fe-safe 2017 TUTORIALS

Transcription

1 fe-safe 2017 TUTORIALS

2

3 Trademarks fe-safe, Abaqus, Isight, Tosca, the 3DS logo, and SIMULIA are commercial trademarks or registered trademarks of Dassault Systèmes or its subsidiaries in the United States and/or other countries. Use of any Dassault Systèmes or its subsidiaries trademarks is subject to their express written approval. Other company, product, and service names may be trademarks or service marks of their respective owners. Legal Notices fe-safe and this documentation may be used or reproduced only in accordance with the terms of the software license agreement signed by the customer, or, absent such an agreement, the then current software license agreement to which the documentation relates. This documentation and the software described in this documentation are subject to change without prior notice. Dassault Systèmes and its subsidiaries shall not be responsible for the consequences of any errors or omissions that may appear in this documentation. Dassault Systèmes Simulia Corp, 2016.

4 Third-Party Copyright Notices Certain portions of fe-safe contain elements subject to copyright owned by the entities listed below. Battelle Endurica LLC Amec Foster Wheeler Nuclear UK Limited fe-safe Licensed Programs may include open source software components. Source code for these components is available if required by the license. The open source software components are grouped under the applicable licensing terms. Where required, links to common license terms are included below. IP Asset Name IP Asset Version Copyright Notice Under BSD 2-Clause UnZip Info-ZIP) (from 2.4 Copyright (c) Info-ZIP. All rights reserved. Under BSD 3-Clause Qt Solutions 2.6 Copyright (c) 2014 Digia Plc and/or its subsidiary(-ies) All rights reserved.

5 Tutorial 101 : Importing ASCII data in fe-safe 101 Tutorial 101 : Importing ASCII data into fe-safe To create an ASCII file, use a text editor. Create a two column ASCII file by entering the following sequence of numbers: Save the file as test1.asc and exit. Start fe-safe by selecting fe-safe from the Windows Start menu (Windows) or by running the script fe-safe (UNIX). Select an existing project, or create a new one from the welcome page Select Open Data File from the Data Files section of the File menu and open the created data file test1.asc. The two signals in the ASCII file will be added to the list of open data files as shown in Figure Figure Volume 1 Tutorial Vol. 1 Section 101 Issue: 15 Date:

6 Tutorial 101 : Importing ASCII data in fe-safe Select these two signals and then press the Stack Plot(s) button in Figure as shown below. in the main toolbar. This will display the plots Figure Volume 1 Tutorial Vol. 1 Section 101 Issue: 15 Date:

7 Tutorial 102 : Peak picking histories 102 Tutorial 102 : Peak picking histories After completing tutorial 101 you will now have 2 time histories stored in the data file test1.asc. These can be rationalised using the multichannel peak-picking function as described in section 10. Ensure that the data file test1.asc is loaded into the list of open data files as shown in Figure Figure Select both of the data signals and from the Amplitude menu item select the Multi-channel Peak Valley function. This will display the dialog as shown in Figure Figure Select a Gate of 10 and enable the Add time information as an additional results signal check box and press OK to start the peak picking process. Vol. 1 Section 102 Issue: 17 Date: Volume 1 Tutorial 102-1

8 Tutorial 102 : Peak picking histories After the analysis is completed the peak picked data signals will be added to the Generated Results section in the Loaded Data Files window as shown in Figure Figure This will have reduced the 2 time histories to 6 points per signal. To view the data select the 3 new signals and select View >> Stack Plot(s). Figure Volume 1 Tutorial Vol. 1 Section 102 Issue: 17 Date:

9 Tutorial 102 : Peak picking histories The X-axis shows the time basis for the new files, based on the originals. To compare the original to the new file, select each history corresponding to signal #1 as shown in Figure Figure Select View >> Stack Plot(s): Figure Vol. 1 Section 102 Issue: 17 Date: Volume 1 Tutorial 102-3

10 Tutorial 102 : Peak picking histories Finally, select View >> Numerical Listing: Figure As can be seen samples 4 and 5 from the original data signal was omitted as they were not peaks or valleys on either of the data signals. Volume 1 Tutorial Vol. 1 Section 102 Issue: 17 Date:

11 103 This tutorial has been intentionally removed

12

13 Tutorial 104 : Using fe-safe with I-DEAS universal (UNV) files 104 Tutorial 104 : Using fe-safe with I-DEAS universal.unv files Introduction The tutorials in this section demonstrate the use of fe-safe with I-DEAS universal (.unv) files, using a Brown-Miller strain-based fatigue algorithm to evaluate the fatigue life of a uniaxial FE stress solution. The use of I-DEAS.unv files in fe-safe is discussed in detail in Appendix G. The sample files used for this tutorial are located in the directory <DataDir>\Ideas. NOTE: The nomenclature used throughout this tutorial when referring to files and directories is as described in Appendix B Preparation Start the program by selecting fe-safe from the Windows Start menu (Windows) or by running the script fe-safe (Linux). Select an existing project, or create a new one from the welcome page Ensure that the following basic settings are correctly configured. If fe-safe is being run for the first time then it is possible to skip this preparatory section. Volume 1 Tutorial Vol. 1 Section 104 Issue: 15 Date:

14 Tutorial 104 : Using fe-safe with I-DEAS universal (UNV) files Reset any existing analysis options to their defaults in the Clear Data and Settings dialogue [Tools >> Clear Data and Settings...], shown in Figure 104-1, below, by selecting the Select all option and clicking OK. Figure I-DEAS UNV interface options The I-DEAS / Master Series UNV Interface Options dialogue [FEA Fatigue >> I-DEAS / Masterseries UNV Interface Options...] should be configured as shown in Figure 104-2, below. Figure Volume 1 Tutorial Vol. 1 Section 104 Issue: 15 Date:

15 Tutorial 104 : Using fe-safe with I-DEAS universal (UNV) files The sample UNV file contains stress data at element nodes but this option will not be used as pre-scanning will be used Opening the sample FE model The sample model for this tutorial is one quarter of a notched shaft as shown in Figure Figure To open the model, select Open Finite Element Model... from the FEA Solutions section of the File menu. From the file selection dialog, select the sample file shaft_sae.unv from the directory <DataDir>\Ideas. A Pre-Scan File dialogue will be displayed as shown in Figure 104-4, select Yes. Figure As fe-safe pre-scans the model, information about the file is written to the file: <ProjectDir>\Model\scan This information is also displayed in the Message Log window. Volume 1 Tutorial Vol. 1 Section 104 Issue: 15 Date:

16 Tutorial 104 : Using fe-safe with I-DEAS universal (UNV) files When the pre-scan of the file is complete, the Select Datasets to Read dialogue will be displayed as shown in Figure The file shaft_sae.unv contains only two datasets of elemental stresses, both of which are required for the tutorial and will be checked. Select OK to load these checked datasets. Figure As fe-safe loads the model, information about the file and the data it contains is written to the file: <ProjectDir>\Model\reader.log. This information is also displayed in the Message Log window. Volume 1 Tutorial Vol. 1 Section 104 Issue: 15 Date:

17 Tutorial 104 : Using fe-safe with I-DEAS universal (UNV) files When the model has finished loading, the Loaded FEA Models Properties dialogue box appears, as shown in Figure Figure If the dialogue box does not appear automatically, then it can be displayed by right-clicking on the Current FE Models window and selecting Properties. icon in the Figure Volume 1 Tutorial Vol. 1 Section 104 Issue: 15 Date:

18 Tutorial 104 : Using fe-safe with I-DEAS universal (UNV) files Ensure that the units are as shown in Figure 104-6, then click OK. A dialogue will show prompting to edit element groups loaded from the model, as shown in Figure 104-8, click No. Figure A summary of the open model appears in the Current FE Models window, showing the loaded datasets and element group information see Figure Figure Note: if the window does not appear exactly as shown in Figure 104-9, then expand the tree view to show more details. Volume 1 Tutorial Vol. 1 Section 104 Issue: 15 Date:

19 Tutorial 104 : Using fe-safe with I-DEAS universal (UNV) files The process of loading an FE model into fe-safe involves extracting pertinent data from the FE model, and writing it to the working FED folder (see Appendix E). Therefore, the Current FE Models window is a summary of the contents of the working FED folder. In this case there are two stress datasets each containing elemental data with 1426 elements in each dataset. The source of the dataset (the filename of the source FE model, the step, increment and timestamp) are also shown. fe-safe only extracts group information of the same type as the loaded datasets. In this example, the datasets are elemental, so only elemental groups are shown. When a new model is loaded, the output filename automatically defaults to: <ResultsDir>\{source_file_name}Results.{source_file_extension} which in this example is: <ResultsDir>\shaft_saeResults.unv The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button: Exercise Objective: To perform a Brown-Miller strain-based fatigue analysis to evaluate the fatigue life of a uniaxial FE stress solution. The fatigue load case consists of an elastically calculated unit load FEA stress solution (i.e. a stress dataset) and some load history data. The unit load and the load history are combined using a scale-and-combine method, as described in section 13. Analysis process: The fatigue life for each node is calculated as follows: the stress tensors are multiplied by the time history of the applied loading, to produce a time history of each of the 6 components of the stress tensor; the time histories of the in-plane principal stresses are calculated; the time histories of the three principal strains are calculated from the stresses; a multi-axial cyclic plasticity model is used to convert the elastic stress-strain histories into elastic plastic stress-strain histories; a critical plane method is used to identify the most damaging plane by calculating the damage on planes at 10 intervals between 0 and 180 in the surface of the component; for each of the critical planes, strains are resolved onto the three shear planes (1-2, 2-3 and 1-3); the time history of the damage parameter (which in this case, using the Brown-Miller algorithm, is the shear and normal strain) is cycle counted; individual fatigue cycles are identified using a Rainflow cycle algorithm, the fatigue damage for each cycle is calculated and the total damage is summed; the plane with the shortest life defines the plane of crack initiation, and this life is written to the output file. Volume 1 Tutorial Vol. 1 Section 104 Issue: 15 Date:

20 Tutorial 104 : Using fe-safe with I-DEAS universal (UNV) files During this calculation, fe-safe may modify the endurance limit amplitude. If all cycles (on a plane) are below the endurance limit amplitude, there is no calculated fatigue damage on this plane. If any cycle is damaging, the endurance limit amplitude is reduced to 25% of the constant amplitude value, and the damage curve extended to this new endurance limit. The critical plane method is described and illustrated in detail in the Fatigue Theory Reference Manual. Method: Step 1: Define the loading: The fatigue loading will consist of a unit load stress dataset, combined with a loading history containing five data points: To define the loading: select the Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; select Clear all loadings and click Yes from the tree context menu (right mouse click on the tree) to clear the existing loading definition; create a loading history file by copying the above text into a text editor; ensure that the last line is followed by a carriage-return/line-feed character (see Appendix E); save the file as t104_ex1.txt; open the file in fe-safe using File >> Data Files >> Open Data File... this adds the file to the Loaded Data Files window; in the Loaded Data Files window, highlight the first channel of data, labelled #1 (next to the channel icon ); in the Current FE Models window, highlight the first dataset, labelled Dataset 1: (1.0) S : FORWARD BEND, MODEL_SOLUTION_SOLVE, LOAD SET 1, (next to the stress dataset icon, ); select Add... >> A LOAD * dataset; A prompt will ask if a new block should be created, click Yes Figure Volume 1 Tutorial Vol. 1 Section 104 Issue: 15 Date:

21 Tutorial 104 : Using fe-safe with I-DEAS universal (UNV) files The defined loading appears in the loading details list box, as shown below: Figure Note: if the window does not appear exactly as shown in Figure , then expand the tree view to show more details. select the Analysis Settings tab from the Fatigue from FEA dialogue to switch to the main settings. Step 2: Define the subgroup option: For this tutorial all elements in the model should be used for analysis, not only those on its surface: double-click the Subgroup column header to open the Subgroup Selection dialogue for all groups: Figure select Whole group; click OK. Volume 1 Tutorial Vol. 1 Section 104 Issue: 15 Date:

22 Tutorial 104 : Using fe-safe with I-DEAS universal (UNV) files Step 3: Define the surface finish: It is assumed that the whole component has a mirror-polished surface finish, (i.e. a Kt factor of 1). To define this surface finish for the whole component (i.e. all element groups): double-click the Surface column header to open the Surface Finish Definition dialogue for all groups: Figure select Select Surface Finish from list; click on the browse button,, to open the Select a surface finish file (*.kt) file dialogue; select the surface finish database file default.kt from the <KtDir> directory; from the drop-down Surface finish list, select Mirror Polished Ra <= 0.25µm; click OK. Volume 1 Tutorial Vol. 1 Section 104 Issue: 15 Date:

23 Tutorial 104 : Using fe-safe with I-DEAS universal (UNV) files Step 4: Define the material: The component material is SAE 950C (Manten). The material record SAE_950C-Manten from the material database local.dbase will be defined for the whole component. Opened material databases are displayed in the Material Databases window as shown in Figure , below. Figure If the database local.dbase is not currently loaded in the Material Databases window, select File >> Materials >> Open Materials Database... and select local.dbase from the directory <UserDir>. Notice in Figure that the database local.dbase is the user s local copy from the <UserDir> directory. The other two databases shown are from the <DatabaseDir> directory. Expand the tree view to show the materials contained in local.dbase. The contents of the database can be filtered to show only materials of a particular type, by selecting one of the filter icons. To ensure that all materials in the database are displayed double-click on the All filter icon. The parameters for a material can be displayed by extending the material name. To define SAE_950C-Manten for the whole component: highlight the material SAE_950C-Manten in the local.dbase database; double-click the Material column header - a Change Material? confirmation dialogue box appears; Figure Volume 1 Tutorial Vol. 1 Section 104 Issue: 15 Date:

24 Tutorial 104 : Using fe-safe with I-DEAS universal (UNV) files click YES; the material name should appear for all groups in the Material column. Step 5: Define the analysis algorithm: The material database identifies a default analysis algorithm for each material. The default analysis algorithm is normally selected automatically. To confirm that the default algorithm will be used for the whole model (i.e. all element groups): double-click the Algorithm column header to open the in Group Algorithm Selection dialogue box for all groups; Figure select the Analyse with material s default algorithm option; click OK. For SAE 950C (Manten) the default algorithm is Brown-Miller Biaxial Strain Life using Morrow mean-stress correction. Volume 1 Tutorial Vol. 1 Section 104 Issue: 15 Date:

25 Tutorial 104 : Using fe-safe with I-DEAS universal (UNV) files Step 6: Define the in-plane residual stress: For this exercise it is assumed that there are no in-plane residual stresses. To set the residual stress to 0 (zero) for the whole component (i.e. all element groups): double-click the In-plane residual stress column header to open the In-plane Residual Stress dialogue for all groups: Figure enter a residual stress of 0 (zero), and click OK. Step 7: Define the output file: When the FE model was loaded, the output filename automatically defaulted to: <ResultsDir>\shaft_saeResults.unv The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. Volume 1 Tutorial Vol. 1 Section 104 Issue: 15 Date:

26 Tutorial 104 : Using fe-safe with I-DEAS universal (UNV) files Step 8: Run the analysis: fe-safe should now be configured to run the analysis. Press the Analyse! button. A summary of analysis parameters is displayed: Figure Check that the analysis is configured as shown in Figure , and then click Continue. Note that the UTS of the material is used to evaluate Kt from the defined surface finish curve (i.e. surface finish factor versus UTS). In this case, for a mirror-polished surface, Kt =1 for all values of UTS. As the analysis is being performed, the following information is written to the analysis log file. The analysis log file has the same file name as the output file, except that the extension is.log. So, for this analysis, the analysis log file is: <ResultsDir>\shaft_saeResults.log This information is also displayed in the Message Log window and includes: Summary ======= Worst Life-Repeats : at Element Analysis time : 0:00:08 Volume 1 Tutorial Vol. 1 Section 104 Issue: 15 Date:

27 Tutorial 104 : Using fe-safe with I-DEAS universal (UNV) files Step 9: Reviewing the results The analysis log shows that the worst-case life for the whole model is: 4556 repeats of the fatigue loading cycle, at element 677, node 10. Note: fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). In fe-safe, the design life and the calculated fatigue life always refer to the number of repeats of the complete defined fatigue loading cycle. An optional conversion factor can be used to convert the fatigue life in repeats to fatigue life with respect to some other quantity, for example hours or miles (see section 13.2). Step 10: Viewing the fatigue life contours: The results from this exercise were written to the UNV file: <ResultsDir>/shaft_saeResults.unv The exported fatigue lives should look similar to Figure , below, the viewer colour scheme may need to be set to "Reversed Rainbow" and any averaging of values at nodes should be disabled. Figure : Log of Fatigue Lives Volume 1 Tutorial Vol. 1 Section 104 Issue: 15 Date:

28 Tutorial 104 : Using fe-safe with I-DEAS universal (UNV) files Step 11: Viewing the worst critical plane In the Fatigue from FEA dialogue box press the Exports button. In the Contours tab check the Critical planes (worst block) box, click OK and run the analysis again. The exported critical plane should look similar to Figure , below: Figure : Critical plane normals at worst element scaled by log1e7 lognf Volume 1 Tutorial Vol. 1 Section 104 Issue: 15 Date:

29 Tutorial 105 : Using fe-safe with Abaqus.fil files 105 Tutorial 105 : Using fe-safe with Abaqus.fil files Introduction This tutorial demonstrates the use of fe-safe with Abaqus.fil files. The use of Abaqus.fil files in fe-safe is discussed in detail in Appendix G. The tutorial includes opening the FE model and configuring multi-axial analyses of two superimposed fatigue load cases and of a dataset sequence, including Factors of Strength (FOS) evaluation. The sample files used for this tutorial are located in the directory <DataDir>\Abaqus. ASCII and binary versions of the sample files are available. The ASCII FIL file format is portable between platforms. The binary FIL file format is not portable between platforms. This tutorial uses the ASCII version of the sample FIL file. NOTE: The nomenclature used throughout this tutorial when referring to files and directories is as described in Appendix B Preparation Start the program by selecting fe-safe from the Windows Start menu (Windows) or by running the script fe-safe (Linux). Select an existing project, or create a new one from the welcome page Ensure that the following basic settings are correctly configured. If fe-safe is being run for the first time then it is possible to skip this preparatory section. Volume 1 Tutorial Vo.. 1 Section 105 Issue: 15 Date:

30 Tutorial 105 : Using fe-safe with Abaqus.fil files Reset any existing analysis options to their defaults in the Clear Data and Settings dialogue [Tools >> Clear Data and Settings...], shown in Figure below, by selecting the Check all option and clicking OK. Figure Abaqus FIL interface options The Abaqus FIL interface Options dialogue [FEA Fatigue >> Abaqus FIL interface Options...] should be configured as shown in Figure 105-2, below. Figure Volume 1 Tutorial Vol. 1 Section 105 Issue: 15 Date:

31 Tutorial 105 : Using fe-safe with Abaqus.fil files The sample FIL file contains two different types of stress data: nodal-averaged data and stresses at element nodes. This tutorial uses data for stresses at element nodes. As the model will be pre-scanned selection of the data type is done in the Select Datasets to Read dialogue described below. The FIL interface can import and export data from ASCII and binary FIL files. The sample file for this tutorial is in ASCII format. It is recommended that the Auto Detect format option be used. The type of variable that fe-safe uses to export lives and FOS results to is configured in the Export Lives/FOS to FIL section of the dialogue, found by clicking on the Export tab.. The preferred export variable is UVARM, since this is a variable that most viewers can interpret. If the UVARM variable is specified, both the fatigue life, or log10 (fatigue life), and the FOS are exported to the same step. If any other variable is used, a new step is added for each fe-safe export variable. Patran users should click the Patran As Viewer button. This button automatically changes the following settings: the export variable is set to TEMP [variable 2], because Patran does not support the UVARM variable; the Export logarithmic lives to results file option, Analysis Options dialogue, Export tab, is automatically selected, since Patran will not handle large values (e.g ), that may exist if the fatigue life is exported rather than log10(fatigue life). Volume 1 Tutorial Vo.. 1 Section 105 Issue: 15 Date:

32 Tutorial 105 : Using fe-safe with Abaqus.fil files Opening the sample FE model The model for this tutorial is a plate with a keyhole, as shown in Figure 105-3: Figure To open the model select Open Finite Element Model... from the File menu. This will display the file selection dialogue. Select the sample file keyhole.fil from the directory <DataDir>\Abaqus. A Pre-Scan File dialogue will be displayed as shown in Figure 105-4, select Yes. Figure As fe-safe pre-scans the model, information about the file is written to the file: <ProjectDir>\Model\scan This information is also displayed in the Message Log window. Volume 1 Tutorial Vol. 1 Section 105 Issue: 15 Date:

33 Tutorial 105 : Using fe-safe with Abaqus.fil files When the pre-scan of the file is complete, the Select Datasets to Read dialogue will be displayed as shown in Figure The file keyhole.fil contains only two datasets of elemental stresses, both of which are required for the tutorial and will be checked. Select OK to load these checked datasets. Figure As fe-safe loads the model, information about the file and the data it contains is appended to the file: <ProjectDir>\Model\reader.log. This information is also displayed in the Message Log window. Volume 1 Tutorial Vo.. 1 Section 105 Issue: 15 Date:

34 Tutorial 105 : Using fe-safe with Abaqus.fil files When the model has finished loading, the Loaded FEA Models Properties dialogue box appears, as shown in Figure Figure If the dialogue box does not appear automatically, then it can be displayed by right-clicking on the Current FE Models window and selecting Properties. icon in the Figure Volume 1 Tutorial Vol. 1 Section 105 Issue: 15 Date:

35 Tutorial 105 : Using fe-safe with Abaqus.fil files Ensure that the units are as shown in Figure 105-6, then click OK. A dialogue will show prompting to edit element groups loaded from the model, as shown in Figure 105-8, click No. Figure A summary of the open model appears in the Current FE Models window, showing the loaded datasets and element group information see Figure Figure Note: if the window does not appear exactly as shown in Figure 105-9, then expand the tree view to show more details. Volume 1 Tutorial Vo.. 1 Section 105 Issue: 15 Date:

36 Tutorial 105 : Using fe-safe with Abaqus.fil files The process of loading an FE model into fe-safe involves extracting pertinent data from the FE model, and writing it to the working FED folder (see Appendix E). Therefore, the Current FE Models window is a summary of the contents of the working FED folder. In this case there are two stress datasets each containing elemental data with 502 elements in each dataset. The source of the dataset (the filename of the source FE model, the step, increment and timestamp) are also shown. fe-safe only extracts group information of the same type as the loaded datasets. In this example, the datasets are elemental, so only elemental groups are shown. When a new model is loaded, the output filename automatically defaults to: <ResultsDir>\{source_file_name}Results.{source_file_extension} which in this example is: <ResultsDir>\keyholeResults.fil The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button: Exercise 1 : Multiaxial analysis using scale-and-combine loading Objective: To perform a multiaxial analysis of two superimposed fatigue load cases. Each load case consists of an elastically calculated unit load FEA stress solution (i.e. a stress dataset) and some load history data. The unit load and the load history are combined using a scale-and-combine method, as described in section 13. Analysis process: The fatigue life for each node is calculated as follows: the stress tensors are multiplied by the time history of the applied loading, to produce a time history of each of the 6 components of the stress tensor; the time histories of the in-plane principal stresses are calculated; the time histories of the three principal strains are calculated from the stresses; a multiaxial cyclic plasticity model is used to convert the elastic stress-strain histories into elastic plastic stressstrain histories; a critical plane method is used to identify the most damaging plane by calculating the damage on planes at 10 intervals between 0 and 180 in the surface of the component; for each of the critical planes, strains are resolved onto the three shear planes (1-2, 2-3 and 1-3); the time history of the damage parameter (which in this case, using the Brown-Miller algorithm, is the shear and normal strain) is cycle counted; individual fatigue cycles are identified using a Rainflow cycle algorithm, the fatigue damage for each cycle is calculated and the total damage is summed; the plane with the shortest life defines the plane of crack initiation, and this life is written to the output file. Volume 1 Tutorial Vol. 1 Section 105 Issue: 15 Date:

37 Tutorial 105 : Using fe-safe with Abaqus.fil files During this calculation, fe-safe may modify the endurance limit amplitude. If all cycles (on a plane) are below the endurance limit amplitude, there is no calculated fatigue damage on this plane. If any cycle is damaging, the endurance limit amplitude is reduced to 25% of the constant amplitude value, and the damage curve extended to this new endurance limit. The critical plane method is described and illustrated in detail in Volume 2. Method: Step 1: Define the loading: For this exercise two fatigue load cases will be superimposed. Each load case will consist of an elastically calculated unit load stress dataset and some load history data, as follows: the first dataset (Dataset 1: (1.1) S : Unit Y Load) will be combined with channel 1 of the data file test_mcg2.amc; the second dataset (Dataset 2: (2.1) S : Unit X Load) will be combined with channel 2 of the data file test_mcg2.amc. To open the loading history data, select Open Data File from the File menu. Use the file selection dialogue to select the sample file test_mcg2.amc from the <DataDir> directory. The data file is summarised in the Loaded Data Files window. The sample file contains two channels of load data, identified in the tree view by the channel icon,. Figure To combine the unit load stress dataset with the loading history for the first case: in the Current FE Models window, highlight the first dataset, labelled Dataset 1: (1.1) S : Unit Y Load, (next to the stress dataset icon, ); in the Loaded Data Files window, highlight the first channel of data, labelled fe-safe tutorial scaler #1, (next to the channel icon ); select the Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; select Clear all loadings from the context-sensitive menu (right mouse click) to clear the existing loading definition; select Add... >> A LOAD * dataset. A prompt will ask if a new block should be created, click Yes Volume 1 Tutorial Vo.. 1 Section 105 Issue: 15 Date:

38 Tutorial 105 : Using fe-safe with Abaqus.fil files To combine the unit load stress dataset with the loading history for the second case: in the Current FE Models window, highlight the second dataset, labelled Dataset 2: (2.1) S : Unit X Load, (next to the stress dataset icon, ); in the Loaded Data Files window, highlight the second channel of data, labelled fe-safe tutorial scaler #2, (next to the channel icon ); select Add... >> A LOAD * dataset; The defined loading appears in the loading details list box, as shown below: Figure Note: if the window does not appear exactly as shown in Figure , then expand the tree view to show more details. select the Analysis Settings tab from the Fatigue from FEA dialogue to switch to the main settings. Step 2: Define the subgroup option: For this tutorial all elements in the model should be used for analysis, not only those on its surface: double-click the Subgroup column header to open the Subgroup Selection dialogue for all groups: Figure Volume 1 Tutorial Vol. 1 Section 105 Issue: 15 Date:

39 Tutorial 105 : Using fe-safe with Abaqus.fil files select Whole group; click OK. Step 3: Define the surface finish: It is assumed that the whole component has a mirror-polished surface finish, (i.e. a Kt factor of 1). To define this surface finish for the whole component (i.e. all element groups): double-click the Surface column header to open the Surface Finish Definition dialogue for all groups: Figure select Select Surface Finish from list; click on the browse button,, to open the Select a surface finish file (*.kt) file dialogue; select the surface finish database file default.kt from the <KtDir> directory; from the drop-down Surface finish list, select Mirror Polished Ra <= 0.25µm; click OK. Volume 1 Tutorial Vo.. 1 Section 105 Issue: 15 Date:

40 Tutorial 105 : Using fe-safe with Abaqus.fil files Step 4: Define the material: The component material is SAE 950C (Manten). The material record SAE_950C-Manten from the material database local.dbase will be defined for the whole component. Opened material databases are displayed in the Material Databases window as shown in Figure , below. Figure If the database local.dbase is not currently loaded in the Material Databases window, select File >> Open Materials Database... and select local.dbase from the directory <UserDir>. Notice in Figure that the database local.dbase is the user s local copy from the <UserDir> directory. The other two databases shown are from the <DatabaseDir> directory. Expand the tree view to show the materials contained in local.dbase. The contents of the database can be filtered to show only materials of a particular type, by selecting one of the filter icons. To ensure that all materials in the database are displayed double-click on the All filter icon. The parameters for a material can be displayed by expanding the material name. To define SAE_950C-Manten for the whole component: highlight the material SAE_950C-Manten in the local.dbase database; double-click the Material column header - a Change Material? confirmation dialogue box appears; Figure click YES; the material name should appear for all groups in the Material column. Volume 1 Tutorial Vol. 1 Section 105 Issue: 15 Date:

41 Tutorial 105 : Using fe-safe with Abaqus.fil files Step 5: Define the analysis algorithm: The material database identifies a default analysis algorithm for each material. The default analysis algorithm is normally selected automatically. To confirm that the default algorithm will be used for the whole model (i.e. all element groups): double-click the Algorithm column header to open the in Group Algorithm Selection dialogue box for all groups; Figure select the Analyse with material s default algorithm option; click OK. For SAE 950C (Manten) the default algorithm is Brown-Miller Biaxial Strain Life using Morrow mean-stress correction. Volume 1 Tutorial Vo.. 1 Section 105 Issue: 15 Date:

42 Tutorial 105 : Using fe-safe with Abaqus.fil files Step 6: Define the in-plane residual stress: For this exercise it is assumed that there are no in-plane residual stresses. To set the residual stress to 0 (zero) for the whole component (i.e. all element groups): double-click the In-plane residual stress column header to open the In-plane Residual Stress dialogue for all groups: Figure enter a residual stress of 0 (zero), and click OK. Step 7: Define the output file: When the FE model was loaded, the output filename automatically defaulted to: <ResultsDir>\keyholeResults.fil Before running the analysis, change the output filename to: <ResultsDir>\keyholeResults_ex01.fil The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. Volume 1 Tutorial Vol. 1 Section 105 Issue: 15 Date:

43 Tutorial 105 : Using fe-safe with Abaqus.fil files Step 8: Run the analysis: fe-safe should now be configured to run the analysis. Press the Analyse! button. A summary of analysis parameters is displayed: Figure Check that the analysis is configured as shown in Figure , and then click Continue. Note that the UTS of the material is used to evaluate Kt from the defined surface finish curve (i.e. surface finish factor versus UTS). In this case, for a mirror-polished surface, Kt =1 for all values of UTS. As the analysis is being performed, the following information is written to the analysis log file. The analysis log file has the same file name as the output file, except that the extension is.log. So, for this analysis, the analysis log file is: <ResultsDir>\keyholeResults_ex01.log This information is also displayed in the Message Log window and includes. Summary ======= Worst Life-Repeats : at Element Analysis time : 0:00:03 Volume 1 Tutorial Vo.. 1 Section 105 Issue: 15 Date:

44 Tutorial 105 : Using fe-safe with Abaqus.fil files Step 9: Reviewing the results The analysis log shows that the worst-case life for the whole model is: repeats of the fatigue loading cycle, at element 144, node 2. Note: fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). In fe-safe, the design life and the calculated fatigue life always refer to the number of repeats of the complete defined fatigue loading cycle. An optional conversion factor can be used to convert the fatigue life in repeats to fatigue life with respect to some other quantity, for example hours or miles (see section 13). Step 10: Viewing the fatigue life contours: A copy of the original.fil file was created, onto which a new step containing the fatigue results was appended. The type of variable that the results are exported to will depend on the configuration in the Abaqus FIL Interface Options dialogue. In the last step of the file <ResultsDir>/keyholeResults_ex01.fil, the results for the exported variable should look similar to Figure , the viewer colour scheme may need to be set to "Reversed Rainbow" and any averaging of values at nodes should be disabled. Figure : Log of Fatigue Lives. Volume 1 Tutorial Vol. 1 Section 105 Issue: 15 Date:

45 Tutorial 105 : Using fe-safe with Abaqus.fil files Additional notes for Exercise 1: 1. In this exercise, the two fatigue load cases are superimposed. Therefore, it does not matter in which order the loads are defined. For example: Loading is the same as: Loading Loading is 1 Repeats DS#1 * test_mcg2.amc:1 DS#2 * test_mcg2.amc:2 Loading is 1 Repeats DS#2 * test_mcg2.amc:2 DS#1 * test_mcg2.amc:1 2. In this example, the load history is very short, consisting of only five data points. For short load histories it is often more convenient to define the loading using a user-defined load history, rather than reading a load history from a data file (see section ). This is achieved using the A user-defined LOAD * dataset option. To re-define the loading for this exercise using user-defined load histories: select the Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; select Clear all loadings and click Yes from the context-sensitive menu (right mouse click) to clear the existing loading definition; in the Loaded Data Files window, expand the filename test_mcg2.amc, so that both channels of data are displayed; highlight both channels of data (to select multiple channels highlight the first channel by clicking on it with the left mouse button, then hold down the CTRL key on the keyboard while clicking on any additional files); display a numerical listing of the two data channels by selecting View >> Numerical Listing (or just click the icon): Figure Volume 1 Tutorial Vo.. 1 Section 105 Issue: 15 Date:

46 Tutorial 105 : Using fe-safe with Abaqus.fil files highlight the first unit stress dataset (labelled Dataset 1: (1.1) S : Unit Y Load) in the Current FE Models window; select Add... >> A user-defined LOAD * dataset to display the Dataset Embedded Load History dialogue, and copy the five data points from the first column of the numerical listing display (scaler #1) into the Loading Scale box: Figure click OK; highlight the second unit stress dataset (labelled Dataset 2: (2.1) S : Unit X Load) in the Current FE Models window; define a load sequence for the second case, as described above, using the data from the second column of the numerical listing display (scaler #2). The new loading definition appears in the Loading Details area of the Fatigue from FEA dialogue, as shown in Figure , below. Figure Note: if the window does not appear exactly as shown in Figure , then expand the tree view to Volume 1 Tutorial Vol. 1 Section 105 Issue: 15 Date:

47 Tutorial 105 : Using fe-safe with Abaqus.fil files show more details. 3. The load definition (LDF) file can be used to define simple and complex loading scenarios. Section 13 includes a full description of the LDF file, including syntax. The loading for this exercise can be seen by saving the loading to a load definition file: select File >> Loadings >> Save Current FEA Loadings As...; save the file as ex01_s-c.ldf and click Save; open the file in a text editor to display the contents (comments may vary): #.ldf file created by fe-safe [mswin] INIT END # Block number 1 BLOCK lh= , ds=1 lh= , ds=2 END 4. In this exercise the surface finish was defined by selecting a surface type (in this case mirror-polished ) from a surface finish database. If the actual surface finish factor, Kt, for the component is known (for mirror-polished, the Kt factor has a value of 1) then it can be specified as a value. To define a userdefined value for Kt, select Define Kt as a value, in the Surface Finish Definition dialogue box: Figure The results data can be exported to an alternative file format at the end of the analysis, by changing the extension of the output file (Fatigue from FEA >> Output File) to a recognised type. Volume 1 Tutorial Vo.. 1 Section 105 Issue: 15 Date:

48 Tutorial 105 : Using fe-safe with Abaqus.fil files For example: to export to an ASCII CSV results file, change the extension to.txt,.csv or.asc (this is useful for viewing a table of results in an editor or spreadsheet). Alternatively, after the analysis is complete, and the FIL file has been created, the results data can be written to another output file in addition to the original output FIL file, using the Save FEA Fatigue Results As... option in the File menu. This option displays the Save FEA Fatigue Results As... dialogue box, as shown in Figure , below: Figure The FER (.fer) file (see Appendix E) is an intermediate file containing the results of the analysis. This new output file type is determined by the extension of the file entered in the Output File box. A copy of the original output FIL file can be created if the extension.fil is used. 6. To analyse individual elements or nodes, list the required items in the Exports and Outputs dialogue, and select the Only analyse listed items dialogue. Additional outputs and diagnostics options can also be specified. Diagnostics and additional outputs are discussed in detail in section To save the current analysis configuration, select Save FEA Fatigue Definition File..., and enter a filename ending with the extension.stlx. The analysis can be reloaded at a later date by restoring the keyword file, using Open FEA Fatigue Definition File Exercise 2 : Multiaxial analysis of a data sets sequence, including Factor Of Strength evaluation Volume 1 Tutorial Vol. 1 Section 105 Issue: 15 Date:

49 Tutorial 105 : Using fe-safe with Abaqus.fil files Objective: To perform a multiaxial analysis of a series of events in this case a sequence of two elastically calculated FEA stress solution (i.e. stress datasets). The analysis will also include an evaluation of the Factor of Strength (FOS). This is the factor by which the loading must be scaled to achieve a specified design life. The FOS method is described in detail in section 17. Analysis process: The Strength Factor (FOS) for each node is calculated as follows: the calculated life is compared with the design life: - if the calculated life is lower than the design life, the elastic stresses at the node are scaled by a factor less than 1.0; - if the calculated life is greater than the design life, the elastic stresses at the node are scaled by a factor greater than 1.0. the elastic stress history is recalculated using the re-scaled nodal stresses; for local strain analysis, the cyclic plasticity model is used to recalculate the time history of elastic-plastic stress-strains - the fatigue life is then recalculated; in the critical plane analysis, the critical plane orientation is re-calculated; the process is repeated with different scale factors until: (i) (ii) the calculated life is within 5% of the design life or the step change of 0.01 or 0.1 in the FOS value causes the design life to be bracketed, or (iii) the FOS exceeds the max factor (default 2.0) or is less than the min factor (default 0.5). Method: Step 1: Define the loading: The series of events being analysed in this exercise consists of a sequence of two elastically calculated FEA stress solution (i.e. stress datasets) scaled by a defined scale factor. The definition of the sequence will be as follows: the first dataset (Dataset 1: (1.1) S : Unit Y Load) multiplied by a scale factor of 10000, followed by: the second dataset (Dataset 2: (2.1) S : Unit X Load) multiplied by a scale factor of The loading for this loading sequence can be defined in a single loading block: select Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; select Clear all loadings and click Yes from the tree context menu (right mouse click on the tree) to clear the existing loading definition; highlight the first unit stress dataset in the Current FE Models window; Volume 1 Tutorial Vo.. 1 Section 105 Issue: 15 Date:

50 Tutorial 105 : Using fe-safe with Abaqus.fil files select Add... >> Dataset; highlight the second unit stress dataset in the Current FE Models window; select Add... >> Dataset; highlight the dataset item in the loading tree of the Fatigue from FEA dialogue; select Scale from the tree context menu (right mouse click on the tree) and enter the value 10000; press enter to accept the value. If saved as a.ldf it would look like: #.ldf file created by fe-safe [mswin] INIT END # Block number 1 BLOCK ds=1, scale=10000 ds=2, scale=10000 END The new loading definition appears in the Loading Details area of the Fatigue from FEA dialogue, as shown in Figure Figure select the Analysis Settings tab from the Fatigue from FEA dialogue to switch to the main settings. Volume 1 Tutorial Vol. 1 Section 105 Issue: 15 Date:

51 Tutorial 105 : Using fe-safe with Abaqus.fil files Step 2: Define the subgroup option: As in Exercise 1, all elements in the model should be used for analysis - see (Exercise 1), Step 2. Step 3: Define the surface finish: As in Exercise 1, the component is assumed to have a mirror-polished surface finish, (i.e. a Kt factor of 1) - see (Exercise 1), Step 3. Step 4: Define the material: As in Exercise 1, the component is assumed to be made from SAE 950C (Manten) see (Exercise 1), Step 4. Step 5: Define the analysis algorithm: As in Exercise 1, the default analysis algorithm for the material will be used, which for SAE 950C (Manten) is Brown-Miller Biaxial Strain Life using Morrow mean-stress correction. Step 6: Define the in-plane residual stress: As in Exercise 1, it is assumed that there are no in-plane residual stresses - see (Exercise 1), Step 6. Step 7: Configuring the Factor of Strength (FOS) analysis: To configure the Factor of Strength (FOS) analysis: click on the Factor of Strength... button in the Fatigue from FEA window to open the Factors of Strength Calculations dialogue box: Figure select the Perform Factor of Strength (FOS) Calculations? option to enable the FOS analysis.; Volume 1 Tutorial Vo.. 1 Section 105 Issue: 15 Date:

52 Tutorial 105 : Using fe-safe with Abaqus.fil files select Infinite design life (use material s Endurance Limit) this uses the constant amplitude endurance limit for the component material, which for SAE 950C (Manten) is: reversals; Note: fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). click OK; specify the FOS band limits in the Analysis Options dialogue [FEA Fatigue >> Analysis Options...] Safety Factors tab as shown in Figure , to determine the limits and precision of the FOS analysis: - between the fine limits, the FOS is calculated to a resolution of approximately 0.01 repeats; - between maximum and minimum, the FOS is calculated to a resolution of approximately 0.1 repeats; - if the evaluated FOS is greater than 2, then a FOS of 2 is exported for the node; - if the evaluated FOS is less than 0.5, then a FOS of 0.5 is exported for the node. Figure Step 8: Define the output file: Before running the analysis, change the output filename to: <ResultsDir>\keyholeResults_ex02.fil The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. Volume 1 Tutorial Vol. 1 Section 105 Issue: 15 Date:

53 Tutorial 105 : Using fe-safe with Abaqus.fil files Step 9: Run the analysis: fe-safe should now be configured to run the analysis. Press the Analyse! button. A summary of analysis parameters is displayed: Figure Check that the analysis is configured as shown in Figure , and then click Continue. Note that the UTS of the material is used to evaluate Kt from the defined surface finish curve (i.e. surface finish factor versus UTS). In this case, for a mirror-polished surface, Kt =1 for all values of UTS. As the analysis is being performed, the following information is written to the analysis log file. The analysis log file has the same file name as the output file, except that the extension is.log. So, for this analysis, the analysis log file is: <ResultsDir>\keyholeResults_ex02.log This information is also displayed in the Message Log window and includes the following: Summary ======= Worst Life-Repeats : at Element 67.2 Worst FOS@Life=Infinite : at Element 65.3 Analysis time : 0:00:05 Volume 1 Tutorial Vo.. 1 Section 105 Issue: 15 Date:

54 Tutorial 105 : Using fe-safe with Abaqus.fil files Step 10: Reviewing the results The analysis log shows that the worst-case life for the whole model is: repeats of the loading, at element 67, node 2. The worst-case Factor of Strength (FOS) for the analysis is: at element 65, node 3. In the configuration of the Factor of Strength analysis, the design life specified was the Infinite design life, which is assumed to be the materials constant amplitude endurance limit, which for SAE 950C (Manten) is: reversals. The worst-case fatigue lives are of the order repeats of the fatigue loading cycle, which is less than the design life ( repeats of the loading). This is why the worst-case strength factor (the factor by which the loading must be scaled to achieve the design life) is somewhat less than 1. The FOS method is described in detail in section 17. Note: fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). In fe-safe, the design life and the calculated fatigue life always refer to the number of repeats of the complete defined fatigue loading cycle. An optional conversion factor can be used to convert the fatigue life in repeats to fatigue life with respect to some other quantity, for example hours or miles (see section 13). Step 11: Viewing the fatigue life contour: A copy of the original.fil file was created, onto which a new step containing the fatigue results was appended. The type of variable that the results are exported to will depend on the configuration in the Abaqus FIL Interface Options dialogue. In this exercise, two fatigue results sets are exported the fatigue life and the strength factor (FOS). If the UVARM export variable is used, then the two sets of results get written as two separate variables in one step. For all other variable types, the two sets of results get written to two separate steps. The results from this exercise were written to the file: <ResultsDir>/keyholeResults_ex02.fil. Volume 1 Tutorial Vol. 1 Section 105 Issue: 15 Date:

55 Tutorial 105 : Using fe-safe with Abaqus.fil files The first set of exported fatigue results in the file contains the fatigue lives, which should look similar to Figure , the viewer colour scheme may need to be set to "Reversed Rainbow" and any averaging of values at nodes should be disabled. Figure Volume 1 Tutorial Vo.. 1 Section 105 Issue: 15 Date:

56 Tutorial 105 : Using fe-safe with Abaqus.fil files The second set of exported fatigue results in the file contains the strength factors (FOS), which should look similar to Figure , the viewer colour scheme may need to be set to "Reversed Rainbow" and any averaging of values at nodes should be disabled. Figure Volume 1 Tutorial Vol. 1 Section 105 Issue: 15 Date:

57 Tutorial 106 : Using fe-safe with Abaqus.odb files 106 Tutorial 106 : Using fe-safe with Abaqus.odb files Introduction This tutorial demonstrates the use of fe-safe with Abaqus.odb files. The use of Abaqus.odb files in fe-safe is discussed in detail in Appendix G. The tutorial includes opening the FE model and configuring multi-axial analyses of two superimposed fatigue load cases and of a dataset sequence, including Factors of Strength (FOS) evaluation. The sample files used for this tutorial are located in the directory <DataDir>\Abaqus. The ODB file format is portable between platforms. NOTE: The nomenclature used throughout this tutorial when referring to files and directories is as described in Appendix B, section Preparation Start the program by selecting fe-safe from the Windows Start menu (Windows) or by running the script fe-safe (Linux) (see section 5.2). Select an existing project, or create a new one from the welcome page Ensure that the following basic settings are correctly configured. If fe-safe is being run for the first time then it is possible to skip this preparatory section. Vol.. 1 Section 106 Issue: 15 Date: Volume 1 Tutorial 106-1

58 Tutorial 106 : Using fe-safe with Abaqus.odb files Reset any existing analysis options to their defaults in the Clear Data and Settings dialogue [Tools >> Clear Data and Settings...], shown in Figure 106-1, below, by selecting the Check all option and clicking OK. Figure Opening the sample FE model The model for this tutorial is a plate with a keyhole, as shown in Figure 106-2: Figure Volume 1 Tutorial Vol. 1 Section 106 Issue: 15 Date:

59 Tutorial 106 : Using fe-safe with Abaqus.odb files To open the model, select Open Finite Element Model... from the FEA Solutions section of the File menu. This will display the file selection dialogue. Select the sample file keyhole_xxx.odb from the directory <DataDir>\Abaqus. A Pre-Scan File dialogue will be displayed as shown in Figure 106-3, select Yes. Figure As fe-safe loads the model, information about the file and the data it contains is written to the file: <ProjectDir>\Model\scan This information is also displayed in the Message Log window. When the pre-scan of the file is complete, the Select Datasets to Read dialogue will be displayed as shown in Figure The file keyhole2016.odb contains four datasets of elemental stresses. The strain and temperature datasets as well as stress datasets for the initial increment do not need to be loaded. Check only the Stresses and Last increment only boxes, click Apply to Dataset List to apply the selection and select OK to load the remaining stress datasets. Figure Vol.. 1 Section 106 Issue: 15 Date: Volume 1 Tutorial 106-3

60 Tutorial 106 : Using fe-safe with Abaqus.odb files As fe-safe loads the model, information about the file and the data it contains is appended to the file: <ProjectDir>\Model\reader.log. This information is also displayed in the Message Log window. When the model has finished loading, the Loaded FEA Models Properties dialogue box appears, as shown in Figure Figure Volume 1 Tutorial Vol. 1 Section 106 Issue: 15 Date:

61 Tutorial 106 : Using fe-safe with Abaqus.odb files If the dialogue box does not appear automatically, then it can be displayed by right-clicking on the Current FE Models window and selecting Properties. icon in the Figure Ensure that the units are as shown in Figure 106-5, then click OK. A dialogue will show prompting to edit element groups loaded from the model, as shown in Figure 106-7, click No. Figure Vol.. 1 Section 106 Issue: 15 Date: Volume 1 Tutorial 106-5

62 Tutorial 106 : Using fe-safe with Abaqus.odb files A summary of the open model appears in the Current FE Models window, showing the loaded datasets and element group information see Figure Figure Note: if the window does not appear exactly as shown in Figure , then expand the tree view to show more details. The process of loading an FE model into fe-safe involves extracting pertinent data from the FE model, and writing it to the working FED folder (see Appendix E). Therefore, the Current FE Models window is a summary of the contents of the working FED folder. In this case there are two stress datasets each containing elemental data with 502 elements in each dataset. The source of the dataset (the filename of the source FE model, the step, increment and timestamp) are also shown fe-safe also extracts group information of the same type as the loaded datasets. In this example, the datasets are elemental, so only elemental groups are shown. When a new model is loaded, the output filename automatically defaults to: <ResultsDir>\{source_file_name}Results.{source_file_extension} which in this example is: <ResultsDir>\keyhole2016Results.odb The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. Volume 1 Tutorial Vol. 1 Section 106 Issue: 15 Date:

63 Tutorial 106 : Using fe-safe with Abaqus.odb files Exercise 1 : Multiaxial analysis using scale-and-combine loading Objective: To perform a multiaxial analysis of two superimposed fatigue load cases. Each load case consists of an elastically calculated unit load FEA stress solution (i.e. a stress dataset) and some load history data. The unit load and the load history are combined using a scale-and-combine method, as described in section 13. Analysis process: The fatigue life for each node is calculated as follows: the stress tensors are multiplied by the time history of the applied loading, to produce a time history of each of the 6 components of the stress tensor; the time histories of the in-plane principal stresses are calculated; the time histories of the three principal strains are calculated from the stresses; a multiaxial cyclic plasticity model is used to convert the elastic stress-strain histories into elastic plastic stressstrain histories; a critical plane method is used to identify the most damaging plane by calculating the damage on planes at 10 intervals between 0 and 180 in the surface of the component; for each of the critical planes, strains are resolved onto the three shear planes (1-2, 2-3 and 1-3); the time history of the damage parameter (which in this case, using the Brown-Miller algorithm, is the shear and normal strain) is cycle counted; individual fatigue cycles are identified using a Rainflow cycle algorithm, the fatigue damage for each cycle is calculated and the total damage is summed; the plane with the shortest life defines the plane of crack initiation, and this life is written to the output file. During this calculation, fe-safe may modify the endurance limit amplitude. If all cycles (on a plane) are below the endurance limit amplitude, there is no calculated fatigue damage on this plane. If any cycle is damaging, the endurance limit amplitude is reduced to 25% of the constant amplitude value, and the damage curve extended to this new endurance limit. The critical plane method is described and illustrated in detail in Volume 2, section 7.5. Method: Step 1: Define the loading: For this exercise two fatigue load cases will be superimposed. Each load case will consist of an elastically calculated unit load stress dataset and some load history data, as follows: the first dataset (Dataset 1: (1.1) S : Unit Y Load) will be combined with channel 1 of the data file test_mcg2.amc; the second dataset (Dataset 2: (2.1) S : Unit X Load) will be combined with channel 2 of the data file test_mcg2.amc. Vol.. 1 Section 106 Issue: 15 Date: Volume 1 Tutorial 106-7

64 Tutorial 106 : Using fe-safe with Abaqus.odb files To open the loading history data, select Open Data File from the Data Files section of the File menu. Use the file selection dialogue to select the sample file test_mcg2.amc from the <DataDir> directory. The data file is summarised in the Loaded Data Files window. The sample file contains two channels of load data, identified in the tree view by the channel icon,. Figure To combine the unit load stress dataset with the loading history for the first case: in the Current FE Models window, highlight the first dataset, labelled Dataset 1: (1.1) S : Unit Y Load, (next to the stress dataset icon, ); in the Loaded Data Files window, highlight the first channel of data, labelled fe-safe tutorial scaler #1, (next to the channel icon ); select the Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; select Clear all loadings from the context-sensitive menu (right click) to clear the existing loading definition; select Add... >> A LOAD * dataset. To combine the unit load stress dataset with the loading history for the second case: in the Current FE Models window, highlight the second dataset, labelled Dataset 2: (2.1) S : Unit X Load, (next to the stress dataset icon, ); in the Loaded Data Files window, highlight the second channel of data, labelled fe-safe tutorial scaler #2, (next to the channel icon ). select Add... >> A LOAD * dataset. Volume 1 Tutorial Vol. 1 Section 106 Issue: 15 Date:

65 Tutorial 106 : Using fe-safe with Abaqus.odb files The defined loading appears in the loading details list box, as shown below: Figure Note: if the window does not appear exactly as shown in Figure , then expand the tree view to show more details. select the Analysis Settings tab from the Fatigue from FEA dialogue to switch to the main settings. Step 2: Define the subgroup option: For this tutorial all elements in the model should be used for analysis, not only those on its surface: double-click the Subgroup column header to open the Subgroup Selection dialogue for all groups: Figure select Whole group; click OK. Vol.. 1 Section 106 Issue: 15 Date: Volume 1 Tutorial 106-9

66 Tutorial 106 : Using fe-safe with Abaqus.odb files Step 3: Define the surface finish: It is assumed that the whole component has a mirror-polished surface finish, (i.e. a Kt factor of 1). To define this surface finish for the whole component (i.e. all element groups): double-click the Surface column header to open the Surface Finish Definition dialogue for all groups: Figure select Select Surface Finish from list; click on the browse button,, to open the Select a surface finish file (*.kt) file dialogue; select the surface finish database file default.kt from the <KtDir> directory; from the drop-down Surface finish list, select Mirror Polished Ra <= 0.25µm; click OK. Volume 1 Tutorial Vol. 1 Section 106 Issue: 15 Date:

67 Tutorial 106 : Using fe-safe with Abaqus.odb files Step 4: Define the material: The component material is SAE 950C (Manten). The material record SAE_950C-Manten from the material database local.dbase will be defined for the whole component. Opened material databases are displayed in the Material Databases window as shown in Figure , below. Figure If the database local.dbase is not currently loaded in the Material Databases window, select File >> Materials >> Open Materials Database... and select local.dbase from the directory <UserDir>. Notice in Figure that the database local.dbase is the user s local copy from the <UserDir> directory. The other two databases shown are from the <DatabaseDir> directory. Expand the tree view to show the materials contained in local.dbase. The contents of the database can be filtered to show only materials of a particular type, by selecting one of the filter icons. To ensure that all materials in the database are displayed double-click on the All filter icon. The parameters for a material can be displayed by expanding the material name. To define SAE_950C-Manten for the whole component: highlight the material SAE_950C-Manten in the local.dbase database; double-click the Material column header - a Change Material? confirmation dialogue box appears; Figure click YES; the material name should appear for all groups in the Material column. Vol.. 1 Section 106 Issue: 15 Date: Volume 1 Tutorial

68 Tutorial 106 : Using fe-safe with Abaqus.odb files Step 5: Define the analysis algorithm: The material database identifies a default analysis algorithm for each material. The default analysis algorithm is normally selected automatically. To confirm that the default algorithm will be used for the whole model (i.e. all element groups): double-click the Algorithm column header to open the in Group Algorithm Selection dialogue box for all groups; Figure select the Analyse with material s default algorithm option; click OK. For SAE 950C (Manten) the default algorithm is Brown-Miller Biaxial Strain Life using Morrow mean-stress correction. Step 6: Define the in-plane residual stress: For this exercise it is assumed that there are no in-plane residual stresses. To set the residual stress to 0 (zero) for the whole component (i.e. all element groups): double-click the In-plane residual stress column header to open the In-plane Residual Stress dialogue for all groups: Figure enter a residual stress of 0 (zero), and click OK. Volume 1 Tutorial Vol. 1 Section 106 Issue: 15 Date:

69 Tutorial 106 : Using fe-safe with Abaqus.odb files Step 7: Define the output file: When the FE model was loaded, the output filename automatically defaulted to: <ResultsDir>\keyhole2016Results.odb Before running the analysis, change the output filename to: <ResultsDir>\keyhole2016Results_ex01.odb The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. Step 8: Run the analysis: fe-safe should now be configured to run the analysis. Press the Analyse button. A summary of analysis parameters is displayed: Figure Check that the analysis is configured as shown in Figure , and then click Continue. Note that the UTS of the material is used to evaluate Kt from the defined surface finish curve (i.e. surface finish factor versus UTS). In this case, for a mirror-polished surface, Kt =1 for all values of UTS. Vol.. 1 Section 106 Issue: 15 Date: Volume 1 Tutorial

70 Tutorial 106 : Using fe-safe with Abaqus.odb files As the analysis is being performed, the following information is written to the analysis log file. The analysis log file has the same file name as the output file, except that the extension is.log. So, for this analysis, the analysis log file is: <ResultsDir>\keyhole2016Results_ex01.log This information is also displayed in the Message Log window and includes: Summary ======= Worst Life-Repeats : at Element [0]144.2 Analysis time : 0:00:00 Step 9: Reviewing the results The analysis log shows that the worst-case life for the whole model is: repeats of the fatigue loading cycle, at element 144, node 2. Note: fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). In fe-safe, the design life and the calculated fatigue life always refer to the number of repeats of the complete defined fatigue loading cycle. An optional conversion factor can be used to convert the fatigue life in repeats to fatigue life with respect to some other quantity, for example hours or miles (see section 13). Step 10: Viewing the fatigue life contours: A copy of the original.odb file was created, onto which a new step containing the fatigue results was appended. The type of variable that the results are exported to will depend on the configuration in the Abaqus ODB Interface Options dialogue (see 106.2, above). Volume 1 Tutorial Vol. 1 Section 106 Issue: 15 Date:

71 Tutorial 106 : Using fe-safe with Abaqus.odb files In the last step of the file <ResultsDir>/keyhole2016Results_ex01.odb, the results for the exported variable should look similar to Figure , the viewer colour scheme may need to be set to "Reversed Rainbow" and any averaging of values at nodes should be disabled. Figure : Log of Fatigue Lives. Vol.. 1 Section 106 Issue: 15 Date: Volume 1 Tutorial

72 Tutorial 106 : Using fe-safe with Abaqus.odb files Additional notes for Exercise 1: 1. In this exercise, the two fatigue load cases are superimposed. Therefore, it does not matter in which order the loads are defined. For example: Loading is the same as: Loading Loading is 1 Repeats DS#1 * test_mcg2.amc:1 DS#2 * test_mcg2.amc:2 Loading is 1 Repeats DS#2 * test_mcg2.amc:2 DS#1 * test_mcg2.amc:1 2. In this example, the load history is very short, consisting of only five data points. For short load histories it is often more convenient to define the loading using a user-defined load history, rather than reading a load history from a data file (see section ). This is achieved using the A user-defined LOAD * dataset option. To re-define the loading for this exercise using user-defined load histories: select the Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; select Clear all loadings from the context sensitive menu (right-click) to clear the existing loading definition; in the Loaded Data Files window expand the filename test_mcg2.amc, so that both channels of data are displayed; highlight both channels of data (to select multiple channels highlight the first channel by clicking on it with the left mouse button, then hold down the CTRL key on the keyboard while clicking on any additional files); display a numerical listing of the two data channels by selecting View >> Numerical Listing (or just click the icon): Figure Volume 1 Tutorial Vol. 1 Section 106 Issue: 15 Date:

73 Tutorial 106 : Using fe-safe with Abaqus.odb files highlight the first unit stress dataset (labelled Dataset 1: (1.1) S : Unit Y Load) in the Current FE Models window; select Add... >> A user-defined LOAD * dataset to display the Dataset Embedded Load History dialogue, and copy the five data points from the first column of the numerical listing display (scaler #1) into the Loading Scale box: Figure click OK; highlight the second unit stress dataset (labelled Dataset 2: (2.1) S : Unit X Load) in the Currrent FE Models window; define a load sequence for the second case, as described above, using the data from the second column of the numerical listing display (scaler #2). The new loading definition appears in the Loading Details area of the Fatigue from FEA dialogue, as shown in Figure , below. Figure Note: if the window does not appear exactly as shown in Figure , then expand the tree view to show more details. Vol.. 1 Section 106 Issue: 15 Date: Volume 1 Tutorial

74 Tutorial 106 : Using fe-safe with Abaqus.odb files 3. The load definition (LDF) file can be used to define simple and complex loading scenarios. Section 13 includes a full description of the LDF file, including syntax. The loading for this exercise can be seen by saving the loading to a load definition file: select File >> Loadings >> Save Current FEA Loadings As...; save the file as ex01_s-c.ldf and click Save; open the file in a text editor to display the contents (comments may vary): #.ldf file created by fe-safe [mswin] INIT END # Block number 1 BLOCK lh= , ds=1 lh= , ds=2 END 4. In this exercise the surface finish was defined by selecting a surface type (in this case mirror-polished ) from a surface finish database. If the actual surface finish factor, Kt, for the component is known (for mirror-polished, the Kt factor has a value of 1) then it can be specified as a value. To define a userdefined value for Kt, select Define Kt as a value, in the Surface Finish Definition dialogue box: Figure Volume 1 Tutorial Vol. 1 Section 106 Issue: 15 Date:

75 Tutorial 106 : Using fe-safe with Abaqus.odb files 5. The results data can be exported to an alternative file format at the end of the analysis, by changing the extension of the output file (Fatigue from FEA >> Output File) to a recognised type. For example: to export to an ASCII CSV results file, change the extension to.txt,.csv or.asc (this is useful for viewing a table of results in an editor or spreadsheet). Alternatively, after the analysis is complete, and the ODB file has been created, the results data can be written to another output file in addition to the original output ODB file, using the Save FEA Fatigue Results As... option in the File menu. This option displays the Save FEA Fatigue Results As... dialogue box, as shown in Figure , below: Figure The FER (.fer) file (see Appendix E) is an intermediate file containing the results of the analysis. This new output file type is determined by the extension of the file entered in the Output File box. A copy of the original output ODB file can be created if the extension.odb is used. 6. To analyse individual elements or nodes, list the required items in the Exports and Outputs dialogue, and select the Only analyse listed items dialogue. Additional outputs and diagnostics options can also be specified. Diagnostics and additional outputs are discussed in detail in section To save the current analysis configuration, select Save FEA Fatigue Definition File..., and enter a filename ending with the extension.stlx. The analysis can be reloaded at a later date by restoring the keyword file, using Open FEA Fatigue Definition File... Vol.. 1 Section 106 Issue: 15 Date: Volume 1 Tutorial

76 Tutorial 106 : Using fe-safe with Abaqus.odb files Exercise 2 : Multiaxial analysis of a data sets sequence, including Factor Of Strength evaluation Objective: To perform a multiaxial analysis of a series of events in this case a sequence of two elastically calculated FEA stress solution (i.e. stress datasets). The analysis will also include an evaluation of the Factor of Strength (FOS). This is the factor by which the loading must be scaled to achieve a specified design life. The FOS method is described in detail in section 17. Analysis process: The Strength Factor (FOS) for each node is calculated as follows: the calculated life is compared with the design life: - if the calculated life is lower than the design life, the elastic stresses at the node are scaled by a factor less than 1.0; - if the calculated life is greater than the design life, the elastic stresses at the node are scaled by a factor greater than 1.0. the elastic stress history is recalculated using the re-scaled nodal stresses; for local strain analysis, the cyclic plasticity model is used to recalculate the time history of elastic-plastic stress-strains - the fatigue life is then recalculated; in the critical plane analysis, the critical plane orientation is re-calculated; the process is repeated with different scale factors until: (i) (ii) the calculated life is within 5% of the design life or the step change of 0.01 or 0.1 in the FOS value causes the design life to be bracketed, or (iii) the FOS exceeds the max factor (default 2.0) or is less than the min factor (default 0.5). Method: Step 1: Define the loading: The series of events being analysed in this exercise consists of a sequence of two elastically calculated FEA stress solution (i.e. stress datasets) scaled by a defined scale factor. The definition of the sequence will be as follows: the first dataset (Dataset 1: (1.1) S : Unit Y Load) multiplied by a scale factor of 10000, followed by: the second dataset (Dataset 2: (2.1) S : Unit X Load) multiplied by a scale factor of The loading for this loading sequence can be defined in a single loading block: select Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; select Clear all loadings and click Yes from the tree context menu (right mouse click on the tree) to clear the existing loading definition; Volume 1 Tutorial Vol. 1 Section 106 Issue: 15 Date:

77 Tutorial 106 : Using fe-safe with Abaqus.odb files highlight the first unit stress dataset in the Current FE Models window; select Add... >> Dataset; highlight the second unit stress dataset in the Current FE Models window; select Add... >> Dataset; highlight the dataset item in the loading tree of the Fatigue from FEA dialogue; select Scale from the tree context menu (right mouse click on the tree) and enter the value 10000; press enter to accept the value. If saved as a.ldf it would look like: #.ldf file created by fe-safe [mswin] INIT END # Block number 1 BLOCK n=1 ds=1, scale=10000 ds=2, scale=10000 END The new loading definition appears in the Loading Details area of the Fatigue from FEA dialogue, as shown in Figure Figure select the Analysis Settings tab from the Fatigue from FEA dialogue to switch to the main settings. Step 2: Define the subgroup option: As in Exercise 1, all elements in the model should be used for analysis - see (Exercise 1), Step 2. Vol.. 1 Section 106 Issue: 15 Date: Volume 1 Tutorial

78 Tutorial 106 : Using fe-safe with Abaqus.odb files Step 3: Define the surface finish: As in Exercise 1, the component is assumed to have a mirror-polished surface finish, (i.e. a Kt factor of 1) - see (Exercise 1), Step 3. Step 4: Define the material: As in Exercise 1, the component is assumed to be made from SAE 950C (Manten) see (Exercise 1), Step 4. Step 5: Define the analysis algorithm: As in Exercise 1, the default analysis algorithm for the material will be used, which for SAE 950C (Manten) is Brown-Miller Biaxial Strain Life using Morrow mean-stress correction. Step 6: Define the in-plane residual stress: As in Exercise 1, it is assumed that there are no in-plane residual stresses - see (Exercise 1), Step 6. Step 6: Configuring the Factor of Strength (FOS) analysis: To configure the Factor of Strength (FOS) analysis: click on the Factor of Strength... button in the Fatigue from FEA window to open the Design Life (Factors of Strength Calculations) dialogue box: Figure select the Perform Factor of Strength (FOS) Calculations? option to enable the FOS analysis.; select Infinite design life (use material s Endurance Limit) this uses the constant amplitude endurance limit for the component material, which for SAE 950C (Manten) is: reversals; Note: fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). click OK; Volume 1 Tutorial Vol. 1 Section 106 Issue: 15 Date:

79 Tutorial 106 : Using fe-safe with Abaqus.odb files specify the FOS band limits in the Analysis Options dialogue [FEA Fatigue >> Analysis Options...] Safety Fators tab as shown in Figure , to determine the limits and precision of the FOS analysis: - between the fine limits, the FOS is calculated to a resolution of approximately 0.01 repeats; - between maximum and minimum, the FOS is calculated to a resolution of approximately 0.1 repeats; - if the evaluated FOS is greater than 2, then a FOS of 2 is exported for the node; - if the evaluated FOS is less than 0.5, then a FOS of 0.5 is exported for the node. Figure Step 8: Define the output file: Before running the analysis, change the output filename to: <ResultsDir>\keyhole2016Results_ex02.odb The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. Vol.. 1 Section 106 Issue: 15 Date: Volume 1 Tutorial

80 Tutorial 106 : Using fe-safe with Abaqus.odb files Step 9: Run the analysis: fe-safe should now be configured to run the analysis. Press the Analyse button. A summary of analysis parameters is displayed: Figure Check that the analysis is configured as shown in Figure , and then click Continue. Note that the UTS of the material is used to evaluate Kt from the defined surface finish curve (i.e. surface finish factor versus UTS). In this case, for a mirror-polished surface, Kt =1 for all values of UTS. As the analysis is being performed, the following information is written to the analysis log file. The analysis log file has the same file name as the output file, except that the extension is.log. So, for this analysis, the analysis log file is: <ResultsDir>\keyhole2016Results_ex02.log This information is also displayed in the Message Log window and includes: Summary ======= Worst Life-Repeats : at Element [0]67.2 Worst FOS@Life=Infinite : at Element [0]65.3 Analysis time : 0:00:00 Volume 1 Tutorial Vol. 1 Section 106 Issue: 15 Date:

81 Tutorial 106 : Using fe-safe with Abaqus.odb files Step 10: Reviewing the results The analysis log shows that the worst-case life for the whole model is: repeats of the loading, at element 67, node 2. The worst-case Factor of Strength (FOS) for the analysis is: at element 65, node 3. In the configuration of the Factor of Strength analysis, the design life specified was the Infinite design life, which is assumed to be the materials constant amplitude endurance limit, which for SAE 950C (Manten) is: reversals. The worst-case fatigue lives are of the order repeats of the fatigue loading cycle, which is less than the design life ( repeats of the loading). This is why the worst-case strength factor (the factor by which the loading must be scaled to achieve the design life) is somewhat less than 1. The FOS method is described in detail in section 17. Note: fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). In fe-safe, the design life and the calculated fatigue life always refer to the number of repeats of the complete defined fatigue loading cycle. An optional conversion factor can be used to convert the fatigue life in repeats to fatigue life with respect to some other quantity, for example hours or miles (see section 13). Step 11: Viewing the fatigue life contour: A copy of the original.odb file was created, onto which a new step containing the fatigue results was appended. In this exercise, two fatigue results sets the fatigue life and the strength factor (FOS) are exported to one step/frame using the following variables: LOGLife-Repeats FOS@Life=Infinite The results from this exercise were written to the file: <ResultsDir>/keyhole2016Results_ex02.odb. Volume 1 Tutorial Vol.. 1 Section 106 Issue: 15 Date:

82 Tutorial 106 : Using fe-safe with Abaqus.odb files The first set of exported fatigue results in the file contains the fatigue lives, which should look similar to Figure , the viewer colour scheme may need to be set to "Reversed Rainbow" and any averaging of values at nodes should be disabled. Figure Volume 1 Tutorial Vol. 1 Section 106 Issue: 15 Date:

83 Tutorial 106 : Using fe-safe with Abaqus.odb files The second set of exported fatigue results in the file contains the strength factors (FOS), which should look similar to Figure , the viewer colour scheme may need to be set to "Reversed Rainbow" and any averaging of values at nodes should be disabled. Figure Vol.. 1 Section 106 Issue: 15 Date: Volume 1 Tutorial

84 Tutorial 106 : Using fe-safe with Abaqus.odb files Volume 1 Tutorial Vol. 1 Section 106 Issue: 15 Date:

85 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files 107 Tutorial 107 : Using fe-safe with NASTRAN.f06 files Introduction This tutorial demonstrates the use of fe-safe with NASTRAN results (*.f06) files. The use of NASTRAN.f06 files in fe-safe is discussed in detail in Appendix G. The tutorial includes opening the FE model and configuring multi-axial analyses of two superimposed fatigue load cases and of a dataset sequence, including Factors of Strength (FOS) evaluation. The sample files used for this tutorial are located in the directory <DataDir>\Nastran. NOTE: The nomenclature used throughout this tutorial when referring to files and directories is as described in Appendix B Preparation Start the program by selecting fe-safe from the Windows Start menu (Windows) or by running the script fe-safe (Linux). Select an existing project, or create a new one from the welcome page Ensure that the following basic settings are correctly configured. If fe-safe is being run for the first time then it is possible to skip this preparatory section. Vol.. 1 Section 10 Issue: 15 Date: Volume 1 Tutorial 107-1

86 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files Reset any existing analysis options to their defaults in the Clear Data and Settings dialogue [Tools >> Clear Data and Settings...], shown in Figure 107-1, below, by selecting the Check all option and clicking OK. Figure Opening the sample FE model The model for this tutorial is a plate with a keyhole, as shown in Figure 107-2: Figure Volume 1 Tutorial Vol. 1 Section 107 Issue: 15 Date:

87 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files To open the model select Open Finite Element Model... from the File menu. This will display the file selection dialogue. Select the sample file keyhole_01.f06 from the directory <DataDir>\Nastran. The Pre-Scan File dialogue will be displayed as shown in Figure 107-3, select Yes. Figure As fe-safe pre-scans the model, information about the file is written to the file: <ProjectDir>\Model\scan This information is also displayed in the Message Log window. When the pre-scan of the file is complete, the Select Datasets to Read dialogue will be displayed as shown in Figure The file keyhole_01.f06 contains four datasets, two of which are stress and two are strain datasets. This tutorial only requires the stress datasets, the strain datasets do not need to be loaded. Check the Stresses and Select last increment only boxes, click Apply to Dataset List to apply the selection. Change the Available Positions combo box to Elemental & Centroidal and select OK to load the stress datasets. As fe-safe loads the model, information about the file and the data it contains is appended to the file: <ProjectDir>\Model\reader.log. This information is also displayed in the Message Log window: Figure Vol.. 1 Section 10 Issue: 15 Date: Volume 1 Tutorial 107-3

88 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files When the model has finished loading, the Loaded FEA Models Properties dialogue box appears, as shown in Figure Figure If the dialogue box does not appear automatically, then it can be displayed by right-clicking on the Current FE Models window and selecting Properties. icon in the Figure Volume 1 Tutorial Vol. 1 Section 107 Issue: 15 Date:

89 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files Ensure that the units are as shown in Figure 107-5, then click OK. A dialogue will show prompting to edit element groups loaded from the model, as shown in Figure 107-7, click No. Figure A summary of the open model appears in the Current FE Models window, showing the loaded datasets and element group information see Figure Figure Note: if the window does not appear exactly as shown in Figure 107-8, then expand the tree view to show more details. Vol.. 1 Section 10 Issue: 15 Date: Volume 1 Tutorial 107-5

90 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files The process of loading an FE model into fe-safe involves extracting pertinent data from the FE model, and writing it to the working FED folder (see Appendix E). Therefore, the Current FE Models window is a summary of the contents of the working FED folder. In this case there are two stress datasets each containing elemental and centroidal data with 1004 elements (502 on the top shell and 502 on the bottom shell) in each dataset. The source of the datasets (the filename of the source FE model, the step, increment and timestamp) are also shown. fe-safe also extracts group information from the SETS defined in the Case Control deck of the.f06 file. When a new model is loaded, the output filename automatically defaults to: <ResultsDir>\{source_file_name}Results.{default_output_file_extension} For NASTRAN.f06 files, the default output file type is.csv, so in this case, the output filename automatically defaults to: <ResultsDir>\ keyhole_01results.csv The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button: Exercise 1 : Multiaxial analysis using scale-and-combine loading Objective: To perform a multiaxial analysis of two superimposed fatigue load cases. Each load case consists of an elastically calculated unit load FEA stress solution (i.e. a stress dataset) and some load history data. The unit load and the load history are combined using a scale-and-combine method, as described in section 13. Analysis process: The fatigue life for each node is calculated as follows: the stress tensors are multiplied by the time history of the applied loading, to produce a time history of each of the 6 components of the stress tensor; the time histories of the in-plane principal stresses are calculated; the time histories of the three principal strains are calculated from the stresses; a multiaxial cyclic plasticity model is used to convert the elastic stress-strain histories into elastic plastic stressstrain histories; a critical plane method is used to identify the most damaging plane by calculating the damage on planes at 10 intervals between 0 and 180 in the surface of the component; for each of the critical planes, strains are resolved onto the three shear planes (1-2, 2-3 and 1-3); the time history of the damage parameter (which in this case, using the Brown-Miller algorithm, is the shear and normal strain) is cycle counted; individual fatigue cycles are identified using a Rainflow cycle algorithm, the fatigue damage for each cycle is calculated and the total damage is summed; the plane with the shortest life defines the plane of crack initiation, and this life is written to the output file. Volume 1 Tutorial Vol. 1 Section 107 Issue: 15 Date:

91 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files During this calculation, fe-safe may modify the endurance limit amplitude. If all cycles (on a plane) are below the endurance limit amplitude, there is no calculated fatigue damage on this plane. If any cycle is damaging, the endurance limit amplitude is reduced to 25% of the constant amplitude value, and the damage curve extended to this new endurance limit. The critical plane method is described and illustrated in detail in Volume 2, section 7.5. Method: Step 1: Define the loading: For this exercise two fatigue load cases will be superimposed. Each load case will consist of an elastically calculated unit load stress dataset and some load history data, as follows: the first dataset (Dataset 1: (1.1) S : KEYHOLE TUTORIAL LS1 CS1) will be combined with channel 1 of the data file test_mcg2.amc; the second dataset (Dataset 2: (2.1) S : KEYHOLE TUTORIAL LS2 CS2) will be combined with channel 2 of the data file test_mcg2.amc. To open the loading history data, select Open Data File from the File menu. Use the file selection dialogue to select the sample file test_mcg2.amc from the <DataDir> directory. The data file is summarised in the Loaded Data Files window. The sample file contains two channels of load data, identified in the tree view by the channel icon,. Figure To combine the unit load stress dataset with the loading history for the first case: select the Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; select Clear all loadings and click Yes from the tree context menu (right mouse click on the tree) to clear the existing loading definition; in the Current FE Models window, highlight the first dataset, labelled Dataset 1: (1.1) S : KEYHOLE TUTORIAL LS1 CS1, (next to the stress dataset icon, ); in the Loaded Data Files window, highlight the first channel of data, labelled fe-safe tutorial scaler #1, (next to the channel icon ); select Add... >> A LOAD * dataset. Vol.. 1 Section 10 Issue: 15 Date: Volume 1 Tutorial 107-7

92 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files To combine the unit load stress dataset with the loading history for the second case: in the Current FE Models window, highlight the second dataset, labelled Dataset 2: (2.1) S : KEYHOLE TUTORIAL LS2 CS2, (next to the stress dataset icon, ); in the Loaded Data Files window, highlight the second channel of data, labelled fe-safe tutorial scaler #2, (next to the channel icon ). select Add... >> A LOAD * dataset. The defined loading appears in the loading details list box, as shown below: Figure Note: if the window does not appear exactly as shown in Figure , then expand the tree view to show more details. select the Analysis Settings tab from the Fatigue from FEA dialogue to switch to the main settings. Step 2: Define the subgroup option: The.f06 file format interface does not support reading geometry data from the FE model, required by the surface detection algorithm. Therefore for this tutorial all elements in the model should be used for analysis, not only those on its surface: double-click the Subgroup column header to open the Subgroup Selection dialogue for all groups: Figure Volume 1 Tutorial Vol. 1 Section 107 Issue: 15 Date:

93 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files select Whole group; click OK. Step 3: Define the surface finish: It is assumed that the whole component has a mirror-polished surface finish, (i.e. a Kt factor of 1). To define this surface finish for the whole component (i.e. all element groups): double-click the Surface column header to open the Surface Finish Definition dialogue for all groups: Figure select Select Surface Finish from list; click on the browse button,, to open the Select a surface finish file (*.kt) file dialogue; select the surface finish database file default.kt from the <KtDir> directory; from the drop-down Surface finish list, select Mirror Polished Ra <= 0.25µm; click OK. Vol.. 1 Section 10 Issue: 15 Date: Volume 1 Tutorial 107-9

94 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files Step 4: Define the material: The component material is SAE 950C (Manten). The material record SAE_950C-Manten from the material database local.dbase will be defined for the whole component. Opened material databases are displayed in the Material Databases window as shown in Figure , below. Figure If the database local.dbase is not currently loaded in the Material Databases window, select File >> Materials >> Open Materials Database... and select local.dbase from the directory <UserDir>. Notice in Figure that the database local.dbase is the user s local copy from the <UserDir> directory. The other two databases shown are from the <DatabaseDir> directory. Expand the tree view to show the materials contained in local.dbase. The contents of the database can be filtered to show only materials of a particular type, by selecting one of the filter icons. To ensure that all materials in the database are displayed double-click on the All filter icon. The parameters for a material can be displayed by clicking the symbol next to the material name. To define SAE_950C-Manten for the whole component: highlight the material SAE_950C-Manten in the local.dbase database; double-click the Material column header - a Change Material? confirmation dialogue box appears; Figure click YES; the material name should appear for all groups in the Material column. Volume 1 Tutorial Vol. 1 Section 107 Issue: 15 Date:

95 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files Step 5: Define the analysis algorithm: The material database identifies a default analysis algorithm for each material. The default analysis algorithm is normally selected automatically. To confirm that the default algorithm will be used for the whole model (i.e. all element groups): double-click the Algorithm column header to open the in Group Algorithm Selection dialogue box for all groups; Figure select the Analyse with material s default algorithm option; click OK. For SAE 950C (Manten) the default algorithm is Brown-Miller Biaxial Strain Life using Morrow mean-stress correction. Step 6: Define the in-plane residual stress: For this exercise it is assumed that there are no in-plane residual stresses. To set the residual stress to 0 (zero) for the whole component (i.e. all element groups): double-click the In-plane residual stress column header to open the In-plane Residual Stress dialogue for all groups: Figure enter a residual stress of 0 (zero), and click OK. Vol.. 1 Section 10 Issue: 15 Date: Volume 1 Tutorial

96 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files Step 7: Define the output file: When the FE model was loaded, the output filename automatically defaulted to: <ResultsDir>\ keyhole_01results.csv The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. Step 8: Run the analysis: fe-safe should now be configured to run the analysis. Press the Analyse! button. A summary of analysis parameters is displayed: Figure Check that the analysis is configured as shown in Figure , and then click Continue. Note that the UTS of the material is used to evaluate Kt from the defined surface finish curve (i.e. surface finish factor versus UTS). In this case, for a mirror-polished surface, Kt =1 for all values of UTS. Volume 1 Tutorial Vol. 1 Section 107 Issue: 15 Date:

97 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files As the analysis is being performed, the following information is written to the analysis log file. The analysis log file has the same file name as the output file, except that the extension is.log. So, for this analysis, the analysis log file is: <ResultsDir>\keyhole_01Results_ex01.log This information is also displayed in the Message Log window and includes Summary ======= Worst Life-Repeats : at Element 1.4:1 Analysis time : 0:00:03 Step 9: Reviewing the results The analysis log shows that the worst-case life for the whole model is: repeats of the fatigue loading cycle, at element 1, node 4, shell section 1. Note: fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). In fe-safe, the design life and the calculated fatigue life always refer to the number of repeats of the complete defined fatigue loading cycle. An optional conversion factor can be used to convert the fatigue life in repeats to fatigue life with respect to some other quantity, for example hours or miles (see section 13). Volume 1 Tutorial Vol.. 1 Section 10 Issue: 15 Date:

98 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files Step 10: Viewing the fatigue life contours: Since the original.f06 file contains two layers (sections) the output file also contains two sets of results data. In this example, the stresses in both sections are the same. Therefore, the fatigue results are also the same. When the results are exported to an ASCII.csv file, then the fatigue results for each layer are written to a separate file. The fatigue life should look similar to Figure , the viewer colour scheme may need to be set to "Reversed Rainbow" and any averaging of values at nodes should be disabled. Figure : Log of Fatigue Lives. Volume 1 Tutorial Vol. 1 Section 107 Issue: 15 Date:

99 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files Additional notes for Exercise 1: 1. In this exercise, the two fatigue load cases are superimposed. Therefore, it does not matter in which order the loads are defined. For example: Loading is the same as: Loading Loading is 1 Repeats DS#1 * test_mcg2.amc:1 DS#2 * test_mcg2.amc:2 Loading is 1 Repeats DS#2 * test_mcg2.amc:2 DS#1 * test_mcg2.amc:1 2. In this example, the load history is very short, consisting of only five data points. For short load histories it is often more convenient to define the loading using a user-defined load history, rather than reading a load history from a data file (see section ). This is achieved using the A user-defined LOAD * dataset option. To re-define the loading for this exercise using user-defined load histories: select Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; select Clear all loadings and click Yes from the tree context menu (right mouse click on the tree) to clear the existing loading definition; in the Loaded Data Files window expand the filename test_mcg2.amc, so that both channels of data are displayed; highlight both channels of data (to select multiple channels highlight the first channel by clicking on it with the left mouse button, then hold down the CTRL key on the keyboard while clicking on any additional files); display a numerical listing of the two data channels by selecting View >> Numerical Listing (or just click the icon): Figure Vol.. 1 Section 10 Issue: 15 Date: Volume 1 Tutorial

100 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files highlight the first unit stress dataset (labelled Dataset 1: (1.1) S : KEYHOLE TUTORIAL LS1 CS1) in the Current FE Models window; select Add... >> A user-defined LOAD * dataset to display the Dataset Embedded Load History dialogue, and copy the five data points from the first column of the numerical listing display (scaler #1) into the Loading Scale box: Figure click OK; highlight the second unit stress dataset (labelled Dataset 2: (2.1) S : KEYHOLE TUTORIAL LS2 CS2) in the Current FE Models window; define a load sequence for the second case, as described above, using the data from the second column of the numerical listing display (scaler #2). The new loading definition appears in the Loading Details area of the Fatigue from FEA dialogue, as shown in Figure , below. Figure Note: if the window does not appear exactly as shown in Figure , then expand the tree view to show more details. Volume 1 Tutorial Vol. 1 Section 107 Issue: 15 Date:

101 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files 3. The load definition (LDF) file can be used to define simple and complex loading scenarios. Section 13 includes a full description of the LDF file, including syntax. The loading for this exercise can be seen by saving the loading to a load definition file: select File >> Loadings >> Save Current FEA Loadings As...; save the file as ex01_s-c.ldf and click Save; open the file in a text editor to display the contents (comments may vary): #.ldf file created by fe-safe [mswin] INIT END # Block number 1 BLOCK n=1 lh= , ds=1 lh= , ds=2 END 4. In this exercise the surface finish was defined by selecting a surface type (in this case mirror-polished ) from a surface finish database. If the actual surface finish factor, Kt, for the component is known (for mirror-polished, the Kt factor has a value of 1) then it can be specified as a value. To define a userdefined value for Kt, select Define Kt as a value, in the Surface Finish Definition dialogue box: Figure Vol.. 1 Section 10 Issue: 15 Date: Volume 1 Tutorial

102 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files 5. The results data can be exported to an alternative file format at the end of the analysis, by changing the extension of the output file (Fatigue from FEA >> Output File) to a recognised type. For example: to export to an ASCII CSV results file, change the extension to.txt,.csv or.asc (this is useful for viewing a table of results in an editor or spreadsheet). Alternatively, after the analysis is complete, and the.csv file has been created, the results data can be written to another output file in addition to the original output.csv file, using the Save FEA Fatigue Results As... option in the File menu. This option displays the Save FEA Fatigue Results As... dialogue box, as shown in Figure , below: Figure The FER (.fer) file (see Appendix E) is an intermediate file containing the results of the analysis. This new output file type is determined by the extension of the file entered in the Output File box. A copy of the original output.csv file can be created if the extension.csv is used. 6. To analyse individual elements or nodes, list the required items in the Exports and Outputs dialogue, and select the Only analyse listed items dialogue. Additional outputs and diagnostics options can also be specified. Diagnostics and additional outputs are discussed in detail in section To save the current analysis configuration, select Save FEA Fatigue Definition File..., and enter a filename ending with the extension.stlx. The analysis can be reloaded at a later date by restoring the keyword file, using Open FEA Fatigue Definition File...,. Volume 1 Tutorial Vol. 1 Section 107 Issue: 15 Date:

103 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files Exercise 2 : Multiaxial analysis of a data sets sequence, including Factor Of Strength evaluation Objective: To perform a multiaxial analysis of a series of events in this case a sequence of two elastically calculated FEA stress solution (i.e. stress datasets). The analysis will also include an evaluation of the Factor of Strength (FOS). This is the factor by which the loading must be scaled to achieve a specified design life. The FOS method is described in detail in section 17. Analysis process: The Strength Factor (FOS) for each node is calculated as follows: the calculated life is compared with the design life: - if the calculated life is lower than the design life, the elastic stresses at the node are scaled by a factor less than 1.0; - if the calculated life is greater than the design life, the elastic stresses at the node are scaled by a factor greater than 1.0. the elastic stress history is recalculated using the re-scaled nodal stresses; for local strain analysis, the cyclic plasticity model is used to recalculate the time history of elastic-plastic stress-strains - the fatigue life is then recalculated; in the critical plane analysis, the critical plane orientation is re-calculated; the process is repeated with different scale factors until: (i) (ii) the calculated life is within 5% of the design life or the step change of 0.01 or 0.1 in the FOS value causes the design life to be bracketed, or (iii) the FOS exceeds the max factor (default 2.0) or is less than the min factor (default 0.5). Method: Step 1: Define the loading: The series of events being analysed in this exercise consists of a sequence of two elastically calculated FEA stress solution (i.e. stress datasets) scaled by a defined scale factor. The definition of the sequence will be as follows: the first dataset (Dataset 1: (1.1) S : KEYHOLE TUTORIAL LS1 CS1) multiplied by a scale factor of 20000, followed by: the second dataset (Dataset 2: (2.1) S : KEYHOLE TUTORIAL LS2 CS2) multiplied by a scale factor of The loading for this loading sequence can be defined in a single loading block: select Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; Vol.. 1 Section 10 Issue: 15 Date: Volume 1 Tutorial

104 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files select Clear all loadings and click Yes from the tree context menu (right mouse click on the tree) to clear the existing loading definition; highlight the first unit stress dataset in the Current FE Models window; select Add... >> Dataset; highlight the second unit stress dataset in the Current FE Models window; select Add... >> Dataset; highlight the dataset item in the loading tree of the Fatigue from FEA dialogue; select Scale from the tree context menu (right mouse click on the tree) and enter the value 20000; press enter to accept the value. If saved as a.ldf it would look like: #.ldf file created by fe-safe [mswin] INIT END # Block number 1 BLOCK ds=1, scale=20000 ds=2, scale=20000 END The new loading definition appears in the Loading Details area of the Fatigue from FEA dialogue, as shown in Figure Figure select the Analysis Settings tab from the Fatigue from FEA dialogue to switch to the main settings. Volume 1 Tutorial Vol. 1 Section 107 Issue: 15 Date:

105 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files Step 2: Define the subgroup option: As in Exercise 1, all elements in the model should be used for analysis - see (Exercise 1), Step 2. Step 3: Define the surface finish: As in Exercise 1, the component is assumed to have a mirror-polished surface finish, (i.e. a Kt factor of 1) - see (Exercise 1), Step 3. Step 4: Define the material: As in Exercise 1, the component is assumed to be made from SAE 950C (Manten) see (Exercise 1), Step 4. Step 5: Define the analysis algorithm: As in Exercise 1, the default analysis algorithm for the material will be used, which for SAE 950C (Manten) is Brown-Miller Biaxial Strain Life using Morrow mean-stress correction. Step 6: Define the in-plane residual stress: As in Exercise 1, it is assumed that there are no in-plane residual stresses - see (Exercise 1), Step 6. Step 7: Configuring the Factor of Strength (FOS) analysis: To configure the Factor of Strength (FOS) analysis: click on the Factor of Strength... button in the Fatigue from FEA window to open the Factors of Strength Calculations dialogue box: Figure select the Perform Factor of Strength (FOS) Calculations? option to enable the FOS analysis.; select Infinite design life (use material s Endurance Limit) this uses the constant amplitude endurance limit for the component material, which for SAE 950C (Manten) is: reversals; Vol.. 1 Section 10 Issue: 15 Date: Volume 1 Tutorial

106 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files Note: fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). click OK; specify the FOS band limits in the Analysis Options dialogue [FEA Fatigue >> Analysis Options...] Safety Factors tab as shown in Figure , to determine the limits and precision of the FOS analysis: - between the fine limits, the FOS is calculated to a resolution of approximately 0.01 repeats; - between maximum and minimum, the FOS is calculated to a resolution of approximately 0.1 repeats; - if the evaluated FOS is greater than 2, then a FOS of 2 is exported for the node; - if the evaluated FOS is less than 0.5, then a FOS of 0.5 is exported for the node. Figure Step 8: Define the output file: Before running the analysis the output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. Volume 1 Tutorial Vol. 1 Section 107 Issue: 15 Date:

107 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files Step 9: Run the analysis: fe-safe should now be configured to run the analysis. Press the Analyse! button. A summary of analysis parameters is displayed: Figure Check that the analysis is configured as shown in Figure , and then click Continue. Note that the UTS of the material is used to evaluate Kt from the defined surface finish curve (i.e. surface finish factor versus UTS). In this case, for a mirror-polished surface, Kt =1 for all values of UTS. As the analysis is being performed, the following information is written to the analysis log file. The analysis log file has the same file name as the output file, except that the extension is.log. So, for this analysis, the analysis log file is: <ResultsDir>\keyhole_01Results_ex02.log This information displayed in the Message Log window includes the following Summary ======= Worst Life-Repeats : at Element 1.4:1 Worst FOS@Life=Infinite : at Element 1.4:1 Analysis time : 0:00:09 Vol.. 1 Section 10 Issue: 15 Date: Volume 1 Tutorial

108 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files Step 10: Reviewing the results The analysis log shows that the worst-case life for the whole model is: repeats of the loading, at element 1, node 4, shell section 1. The worst-case Factor of Strength (FOS) for the analysis is: at element 1, node 4, shell section 1. In the configuration of the Factor of Strength analysis, the design life specified was the Infinite design life, which is assumed to be the materials constant amplitude endurance limit, which for SAE 950C (Manten) is: reversals. The worst-case fatigue lives are of the order repeats of the fatigue loading cycle, which is less than the design life ( repeats of the loading). This is why the worst-case strength factor (the factor by which the loading must be scaled to achieve the design life) is somewhat less than 1. The FOS method is described in detail in section 17. Note: fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). In fe-safe, the design life and the calculated fatigue life always refer to the number of repeats of the complete defined fatigue loading cycle. An optional conversion factor can be used to convert the fatigue life in repeats to fatigue life with respect to some other quantity, for example hours or miles (see section 13). Volume 1 Tutorial Vol. 1 Section 107 Issue: 15 Date:

109 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files Step 11: Viewing the fatigue life contour: Since the original.f06 file contains two layers (sections) the output file also contains two sets of results data for both the fatigue life and the FOS. In this example, the stresses in both sections are the same. Therefore, the fatigue results and the FOS are also the same for both sections. When the results are exported an ASCII.csv file, then the results are written to separate files. The fatigue should look similar to Figure , the viewer colour scheme may need to be set to "Reversed Rainbow" and any averaging of values at nodes should be disabled. Figure Vol.. 1 Section 10 Issue: 15 Date: Volume 1 Tutorial

110 Tutorial 107 : Using fe-safe with NASTRAN results (*.f06) files The strength factors (FOS), should look similar to Figure , the viewer colour scheme may need to be set to "Reversed Rainbow" and any averaging of values at nodes should be disabled. Figure Volume 1 Tutorial Vol. 1 Section 107 Issue: 15 Date:

111 Tutorial 108 : Using the ANSYS results (.rst) file 108 Tutorial 108 : Using fe-safe with ANSYS.rst files Introduction This tutorial demonstrates the use of fe-safe with the ANSYS results (.rst) file. The use of ANSYS results.rst files in fe-safe is discussed in detail in Appendix G. The tutorial includes opening the FE model and configuring multi-axial analyses of two superimposed fatigue load cases and of a dataset sequence, including Factors of Strength (FOS) evaluation. The sample files used for this tutorial are located in the directory <DataDir>\Ansys. NOTE: The nomenclature used throughout this tutorial when referring to files and directories is as described in Appendix B Preparation Start the program by selecting fe-safe from the Windows Start menu (Windows) or by running the script fe-safe (Linux). Select an existing project, or create a new one from the welcome page Ensure that the following basic settings are correctly configured. If fe-safe is being run for the first time then it is possible to skip this preparatory section. Vol. 1 Section 108 Issue: 15 Date: Volume 1 Tutorial 108-1

112 Tutorial 108 : Using the ANSYS results (.rst) file Reset any existing analysis options to their defaults in the Clear Data and Settings dialogue [Tools >> Clear Data and Settings...], shown in Figure , below, by selecting the Check all option and clicking OK. Figure Opening the sample FE model The model for this tutorial is a plate with a keyhole, as shown in Figure : Figure Volume 1 Tutorial Vol. 1 Section 108 Issue: 15 Date:

113 Tutorial 108 : Using the ANSYS results (.rst) file To open the model, select Open Finite Element Model... from the File menu. This will display the file selection dialogue. Select the sample file keyhole_01.rst from the directory <DataDir>\Ansys. The Pre-Scan File dialogue will be displayed as shown in Figure , select Yes. Figure As fe-safe pre-scans the model, information about the file is written to the file: <ProjectDir>\Model\scan This information is also displayed in the Message Log window. When the pre-scan of the file is complete, the Select Datasets to Read dialogue will be displayed as shown in Figure The file keyhole_01.rst contains two datasets of elemental stresses that are required for this tutorial. The strain, temperature and forces datasets do not need to be loaded. Check only the Stresses and Select last increment only boxes, click Apply to Dataset List to apply the selection and select OK to load the remaining stress datasets. As fe-safe loads the model, information about the file and the data it contains is appended to the file: <ProjectDir>\Model\reader.log. This information is also displayed in the Message Log window. Figure Vol. 1 Section 108 Issue: 15 Date: Volume 1 Tutorial 108-3

114 Tutorial 108 : Using the ANSYS results (.rst) file When the model has finished loading, the Loaded FEA Models Properties dialogue box appears, as shown in Figure Figure If the dialogue box does not appear automatically, then it can be displayed by right-clicking on the Open FE Models window and selecting Properties. icon in the Figure Ensure that the units are as shown in Figure , then click OK. Volume 1 Tutorial Vol. 1 Section 108 Issue: 15 Date:

115 Tutorial 108 : Using the ANSYS results (.rst) file A dialogue will show prompting to edit element groups loaded from the model, as shown in Figure , click No. Figure A summary of the open model appears in the Open FE Models window, showing the loaded datasets and element group information see Figure Figure Note: if the window does not appear exactly as shown in Figure , then expand the tree view to show more details. The process of loading an FE model into fe-safe involves extracting pertinent data from the FE model, and writing it to the working FED folder (see Appendix E). Therefore, the Open FE Models window is a summary of the contents of the working FED folder. In this case there are two stress datasets each containing elemental data with 502 Vol. 1 Section 108 Issue: 15 Date: Volume 1 Tutorial 108-5

116 Tutorial 108 : Using the ANSYS results (.rst) file elements in each dataset. The source of the dataset (the filename of the source FE model, the step, increment and timestamp) are also shown. For ANSYS models, element groups can be defined by setting different regions in the model to have different material numbers (although the material data can be the same). fe-safe then extracts group information from the RST file by grouping elements that have the same ANSYS material number. When a new model is loaded, the output filename automatically defaults to: <ResultsDir>\{source_file_name}Results.{source_file_extension} which in this example is: <ResultsDir>\keyhole_01Results.rst The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button: Exercise 1 : Multiaxial analysis using scale-and-combine loading Objective: To perform a multiaxial analysis of two superimposed fatigue load cases. Each load case consists of an elastically calculated unit load FEA stress solution (i.e. a stress dataset) and some load history data. The unit load and the load history are combined using a scale-and-combine method, as described in section 13. Analysis process: The fatigue life for each node is calculated as follows: the stress tensors are multiplied by the time history of the applied loading, to produce a time history of each of the 6 components of the stress tensor; the time histories of the in-plane principal stresses are calculated; the time histories of the three principal strains are calculated from the stresses; a multiaxial cyclic plasticity model is used to convert the elastic stress-strain histories into elastic plastic stressstrain histories; a critical plane method is used to identify the most damaging plane by calculating the damage on planes at 10 intervals between 0 and 180 in the surface of the component; for each of the critical planes, strains are resolved onto the three shear planes (1-2, 2-3 and 1-3); the time history of the damage parameter (which in this case, using the Brown-Miller algorithm, is the shear and normal strain) is cycle counted; individual fatigue cycles are identified using a Rainflow cycle algorithm, the fatigue damage for each cycle is calculated and the total damage is summed; the plane with the shortest life defines the plane of crack initiation, and this life is written to the output file. Volume 1 Tutorial Vol. 1 Section 108 Issue: 15 Date:

117 Tutorial 108 : Using the ANSYS results (.rst) file During this calculation, fe-safe may modify the endurance limit amplitude. If all cycles (on a plane) are below the endurance limit amplitude, there is no calculated fatigue damage on this plane. If any cycle is damaging, the endurance limit amplitude is reduced to 25% of the constant amplitude value, and the damage curve extended to this new endurance limit. The critical plane method is described and illustrated in detail in Volume 2. Method: Step 1: Define the loading: For this exercise two fatigue load cases will be superimposed. Each load case will consist of an elastically calculated unit load stress dataset and some load history data, as follows: the first dataset (Dataset 1: (1.1) S : Keyhole) will be combined with channel 1 of the data file test_mcg2.amc; the second dataset (Dataset 2: (2.1) S : Keyhole) will be combined with channel 2 of the data file test_mcg2.amc. To open the loading history data, select Open Data File from the File menu. Use the file selection dialogue to select the sample file test_mcg2.amc from the <DataDir> directory. The data file is summarised in the Loaded Data Files window. The sample file contains two channels of load data, identified in the tree view by the channel icon. Figure To combine the unit load stress dataset with the loading history for the first case: select the Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; select Clear all loadings and click Yes from the tree context menu (right mouse click on the tree) to clear the existing loading definition in the Current FE Models window, highlight the first dataset, labelled Dataset 1: (1.1) S : Keyhole, (next to the stress dataset icon, ); in the Loaded Data Files window, highlight the first channel of data, labelled fe-safe tutorial scaler #1, (next to the channel icon ); select Add... >> A LOAD * dataset. Vol. 1 Section 108 Issue: 15 Date: Volume 1 Tutorial 108-7

118 Tutorial 108 : Using the ANSYS results (.rst) file To combine the unit load stress dataset with the loading history for the second case: in the Current FE Models window, highlight the second dataset, labelled Dataset 2: (2.1) S : Keyhole, (next to the stress dataset icon, ); in the Loaded Data Files window, highlight the second channel of data, labelled fe-safe tutorial scaler #2, (next to the channel icon ). select Add... >> A LOAD * dataset. The defined loading appears in the loading details list box, as shown below: Figure Note: if the window does not appear exactly as shown in Figure , then expand the tree view to show more details. select the Analysis Settings tab from the Fatigue from FEA dialogue to switch to the main settings. Step 2: Define the subgroup option: For this tutorial all elements in the model should be used for analysis, not only those on its surface: double-click the Subgroup column header to open the Subgroup Selection dialogue for all groups: Figure Volume 1 Tutorial Vol. 1 Section 108 Issue: 15 Date:

119 Tutorial 108 : Using the ANSYS results (.rst) file select Whole group; click OK. Step 3: Define the surface finish: It is assumed that the whole component has a mirror-polished surface finish, (i.e. a Kt factor of 1). To define this surface finish for the whole component (i.e. all element groups): double-click the Surface column header to open the Surface Finish Definition dialogue for all groups: Figure select Select Surface Finish from list; click on the browse button,, to open the Select a surface finish file (*.kt) file dialogue; select the surface finish database file default.kt from the <KtDir> directory; from the drop-down Surface finish list, select Mirror Polished Ra <= 0.25µm; click OK. Vol. 1 Section 108 Issue: 15 Date: Volume 1 Tutorial 108-9

120 Tutorial 108 : Using the ANSYS results (.rst) file Step 4: Define the material: The component material is SAE 950C (Manten). The material record SAE_950C-Manten from the material database local.dbase will be defined for the whole component. Opened material databases are displayed in the Material Databases window as shown in Figure , below. Figure If the database local.dbase is not currently loaded in the Material Databases window, select File >> Materials >> Open Materials Database... and select local.dbase from the directory <UserDir>. Notice in Figure that the database local.dbase is the user s local copy from the <UserDir> directory. The other two databases shown are from the <DatabaseDir> directory. Expand the tree view to show the materials contained in local.dbase. The contents of the database can be filtered to show only materials of a particular type, by selecting one of the filter icons. To ensure that all materials in the database are displayed double-click on the All filter icon. The parameters for a material can be displayed by extending the material name. To define SAE_950C-Manten for the whole component: highlight the material SAE_950C-Manten in the local.dbase database; double-click the Material column header - a Change Material? confirmation dialogue box appears; check the confirmation dialogue it should say: Are you sure you want to change the material for the groups Default, Material 1, Material 2 to SAE_950C-Manten in database local.dbase? ; click YES; the material name should appear for all groups in the Material column. Volume 1 Tutorial Vol. 1 Section 108 Issue: 15 Date:

121 Tutorial 108 : Using the ANSYS results (.rst) file Step 5: Define the analysis algorithm: The material database identifies a default analysis algorithm for each material. The default analysis algorithm is normally selected automatically. To confirm that the default algorithm will be used for the whole model (i.e. all element groups): double-click the Algorithm column header to open the in Group Algorithm Selection dialogue box for all groups; Figure select the Analyse with material s default algorithm option; click OK. For SAE 950C (Manten) the default algorithm is Brown-Miller Biaxial Strain Life using Morrow mean-stress correction. Step 6: Define the in-plane residual stress: For this exercise it is assumed that there are no in-plane residual stresses. To set the residual stress to 0 (zero) for the whole component (i.e. all element groups): double-click the In-plane residual stress column header to open the In-plane Residual Stress dialogue for all groups: Figure enter a residual stress of 0 (zero), and click OK. Vol. 1 Section 108 Issue: 15 Date: Volume 1 Tutorial

122 Tutorial 108 : Using the ANSYS results (.rst) file Step 7: Define the output file: When the FE model was loaded, the output filename automatically defaulted to: <ResultsDir>\keyhole_01Results.rst Before running the analysis, change the output filename to: <ResultsDir>\keyhole_01Results_ex01.rst The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. Step 8: Run the analysis: fe-safe should now be configured to run the analysis. Press the Analyse! button. A summary of analysis parameters is displayed: Figure Check that the analysis is configured as shown in Figure , and then click Continue. Note that the UTS of the material is used to evaluate Kt from the defined surface finish curve (i.e. surface finish factor versus UTS). In this case, for a mirror-polished surface, Kt =1 for all values of UTS. Volume 1 Tutorial Vol. 1 Section 108 Issue: 15 Date:

123 Tutorial 108 : Using the ANSYS results (.rst) file As the analysis is being performed, the following information is written to the analysis log file. The analysis log file has the same file name as the output file, except that the extension is.log. So, for this analysis, the analysis log file is: <ResultsDir>\keyhole_01Results_ex01.log This information is also displayed in the Message Log window and includes Summary ======= Worst Life-Repeats : at Element 1.3 Analysis time : 0:00:05 Step 9: Reviewing the results The analysis log shows that the worst-case life for the whole model is: repeats of the fatigue loading cycle, at element 1, node 3. Note: fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). In fe-safe, the design life and the calculated fatigue life always refer to the number of repeats of the complete defined fatigue loading cycle. An optional conversion factor can be used to convert the fatigue life in repeats to fatigue life with respect to some other quantity, for example hours or miles (see section 13). Volume 1 Tutorial Vol. 1 Section 108 Issue: 15 Date:

124 Tutorial 108 : Using the ANSYS results (.rst) file Step 10: Viewing the fatigue life contours: A copy of the original.rst file excluding the original steps was created, onto which a new step containing the fatigue results was appended. The fatigue life is written to the ANSYS variable SX. The SX variable in the last set in the file <ResultsDir>/keyhole_01Results_ex01.rst should look similar to Figure , the viewer colour scheme may need to be set to "Reversed Rainbow" and any averaging of values at nodes should be disabled. Figure : Log of Fatigue Lives. Volume 1 Tutorial Vol. 1 Section 108 Issue: 15 Date:

125 Tutorial 108 : Using the ANSYS results (.rst) file Additional notes for Exercise 1: 1. In this exercise, the two fatigue load cases are superimposed. Therefore, it does not matter in which order the loads are defined. For example: Loading is the same as: Loading Loading is 1 Repeats DS#1 * test_mcg2.amc:1 DS#2 * test_mcg2.amc:2 Loading is 1 Repeats DS#2 * test_mcg2.amc:2 DS#1 * test_mcg2.amc:1 2. In this example, the load history is very short, consisting of only five data points. For short load histories it is often more convenient to define the loading using a user-defined load history, rather than reading a load history from a data file (see section ). This is achieved using the A user-defined LOAD * dataset option. To re-define the loading for this exercise using user-defined load histories: select the Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; select Clear all loadings and click Yes from the tree context menu (right mouse click on the tree) to clear the existing loading definition; in the Loaded Data Files window expand the filename test_mcg2.amc, so that both channels of data are displayed; highlight both channels of data (to select multiple channels highlight the first channel by clicking on it with the left mouse button, then hold down the CTRL key on the keyboard while clicking on any additional files); display a numerical listing of the two data channels by selecting View >> Numerical Listing (or just click the icon): Figure Vol. 1 Section 108 Issue: 15 Date: Volume 1 Tutorial

126 Tutorial 108 : Using the ANSYS results (.rst) file highlight the first unit stress dataset (labelled Dataset 1: (1.1) S : Keyhole) in the Current FE Models window; select Add... >> A user-defined LOAD * dataset to display the Dataset Embedded Load History dialogue, and copy the five data points from the first column of the numerical listing display (scaler #1) into the Loading Scale box: Figure click OK; highlight the second unit stress dataset (labelled Dataset 2: (2.1) S : Keyhole) in the Current FE Models window; define a load sequence for the second case, as described above, using the data from the second column of the numerical listing display (scaler #2). The new loading definition appears in the Loading Details area of the Fatigue from FEA dialogue, as shown in Figure , below. Figure Note: if the window does not appear exactly as shown in Figure , then expand the tree view to show more details. Volume 1 Tutorial Vol. 1 Section 108 Issue: 15 Date:

127 Tutorial 108 : Using the ANSYS results (.rst) file 3. The load definition (LDF) file can be used to define simple and complex loading scenarios. Section 13 includes a full description of the LDF file, including syntax. The loading for this exercise can be seen by saving the loading to a load definition file: select File >> Loadings >> Save Current FEA Loadings As...; save the file as ex01_s-c.ldf and click Save; open the file in a text editor to display the contents (comments may vary): #.ldf file created by fe-safe [mswin] INIT END # Block number 1 BLOCK lh= , ds=1 lh= , ds=2 END 4. In this exercise the surface finish was defined by selecting a surface type (in this case mirror-polished ) from a surface finish database. If the actual surface finish factor, Kt, for the component is known (for mirror-polished, the Kt factor has a value of 1) then it can be specified as a value. To define a userdefined value for Kt, select Define Kt as a value, in the Surface Finish Definition dialogue box: Figure The results data can be exported to an alternative file format at the end of the analysis, by changing the extension of the output file (Fatigue from FEA >> Output File) to a recognised type. Vol. 1 Section 108 Issue: 15 Date: Volume 1 Tutorial

128 Tutorial 108 : Using the ANSYS results (.rst) file For example: to export to an ASCII CSV results file, change the extension to.txt,.csv or.asc (this is useful for viewing a table of results in an editor or spreadsheet). Alternatively, after the analysis is complete, and the RST file has been created, the results data can be written to another output file in addition to the original output RST file, using the Save FEA Fatigue Results As... option in the File menu. This option displays the Save FEA Fatigue Results As... dialogue box, as shown in Figure , below: Figure The FER (.fer) file (see Appendix E) is an intermediate file containing the results of the analysis. This new output file type is determined by the extension of the file entered in the Output File box. A copy of the original output RST file can be created if the extension.rst is used. 6. To analyse individual elements or nodes, list the required items in the Exports and Outputs dialogue, and select the Only analyse listed items dialogue. Additional outputs and diagnostics options can also be specified. Diagnostics and additional outputs are discussed in detail in section To save the current analysis configuration, select Save FEA Fatigue Definition File..., and enter a filename ending with the extension.stlx. The analysis can be reloaded at a later date by restoring the keyword file, using Open FEA Fatigue Definition File...,. Volume 1 Tutorial Vol. 1 Section 108 Issue: 15 Date:

129 Tutorial 108 : Using the ANSYS results (.rst) file Exercise 2 : Multiaxial analysis of a data sets sequence, including Factor Of Strength evaluation Objective: To perform a multiaxial analysis of a series of events in this case a sequence of two elastically calculated FEA stress solution (i.e. stress datasets). The analysis will also include an evaluation of the Factor of Strength (FOS). This is the factor by which the loading must be scaled to achieve a specified design life. The FOS method is described in detail in section 17. Analysis process: The Strength Factor (FOS) for each node is calculated as follows: the calculated life is compared with the design life: - if the calculated life is lower than the design life, the elastic stresses at the node are scaled by a factor less than 1.0; - if the calculated life is greater than the design life, the elastic stresses at the node are scaled by a factor greater than 1.0. the elastic stress history is recalculated using the re-scaled nodal stresses; for local strain analysis, the cyclic plasticity model is used to recalculate the time history of elastic-plastic stress-strains - the fatigue life is then recalculated; in the critical plane analysis, the critical plane orientation is re-calculated; the process is repeated with different scale factors until: (i) (ii) the calculated life is within 5% of the design life or the step change of 0.01 or 0.1 in the FOS value causes the design life to be bracketed, or (iii) the FOS exceeds the max factor (default 2.0) or is less than the min factor (default 0.5). Method: Step 1: Define the loading: The series of events being analysed in this exercise consists of a sequence of two elastically calculated FEA stress solution (i.e. stress datasets) scaled by a defined scale factor. The definition of the sequence will be as follows: the first dataset (Dataset 1: (1.1) S : Keyhole) multiplied by a scale factor of 30000, followed by: the second dataset (Dataset 2: (2.1) S : Keyhole) multiplied by a scale factor of The loading for this loading sequence can be defined in a single loading block: select the Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; select Clear all loadings and click Yes from the tree context menu (right mouse click on the tree) to clear the existing loading definition; Vol. 1 Section 108 Issue: 15 Date: Volume 1 Tutorial

130 Tutorial 108 : Using the ANSYS results (.rst) file highlight the first unit stress dataset in the Current FE Models window; select Add... >> Dataset; highlight the second unit stress dataset in the Current FE Models window; select Add... >> Dataset; highlight the dataset item in the loading tree of the Fatigue from FEA dialogue; select Scale from the tree context menu (right mouse click on the tree) and enter the value 30000; press enter to accept the value. If saved as a.ldf it would look like: #.ldf file created by fe-safe [mswin] INIT END # Block number 1 BLOCK ds=1, scale=30000 ds=2, scale=30000 END The new loading definition appears in the Loading Details area of the Fatigue from FEA dialogue, as shown in Figure Figure select the Analysis Settings tab from the Fatigue from FEA dialogue to switch to the main settings. Step 2: Define the subgroup option: As in Exercise 1, all elements in the model should be used for analysis - see (Exercise 1), Step 2. Volume 1 Tutorial Vol. 1 Section 108 Issue: 15 Date:

131 Tutorial 108 : Using the ANSYS results (.rst) file Step 3: Define the surface finish: As in Exercise 1, the component is assumed to have a mirror-polished surface finish, (i.e. a Kt factor of 1) - see (Exercise 1), Step 3. Step 4: Define the material: As in Exercise 1, the component is assumed to be made from SAE 950C (Manten) see (Exercise 1), Step 4. Step 5: Define the analysis algorithm: As in Exercise 1, the default analysis algorithm for the material will be used, which for SAE 950C (Manten) is Brown-Miller Biaxial Strain Life using Morrow mean-stress correction. Step 6: Define the in-plane residual stress: As in Exercise 1, it is assumed that there are no in-plane residual stresses - see (Exercise 1), Step 6. Step 7: Configuring the Factor of Strength (FOS) analysis: To configure the Factor of Strength (FOS) analysis: click on the Factor of Strength... button in the Fatigue from FEA window to open the Factor of Strength Calculations dialogue box: Figure select the Perform Factor of Strength (FOS) Calculations? option to enable the FOS analysis.; select Infinite design life (use material s Endurance Limit) this uses the constant amplitude endurance limit for the component material, which for SAE 950C (Manten) is: reversals; Note: fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). click OK; Volume 1 Tutorial Vol. 1 Section 108 Issue: 15 Date:

132 Tutorial 108 : Using the ANSYS results (.rst) file specify the FOS band limits in the Analysis Options dialogue [FEA Fatigue >> Analysis Options...] Safety Factors tab as shown in Figure , to determine the limits and precision of the FOS analysis: - between the fine limits, the FOS is calculated to a resolution of approximately 0.01 repeats; - between maximum and minimum, the FOS is calculated to a resolution of approximately 0.1 repeats; - if the evaluated FOS is greater than 2, then a FOS of 2 is exported for the node; - if the evaluated FOS is less than 0.5, then a FOS of 0.5 is exported for the node. Figure Step 7: Define the output file: Before running the analysis, change the output filename to: <ResultsDir>\keyhole_01Results_ex02.rst The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. Volume 1 Tutorial Vol. 1 Section 108 Issue: 15 Date:

133 Tutorial 108 : Using the ANSYS results (.rst) file Step 8: Run the analysis: fe-safe should now be configured to run the analysis. Press the Analyse! button. A summary of analysis parameters is displayed: Figure Check that the analysis is configured as shown in Figure , and then click Continue. Note that the UTS of the material is used to evaluate Kt from the defined surface finish curve (i.e. surface finish factor versus UTS). In this case, for a mirror-polished surface, Kt =1 for all values of UTS. As the analysis is being performed, the following information is written to the analysis log file. The analysis log file has the same file name as the output file, except that the extension is.log. So, for this analysis, the analysis log file is: <ResultsDir>\keyhole_01Results_ex02.log This information is also displayed in the Message Log window and includes Summary ======= Worst Life-Repeats : at Element 71.3 Worst FOS@Life=Infinite : at Element 71.2 Analysis time : 0:00:07 Vol. 1 Section 108 Issue: 15 Date: Volume 1 Tutorial

134 Tutorial 108 : Using the ANSYS results (.rst) file Step 9: Reviewing the results The analysis log shows that the worst-case life for the whole model is: repeats of the loading, at element 71, node 3. The worst-case Factor of Strength (FOS) for the analysis is: at element 71, node 2. In the configuration of the Factor of Strength analysis, the design life specified was the Infinite design life, which is assumed to be the materials constant amplitude endurance limit, which for SAE 950C (Manten) is: reversals. The worst-case fatigue lives are of the order repeats of the fatigue loading cycle, which is less than the design life ( repeats of the loading). This is why the worst-case strength factor (the factor by which the loading must be scaled to achieve the design life) is somewhat less than 1. The FOS method is described in detail in section 17. Note: fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). In fe-safe, the design life and the calculated fatigue life always refer to the number of repeats of the complete defined fatigue loading cycle. An optional conversion factor can be used to convert the fatigue life in repeats to fatigue life with respect to some other quantity, for example hours or miles (see section 13.2). Volume 1 Tutorial Vol. 1 Section 108 Issue: 15 Date:

135 Tutorial 108 : Using the ANSYS results (.rst) file Step 10: Viewing the fatigue life contour: A copy of the original.rst file excluding the steps was created, onto which a new step containing the fatigue results was appended. The fatigue life is written to the ANSYS variable SX; the FOS is written to the ANSYS variable SY. The SX variable in the last set in the file <ResultsDir>/keyhole_01Results_ex02.rst should look similar to Figure , the viewer colour scheme may need to be set to "Reversed Rainbow" and any averaging of values at nodes should be disabled. Figure Vol. 1 Section 108 Issue: 15 Date: Volume 1 Tutorial

136 Tutorial 108 : Using the ANSYS results (.rst) file The SY variable in the last set in the file <ResultsDir>/keyhole_01Results_ex02.rst should look similar to Figure , the viewer colour scheme may need to be set to "Reversed Rainbow" and any averaging of values at nodes should be disabled. Figure Volume 1 Tutorial Vol. 1 Section 108 Issue: 15 Date:

137 Tutorial 109 : Analysing the fatigue life of a weld 109 Tutorial 109 : Analysing the fatigue life of a weld Introduction This tutorial demonstrates how to perform an analysis of a welded joint and should be read in conjunction with section 16, Fatigue Analysis of Welded Steel Joints. The sample files used for this tutorial are located in the directory <DataDir>\ weld_tutorial\ Preparation The tutorial uses an ANSYS.rst model, however, the same techniques can be applied to all FE formats. Sample models and stress result files are provided in the following formats: ANSYS.rst file Abaqus.odb file Abaqus.fil file NASTRAN.f06 file I-DEAS universal.unv file (only the model file is supplied) The results shown below are for illustration only. The actual stresses (and therefore the fatigue results) are different for each model format. In addition to the analysis of the welded joints, a further analysis of the entire model would normally be performed, since the shortest lives are not necessarily at the welds. This tutorial assumes that the user is familiar with the basic program operation. Before attempting this tutorial, it is strongly recommended that one of the introductory tutorials is followed: Tutorial 104: Using fe-safe with IDEAS.unv files Tutorial 105: Using fe-safe with Abaqus.fil files Tutorial 106: Using fe-safe with Abaqus.odb files Tutorial 107: Using fe-safe with NASTRAN.f06 files Tutorial 108: Using fe-safe with ANSYS.rst files Start the program by selecting fe-safe from the Windows Start menu (Windows) or by running the script fe-safe (Linux) (see section 5.2). Volume 1 Tutorial Vol. 1 Section 109 Issue: 15 Date:

138 Tutorial 109 : Analysing the fatigue life of a weld Select an existing project, or create a new one from the welcome page Figure Ensure that the following basic settings are correctly configured. If fe-safe is being run for the first time then it is possible to skip this preparatory section. Reset any existing analysis options to their defaults in the Clear Data and Settings dialogue [Tools >> Clear Data and Settings...], shown in Figure 109-2, below, by selecting the Check all option and clicking OK. Figure Volume 1 Tutorial Vol. 1 Section 109 Issue: 15 Date:

139 Tutorial 109 : Analysing the fatigue life of a weld Sample model The model used in this example consists of a plate with a component welded to one of the large faces, as shown in Figure below: Figure The weld is simulated on the FE model as a solid chamfer. For this analysis, the nominal stresses at the toe of the weld are of interest. However, high stress concentrations will occur at the toe of the weld, as shown in Figure below (showing Principal Stress): Figure Volume 1 Tutorial Vol. 1 Section 109 Issue: 15 Date:

140 Tutorial 109 : Analysing the fatigue life of a weld To avoid the high stress concentration at the toe of each weld, and give the best approximation of the actual stresses at the weld, the stresses within the first 2 to 3 mm of the chamfer/surface junction should be ignored. The stresses in the band of elements adjacent to this gap provide the best approximation of the nominal stresses at the weld itself. Depending on the dimensions of the model, it may be necessary to reduce the size of the elements in the analysis region. A set of stress results were obtained by constraining the base of the component through one hole, and applying a load to the other hole, in a direction away from the constrained hole and in the plane of the plate. The stress results file contains stresses for the whole model, as well as stresses for a defined group of elements in two narrow bands (a few mm wide), close to the weld. The sample model and stress results are contained in the following files: Model Type: ANSYS Abaqus NASTRAN I-DEAS Model Filename: weld_ans.db weld_abaqus.inp weld_nas.mod weld_unv.unv Results file filename: weld_ans.rst weld_abaqus610.odb weld_abaqus661.odb weld_nas.f06 weld_abaqus.fil Note: in ANSYS, groups are supported by using a different material number for different groups of elements. fesafe recognises these groups, and lists them in the Current FE Models window. In this example, the different material numbers have identical properties Setting up the analysis The stress results in <DataDir>\weld_tutorial\Ansys\weld_ans.rst are loaded into fe-safe using the Open Finite Element Model option from the FEA Solutions section of the File menu. If pre-scanning the model only the stress dataset needs to be selected for this tutorial. Figure Volume 1 Tutorial Vol. 1 Section 109 Issue: 15 Date:

141 Tutorial 109 : Analysing the fatigue life of a weld Ensure the model units are MPa, ue and deg.c. To change the units, right click within Current FE Models window and select properties. Then change the values to those shown in Figure 109-6: Figure In the Fatigue from FEA window, Loading Settings tab, configure a user defined load and dataset using data set 1 and a load sequence of [1, 0]: Select the Loading Settings from the Fatigue from FEA dialogue to switch to the loading tree; select Clear all loadings and click Yes from the tree context menu (right mouse click on the tree) to clear the existing loading definition; in the Current FE Models window, highlight the stress dataset (next to the stress dataset icon, ); select Add... >> user-defined LOAD * dataset; enter 1 and 0 in the Dataset Embedded Load History dialogue (i.e. one repeat of the stress load case); select the Analysis Settings tab from the Fatigue from FEA dialogue to switch to the main settings. It is not necessary to define the surface finish, material or in-plane residual stresses for this type of analysis. In this tutorial only the welded joints will be analysed, a further analysis of the entire model would normally be performed, since the shortest lives may not necessarily be at the welds. Volume 1 Tutorial Vol. 1 Section 109 Issue: 15 Date:

142 Tutorial 109 : Analysing the fatigue life of a weld To define the analysis algorithm for the welded joints: double-click the Algorithm column header to open the in Group Algorithm Selection dialogue box for all groups; choose the Do not analyse option; double-click the Algorithm cell for Material3; choose the Select an algorithm to be used option; click the User algorithm browse button,, and select BS5400 Weld Finite Life (CP) from the drop-down menu, as in Figure 109-7; Figure in the BS5400 Weld Definition section of the Group Algorithm Selection dialogue select Weld Class F and enter a design criteria of 2, as in Figure 109-8; Figure click OK. Volume 1 Tutorial Vol. 1 Section 109 Issue: 15 Date:

143 Tutorial 109 : Analysing the fatigue life of a weld Modify the Output File name to: weld_ansresults_01.rst. The Fatigue from FE dialogue should now look similar to Figure 109-9: Figure Performing the analysis fe-safe is now ready to perform the analysis. Click on the Analyse! button and accept the pre-analysis summary. The following text appears in the message log: Summary ======= Worst Life-Repeats : at Element Analysis time : 0:00:01 This fatigue results from this exercise were written to the file: <ResultsDir>/weld_ansResults_01.rst. Volume 1 Tutorial Vol. 1 Section 109 Issue: 15 Date:

144 Tutorial 109 : Analysing the fatigue life of a weld The exported results contain log10 of lives, which can be viewed in ANSYS and should look similar to Figure , the viewer colour scheme may need to be set to "Reversed Rainbow" and any averaging of values at nodes should be disabled. Figure : Log of Fatigue Lives. Regions immediately next to the toe of the welds were NOT included in the analysed region to avoid the areas of high stress concentration at the toe, and to give the best estimate of the fatigue life at the weld. Volume 1 Tutorial Vol. 1 Section 109 Issue: 15 Date:

145 Tutorial 110 : Stress-based thermal fatigue analysis using multiple-temperature S-N data 110 Tutorial 110 : Stress-based thermal fatigue analysis using multiple-temperature S-N data Introduction This tutorial demonstrates a stress-based thermal (temperature-dependent) fatigue analysis of an exhaust manifold assemblage, using multiple-temperature S-N data. This tutorial should be read in conjunction with section 18, Conventional High Temperature Fatigue. The sample files used for this tutorial are located in the directory <DataDir>\Abaqus Preparation The tutorial uses an Abaqus.odb model. However, the same techniques can be applied to all FE formats for which temperatures are supported, which currently include: I-DEAS universal.unv files Abaqus.fil files Abaqus.odb files ANSYS results.rst files This tutorial assumes that the user is familiar with the basic program operation. Before attempting this tutorial, it is strongly recommended that one of the introductory tutorials is followed: Tutorial 104: Using fe-safe with IDEAS.unv files Tutorial 105: Using fe-safe with Abaqus.fil files Tutorial 106: Using fe-safe with Abaqus.odb files Tutorial 108: Using fe-safe with ANSYS.rst files Start the program by selecting fe-safe from the Windows Start menu (Windows) or by running the script fe-safe (Linux). Volume 1 Tutorial Vol. 1 Section 110 Issue : 15 Date:

146 Tutorial 110 : Stress-based thermal fatigue analysis using multiple-temperature S-N data Select an existing project, or create a new one from the welcome page Ensure that the following basic settings are correctly configured. If fe-safe is being run for the first time then it is possible to skip this preparatory section. Reset any existing analysis options to their defaults in the Clear Data and Settings dialogue [Tools >> Clear Data and Settings...], shown in Figure , below, by selecting the Check all option and clicking OK. Figure Volume 1 Tutorial Vol. 1 Section 110 Issue : 15 Date:

147 Tutorial 110 : Stress-based thermal fatigue analysis using multiple-temperature S-N data Opening the sample FE model The model for this tutorial is an exhaust manifold assemblage, as shown in Figure : Figure To open the model, select Open Finite Element Model... from the File menu. From the file selection dialog, select the sample file manifold610.odb from the directory <DataDir>\Abaqus. A prompt to pre-scan the file will be displayed if the file has not yet been pre-scanned. The stress and temperature datasets for the initial step increment do not need to be loaded. Check the Stresses, Temperatures and Last increment only boxes, click Apply to Dataset List to apply the selections and select OK to load the remaining datasets, as shown in Figure : Figure Volume 1 Tutorial Vol. 1 Section 110 Issue : 15 Date:

148 Tutorial 110 : Stress-based thermal fatigue analysis using multiple-temperature S-N data As fe-safe loads the model, information about the file and the data it contains is written to the file: <ProjectDir>\Model\reader.log. This information is also displayed in the Message Log window. When the model has finished loading, the Loaded FEA Models Properties dialogue box appears, as shown in Figure Figure If the dialogue box does not appear automatically, then it can be displayed by right-clicking on the Current FE Models window and selecting Properties. icon in the Ensure that the stress, strain and temperature units are MPa, µe and deg.c, respectively, as shown in Figure , then click OK. Volume 1 Tutorial Vol. 1 Section 110 Issue : 15 Date:

149 Tutorial 110 : Stress-based thermal fatigue analysis using multiple-temperature S-N data A summary of the open model appears in the Current FE Models window, showing the loaded datasets and element group information see Figure Figure The dataset and group details in the tree view can be expanded to show more details. The model contains three stress datasets, three temperature datasets. fe-safe also extracts element group information from the ODB file. When a new model is loaded, the output filename automatically defaults to: <ResultsDir>\{source_file_name}Results.{source_file_extension} which in this example is: <ResultsDir>\manifold610Results.odb Exercise : Thermal fatigue analysis This tutorial should be read in conjunction with section 18, Conventional High Temperature Fatigue. Objective: To perform a stress-based thermal (temperature-dependent) fatigue analysis of a sequence of two fatigue load cases, using multiple-temperature S-N data. Each load case consists of an elastically calculated FEA stress solution (i.e. a stress dataset). Each stress dataset has a corresponding temperature dataset containing the temperature of each node. The analysis will also include an evaluation of the Factor of Strength (FOS). This is the factor by which the loading must be scaled to achieve a specified design life. The FOS method is described in section 17. Volume 1 Tutorial Vol. 1 Section 110 Issue : 15 Date:

150 Tutorial 110 : Stress-based thermal fatigue analysis using multiple-temperature S-N data Analysis process: For each node: the maximum temperature from all temperature results sets in the FEA model is determined; the material properties are modified so that they apply at the maximum temperature of the node; the modified material properties are used to calculate the fatigue life for the node. It is implicit in this analysis that each node uses materials data specifically modified for the maximum temperature of that node. The temperature-corrected material properties will only be used if the following requirements are satisfied: the materials being used have properties defined at multiple temperatures; temperature data exists in the FE model; the option to disable temperature analysis [FEA Fatigue >> Analysis Options..., General tab, Disable temperature-based analysis option] is not set. Method: Step 1: Define the loading: The loading consists of a single fatigue loading block, cycling between the second dataset (the mechanical load plus the thermal load) and the third dataset (the mechanical load at ambient temperature). Note: The definition of fatigue loading for varying temperature, as discussed in section 13, applies only to thermo-mechanical fatigue analyses, as described in section 20. This definition is not required for conventional high temperature fatigue, as in this tutorial. To define the loading: select the Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; select Clear all loadings and click Yes from the tree context menu (right mouse click on the tree) to clear the existing loading definition; in the Current FE Models window, highlight the fourth dataset, labelled Dataset 2: (2.6) S : Step 2.) APPLY PRESCRIBED THERMAL LOAD, (next to the stress dataset icon, ); select Add... >> Dataset; in the Current FE Models window, highlight the sixth dataset, labelled Dataset 3: (3.4) S : Step 3.) RETURN TO AMBIENT TEMPERATURES, (next to the stress dataset icon, ); select Add... >> Dataset; select the Analysis Settings tab from the Fatigue from FEA dialogue to switch to the main settings. Step 2: Define the surface finish: It is assumed that the whole component has a mirror-polished surface finish, (i.e. a Kt factor of 1). To define this surface finish for the whole component (i.e. all element groups): Volume 1 Tutorial Vol. 1 Section 110 Issue : 15 Date:

151 Tutorial 110 : Stress-based thermal fatigue analysis using multiple-temperature S-N data double-click the Surface column header to open the Surface Finish Definition dialogue for all groups: Figure select Select Surface Finish from list; click on the browse button,, to open the Select a surface finish file (*.kt) file dialogue; select the surface finish database file default.kt from the <KtDir> directory; from the drop-down Surface finish list, select Mirror Polished Ra <= 0.25µm; click OK. Step 3: Define the material: Since this is a thermal analysis, we need temperature-dependent material data. For this exercise a copy of the material SAE_950C-Manten from the material database local.dbase will be created, and then modified to give it some sample temperature-dependent data. This tutorial uses a stress-based algorithm using S-N data, so it is the S-N curve parameters that will be modified. First create the new material: in the Material Databases window, select (highlight) the material SAE_950C_Manten from the list of available materials in the local.dbase material database; select Material >> Copy Material to create a new material called CopyOfSAE_95OC-Manten, which will appear at the bottom of the local.dbase database; double-click the newly created material to edit it change the name to Manifold. Volume 1 Tutorial Vol. 1 Section 110 Issue : 15 Date:

152 Tutorial 110 : Stress-based thermal fatigue analysis using multiple-temperature S-N data Change the constant amplitude endurance limit to : expand the Manifold material to show its properties; select the constant amplitude endurance limit field: gen : Const Amp Endurance Limit (2nf); double-click on the value field to edit it; modify the value to 2.00E+15 Now create a temperature list: select the temperature list field: gen : Temperature List (deg.c); double-click on the value field to edit it a temperature list dialogue will open; modify the list to contain the two temperatures 300 C and 800 C, as shown in Figure : Figure click OK. Next, define some temperature-dependent S-N data: select one of the S-N curve fields (either sn curve : S Values (MPa) or sn curve : N Values (nf)); double-click on the value field to edit it - a SN Values Table (MPa) dialogue will open; modify the table so that it contains S-N curve data for two temperatures, as shown in Figure : Figure Volume 1 Tutorial Vol. 1 Section 110 Issue : 15 Date:

153 Tutorial 110 : Stress-based thermal fatigue analysis using multiple-temperature S-N data To define Manifold for the whole component: highlight the material Manifold in the local.dbase database; double-click the Material header in the Groups Parameter box in the Fatigue from FEA dialogue - a Change Material? confirmation dialogue box appears; check the confirmation dialogue it should say: Are you sure you want to change the material for the groups all to Manifold in database local.dbase? ; click YES; the material name should appear for all groups in the Material column. To plot temperature-dependent S-N curves: highlight the material Manifold in the Material Databases window; open the Material Plot dialogue by selecting Material >> Generate Material Plot Data...; ensure that Material type is set to Manifold; enter the required plot temperature; select only the Stress-life (SN) curve (*.sn) output option; click Apply to create the S-N curve the plot is added to the Loaded Data Files window; enter another temperature, click Apply, and repeat as needed. Click Cancel to exit the dialogue highlight the plot file in the Loaded Data Files window and plot it by selecting View >> Plot; multiple plots can be plotted on the same axis using View >> Overlay Plot(s) see Figure Figure Volume 1 Tutorial Vol. 1 Section 110 Issue : 15 Date:

154 Tutorial 110 : Stress-based thermal fatigue analysis using multiple-temperature S-N data Definition of multiple-temperature S-N parameters as well as the process used for interpolating and extrapolating material data is described in detail in section 8. Step 4: Define the analysis algorithm: This exercise uses a stress-based algorithm, to take advantage of the temperature-dependent S-N data. To define the analysis algorithm for the whole model (i.e. all element groups): double-click the Algorithm column header to open the in Group Algorithm Selection dialogue box for all groups; select the Select an algorithm to be used option; click the User algorithm browse button,, and select Normal Stress (CP) >> Goodman from the drop-down menu: Figure click OK. Volume 1 Tutorial Vol. 1 Section 110 Issue : 15 Date:

155 Tutorial 110 : Stress-based thermal fatigue analysis using multiple-temperature S-N data Step 5: Define the in-plane residual stress: For this exercise it is assumed that there are no in-plane residual stresses. To set the residual stress to 0 (zero) for the whole component (i.e. all element groups): double-click the In-plane residual stress column header to open the In-plane Residual Stress dialogue for all groups: Figure enter a residual stress of 0 (zero), and click OK. Step 6: Configuring the Factor of Strength (FOS) analysis: To configure the Factor of Strength (FOS) analysis: click on the Factor of Strength... button in the Fatigue from FEA window to open the Factor of Strength Calculations dialogue box: Figure select the Perform Factor of Strength (FOS) Calculations? option to enable the FOS analysis.; select User-defined design life and enter a design life of 1E7; click OK; Volume 1 Tutorial Vol. 1 Section 110 Issue : 15 Date:

156 Tutorial 110 : Stress-based thermal fatigue analysis using multiple-temperature S-N data specify the FOS band limits in the Analysis Options dialogue [FEA Fatigue >> Analysis Options...] Safety Factors tab as shown in Figure to determine the limits and precision of the FOS analysis: - between the fine limits, the FOS is calculated to a resolution of approximately 0.01 repeats; - between maximum and minimum, the FOS is calculated to a resolution of approximately 0.1 repeats; - if the evaluated FOS is greater than 5, then a FOS of 5 is exported for the node; - if the evaluated FOS is less than 0.5, then a FOS of 0.5 is exported for the node. Figure Step 7: Define the output file: When the FE model was loaded, the output filename automatically defaulted to: <ResultsDir>\manifold610Results.odb The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. Volume 1 Tutorial Vol. 1 Section 110 Issue : 15 Date:

157 Tutorial 110 : Stress-based thermal fatigue analysis using multiple-temperature S-N data Step 8: Run the analysis: fe-safe is now configured to run the analysis. Press the Analyse! button. A summary of analysis parameters is displayed: Figure Check that the analysis is configured as shown in Figure , and then click Continue. Note that the UTS of the material is used to evaluate Kt from the defined surface finish curve (i.e. surface finish factor versus UTS). In this case, for a mirror-polished surface, Kt =1 for all values of UTS. As the analysis is being performed, the following information is written to the analysis log file. The analysis log file has the same file name as the output file, except that the extension is.log: <ResultsDir>\manifold610Results.log This information is also displayed in the Message Log window and includes Summary ======= Worst Life-Repeats : at Element [0] Worst FOS@Life=1E7-Repeats : 0.65 at Element [0] Analysis time : 0:00:05 Volume 1 Tutorial Vol. 1 Section 110 Issue : 15 Date:

158 Tutorial 110 : Stress-based thermal fatigue analysis using multiple-temperature S-N data Step 9: Reviewing the results The analysis log shows that the worst-case life for the whole model is: repeats of the loading, at element 7273, node 3. The worst-case Factor of Strength (FOS) for the analysis is: 0.65 at element 7273, node 3. In the configuration of the Factor of Strength analysis, the design life specified was 10 7 repeats. The worst-case fatigue lives are of the order repeats of the fatigue loading cycle, which is less than the design life ( repeats of the loading). This is why the worst-case strength factor (the factor by which the loading must be scaled to achieve the design life) is somewhat less than 1. The FOS method is described in detail in section 17. Note: fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). In fe-safe, the design life and the calculated fatigue life always refer to the number of repeats of the complete defined fatigue loading cycle. An optional conversion factor can be used to convert the fatigue life in repeats to fatigue life with respect to some other quantity, for example hours or miles (see section 13.2). Step 10: Viewing the fatigue life contour: A copy of the original.odb file was created, onto which a new step containing the fatigue results was appended. In this exercise, two fatigue results sets the fatigue life and the strength factor (FOS) are exported to one step/frame using the following variables: LOGLife-Repeats FOS@Life=Infinite The results from this exercise were written to the file: <ResultsDir>/manifold610Results.odb. Volume 1 Tutorial Vol. 1 Section 110 Issue : 15 Date:

159 Tutorial 110 : Stress-based thermal fatigue analysis using multiple-temperature S-N data The first set of exported fatigue results in the file contains the fatigue lives, which should look similar to Figure : Figure : Log of Fatigue Lives Volume 1 Tutorial Vol. 1 Section 110 Issue : 15 Date:

160 Tutorial 110 : Stress-based thermal fatigue analysis using multiple-temperature S-N data The second set of exported fatigue results in the file contains the strength factors (FOS), which should look similar to Figure : Figure Volume 1 Tutorial Vol. 1 Section 110 Issue : 15 Date:

161 Tutorial 111 : Modal Transient Fatigue Analysis 111 Tutorial 111 : Modal Transient Fatigue Analysis Introduction This tutorial demonstrates modal transient dynamic fatigue analysis of a simple bracket. The tutorial includes opening the FE model and configuring the analysis. Two different analysis methods are explored: Exercise 1: Exercise 2: Exercise 3: Modal transient analysis of a bracket due to a base excitation including Complete a Factors of Strength (FOS) evaluation of the modal fatigue analysis. A sensitivity analysis to determine the most damaging mode at worst life location. The ODB file format is portable between platforms. The use of Abaqus.odb files in fe-safe is discussed in detail in Appendix G. The sample files used for this tutorial are located in the directory <DataDir>\Abaqus. NOTE: The nomenclature used throughout this tutorial when referring to files and directories is as described in Appendix B Preparation This tutorial assumes that the user is familiar with the basic program operation. Before attempting this tutorial, it is strongly recommended that one of the introductory tutorials is followed: Tutorial 106: Using fe-safe with Abaqus.odb files Start the program by selecting fe-safe from the Windows Start menu (Windows) or by running the script fe-safe (Linux). Select an existing project, or create a new one from the welcome page Vol.. 1 Section 111 Issue: 15 Date: Volume 1 Tutorial 111-1

162 Tutorial 111 : Modal Transient Fatigue Analysis Ensure that the following basic settings are correctly configured. If fe-safe is being run for the first time then it is possible to skip this preparatory section. Reset any existing analysis options to their defaults in the Clear Data and Settings dialogue [Tools >> Clear Data and Settings...], shown in Figure below, by selecting the Select all option and clicking OK Figure Opening the sample FE model The model for this tutorial is a bracket, as shown in Figure : Mass Base acceleration Figure Volume 1 Tutorial Vol. 1 Section 111 Issue: 15 Date:

163 Tutorial 111 : Modal Transient Fatigue Analysis To open the model, select Open Finite Element Model... from the FEA Solutions section of the File menu. This will display the file selection dialogue. Select the sample file modal_bracket610.odb from the directory <DataDir>\Abaqus. The Pre-Scan File dialogue will be displayed as shown in Figure , select Yes. Figure As fe-safe pre-scans the model information about the file is written to the folder: <ProjectDir>\Model\scan This information is also displayed in the Message Log window. When the pre-scan of the file is complete, the Select Datasets to Read dialogue will be displayed as shown in Figure The file modal_bracket610.odb contains 10 datasets of elemental stresses from normal mode analysis and generalized displacements. Check the Stresses and Others boxes, click Apply to Dataset List to apply the selection and select OK to load the stress datasets and histories. Figure As fe-safe loads the model, information about the file and the data it contains is appended to the file: <ProjectDir>\Model\reader.log. This information is also displayed in the Message Log window. Vol.. 1 Section 111 Issue: 15 Date: Volume 1 Tutorial 111-3

164 Tutorial 111 : Modal Transient Fatigue Analysis When the model has finished loading, the Loaded FEA Models Properties dialogue box appears, as shown in Figure Figure If the dialogue box does not appear automatically, then it can be displayed by right-clicking on the Current FE Models window and selecting Properties as shown in Figure icon in the Figure Ensure that the units are as shown in Figure , then click OK. Volume 1 Tutorial Vol. 1 Section 111 Issue: 15 Date:

165 Tutorial 111 : Modal Transient Fatigue Analysis A dialogue will show prompting to edit element groups loaded from the model, as shown in Figure , click No. Figure A summary of the open model appears in the Current FE Models window, showing the loaded datasets and element group information see below Figure Figure Note: if the window does not appear exactly as shown in Figure , then expand the tree view to show more details. Vol.. 1 Section 111 Issue: 15 Date: Volume 1 Tutorial 111-5

166 Tutorial 111 : Modal Transient Fatigue Analysis The process of loading an FE model into fe-safe involves extracting pertinent data from the FE model, and writing it to the working FED folder (see Appendix E, section ). Therefore, the Current FE Models window is a summary of the contents of the working FED folder. In this case there are 11 normal modes stress datasets each containing elemental data with elements in each dataset. The source of the dataset (the filename of the source FE model, the step, increment and timestamp) are also shown. fe-safe also extracts element group information from the ODB file. The Abaqus odb file also included the modal participation factors. The data is summarised in the Loaded Data Files window. The sample file contains 11 participation factors, identified in the tree view by the channel icon, as shown in Figure Figure When a new model is loaded, the output filename automatically defaults to: <ResultsDir>\{source_file_name}Results.{source_file_extension} which in this example is: <ResultsDir>\modal_bracket610Results.odb The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button: Exercise 1 : Modal Transient Fatigue Analysis Objective: To perform a dynamic analysis combining the 10 modal stress conditions and the modal participation factors corresponding to a base excitation. The excitation at the base consists of a described vertical displacement in the z-direction, and two rotations about the x and y-axes for a duration of 1 second. A modal transient finite element analysis is performed using Abaqus in two steps. First, the normal modes analysis is done, and the modal stresses are written out to the output database (odb). In the following step, the forced response is performed and ONLY the generalized displacements (a.k.a. modal participation factors) are written to the output database. The odb file is read into fe-safe for fatigue analysis based on these two steps. Each fatigue load case consists of an elastic modal stress (a.k.a. stress dataset) and the corresponding generalized displacement (a.k.a. modal participation factor). The stress conditions and modal participation factors are combined in a typical scale-and-combine method. Volume 1 Tutorial Vol. 1 Section 111 Issue: 15 Date:

167 Tutorial 111 : Modal Transient Fatigue Analysis Analysis process: The fatigue life for each node is calculated as follows: the stress tensors due to each mode are multiplied by the generalised displacements due to the base excitation, to produce a time history of each of the 6 components of the stress tensor per mode; contributions from all modes are superimposed to produce a time history of each of the 6 components of the stress tensor for all modes; the time histories of the in-plane principal stresses are calculated; the time histories of the three principal strains are calculated from the stresses; a multiaxial cyclic plasticity model is used to convert the elastic stress-strain histories into elastic plastic stressstrain histories; a critical plane method is used to identify the most damaging plane by calculating the damage on planes at 10 intervals between 0 and 180 in the surface of the component; for each of the critical planes, strains are resolved onto the three shear planes (1-2, 2-3 and 1-3); the time history of the damage parameter (which in this case, using the Brown-Miller algorithm, is the shear and normal strain) is cycle counted; individual fatigue cycles are identified using a Rainflow cycle algorithm, the fatigue damage for each cycle is calculated and the total damage is summed; the plane with the shortest life defines the plane of crack initiation, and this life is written to the output file. During this calculation, fe-safe may modify the endurance limit amplitude. If all cycles (on a plane) are below the endurance limit amplitude, there is no calculated fatigue damage on this plane. If any cycle is damaging, the endurance limit amplitude is reduced to 25% of the constant amplitude value, and the damage curve extended to this new endurance limit. The critical plane method is described and illustrated in detail in Volume 2. Method: Step 1: Automatic loading definition: For this exercise 10 modes and participation factors will be superimposed. Each load case will consist of an elastically calculated modal stress dataset and a corresponding generalised displacement, as follows: the second dataset (Dataset 2 (1.0) ms: Normal Modes Extraction, mode=1) will be combined with generalized displacement 2 from the Abaqus output file modal_bracket610.odb in the Loaded Data Files window: Modal_bracket610.odb[step_2].amc,1; the third dataset (Dataset 3 (1.0) ms: Normal Modes Extraction, mode=2) will be combined with generalized displacement 3 from the Abaqus output file modal_bracket610.odb in the Loaded Data Files window: Modal_bracket610.odb[step_2].amc,2; etc till Mode 10 Vol.. 1 Section 111 Issue: 15 Date: Volume 1 Tutorial 111-7

168 Tutorial 111 : Modal Transient Fatigue Analysis Note: The first Stress Dataset shown in Figure represents a zero solution. The direct and shear stress ranges, and mode number are zero. Accordingly, the first modal participation factor shown in the Loaded Data Files window does not correspond to a mode. Modes 1-10 correspond to stress data sets and generalized displacements 2-11 in each window. To view the automatic loading definitions: select the Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; The defined loading appears in the loading details list box, as shown in Figure Note: if the window does not appear exactly as shown in Figure , then expand the tree view to show more details. Instructions on how to complete the same loading definitions manually are in the notes at the end of this exercise. Figure Volume 1 Tutorial Vol. 1 Section 111 Issue: 15 Date:

169 Tutorial 111 : Modal Transient Fatigue Analysis in the Settings block right click on Loading is equivalent to 1 Repeats and select Edit from the drop down menu in the Conversion factors dialogue click the LDF Time button and then OK. Figure select the Analysis Settings tab from the Fatigue from FEA dialogue to switch to the main settings. Step 2: Define the subgroup option: For this tutorial we ll allow fe-safe to analyse the whole group, although surface detection is available. See section 5 for details on the subgroup selection. double-click the Subgroup column header to open the Subgroup Selection dialogue for all groups: Figure select Whole group; click OK. Vol.. 1 Section 111 Issue: 15 Date: Volume 1 Tutorial 111-9

170 Tutorial 111 : Modal Transient Fatigue Analysis Step 3: Define the surface finish: It is assumed that the whole component has a mirror-polished surface finish, (i.e. a Kt factor of 1). To define this surface finish for the whole component (i.e. all element groups): double-click the Surface column header to open the Surface Finish Definition dialogue for all groups: Figure select Define Kt as a value; click inside the box next to User defined Kt and type 1; click OK. Step 4: Define the material: The component material is SAE The material record SAE-1008 from the material database system.dbase will be defined for the whole component. Opened material databases are displayed in the Material Databases window as shown in Figure , below. If this window is not currently displayed, select Material >> Display Materials Database Window to display it. Figure Volume 1 Tutorial Vol. 1 Section 111 Issue: 15 Date:

171 Tutorial 111 : Modal Transient Fatigue Analysis If the database system.dbase is not currently loaded in the Material Databases window, select File >> Materials >> Open Materials Database... and select system.dbase from the directory <DatabaseDir>. Notice in Figure that the database system.dbase is the System Database from the <DatabaseDir> directory. Expand the tree view to show the materials contained in system.dbase. The contents of the database can be filtered to show only materials of a particular type, by selecting one of the filter icons. To ensure that all materials in the database are displayed double-click on the All filter icon. The parameters for a material can be displayed by expanding the tree view of the material name. To define SAE-1008 for the whole component: highlight the material SAE-1008 in the system.dbase database; select all groups by clicking on the Group column header in the Group Parameters box in the Fatigue from FEA dialogue; double-click the Material column header - a Change Material? confirmation dialogue box appears; check the confirmation dialogue it should say: Are you sure you want to change the material for the groups Default, WanrElemDistorted, EBRACKET, EMASS to SAE-1008 in database system.dbase? ; click YES; the material name should appear for all groups in the Material column. Step 5: Define the analysis algorithm: The material database identifies a default analysis algorithm for each material. The default analysis algorithm is normally selected automatically. To confirm that the default algorithm will be used for the whole model (i.e. all element groups): double-click the Algorithm column header to open the in Group Algorithm Selection dialogue box for all groups; Figure select the Analyse with material s default algorithm option; click OK. For SAE 1008 the default algorithm is Brown-Miller Biaxial Strain Life using Morrow mean-stress correction. Vol.. 1 Section 111 Issue: 15 Date: Volume 1 Tutorial

172 Tutorial 111 : Modal Transient Fatigue Analysis Step 6: Define the in-plane residual stress: For this exercise it is assumed that there are no in-plane residual stresses. To set the residual stress to 0 (zero) for the whole component (i.e. all element groups): in the Group Parameters table, use the scroll bar to the right, in order to double-click the In-plane residual stress column header to open the In-plane Residual Stress dialogue for all groups: Figure enter a residual stress of 0 (zero), and click OK. Step 7: Define the output file: When the FE model was loaded, the output filename automatically defaulted to: <ResultsDir>\modal_bracket610Results.odb Before running the analysis, change the output filename to: <ResultsDir>\modal_bracket610Results_ex01.odb The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. After steps 1 through 6 are complete the Fatigue from FEA dialogue appears as shown in Figure Figure Volume 1 Tutorial Vol. 1 Section 111 Issue: 15 Date:

173 Tutorial 111 : Modal Transient Fatigue Analysis Step 8: Run the analysis: fe-safe should now be configured to run the analysis. Press the Analyse! button. A summary of analysis parameters is displayed: Figure Check that the analysis is configured as shown in Figure , and then click Continue. As the analysis is being performed, information is written to the analysis log file. The analysis log file has the same file name as the output file, except that the extension is.log. So, for this analysis, the analysis log file is: <ResultsDir>\modal_bracket610Results_ex01.log This information is also displayed in the Message Log window and includes: Summary ======= Worst Life-Hours : at Element [0] Analysis time : 0:00:25 Fatigue Analysis Completed. Vol.. 1 Section 111 Issue: 15 Date: Volume 1 Tutorial

174 Tutorial 111 : Modal Transient Fatigue Analysis To save the current analysis configuration, select Save FEA Fatigue Definition File..., and enter a filename ending with the extension.stlx. The analysis can be reloaded at a later date by restoring the keyword file, using Open FEA Fatigue Definition File... Step 9: Reviewing the results The analysis log shows that the worst-case life for the whole model is: Note: hours of the base excitation, at element 5939, node 1. fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). In fe-safe, the Factor of Strength and the calculated fatigue life always refer to the number of repeats of the complete defined fatigue loading cycle. In this case the conversion factor was used to convert the fatigue life in repeats to fatigue life with respect to hours or miles (see section 13). Step 10: Viewing the fatigue life contours: A copy of the original.odb file was created, onto which a new step containing the fatigue results was appended. Open the.odb file with your preferred post-processor and plot a contour of the results. In the last step of the file <ResultsDir>/modal_bracket610Results_ex01.odb, the results for the exported variable should look similar to Figure : Figure : Log of Fatigue Lives. Note: The contour plot above is a reverse-contour. It shows the lowest Log Life as red and the highest Log Life as blue. Depending on which post-processor you use, the method to reverse the contour colours will vary and any averaging of values at nodes should be disabled. Volume 1 Tutorial Vol. 1 Section 111 Issue: 15 Date:

175 Tutorial 111 : Modal Transient Fatigue Analysis Additional notes for Exercise 1: 1. In the case that the modal superposition loading does not automatically populate as indicated in Step 1, the following procedure can be done to effect the same result: in the Current FE Models window, highlight the second stress dataset, labelled Dataset 2 (1.1) ms: Normal Modes Extraction, Mode=1, (next to the stress dataset icon, ); in the Loaded Data Files window, highlight all but the first channel of data, labelled Modal_bracket_610.odb[step_2].amc:GU1 through GU10 (next to the channel icon ); Figure select the Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; select Clear all loadings from the tree context menu (right mouse click on the tree) to clear the existing loading definition; and click Yes in the delete loadings dialogue. select Add... >> A LOAD * dataset. select OK in the Automatic Block Creation dialogue: Figure Vol.. 1 Section 111 Issue: 15 Date: Volume 1 Tutorial

176 Tutorial 111 : Modal Transient Fatigue Analysis Select Yes in the Adding Multiple Load Histories dialogue Figure in the Loaded Data Files window, highlight the first channel of data, labelled Modal_bracket.odb[step2].amc:Time In the Loading Details dialogue right click on the Elastic Block and choose Add Time History. Figure The time base record is loaded into the elastic block with a time history symbol as shown in Figure in the Settings block right click on Loading is equivalent to 1 Repeats and select Edit from the drop down menu in the Conversion factors dialogue click the LDF Time button and then OK. Select Save Current FEA Loadings as... from the Loadings section of the File menu Use the Save Loading as.ldf file dialogue to browse to a file location where you want to save the loadings, and name the ldf file. Click Save. select the Analysis Settings tab from the Fatigue from FEA dialogue to switch to the main settings. Volume 1 Tutorial Vol. 1 Section 111 Issue: 15 Date:

177 Tutorial 111 : Modal Transient Fatigue Analysis In this exercise, the many modal load cases are superimposed. Section 13 includes a full description of the LDF file, including syntax. The file is as follows: #.ldf file created by fe-safe compliant product [mswin] INIT transitions=yes END # Block number 1 BLOCK lhtime=modal_bracket610.odb[step_2].amc, signum=1 lh=modal_bracket610.odb[step_2].amc, signum=2, ds=2 lh=modal_bracket610.odb[step_2].amc, signum=3, ds=3 lh=modal_bracket610.odb[step_2].amc, signum=4, ds=4 lh=modal_bracket610.odb[step_2].amc, signum=5, ds=5 lh=modal_bracket610.odb[step_2].amc, signum=6, ds=6 lh=modal_bracket610.odb[step_2].amc, signum=7, ds=7 lh=modal_bracket610.odb[step_2].amc, signum=8, ds=8 lh=modal_bracket610.odb[step_2].amc, signum=9, ds=9 lh=modal_bracket610.odb[step_2].amc, signum=10, ds=10 lh=modal_bracket610.odb[step_2].amc, signum=11, ds=11 END 2. In this exercise the surface finish was indicated by a user-defined value for Kt. For an example of selecting a surface type (in this case mirror-polished ) from a surface finish database, see Tutorial The results data can be exported to an alternative file format at the end of the analysis, by changing the extension of the output file (Fatigue from FEA >> Output File) to a recognised type. For example: to export to an ASCII CSV results file, change the extension to.txt,.csv or.asc (this is useful for viewing a table of results in an editor or spreadsheet). Alternatively, after the analysis is complete, and the ODB file has been created, the results data can be written to another output file in addition to the original output ODB file, using the Save FEA Fatigue Results As... option in the File menu. This option displays the Save FEA Fatigue Results As... dialogue box, as shown in Figure below: Figure Vol.. 1 Section 111 Issue: 15 Date: Volume 1 Tutorial

178 Tutorial 111 : Modal Transient Fatigue Analysis The FER (.fer) file (see Appendix E) is an intermediate file containing the results of the analysis. This new output file type is determined by the extension of the file entered in the Output File box. A copy of the original output ODB file can be created if the extension.odb is used Exercise 2: Factors of Strength (FOS) evaluation of the modal fatigue problem Objective: Add an evaluation of the Factor of Strength (FOS) to the previously completed Example 1. To be determined is the factor by which the loading must be scaled to achieve a specified Factor of Strength. The FOS method is described in detail in section 17. Analysis process: The Strength Factor (FOS) for each node is calculated as follows: the calculated life is compared with the Factor of Strength: - if the calculated life is lower than the Factor of Strength, the elastic stresses at the node are scaled by a factor less than 1.0; - if the calculated life is greater than the Factor of Strength, the elastic stresses at the node are scaled by a factor greater than 1.0. the elastic stress history is recalculated using the re-scaled nodal stresses; for local strain analysis, the cyclic plasticity model is used to recalculate the time history of elastic-plastic stress-strains - the fatigue life is then recalculated; in the critical plane analysis, the critical plane orientation is re-calculated; the process is repeated with different scale factors until: (i) (ii) the calculated life is within 5% of the Factor of Strength or the step change of 0.01 or 0.1 in the FOS value causes the Factor of Strength to be bracketed, or (iii) the FOS exceeds the max factor (default 2.0) or is less than the min factor (default 0.5). Method: Step 1: This analysis makes use of the previous loading and group definitions set up in section If fe-safe is still open since completion of Example 1, continue on to Step 2 If you have re-opened fe-safe, complete Section 111.2: Preparation again Choose File >> Open FEA Fatigue Definition File Use the Open FEA Fatigue Definition dialogue to choose the.stlx file created in Section 111.2: Exercise 1, Step 8. Select Open Step 2: Define the subgroup option: As in Exercise 1: select subgroup: whole - see (Exercise 1), Step 2. Volume 1 Tutorial Vol. 1 Section 111 Issue: 15 Date:

179 Tutorial 111 : Modal Transient Fatigue Analysis Step 3: Define the surface finish: As in Exercise 1, the component is assumed to have a mirror-polished surface finish, (i.e. a Kt factor of 1) - see (Exercise 1). Step 4: Define the material: As in Exercise 1, the component is assumed to be made from SAE 1008 see (Exercise 1). Step 5: Define the analysis algorithm: As in Exercise 1, the default analysis algorithm for the material will be used, which for SAE 1008 is Brown-Miller Biaxial Strain Life using Morrow mean-stress correction. Step 6: Define the in-plane residual stress: As in Exercise 1, it is assumed that there are no in-plane residual stresses - see (Exercise 1). Step 7: Configuring the Factor of Strength (FOS) analysis: To configure the Factor of Strength (FOS) analysis: click on the Factor of Strength... button in the Fatigue from FEA window to open the Factor of Strength Calculations dialogue box: Figure select the Perform Factor of Strength (FOS) Calculations? option to enable the FOS analysis.; select User-defined Factor of Strength and enter 20 in the box next to Hours; click OK; Vol.. 1 Section 111 Issue: 15 Date: Volume 1 Tutorial

180 Tutorial 111 : Modal Transient Fatigue Analysis specify the FOS band limits in the Analysis Options dialogue [FEA Fatigue >> Analysis Options...] choose the Safety Factors tab as shown in Figure to determine the limits and precision of the FOS analysis: - between the fine limits, the FOS is calculated to a resolution of approximately 0.01 repeats; - between maximum and minimum, the FOS is calculated to a resolution of approximately 0.1 repeats; - if the evaluated FOS is greater than 2, then a FOS of 2 is exported for the node; - if the evaluated FOS is less than 0.5, then a FOS of 0.5 is exported for the node. Figure Step 8: Define the output file: Before running the analysis, change the output filename to: <ResultsDir>\modal_bracket610Results_ex02.odb The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. Volume 1 Tutorial Vol. 1 Section 111 Issue: 15 Date:

181 Tutorial 111 : Modal Transient Fatigue Analysis Step 9: Run the analysis: fe-safe should now be configured to run the analysis. Press the Analyse! button. A summary of analysis parameters is displayed: Figure Check that the analysis is configured as shown in Figure , and then click Continue. As the analysis is being performed, the following information is written to the analysis log file. The analysis log file has the same file name as the output file, except that the extension is.log. So, for this analysis, the analysis log file is: <ResultsDir>\modal_bracket610Results_ex02.log This information is also displayed in the Message Log window and includes: Summary ======= Worst Life-Hours : at Element Worst FOS@Life=20-Hours : 0.95 at Element Analysis time : 0:01:53 Vol.. 1 Section 111 Issue: 15 Date: Volume 1 Tutorial

182 Tutorial 111 : Modal Transient Fatigue Analysis Step 9: Viewing the Factor of Strength (FOS) contours: A copy of the original.odb file was created, onto which a new step containing the fatigue results was appended. The type of variable that the results are exported to will depend on the configuration in the Abaqus ODB Interface Options dialogue (see 111.2, above). Open the.odb file with your preferred post-processor and plot a contour of the results. In the last step of the file <ResultsDir>/modal_bracket610Results_ex02.odb, the results for the exported variable should look similar to Figure : Figure Factor of Strength (FOS) Note: The contour plot above is a reverse-contour. It shows the lowest Log Life as red and the highest Log Life as blue. Depending on which post-processor you use, the method to reverse the contour colours will vary and any averaging of values at nodes should be disabled Exercise 3 : Sensitivity analysis of the modal fatigue analysis Objective: Perform a sensitivity analysis to determine the most damaging mode at worst life location for the modal fatigue analysis completed in Exercise 1. Load Sensitivity Analysis is described in detail in section Analysis process: The Sensitivity calculated for the selected node is calculated as follows: For each node selected : - Remove each modal stress dataset / participation pair in turn - Recalculate fatigue life without the removed pair Tabulate the Load Sensitivity factors as life and as percentage change in life Volume 1 Tutorial Vol. 1 Section 111 Issue: 15 Date:

183 Tutorial 111 : Modal Transient Fatigue Analysis Method: Step 1: This analysis makes use of the previous loading and group definitions set up in section If fe-safe is still open since completion of Example 1, continue on to Step 2 If you have re-opened fe-safe, complete Section 111.2: Preparation again. Choose File >> Open FEA Fatigue Definition File Use the Open FEA Fatigue Definition dialogue to choose the.stlx file created in Section 111.2: Exercise 1, Step 8. Select Open Step 2: Define the subgroup option: As in Exercise 1: select subgroup: whole - see (Exercise 1), Step 2. Step 3: Define the surface finish: As in Exercise 1, the component is assumed to have a mirror-polished surface finish, (i.e. a Kt factor of 1) - see (Exercise 1). Step 4: Define the material: As in Exercise 1, the component is assumed to be made from SAE 1008 see (Exercise 1). Step 5: Define the analysis algorithm: As in Exercise 1, the default analysis algorithm for the material will be used, which for SAE 1008 is Brown-Miller Biaxial Strain Life using Morrow mean-stress correction. Step 6: Define the in-plane residual stress: As in Exercise 1, it is assumed that there are no in-plane residual stresses - see (Exercise 1). Step 7: Configuring the Load Sensitivity analysis: This analysis makes use of the location where the lowest life was recorded in Exercise 1. click on the Factor of Strength... button in the Fatigue from FEA window to open the Factors of Strength Calculations dialogue box. deselect the box next to Perform Factor of Strength Calculations?. Select OK. The Fatigue from FEA window displays FOS disabled next to the Factor of Strength button Click on the Exports button in the Fatigue from FEA window to open the Exports and Outputs dialogue box. Select the List of Items tab and enter the Element and Node number: in the item box. Vol.. 1 Section 111 Issue: 15 Date: Volume 1 Tutorial

184 Tutorial 111 : Modal Transient Fatigue Analysis Select the check box next to Only analyse listed items. as shown in Figure Figure Select the Log for Items tab to the right Select the check box next to Enable Load Sensitivity Analysis. Click OK. Figure Volume 1 Tutorial Vol. 1 Section 111 Issue: 15 Date:

185 Tutorial 111 : Modal Transient Fatigue Analysis Step 8: Define the output file: Before running the analysis, change the output filename to: <ResultsDir>\modal_bracket610Results_ex03.csv The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. Step 9: Run the analysis: fe-safe should now be configured to run the analysis. Press the Analyse! button. A summary of analysis parameters is displayed: Figure Check that the analysis is configured as shown in Figure , and then click Continue. As the analysis is being performed, the sensitivity analysis information is written to the analysis log file. The analysis log file has the same file name as the output file, except that the extension is.log. So, for this analysis, the analysis log file is: <ResultsDir>\modal_bracket610Results_ex03.log Fatigue analysis for the selected node is displayed in the Message Log window and includes: Summary ======= Worst Life-Hours : at Element Analysis time : 0:00:01 Vol.. 1 Section 111 Issue: 15 Date: Volume 1 Tutorial

186 Tutorial 111 : Modal Transient Fatigue Analysis Step 10: Reviewing the results The analysis log shows the sensitivity analysis for Element 5939, Node 1: SENSITIVITY ANALYSIS for Element [0] (The life is for 1 repeat of the block (i.e n=1), it does not consider the n Value if this is an LDF analysis) Life (Reps) % Omission None DS#2 * modal_bracket_2016.odb[step_2].amc:gu DS#3 * modal_bracket_2016.odb[step_2].amc:gu DS#4 * modal_bracket_2016.odb[step_2].amc:gu DS#5 * modal_bracket_2016.odb[step_2].amc:gu DS#6 * modal_bracket_2016.odb[step_2].amc:gu DS#7 * modal_bracket_2016.odb[step_2].amc:gu DS#8 * modal_bracket_2016.odb[step_2].amc:gu DS#9 * modal_bracket_2016.odb[step_2].amc:gu DS#10 * modal_bracket_2016.odb[step_2].amc:gu DS#11 * modal_bracket_2016.odb[step_2].amc:gu10 The percentage change in Life and the percentage life change corresponding to the removal of each data set oneby one are tabulated in the log file. Which modes contribute most of the damage? Volume 1 Tutorial Vol. 1 Section 111 Issue: 15 Date:

187 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files 112 Tutorial 112 : Using fe-safe with NASTRAN.op2 files Introduction This tutorial demonstrates the use of fe-safe with NASTRAN.op2 files. The use of NASTRAN.op2 files in fe-safe is discussed in detail in Appendix G. The tutorial includes opening the FE model and configuring multi-axial analyses of two superimposed fatigue load cases and of a dataset sequence, including Factors of Strength (FOS) evaluation. The sample files used for this tutorial are located in the directory <DataDir>\Nastran. NOTE: The nomenclature used throughout this tutorial when referring to files and directories is as described in Appendix B Preparation Start the program by selecting fe-safe from the Windows Start menu (Windows) or by running the script fe-safe (Linux). Select an existing project, or create a new one from the welcome page Figure Ensure that the following basic settings are correctly configured. If fe-safe is being run for the first time then it is possible to skip this preparatory section. Vol. 1 Section 112 Issue: 15 Date: Volume 1 Tutorial 112-1

188 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files Reset any existing analysis options to their defaults in the Clear Data and Settings dialogue [Tools >> Clear Data and Settings...], shown in Figure below, by selecting the Select all option and clicking OK. Figure Opening the sample FE model The selected model is a plate with a keyhole, as shown in Figure 112-3: Figure Volume 1 Tutorial Vol. 1 Section 112 Issue: 15 Date:

189 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files To open the model, select Open Finite Element Model... from the File menu. From the file selection dialog, select the sample file keyhole_01.op2 from the directory <DataDir>\Nastran. The Pre-Scan File dialogue will be displayed as shown in Figure 112-4, select Yes. Figure As fe-safe pre-scans the model information about the file is written to the folder: <ProjectDir>\Model\scan This information is also displayed in the Message Log window. When the pre-scan of the file is complete, the Select Datasets to Read dialogue will be displayed as shown in Figure The file keyhole_01.op2 contains four datasets, two of which are stress and two are strain datasets. This tutorial only requires the stress datasets, the strain datasets do not need to be loaded. Check the Stresses and Last increment only boxes, click Apply to Dataset List to apply the selection. Change the Available Positions combo box to Elemental & Centroidal and select OK to load the stress datasets. As fe-safe loads the model, information about the file and the data it contains is appended to the file: <ProjectDir>\Model\reader.log. This information is also displayed in the Message Log window. Figure Vol. 1 Section 112 Issue: 15 Date: Volume 1 Tutorial 112-3

190 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files When the model has finished loading, the Loaded FEA Models Properties dialogue box appears, as shown in Figure Figure If the dialogue box does not appear automatically, then it can be displayed by right-clicking on the Current FE Models window and selecting Properties. icon in the Figure Volume 1 Tutorial Vol. 1 Section 112 Issue: 15 Date:

191 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files Ensure that the units are as shown in Figure 112-6, then click OK. A dialogue will show prompting to edit element groups loaded from the model, as shown in Figure click No. Figure A summary of the open model appears in the Current FE Models window, showing the loaded datasets and element group information see Figure Figure Note: if the window does not appear exactly as shown in Figure 112-9, then expand the tree view to show more details. Vol. 1 Section 112 Issue: 15 Date: Volume 1 Tutorial 112-5

192 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files The process of loading an FE model into fe-safe involves extracting pertinent data from the FE model, and writing it to the working FED folder (see Appendix E). Therefore, the Current FE Models window is a summary of the contents of the working FED folder. In this case there are two stress datasets each containing elemental and centroidal data with 1004 elements (502 on the top shell and 502 on the bottom shell) in each dataset. The source of the datasets (the filename of the source FE model, the step, increment and timestamp) are also shown. fe-safe also extracts group information from the SETS defined in the first case control record in the case control data block in the.op2 file. When a new model is loaded, the output filename automatically defaults to: <ResultsDir>\{source_file_name}Results.{source_file_extension} which in this example is: <ResultsDir>\keyhole_01Results.op2 The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button: Exercise 1 : Multiaxial analysis using scale-and-combine loading Objective: To perform a multiaxial analysis of two superimposed fatigue load cases. Each load case consists of an elastically calculated unit load FEA stress solution (i.e. a stress dataset) and some load history data. The unit load and the load history are combined using a scale-and-combine method, as described in section 13. Analysis process: The fatigue life for each node is calculated as follows: the stress tensors are multiplied by the time history of the applied loading, to produce a time history of each of the 6 components of the stress tensor; the time histories of the in-plane principal stresses are calculated; the time histories of the three principal strains are calculated from the stresses; a multi-axial cyclic plasticity model is used to convert the elastic stress-strain histories into elastic plastic stress-strain histories; a critical plane method is used to identify the most damaging plane by calculating the damage on planes at 10 intervals between 0 and 180 in the surface of the component; for each of the critical planes, strains are resolved onto the three shear planes (1-2, 2-3 and 1-3); the time history of the damage parameter (which in this case, using the Brown-Miller algorithm, is the shear and normal strain) is cycle counted; individual fatigue cycles are identified using a Rainflow cycle algorithm, the fatigue damage for each cycle is calculated and the total damage is summed; the plane with the shortest life defines the plane of crack initiation, and this life is written to the output file. During this calculation, fe-safe may modify the endurance limit amplitude. If all cycles (on a plane) are below the Volume 1 Tutorial Vol. 1 Section 112 Issue: 15 Date:

193 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files endurance limit amplitude, there is no calculated fatigue damage on this plane. If any cycle is damaging, the endurance limit amplitude is reduced to 25% of the constant amplitude value, and the damage curve extended to this new endurance limit. The critical plane method is described and illustrated in detail in Volume 2. Method: Step 1: Define the loading: For this exercise two fatigue load cases will be superimposed. Each load case will consist of an elastically calculated unit load stress dataset and some load history data, as follows: the first dataset (Dataset 1: (1.1) S : LS1 CS1, SUBCASE 1) will be combined with channel 1 of the data file test_mcg2.amc; the second dataset (Dataset 2: (2.2) S : LS2 CS2, SUBCASE 2) will be combined with channel 2 of the data file test_mcg2.amc. To open the loading history data, select Open Data File from the File menu. Use the file selection dialogue to select the sample file test_mcg2.amc from the <DataDir> directory. The data file is summarised in the Loaded Data Files window. The sample file contains two channels of load data, identified in the tree view by the channel icon,. Figure To combine the unit load stress dataset with the loading history for the first case: select the Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; select Clear all loadings and click Yes from the tree context menu (right mouse click on the tree) to clear the existing loading definition; in the Current FE Models window, highlight the first dataset, labelled Dataset 1: (1.1) S : LS1 CS1, SUBCASE 1, (next to the stress dataset icon, ); in the Loaded Data Files window, highlight the first channel of data, labelled fe-safe tutorial scaler #1, (next to the channel icon ); select Add... >> A LOAD * dataset. Vol. 1 Section 112 Issue: 15 Date: Volume 1 Tutorial 112-7

194 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files To combine the unit load stress dataset with the loading history for the second case: in the Current FE Models window, highlight the second dataset, labelled Dataset 2: (2.1) S : LS2 CS2, SUBCASE 2, (next to the stress dataset icon, ); in the Loaded Data Files window, highlight the second channel of data, labelled fe-safe tutorial scaler #2, (next to the channel icon ). select Add... >> A LOAD * dataset. The defined loading appears in the loading details list box, as shown below: Figure Note: if the window does not appear exactly as shown in Figure , then expand the tree view to show more details. select the Analysis Settings tab from the Fatigue from FEA dialogue to switch to the main settings. Step 2: Define the subgroup option: The.op2 source file does not contain any geometry data for the FE model, required by the surface detection algorithm. Therefore for this tutorial all elements in the model should be used for analysis, not only those on its surface: double-click the Subgroup column header to open the Subgroup Selection dialogue for all groups: Figure Volume 1 Tutorial Vol. 1 Section 112 Issue: 15 Date:

195 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files select Whole group; click OK. Step 3: Define the surface finish: It is assumed that the whole component has a mirror-polished surface finish, (i.e. a Kt factor of 1). To define this surface finish for the whole component (i.e. all element groups): double-click the Surface column header to open the Surface Finish Definition dialogue for all groups: Figure select Select Surface Finish from list; click on the browse button,, to open the Select a surface finish file (*.kt) file dialogue; select the surface finish database file default.kt from the <KtDir> directory; from the drop-down Surface finish list, select Mirror Polished Ra <= 0.25µm; click OK. Vol. 1 Section 112 Issue: 15 Date: Volume 1 Tutorial 112-9

196 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files Step 4: Define the material: The component material is SAE 950C (Manten). The material record SAE_950C-Manten from the material database local.dbase will be defined for the whole component. Opened material databases are displayed in the Material Databases window as shown in Figure , below. Figure If the database local.dbase is not currently loaded in the Material Databases window, select File >> Materials >> Open Materials Database... and select local.dbase from the directory <UserDir>. Notice in Figure that the database local.dbase is the user s local copy from the <UserDir> directory. The other two databases shown are from the <DatabaseDir> directory. Expand the tree view to show the materials contained in local.dbase. The contents of the database can be filtered to show only materials of a particular type, by selecting one of the filter icons. To ensure that all materials in the database are displayed double-click on the All filter icon. The parameters for a material can be displayed by extending the material name. To define SAE_950C-Manten for the whole component: highlight the material SAE_950C-Manten in the local.dbase database; double-click the Material column header - a Change Material? confirmation dialogue box appears; Figure click YES; the material name should appear for all groups in the Material column. Volume 1 Tutorial Vol. 1 Section 112 Issue: 15 Date:

197 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files Step 5: Define the analysis algorithm: The material database identifies a default analysis algorithm for each material. The default analysis algorithm is normally selected automatically. To confirm that the default algorithm will be used for the whole model (i.e. all element groups): double-click the Algorithm column header to open the in Group Algorithm Selection dialogue box for all groups; Figure select the Analyse with material s default algorithm option; click OK. For SAE 950C (Manten) the default algorithm is Brown-Miller Biaxial Strain Life using Morrow mean-stress correction. Step 6: Define the in-plane residual stress: For this exercise it is assumed that there are no in-plane residual stresses. To set the residual stress to 0 (zero) for the whole component (i.e. all element groups): double-click the In-plane residual stress column header to open the In-plane Residual Stress dialogue for all groups: Figure enter a residual stress of 0 (zero), and click OK. Vol. 1 Section 112 Issue: 15 Date: Volume 1 Tutorial

198 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files Step 7: Define the output file: When the FE model was loaded, the output filename automatically defaulted to: <ResultsDir>\keyhole_01Results.op2 Before running the analysis, change the output filename to: <ResultsDir>\keyhole_01Results_ex01.op2 The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. Step 8: Run the analysis: fe-safe should now be configured to run the analysis. Press the Analyse! button. A summary of analysis parameters is displayed: Figure Check that the analysis is configured as shown in Figure , and then click Continue. Note that the UTS of the material is used to evaluate Kt from the defined surface finish curve (i.e. surface finish factor versus UTS). In this case, for a mirror-polished surface, Kt =1 for all values of UTS. Volume 1 Tutorial Vol. 1 Section 112 Issue: 15 Date:

199 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files As the analysis is being performed, the following information is written to the analysis log file. The analysis log file has the same file name as the output file, except that the extension is.log. So, for this analysis, the analysis log file is: <ResultsDir>\keyhole_01Results_ex01.log This information is also displayed in the Message Log window and includes: Summary ======= Worst Life-Repeats : at Element 1.4:1 Analysis time : 0:00:05 Step 9: Reviewing the results The analysis log shows that the worst-case life for the whole model is: repeats of the fatigue loading cycle, at element 1, node 4, shell section 1. Note: fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). In fe-safe, the design life and the calculated fatigue life always refer to the number of repeats of the complete defined fatigue loading cycle. An optional conversion factor can be used to convert the fatigue life in repeats to fatigue life with respect to some other quantity, for example hours or miles (see section 13). Volume 1 Tutorial Vol. 1 Section 112 Issue: 15 Date:

200 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files Step 10: Viewing the fatigue life contours: A copy of the original OP2 file was created, with a single stress dataset to hold the fatigue results see Appendix G for a description of this process. The fatigue life is written to the variable: X Normal Stress. In the file: <ResultsDir>/keyhole_01Results_ex01.op2, the fatigue life (written to the variable Strain X Normal) should look similar to Figure , the viewer colour scheme may need to be set to "Reversed Rainbow" and any averaging of values at nodes should be disabled. Figure : Log of Fatigue Lives. Volume 1 Tutorial Vol. 1 Section 112 Issue: 15 Date:

201 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files Additional notes for Exercise 1: 1. In this exercise, the two fatigue load cases are superimposed. Therefore, it does not matter in which order the loads are defined. For example: Loading is the same as: Loading Loading is 1 Repeats DS#1 * test_mcg2.amc:1 DS#2 * test_mcg2.amc:2 Loading is 1 Repeats DS#2 * test_mcg2.amc:2 DS#1 * test_mcg2.amc:1 2. In this example, the load history is very short, consisting of only five data points. For short load histories it is often more convenient to define the loading using a user-defined load history, rather than reading a load history from a data file (see section ). This is achieved using the A user-defined LOAD * dataset option. To re-define the loading for this exercise using user-defined load histories: Select the Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; select Clear all loadings and click Yes from the tree context menu (right mouse click on the tree) to clear the existing loading definition; in the Loaded Data Files window expand the filename test_mcg2.amc, so that both channels of data are displayed; highlight both channels of data (to select multiple channels highlight the first channel by clicking on it with the left mouse button, then hold down the CTRL key on the keyboard while clicking on any additional files); display a numerical listing of the two data channels by selecting View >> Numerical Listing (or just click the icon): Figure highlight the first unit stress dataset (labelled Dataset 1: (1.1) S : LS1 CS1, SUBCASE 1) in the Current FE Models window; Vol. 1 Section 112 Issue: 15 Date: Volume 1 Tutorial

202 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files select Add... >> A user-defined LOAD * dataset to display the Dataset Embedded Load History dialogue, and copy the five data points from the first column of the numerical listing display (scaler #1) into the Loading Scale box: Figure click OK; highlight the second unit stress dataset (labelled Dataset 2: (2.1) S : LS2 CS2, SUBCASE 2) in the Current FE Models window; define a load sequence for the second case, as described above, using the data from the second column of the numerical listing display (scaler #2). The new loading definition appears in the Loading Details area of the Fatigue from FEA dialogue, as shown in Figure , below. Figure Note: if the window does not appear exactly as shown in Figure , then expand the tree view to show more details. Volume 1 Tutorial Vol. 1 Section 112 Issue: 15 Date:

203 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files 3. The load definition (LDF) file can be used to define simple and complex loading scenarios. Section 13 includes a full description of the LDF file, including syntax. The loading for this exercise can be seen by saving the loading to a load definition file: select File >> Save Current FEA Loadings As...; save the file as ex01_s-c.ldf and click Save; open the file in a text editor to display the contents (comments may vary): #.ldf file created by fe-safe [mswin] INIT END # Block number 1 BLOCK lh= , ds=1 lh= , ds=2 END 4. In this exercise the surface finish was defined by selecting a surface type (in this case mirror-polished ) from a surface finish database. If the actual surface finish factor, Kt, for the component is known (for mirror-polished, the Kt factor has a value of 1) then it can be specified as a value. To define a userdefined value for Kt, select Define Kt as a value, in the Surface Finish Definition dialogue box: Figure The results data can be exported to an alternative file format at the end of the analysis, by changing the extension of the output file (Fatigue from FEA >> Output File) to a recognised type. Vol. 1 Section 112 Issue: 15 Date: Volume 1 Tutorial

204 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files For example: to export to an ASCII CSV results file, change the extension to.txt,.csv or.asc (this is useful for viewing a table of results in an editor or spreadsheet). Alternatively, after the analysis is complete, and the OP2 file has been created, the results data can be written to another output file in addition to the original output OP2 file, using the Save FEA Fatigue Results As... option in the File menu. This option displays the Save FEA Fatigue Results As... dialogue box, as shown in Figure , below: Figure The FER (.fer) file (see Appendix E) is an intermediate file containing the results of the analysis. This new output file type is determined by the extension of the file entered in the Output File box. A copy of the original output OP2 file can be created if the extension.op2 is used. 6. To analyse individual elements or nodes, list the required items in the Exports and Outputs dialogue, and select the Only analyse listed items dialogue. Additional outputs and diagnostics options can also be specified. Diagnostics and additional outputs are discussed in detail in section To save the current analysis configuration, select Save FEA Fatigue Definition File..., and enter a filename ending with the extension.stlx. The analysis can be reloaded at a later date by restoring the project definition file, using Open FEA Fatigue Definition File...,. Volume 1 Tutorial Vol. 1 Section 112 Issue: 15 Date:

205 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files Exercise 2 : Multiaxial analysis of a data sets sequence, including Factor Of Strength evaluation Objective: To perform a multiaxial analysis of a series of events in this case a sequence of two elastically calculated FEA stress solution (i.e. stress datasets). The analysis will also include an evaluation of the Factor of Strength (FOS). This is the factor by which the loading must be scaled to achieve a specified design life. The FOS method is described in detail in section 17. Analysis process: The Strength Factor (FOS) for each node is calculated as follows: the calculated life is compared with the design life: - if the calculated life is lower than the design life, the elastic stresses at the node are scaled by a factor less than 1.0; - if the calculated life is greater than the design life, the elastic stresses at the node are scaled by a factor greater than 1.0. the elastic stress history is recalculated using the re-scaled nodal stresses; for local strain analysis, the cyclic plasticity model is used to recalculate the time history of elastic-plastic stress-strains - the fatigue life is then recalculated; in the critical plane analysis, the critical plane orientation is re-calculated; the process is repeated with different scale factors until: (i) (ii) the calculated life is within 5% of the design life or the step change of 0.01 or 0.1 in the FOS value causes the design life to be bracketed, or (iii) the FOS exceeds the max factor (default 2.0) or is less than the min factor (default 0.5). Method: Step 1: Define the loading: The series of events being analysed in this exercise consists of a sequence of two elastically calculated FEA stress solution (i.e. stress datasets) scaled by a defined scale factor. The definition of the sequence will be as follows: the first dataset (Dataset 1: (1.1) S : LS1 CS1, SUBCASE 1) multiplied by a scale factor of 20000, followed by: the second dataset (Dataset 2: (2.1) S : LS2 CS2, SUBCASE 2) multiplied by a scale factor of The loading for this loading sequence can be defined in a single loading block: select the Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree; select Clear all loadings and click Yes from the tree context menu (right mouse click on the tree) to clear the existing loading definition; Vol. 1 Section 112 Issue: 15 Date: Volume 1 Tutorial

206 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files highlight the first unit stress dataset in the Current FE Models window; select Add... >> Dataset; highlight the second unit stress dataset in the Current FE Models window; select Add... >> Dataset; highlight the dataset item in the loading tree of the Fatigue from FEA dialogue; select Scale from the tree context menu (right mouse click on the tree) and enter the value 20000; press enter to accept the value. If saved as a.ldf it would look like: #.ldf file created by fe-safe INIT END # Block number 1 BLOCK ds=1, scale=20000 ds=2, scale=20000 END The new loading definition appears in the Loading Details area of the Fatigue from FEA dialogue, as shown in Figure Figure select the Analysis Settings tab from the Fatigue from FEA dialogue to switch to the main settings. Step 2: Define the subgroup option: As in Exercise 1, all elements in the model should be used for analysis - see (Exercise 1), Step 2. Volume 1 Tutorial Vol. 1 Section 112 Issue: 15 Date:

207 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files Step 3: Define the surface finish: As in Exercise 1, the component is assumed to have a mirror-polished surface finish, (i.e. a Kt factor of 1) - see (Exercise 1), Step 3. Step 4: Define the material: As in Exercise 1, the component is assumed to be made from SAE 950C (Manten) see (Exercise 1), Step 4. Step 5: Define the analysis algorithm: As in Exercise 1, the default analysis algorithm for the material will be used, which for SAE 950C (Manten) is Brown-Miller Biaxial Strain Life using Morrow mean-stress correction. Step 6: Define the in-plane residual stress: As in Exercise 1, it is assumed that there are no in-plane residual stresses - see (Exercise 1), Step 6. Step 7: Configuring the Factor of Strength (FOS) analysis: To configure the Factor of Strength (FOS) analysis: click on the Factor of Strength button in the Fatigue from FEA window to open the Factor of Strength Calculations dialogue box: Figure select the Perform Factor of Strength (FOS) Calculations? option to enable the FOS analysis.; select Infinite design life (use material s Endurance Limit) this uses the constant amplitude endurance limit for the component material, which for SAE 950C (Manten) is: reversals; Note: fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). click OK; Volume 1 Tutorial Vol. 1 Section 112 Issue: 15 Date:

208 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files specify the FOS band limits in the Analysis Options dialogue [FEA Fatigue >> Analysis Options...] Safety Factors tab as shown in Figure , to determine the limits and precision of the FOS analysis: - between the fine limits, the FOS is calculated to a resolution of approximately 0.01 repeats; - between maximum and minimum, the FOS is calculated to a resolution of approximately 0.1 repeats; - if the evaluated FOS is greater than 2, then a FOS of 2 is exported for the node; - if the evaluated FOS is less than 0.5, then a FOS of 0.5 is exported for the node. Figure Step 8: Define the output file: Before running the analysis, change the output filename to: <ResultsDir>\keyhole_01Results_ex02.op2 The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. Volume 1 Tutorial Vol. 1 Section 112 Issue: 15 Date:

209 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files Step 9: Run the analysis: fe-safe should now be configured to run the analysis. Press the Analyse! button. A summary of analysis parameters is displayed: Figure Check that the analysis is configured as shown in Figure , and then click Continue. Note that the UTS of the material is used to evaluate Kt from the defined surface finish curve (i.e. surface finish factor versus UTS). In this case, for a mirror-polished surface, Kt =1 for all values of UTS. As the analysis is being performed, the following information is written to the analysis log file. The analysis log file has the same file name as the output file, except that the extension is.log. So, for this analysis, the analysis log file is: <ResultsDir>\keyhole_01Results_ex02.log This information displayed in the Message Log window includes the following Summary ======= Worst Life-Repeats : at Element 1.4:1 Worst FOS@Life=Infinite : at Element 1.4:1 Analysis time : 0:00:09 Vol. 1 Section 112 Issue: 15 Date: Volume 1 Tutorial

210 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files Step 10: Reviewing the results The analysis log shows that the worst-case life for the whole model is: repeats of the loading, at element 1, node 4, shell section 1. The worst-case Factor of Strength (FOS) for the analysis is: at element 1, node 4, shell section 1. In the configuration of the Factor of Strength analysis, the target life specified was the Infinite design life, which is assumed to be the materials constant amplitude endurance limit, which for SAE 950C (Manten) is: reversals. The worst-case fatigue lives are of the order repeats of the fatigue loading cycle, which is less than the design life ( repeats of the loading). This is why the worst-case strength factor (the factor by which the loading must be scaled to achieve the design life) is somewhat less than 1. The FOS method is described in detail in section 17. Note: fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). In fe-safe, the design life and the calculated fatigue life always refer to the number of repeats of the complete defined fatigue loading cycle. An optional conversion factor can be used to convert the fatigue life in repeats to fatigue life with respect to some other quantity, for example hours or miles (see section 13). Volume 1 Tutorial Vol. 1 Section 112 Issue: 15 Date:

211 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files Step 11: Viewing the fatigue life contour: Since the original.op2 file contains two layers (sections) the output file also contains two sets of results data for both the fatigue life and the FOS. In this example, the stresses in both sections are the same. Therefore, the fatigue results and the FOS are also the same for both sections. In the file <ResultsDir>/keyhole_01Results_ex02.op2, the fatigue life (written to variable Strain X Normal) should look similar to Figure , the viewer colour scheme may need to be set to "Reversed Rainbow" and any averaging of values at nodes should be disabled. Figure Vol. 1 Section 112 Issue: 15 Date: Volume 1 Tutorial

212 Tutorial 112 : Using fe-safe with NASTRAN OUTPUT2 results (*.OP2) files In the file <ResultsDir>/keyhole_01Results_ex02.op2, the strength factors FOS (written to variable Strain Y Normal) should look similar to Figure , the viewer colour scheme may need to be set to "Reversed Rainbow" and any averaging of values at nodes should be disabled. Figure Volume 1 Tutorial Vol. 1 Section 112 Issue: 15 Date:

213 Tutorial 113 : Analysis of an axially symmetric model using fe-safe/rotate 113 Tutorial 113 : Analysis of an axially symmetric model using fe-safe/rotate Introduction This tutorial demonstrates the application of fe-safe/rotate to models of rotating components that exhibit axial symmetry. This tutorial should be read in conjunction with section 21, Analysis of Axially Symmetric Models Using fesafe/rotate. The following sample files used for this tutorial are located in the directory <DataDir>\fe-safe_rotate: wheel_01.db : Ansys FE model file. wheel_01.s01 : Load step file for load step 1. wheel_01.s02 : Load step file for load step 2. wheel_01.s03 : Load step file for load step 3. wheel_01.s04 : Load step file for load step 4. wheel_a_01.rst : Results of FE stress analysis for load steps 1, 2, 3 and Preparation The tutorial uses an Ansys RST model. However, the same techniques can be applied to all FE formats supported by fe-safe/rotate, which currently include: Ansys results (*.rst) files Abaqus FIL files This tutorial assumes that the user is familiar with the basic program operation. Before attempting this tutorial, it is strongly recommended that one of the introductory tutorials is followed: Tutorial 105: Using fe-safe with Abaqus.fil files Tutorial 108: Using fe-safe with ANSYS.rst files Start the program by selecting fe-safe from the Windows Start menu (Windows) or by running the script fe-safe (Linux) see section 5. Volume 1 Tutorial Vol. 1 Section 113 Issue: 17 Date:

214 Tutorial 113 : Analysis of an axially symmetric model using fe-safe/rotate Select an existing project, or create a new one from the welcome page Figure Ensure that the following basic settings are correctly configured. If fe-safe is being run for the first time then it is possible to skip this preparatory section. Reset any existing analysis options to their defaults in the Clear Data and Settings dialogue [Tools >> Clear Data and Settings...], shown in Figure 113-2, below, by selecting the Select all option and clicking OK. Figure Volume 1 Tutorial Vol. 1 Section 113 Issue: 17 Date:

215 Tutorial 113 : Analysis of an axially symmetric model using fe-safe/rotate Sample model. The model used for this tutorial is a simple wheel, as shown in Figure 113-3: Figure The elements in the model exhibit axial symmetry in 64 orientations. For this tutorial, we will take advantage of this symmetry to divide the model into four 90 axisymmetric segments. The master segment needs to be defined by listing the group/material numbers that make up the segment (Ansys uses material numbers to define groups of elements). The complete sample model is actually defined by seven different material numbers, as shown in Figure 113-4: Figure Volume 1 Tutorial Vol. 1 Section 113 Issue: 17 Date:

216 Tutorial 113 : Analysis of an axially symmetric model using fe-safe/rotate We can define a 90 master segment by specifying that it consists of materials 1, 2, 3, 4 and 5. In Ansys, four load steps (wheel_01.s01, wheel_01.s02, wheel_01.s03 and wheel_01.s04) were created. The first load step was generated for the model in its original orientation. The second load step was generated as if the model had been rotated through The third and fourth load steps were generated as if the model had been rotated through 45 and 67.5, respectively. An FE analysis of static stresses was performed by solving the four load steps, and the results were written to the Ansys results file wheel_a_01.rst. The stresses produced can be visualised by plotting element solutions for the four results sets in wheel_a_01.rst. These are illustrated in Figure 113-5, which shows the von Mises stresses for each solution. Figure Volume 1 Tutorial Vol. 1 Section 113 Issue: 17 Date:

217 Tutorial 113 : Analysis of an axially symmetric model using fe-safe/rotate Opening the sample FE model using fe-safe/rotate. Select File >> FEA Solutions >> Open Finite Element Model Using Rotational Symmetry... from the main fe-safe menu. The fe-safe/rotate dialogue appears, configure the options as follows: In General Options, select the FE results file to import: <DataDir>\fe-safe_rotate\wheel_a_01.rst; select the Axis of rotational symmetry as the Z-Axis from the drop-down list; set the Num. of rotations of master segment needed (n) to 4 (as the model has four 90 segments); set the No. of solutions in master segment (n2) to 4 (as there are 4 load steps in each segment); leave the Warning tolerance for finding rotated elements box blank for fe-safe/rotate to calculate the tolerance automatically. set the List of group names defining master segment to 1,2,3,4,5 (as materials 1-5 contain elements of the master segment, see section ); The fe-safe/rotate dialogue should now look similar to Figure 113-6: Figure fe-safe/rotate is now configured, and ready to process the FE results file. Press the OK button. Volume 1 Tutorial Vol. 1 Section 113 Issue: 17 Date:

218 Tutorial 113 : Analysis of an axially symmetric model using fe-safe/rotate A prompt to pre-scan the file will be displayed if the file has not yet been pre-scanned. When the pre-scan of the file is complete, the Select Datasets to Read dialogue will be displayed. The file wheel_a_01.rst contains four stress datasets corresponding to the four solutions identified earlier and corresponding temperature datasets. Only the stress datasets are required for the tutorial, the temperature datasets do not need to be loaded. Check the Stresses and Last increment only boxes, click Apply to Dataset List to apply the selection and select OK to load the remaining datasets, as shown in Figure Figure When the model has finished loading, ensure that the stress, strain and temperature units are set to MPa, µe and deg.c, respectively. If the Units dialogue is not shown automatically, right click within Current FE Models window and select Properties. Then change the values to those shown in Figure and click OK. Figure Volume 1 Tutorial Vol. 1 Section 113 Issue: 17 Date:

219 Tutorial 113 : Analysis of an axially symmetric model using fe-safe/rotate As fe-safe loads the model, information about the file and the data it contains is appended to the file: <ProjectDir>\Model\reader.log. This information is also displayed in the Message Log window. A summary of the open model appears in the Current FE Models window, showing the loaded datasets and element group information, as in Figure Figure Volume 1 Tutorial Vol. 1 Section 113 Issue: 17 Date:

220 Tutorial 113 : Analysis of an axially symmetric model using fe-safe/rotate Performing the analysis. Step 1: Define the loading: During the loading process, fe-safe/rotate automatically creates loading information in the form of an LDF file, containing a series of loading blocks, ready for use in the fatigue analysis, and automatically updates fe-safe loading options to use the new LDF file. Step 2: Define the subgroup option: The surface detection algorithm is not supported with fe-safe/rotate, therefore all elements in the model should be used for analysis, not only those on its surface double-click the Subgroup column header to open the Subgroup Selection dialogue for all groups: Figure select Whole group; click OK. Step 3: Define the surface finish: The component is assumed to have a mirror-polished surface finish, set the Surface option to Mirror Polished Ra <= 0.25µm (i.e. a Kt factor of 1). double-click the Surface column header to open the Surface Finish Definition dialogue for all groups: Figure select Select Surface Finish from list; click on the browse button,, to open the Select a surface finish file (*.kt) file dialogue; Volume 1 Tutorial Vol. 1 Section 113 Issue: 17 Date:

221 Tutorial 113 : Analysis of an axially symmetric model using fe-safe/rotate select the surface finish database file default.kt from the <KtDir> directory; from the drop-down Surface finish list, select Mirror Polished Ra <= 0.25µm; click OK. Step 4: Define the material: The component is assumed to be made from SAE 950C (Manten), set the Material option to SAE_950C-Manten. The material record SAE_950C-Manten from the material database local.dbase will be defined for the whole component. Opened material databases are displayed in the Material Databases window as shown in Figure , below. Figure If the database local.dbase is not currently loaded in the Material Databases window, select File >> Materials >> Open Materials Database... and select local.dbase from the directory <UserDir>. Notice in Figure that the database local.dbase is the user s local copy from the <UserDir> directory. The other two databases shown are from the <DatabaseDir> directory. Expand the tree view to show the materials contained in local.dbase. The contents of the database can be filtered to show only materials of a particular type, by selecting one of the filter icons. To ensure that all materials in the database are displayed double-click on the All filter icon. The parameters for a material can be displayed by expanding the material name. To define SAE_950C-Manten for the whole component: highlight the material SAE_950C-Manten in the local.dbase database; double-click the Material column header - a Change Material? confirmation dialogue box appears; Figure click YES; the material name should appear for all groups in the Material column. Volume 1 Tutorial Vol. 1 Section 113 Issue: 17 Date:

222 Tutorial 113 : Analysis of an axially symmetric model using fe-safe/rotate Step 5: Define the analysis algorithm: The default analysis algorithm for the material will be used, which for SAE 950C (Manten) is Brown-Miller Biaxial Strain Life using Morrow mean-stress correction. Step 6: Define the in-plane residual stress: It is assumed that there are no in-plane residual stresses. Step 7: Run the analysis: fe-safe is now ready to perform the analysis. Press the Analyse! button and accept the pre-analysis summary. The following text appears in the message log: Summary ======= Worst Life-Repeats : at Element Analysis time : 0:00:17 This fatigue results from this exercise were written to the file: <ResultsDir>/wheel_a_01Results.rst The fatigue results can now be viewed in Ansys by loading the results file and selecting the last result set in the file. The fatigue life is saved in place of the SX (stresses in X direction) parameter, plotting SX displays a contour plot of the log of the fatigue life, as shown in Figure The viewer colour scheme may need to be set to "Reversed Rainbow" and any averaging of values at nodes should be disabled. Figure Volume 1 Tutorial Vol. 1 Section 113 Issue: 17 Date:

223 Tutorial 114 : PSD Fatigue Analysis 114 Tutorial 114 : PSD Fatigue Analysis Introduction This tutorial demonstrates PSD fatigue analysis of a flat plate. The tutorial includes opening the FE model and configuring the analysis, followed by calculating life using the Dirlik algorithm with Von Mises stress. A later section demonstrates the use of the alternative Tovo-Benasciutti algorithm using an appended residual stress dataset to provide a non-zero cycle mean. The ODB, RST and OP2 file formats are portable between platforms. The use of Abaqus.odb files in fe-safe is discussed in detail in Appendix G. The sample *.psd files used for this tutorial are located in the directory <DataDir>. The sample Abaqus files used for this tutorial are located in the directory <DataDir>\Abaqus. The sample ANSYS files used for this tutorial are located in the directory <DataDir>\ANSYS. The sample NASTRAN files used for this tutorial are located in the directory <DataDir>\Nastran. NOTE: The nomenclature used throughout this tutorial when referring to files and directories is as described in Appendix B Model Description The model for the first tutorial is a flat plate, as shown in Figure 114-1: Figure The FE model under investigation is the steel plate illustrated above. The actual FE mesh is comprised of second order hexahedral elements. Boundary conditions ensure that points A and B are fixed in DOF 1-6. A natural frequency analysis was run to retrieve the first 10 natural frequencies and their corresponding stress states, resulting in abaqus_plate.odb, ansys_plate.rst or nastran_plate.op2 depending on the selected solver. Two Frequency sweep analyses were then run on each model. These are called Steady State Dynamic Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial 114-1

224 Tutorial 114 : PSD Fatigue Analysis (Abaqus), Harmonic (ANSYS) or Frequency Response (NASTRAN) analyses depending on the solver. Each response analysis is characterised by a 1N force applied in the Z direction at one of the pilot nodes displayed as points C (channel 1) or D (channel 2). In the case of Abaqus, the Steady State Dynamic Analysis steps resulted in file abaqus_plate_mpfs.odb for both steps. In the case of ANSYS two.mcf files were generated from the Harmonic Analysis corresponding to the two channels. The ANSYS.mcf files were renamed with respect to channel number (resulting in plate_1.mcf and plate_2.mcf) in order to satisfy the file name convention detailed in section 27 of the fe-safe User Guide. In the case of NASTRAN two.pch files were generated from the Frequency Response Analysis corresponding to the two channels. The NASTRAN.pch files were renamed with respect to channel number (resulting in plate_1.pch and plate_2.pch) in order to satisfy the file name convention detailed in section 27 of the fe-safe User Guide. The PSD spectrum shown in Figure will be used in the loading, and is repeated twice in the file plate.psd so that there are two PSD channels, one corresponding to each channel in the Generalized Displacement data (also called Modal Participation Factors in ANSYS). Figure Note: Due to differences in implementation of damping, frequency sweep responses from Abaqus, ANSYS and NASTRAN models are different, but the same process flow can be applied for each solver for the purposes of this tutorial Preparation This tutorial uses Abaqus ODB models, an ANSYS RST model with associated.mcf files, or a NASTRAN OP2 model with associated.pch files. It is assumed that the user is familiar with the basic program operation. Before attempting this tutorial, it is strongly recommended that one of the introductory tutorials is followed: Tutorial 106: Using fe-safe with Abaqus.odb files Tutorial 108: Using fe-safe with ANSYS.rst files Tutorial 112: Using fe-safe with NASTRAN.op2 files Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

225 Tutorial 114 : PSD Fatigue Analysis Start the program by selecting fe-safe from the Windows Start menu (Windows) or by running the script fe-safe (Linux). Select an existing project, or create a new one from the welcome page Figure If an existing project directory is chosen, existing data in that project will be retained. This includes FE data, load history files, analysis settings and more. Ensure that the following basic settings are correctly configured. If fe-safe is being run for the first time then it is possible to skip this preparatory section. Reset any existing analysis options to their defaults in the Clear Data and Settings dialogue [Tools >> Clear Data and Settings...], shown in Figure below, by selecting the Select all option and clicking OK. Figure For Opening the sample FE model (Abaqus Model) continue to section For Opening the sample FE model (ANSYS Model) continue to section For Opening the sample FE model (NASTRAN Model) continue to section Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial 114-3

226 Tutorial 114 : PSD Fatigue Analysis Opening the sample FE model (Abaqus Model) To open the model, select File >> FEA Solutions >> Open Finite Element Model For PSD Analysis... This will display the dialogue shown in Figure below. Select the Source FE Model file abaqus_plate_single.odb from the directory <DataDir>\Abaqus. Leave the Use the same source file for Generalized Displacement data checkbox selected, and leave the Polar (degrees) radio button selected. Note that the checkbox and radio button selection are defaulted to these settings when the source FE model is an ODB. Finally, select the PSD file plate.psd from the directory <DataDir>. Click OK. Figure Note: The complex Generalized Displacement Data being imported into fe-safe can be expressed in either polar or rectangular form. By default, a Steady State Dynamic Analysis in Abaqus exports such data in polar form, i.e. with modulus and argument components (where the angles are expressed in degrees), hence the Complex number notation field setting above. Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

227 Tutorial 114 : PSD Fatigue Analysis The Select Datasets to Read dialogue will appear as shown in Figure Check the Quick-select boxes for Stresses and Other, and if it is selected, deselect the box for Last Increment Only. Click Apply to Dataset List. Deselect the dataset marked Mode 0 (this Initial State is not used in PSD loading) as shown in Figure Click OK. Figure Scroll down and make sure that Steps 2 and 3 (the Generaized Displacements and Phase Angle Histories) are selected. As fe-safe loads the model, information about the file and the data it contains is appended to the file: <ProjectDir>\Model\reader.log. This information is also displayed in the Message Log window. Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial 114-5

228 Tutorial 114 : PSD Fatigue Analysis When the model has finished loading, the Loaded FEA Models Properties dialogue box appears, as shown in Figure Set the units to MPa, N, mm. Figure If the dialogue box does not appear automatically, then it can be displayed by double-clicking on the Current FE Models window. icon in the Ensure that the units are as shown in Figure 114-7, then click OK. A dialogue will appear prompting to edit element groups loaded from the model, click Yes. Use the button to move all groups to the list of Unused Groups. Click OK. Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

229 Tutorial 114 : PSD Fatigue Analysis A summary of the open model appears in the Current FE Models window, showing the loaded datasets and element group information see below. Figure Note: If the window does not appear exactly as shown in Figure 114-8, then expand the tree view to show more details. The process of loading an FE model into fe-safe involves extracting pertinent data from the FE model, and writing it to the /model subdirectory of the project directory (see Appendix E, section ). Therefore, the Current FE Models window is a summary of the contents of the working FED folder. In this case there are 10 modal stress datasets each containing elemental data with 925 elements in each dataset. The source of the dataset (the filename of the source FE model, the step, increment and timestamp) are also shown. fe-safe also extracts element group information from the FE model file. Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial 114-7

230 Tutorial 114 : PSD Fatigue Analysis The Generalized Displacements (GDs) were loaded from Steps 2 and 3 of the FE model. These define weightings for each node for each mode within each channel, and are used to convert the input channel PSDs to the nodal response PSDs which are the basis of the fatigue calculations. The data is summarised in the Generalized Displacements item in the Current FE Models window. The sample file contains 10 modes, and two channels of GDs from 0 to 300 Hz as shown above. When a new model is loaded, the output filename automatically defaults to: <ResultsDir>\{source_file_name}Results.{source_file_extension} The output filename can be modified by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. Continue to section Exercise 1: Finite life using the Dirlik algorithm with Von Mises stress. Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

231 Tutorial 114 : PSD Fatigue Analysis Opening the sample FE model (ANSYS Model) To open the model, select File >> FEA Solutions >> Open Finite Element Model For PSD Analysis... This will display the dialogue shown in Figure Select the Source FE Model file ansys_plate.rst from the directory <DataDir>\Ansys. Select the Generalized Displacement data (Modal Participation Factors in ANSYS terminology) files plate_1.mcf and plate_2.mcf from the directory <DataDir>\Ansys then click on the Rectangula radio button. Finally, select the PSD data file plate.psd from the directory <DataDir>. Click OK. Figure Note: The default settings for a Harmonic Analysis in ANSYS result in complex-valued Generalized Displacement data (also called Modal Participation Factors in ANSYS) which are exported in rectangular form, i.e. with real and imaginary components, hence the Complex number notation field setting above. Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial 114-9

232 Tutorial 114 : PSD Fatigue Analysis A dialogue will be shown prompting the user Do you want to Pre-scan? Click Yes. The Select Datasets to Read dialogue will appear as shown in Figure Check the Quick-select box for Stresses, and if it is selected, deselect the box for Last Increment Only. Click Apply to Dataset List. The Generalized Displacements (GDs) will not appear in the list. This is expected, as these are loaded from separate.mcf text files for ANSYS models. Click OK. Figure As fe-safe loads the model, information about the file and the data it contains is appended to the file: <ProjectDir>\Model\reader.log. This information is also displayed in the Message Log window. Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

233 Tutorial 114 : PSD Fatigue Analysis When the model has finished loading, the Loaded FEA Models Properties dialogue box appears, as shown in Figure Set the units to Pa, N, m. Figure If the dialogue box does not appear automatically, then it can be displayed by double-clicking on the Current FE Models window. icon in the Ensure that the units are as shown in Figure , then click OK. A dialogue will appear prompting to edit element groups loaded from the model, click Yes. Use the button to move all groups to the list of Unused Groups. Click OK. Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial

234 Tutorial 114 : PSD Fatigue Analysis A summary of the open model appears in the Current FE Models window, showing the loaded datasets and element group information see below Figure Figure Note: If the window does not appear exactly as shown in Figure , then expand the tree view to show more details. The process of loading an FE model into fe-safe involves extracting pertinent data from the FE model, and writing it to the /model subdirectory of the project directory (see Appendix E, section ). Therefore, the Current FE Models window is a summary of the contents of the working FED folder. In this case there are 10 modal stress datasets each containing elemental data with 925 elements in each dataset. The source of the dataset (the filename of the source FE model, the step, increment and timestamp) are also shown. fe-safe also extracts element group information from the FE model file. Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

235 Tutorial 114 : PSD Fatigue Analysis The FE analysis files (.mcf files for ANSYS) containing the Generalized Displacements were loaded. The data is summarised in the Generalized Displacements item in the Current FE Models window. The sample file contains 10 modes, and two channels of GDs from 0 to 100 Hz as shown above. When a new model is loaded, the output filename automatically defaults to: <ResultsDir>\{source_file_name}Results.{source_file_extension} The output filename can be modified by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. Continue to section Exercise 1: Finite life using the Dirlik algorithm with Von Mises stress. Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial

236 Tutorial 114 : PSD Fatigue Analysis Opening the sample FE model (NASTRAN Model) To open the model, select File >> FEA Solutions >> Open Finite Element Model For PSD Analysis... This will display the dialogue shown in Figure Select the Source FE Model file nastran_plate.op2 from the directory <DataDir>\Nastran. Select the Generalized Displacement data plate_1.pch and plate_2.pch from the directory <DataDir>\Nastran then click on the Rectangular radio button. Finally, select the PSD data file plate.psd from the directory <DataDir>. Click OK. Figure A dialogue will be shown prompting the user Do you want to Pre-scan? Click Yes. Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

237 Tutorial 114 : PSD Fatigue Analysis The Select Datasets to Read dialogue will appear as shown in Figure Check the Quick-select box for Stresses, and if it is selected, deselect the box for Last Increment Only. Click Apply to Dataset List. The Generalized Displacements (GDs) will not appear in the list. This is expected. Click OK. Figure As fe-safe loads the model, information about the file and the data it contains is appended to the file: <ProjectDir>\Model\reader.log. This information is also displayed in the Message Log window. Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial

238 Tutorial 114 : PSD Fatigue Analysis When the model has finished loading, the Loaded FEA Models Properties dialogue box appears, as shown in Figure Set the units to MPa, N, m. Figure If the dialogue box does not appear automatically, then it can be displayed by double-clicking on the Current FE Models window. icon in the Ensure that the units are as shown in Figure , then click OK. A dialogue will appear prompting to edit element groups loaded from the model, click Yes. Use the button to move all groups to the list of Unused Groups. Click OK. Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

239 Tutorial 114 : PSD Fatigue Analysis A summary of the open model appears in the Current FE Models window, showing the loaded datasets and element group information see below Figure Figure Note: If the window does not appear exactly as shown in Figure , then expand the tree view to show more details. The process of loading an FE model into fe-safe involves extracting pertinent data from the FE model, and writing it to the /model subdirectory of the project directory (see Appendix E, section ). Therefore, the Current FE Models window is a summary of the contents of the working FED folder. In this case there are 10 modal stress datasets each containing elemental data with 925 elements in each dataset. The source of the dataset (the filename of the source FE model, the step, increment and timestamp) are also shown. fe-safe also extracts element group information from the FE model file. Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial

240 Tutorial 114 : PSD Fatigue Analysis The FE analysis files (.pch files for NASTRAN) containing the Generalized Displacements were loaded. The data is summarised in the Generalized Displacements item in the Current FE Models window. The sample file contains 10 modes, and two channels of GDs from 0 to 100 Hz as shown above. When a new model is loaded, the output filename automatically defaults to: <ResultsDir>\{source_file_name}Results.{source_file_extension} The output filename can be modified by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

241 Tutorial 114 : PSD Fatigue Analysis Exercise 1: Finite life using the Dirlik algorithm with Von Mises stress Objective: Calculate fatigue life of the plate using the loaded Generalized Displacements and 2-channel PSD signal. This procedure is applicable to Abaqus, ANSYS and NASTRAN-derived input files (as summarised in sections 114.4, and 114.6); however, the screenshots will focus on the ANSYS-related procedure and results. Analysis process: The finite life for each node is calculated as follows: Modal stresses and GDs are collected and used to calculate frequency response functions. The frequency response functions and the PSD data are used to calculate the Von Mises equivalent stress. The Dirlik method makes use of the Von Mises equivalent stress to provide a closed form solution to estimate the Probability Density Function (PDF) of stress range and produce a cycle histogram of stress ranges. Fatigue damage per block is calculated from the cycle histogram: o o The number of bins in the cycle histogram is configured by setting the Number of stress range intervals. The maximum stress range in the histogram is configured by setting the RMS stress cut-off multiple (see section 27 of the fe-safe User Guide). Method: Step 1: Automatic loading definition: For this exercise 10 modes and GDs for two channels will be combined with a two channel PSD file to create the PSD loading. The necessary loading definition was generated automatically. To view the automatic loading definitions: Select the Loading Settings tab from the Fatigue from FEA dialogue to switch to the loading tree. The defined loading appears in the loading details list box, as shown in Figure Note: If the window does not appear exactly as shown in Figure , then expand the tree view to show more details. Instructions on how to complete the same loading definitions manually are in the notes at the end of this exercise. Figure Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial

242 Tutorial 114 : PSD Fatigue Analysis The signal time length of 1 seconds is specified in the plate.psd file header. If a psd file is used without this optional header line, then the time would display as zero, and you would need to double click on the Length per repeat field to set the time length of the signal. Select the Analysis Settings tab from the Fatigue from FEA dialogue to switch to the main settings. Step 2: Define the subgroup option: For this tutorial we ll allow fe-safe to analyse the whole group, although surface detection is available. See section 5 of the fe-safe User Guide for details on the subgroup selection. Double-click the Subgroup column header to open the Subgroup Selection dialogue for all groups: Figure Select Whole group. Click OK. Step 3: Define the surface finish: It is assumed that the whole component has a mirror-polished surface finish, (i.e. a Kt factor of 1). To define this surface finish for the whole component (i.e. all element groups): double-click the Surface column header to open the Surface Finish Definition dialogue for all groups: Figure Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

243 Tutorial 114 : PSD Fatigue Analysis select Select Surface Finish from list; click on the browse button,, to open the Select a surface finish file (*.kt) file dialogue; select the surface finish database file default.kt from the <KtDir> directory; from the drop-down Surface finish list, select Mirror Polished Ra <= 0.25µm; click OK. Step 4: Define the material: The component material is SAE The material record SAE from the material database system.dbase will be defined for the whole component. Opened material databases are displayed in the Material Databases window as shown in Figure If this window is not displayed, select Window Auto Arrange to display it. Click in the <New Filter> field next to the Filter: drop-down and enter the string 1045 as shown. Figure If the database system.dbase is not currently loaded in the Material Databases window, select File >> Materials >> Open Materials Database... and select system.dbase from the directory <DatabaseDir>. Notice in Figure that the database system.dbase is the System Database from the <DatabaseDir> directory. The parameters for a material can be displayed by expanding the tree view of the material name. To define SAE for the whole component: In the Material Databases window, highlight the material SAE in the system.dbase database. In the Fatigue from FEA dialogue (group parameters table), double-click the Material column header - a Change Material? confirmation dialogue box appears; click YES. The material name should appear for all groups in the Material column. Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial

244 Tutorial 114 : PSD Fatigue Analysis Step 5: Define the analysis algorithm: The method of opening the model was used to default the PSD Group Algorithm: Double-click the Algorithm column header to open the PSD Group Algorithm Selection dialogue box for all groups: Figure Select the default Dirlik option then click OK. Step 6: Define the PSD settings: Specify the PSD settings in the Analysis Options dialogue. Configure the PSD settings by accessing the Analysis Options: Specify the PSD settings in the Analysis Options dialogue [FEA Fatigue Analysis Options ] Scroll the tabs to the right in the dialogue to access the PSD tab as shown in Figure below. Use the default PSD Response setting (Von Mises radio button). Use the default value for the Number of stress range intervals value: Set the RMS stress cut-off multiple to 4. Leave the Bound Dirlik at UTS checkbox unchecked click OK. Note that although the use of the RMS stress cut-off multiple is illustrated here, it is recommended that the default value be normally retained. Also note that these settings are only applied to the Dirlik algorithm. The damage is upper bounded at the value implied by the limit, and the remaining tail of the stress PDF is integrated using this damage upper bound (or 1 if this damage would be more than 1). Also note that Dirlik s algorithm is defined in terms of stress ranges (not amplitudes), and so the limit in the case of Dirlik is applied to the stress range (not amplitude). Hence the default setting of 10 can be thought of as covering 5 standard deviations of the amplitude distribution. The Tovo-Benasciutti method has a more complicated way of handling the integral, and limits are affected by the mean stress under consideration. Therefore for Tovo-Benasciutti the amplitude limits are always the lower of the SN curve intercept point (stress where damage reaches 1) subsequently modified by the current mean, Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

245 Tutorial 114 : PSD Fatigue Analysis or 5 RMS values. Finally the Number of stress range intervals is also only applied to Dirlik, since with Tovo- Benasciutti there is a closed form for the integral for single-segment SN curves, and otherwise a lower number of 100 intervals is used when also doing a double integral over the randomly varying mean. There is a further option, selectable by checkbox, to bound the Dirlik damage integral at the Ultimate Tensile Strength (UTS) of the configured material as shown in Figure If the UTS is lower than the SN curve intercept point, then the effect is to use the UTS in place of the SN curve intercept as the upper limit to the integral, after which the tail is treated as having damage of 1. Use of this option is usually over-conservative at low life, as for most materials the UTS is lower than the SN curve intercept, but is provided for backwards compatibility with earlier versions of fe-safe, or for when a material s SN curve is not regarded as valid beyond the UTS. Figure Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial

246 Tutorial 114 : PSD Fatigue Analysis Step 7: Define the output file: When the FE model was loaded, the output filename automatically defaulted to: <ResultsDir>\abaqus_plateResults.odb or <ResultsDir>\ansys_plateResults.rst or <ResultsDir>\nastran_plateResults.op2 Before running the analysis, change the output filename to: <ResultsDir>\abaqus_plateResults_ex01.odb or <ResultsDir>\ansys_plateResults_ex01.rst or <ResultsDir>\nastran_plateResults_ex01.op2 The output filename can be modified either by manually editing the Output File field in the Fatigue from FEA dialogue, or by clicking the adjacent browse button:. After steps 1 through 7 are complete the Fatigue from FEA dialogue appears as shown in Figure Figure Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

247 Tutorial 114 : PSD Fatigue Analysis Step 8: Run the analysis: fe-safe is now configured to run the analysis. Press the Analyse button. A summary of analysis parameters is displayed: Figure Check that the analysis is configured as shown in Figure , and then click Continue. As the analysis is being performed, information is written to the analysis log file. The analysis log file has the same file name as the output file, except that the extension is.log. So, for this analysis, the analysis log file is: <ResultsDir>\*_plateResults_ex01.log This information is also displayed in the Message Log window and includes: Summary ======= Worst Life-Repeats : at Element [0]25.7 Analysis time : 0:00: Note: these are figures taken from the log of the analysis on the Abaqus model, continue reading for the results from both Abaqus and Ansys examples. Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial

248 Tutorial 114 : PSD Fatigue Analysis To save the current analysis configuration, select Save FEA Fatigue Definition File..., and enter a filename ending with the extension.stlx. The analysis can be reloaded at a later date by restoring the project definition file, using Open FEA Fatigue Definition File... Step 9: Reviewing the results The analysis log shows that the worst-case life for the whole model is: Abaqus: repeats of the 1 second loading block, at element 25, node 7. ANSYS: repeats of the 1 second loading block, at element 925, node 3. NASTRAN: repeats of the 1 second loading block, at element 25, node 7. Note: fe-safe adopts the conventional method of expressing the endurance limit, as the number of reversals, or half cycles ( 2 N f ), whereas fatigue lives are expressed in terms of cycles ( N f ). In fe-safe, the calculated fatigue life always refers to the number of repeats of the complete defined fatigue loading cycle. If necessary, a conversion factor can be used to convert the fatigue life in repeats to fatigue life with respect to hours or miles (see section 13 of the fe-safe User Guide). Step 10: Viewing the fatigue life contours: A copy of the original FEA Model file was created, onto which the fatigue results were written, depending on the FEA Model format. Open the FEA Model file with your preferred post-processor and plot a contour of the results. For example, in the last step of the file <ResultsDir>/abaqus_plate_singleResults_ex01.odb, the results for the exported variable should look similar to Figure : Figure : Log of Fatigue Lives. Note: The contour plot above is a reverse-contour. It shows the lowest Log Life as red and the highest Log Life as blue. Depending on which post-processor you use, the method to reverse the contour colours will vary. Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

249 log 10 (worst life) Tutorial 114 : PSD Fatigue Analysis Additional notes for Exercise 1: 1. Recall that the RMS stress cut-off multiple was set to 4. Note that a higher value will increase the stress range under investigation. To illustrate this point the same analysis using ANSYS files was run for a number of different RMS stress cut-off multiple values. The greatest damage was always at element 925 (similar to Figure ), leading to the results (in log base 10 notation) displayed in Figure Such results will vary on a case by case basis; however, the general trend is always the same. This illustrates why, for a conservative worst life estimate, a large RMS stress cut-off multiple is recommended (which is why the default value is set to 10) RMS stress cut-off multiple Figure Additional Output can be used to explore the fatigue analysis. a. Clicking on the Exports button on the Fatigue from FEA dialogue allows users to view the Contours tab to select contours to export such as Finite Life, Damage and more. b. The List of Items tab allows a node of interest to be entered, such as for the third node defined on element number 925. c. The History for Items tab allows creation of plot files of the response PSD for items on the List of Items to checking the box Export PSD frequency response function plots. This will produce a text file, which can be plotted, of the response PSD against frequency for each input channel in the project fe-results directory. Select File >> Data Files >> Open Data File(s) to open the file(s), which will appear in the fe-results subdirectory of the job. An example is given in the next exercise (Figure ). The plot file names are based on results file name, item ID, and input PSD channel, and have names of the form: <results_file>_psd_frf_plot-<itemid>_block_<n>.txt Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial

250 Tutorial 114 : PSD Fatigue Analysis d. The Log for Items tab allows additional information about the PSD analysis for the nodes on the List of Items to be exported to the results.log file by checking the box to Export PSD Items. The PSD diagnostics table in the log file appears as follows: PSD diagnostics for item e925.3 (block 1): 0th moment = e+17 1st moment = e+19 2nd moment = e+20 4th moment = e+24 Peaks per second = Upward mean crossings per second = Irregularity factor = Central frequency = Hz RMS = e+08 MPa e. For every PSD analysis there is an implicit assumption that all loaded modal stress dataset / GD pairs contribute to the PSD loading block definition(s). The Log for Items tab allows a sensitivity analysis to be performed on such data. To run, check the Enable load sensitivity analysis box. For each item on the list of items, a series of analyses will be run where each analysis is characterised by the omission of a single modal stress dataset and its associated set of GDs, per PSD block, i.e. in this example there would be ten additional analyses where the first analysis omits Dataset 1 and its associated GDs, the second analysis omits Dataset 2 and its associated GDs, etc The results are then exported to the projects.log file. The sensitivity analysis for the ANSYS analysis is shown below: SENSITIVITY ANALYSIS for Element (The life is for 1 repeat of the block (i.e n=1), it does not consider the n Value if this is an LDF analysis) Life (Reps) % Omission None DS#1 and associated GDs DS#2 and associated GDs DS#3 and associated GDs DS#4 and associated GDs DS#5 and associated GDs DS#6 and associated GDs DS#7 and associated GDs DS#8 and associated GDs DS#9 and associated GDs DS#10 and associated GDs Excluding Dataset 1 (Natural Frequency Hz) and its associated GDs increases the life over 3000 times. Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

251 Tutorial 114 : PSD Fatigue Analysis 3. In Figure the Implement Von Mises-based nodal filtering check box is a critical plane searchrelated option, i.e. it will only be enabled when a critical plane option is selected. If checked, the box indicates that fe-safe will implement 'nodal filtering'. More precisely, response PSD moments will be initially calculated (for all nodes) by using the Von Mises stress, and only nodes with lives below the constant amplitude endurance limit will be further processed using a critical plane search. In models where most of the lives are infinite this allows faster processing of the majority of nodes which undergo no damage. A 20% error margin is applied to the Von Mises stress in this filtering, and for speed the life being checked in the filtering process is estimated using a conservative narrowband approximation. Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial

252 Tutorial 114 : PSD Fatigue Analysis Exercise 2. Using the Tovo-Benasciutti algorithm with residual stress effects (ANSYS Model) The second example uses a notched beam model taken from experiments described in [1,2]. This is illustrated below in Figure In the experiments the region labelled as Restrained Nodes in Figure was attached to a vertical rod (Z direction), which was the source of the vibration. The Large Mass Method was use with Ansys Workbench to perform a modal analysis with 10 modes and the frequency range limited to 0.1Hx - 1E8 Hz. The node associated with the Large Mass had all its degrees of freedom removed, apart from movement in the Z direction (i.e. the input oscillation direction). An illustration of the first 4 modes, and their resonant frequencies are shown in Figure Modal Analysis. Figure Notched Beam Model Next a Modal Superposition Harmonic Analysis was performed in Ansys to generate Generalized Displacements (Modal Participation Factors in ANSYS terminology), which are used in fe-safe to weight the contribution of each mode shape when calculating the response PSD. The Generalized Displacements are shown in Figure (Mode 3 has a negligible Generalized Displacement in this case). Thirdly the input PSD was defined (see [1] or PSD #1 in [2]), representing the driving acceleration of the vertical rod, as in Figure Figure Modal Analysis Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

253 Tutorial 114 : PSD Fatigue Analysis Figure Generalized Displacements (Modal Participation Factors in ANSYS terminology) Figure Input PSD (Connecting rod acceleration PSD) In addition a forming analysis was carried out to calculate residual stresses present in the beam. These will be used to provide the background mean stress for the PSD analysis. Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial

254 Tutorial 114 : PSD Fatigue Analysis Opening the notched beam model (ANSYS Model) To open the model, select File >> FEA Solutions >> Open Finite Element Model For PSD Analysis... This will display the dialogue shown in Figure Select the Source FE Model file notched_beam_modal.rst from the directory <DataDir>\Ansys. Select the Generalized Displacement data notched_beam_mpf_1.mcf from the directory <DataDir>\Ansys then click on the Rectangular radio button. Finally, select the PSD data file notched_beam_psd.psd from the directory <DataDir>. Click OK. Figure A dialogue will be shown prompting the user Do you want to Pre-scan? Click Yes. Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

255 Tutorial 114 : PSD Fatigue Analysis The Select Datasets to Read dialogue will appear as shown in Figure Check the Quick-select box for Stresses, and if it is selected, deselect the box for Last Increment Only. Click Apply to Dataset List. Figure The Generalized Displacements (GDs) will not appear in the list. This is expected as they are read in from separate (.mcf) text files. Click OK. Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial

256 Tutorial 114 : PSD Fatigue Analysis When the Loaded FEA Models Properties dialogue appears to conclude the model loading, select MPa as the stress units; other units are left at their defaults (Figure ). Figure A dialogue will be shown prompting to edit the group list or not, choose No Figure Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

257 Tutorial 114 : PSD Fatigue Analysis A warning will be shown listing some unsupported element types, this can be safely ignored Next the residual stress dataset output from the Forming Analysis must be loaded to provide the background mean stress. Use Append Finite Element Model from the File >> FEA Solutions menu. Select file notched_beam_residual_stress.rst from the <DataDir>/Ansys directory. A warning message will appear saying that in PSD analyses only residual stress or temperature datasets may be appended. This is to be expected, click OK on the warning, and then click Yes on the subsequent pre-scan option message to bring up the pre-scan dialogue, and then select stress and strain datasets (Figure ). Note that the associated strain dataset must be loaded as well as the stress dataset. This is not used in the PSD analysis, but the general fe-safe residual stress interface for Loadings expects both to be present, due to its original use in Elastic-Plastic analyses. Figure Next the loading must be defined. There will be an automatic loading defined by the PSD model open process, but it is necessary to define the signal length, and add the residual. Switch to the Loading Settings tab. Double-click on the Length per repeat in seconds field of the PSD Block and set the signal length to 1 (second). To add the residual stress dataset to the loading, first click on it under the appended model on the Current FE models area to the right (Dataset 11).Then click on the Settings field near the top of the loading page. Click the Add button above, then select Residual dataset pair from the menu that appears. Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial

258 Tutorial 114 : PSD Fatigue Analysis Finally double click on the associated Residual strain dataset which must also be added (even though this will not be used in the PSD analysis) and set it to Dataset 12. The loading should look like Figure Figure Then switch back to the Analysis Settings tab to select the material and select Tovo-Benasciutti as the PSD algorithm. Expand the system database of the Material Databases, and select SAE-1045 as the material. Then double-click on the Material column in the Analysis Settings to apply this material. Then double-click on the Algorithm column (which will have defaulted to Dirlik). This will bring up the PSD algorithm selection dialog as shown in Figure Select Tovo-Benasciutti using the Stochastic mean centred on residual stress sub-option, and leave the mean stress correction method at the default Morrow. The stochastic mean sub-option will account for the effect on the mean-stress correction of random variability about the overall mean defined by the residual stress. Figure Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

259 Tutorial 114 : PSD Fatigue Analysis The Analysis Settings should then appear as below in Figure Figure fe-safe is now configured to run the analysis. Press the Analyse button. A summary of analysis parameters is displayed, Click Continue. The results will be written to Ansys RST file notched_beam_modalresults.rst in the project results directory. The worst node result will be displayed in a message box, and to the log file, which should read as below. Summary ======= Worst Life-Repeats : at Element Analysis time : 0:00: The expected life results will be written to stress component Sx in the Ansys results file. This can be viewed back in Ansys and should look like Figure As might be expected the fatigue hotspots are around one of the notches. Figure Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial

260 Tutorial 114 : PSD Fatigue Analysis Figure shows a zoomed in view around the notch containing element 1224 where most of the damage occurs. Figure A more detailed investigation of the response PSD can be carried out for the hotspot node. On the Exports dialog select List of Items tab and enter as the item. Then click on the Histories for Items tab and select Export PSD frequency response function plots. This will produce a plottable text file of the reponse PSD against frequency in the project fe-results directory. Select File >> Data Files >> Open Data File(s) to open file: notched_beam_modalresults_psd_frf_plot-e1224.2_block_1.txt in the jobs/job_01/fe-results sub-directory of the project. Volume 1 Tutorial Vol. 1 Section 114 Issue: 23 Date:

261 Tutorial 114 : PSD Fatigue Analysis This will appear in the Loaded Data Files column. Expand the data tree below this file in the Loaded Data Files column, to reveal the Frequency and PSD Response fields. Select both, then right click and select Cross Plot from the popup menu. Right click on the displayed plot, and select Properties on the popup menu, then change the Vertical Axis scaling to Logarithmic using the Logarithmic Scale checkbox. The response PSD plot should look like Figure Figure Response PSD (Pa^2/Hz) References 1. V. K. Nagulapalli (2005). Fatigue Life of Notched Aluminium Beams at Elevated Stress Levels, MsC Thesis, 2005, Northern Illinois University. 2. V. K. Nagulapalli, A. Gupta, S. Fan (2007). Estimation of Fatigue life of Aluminium Beams subjected to Random Vibration, Department of Mechanical Engineering, Northern Illinois University, in Conference Proceedings: 2007 IMAC-XXV: Conference & Exposition on Structural Dynamics. Vol.. 1 Section 114 Issue: 23 Date: Volume 1 Tutorial