ASME Fatigue DOCUMENTATION. ANSYS Mechanical Application. Extension version Compatible ANSYS version

Transcription

1 ASME Fatigue ANSYS Mechanical Application DOCUMENTATION Extension version Release date 06-Apr-17 Compatible ANSYS version

2 Table of Contents 1 INTRODUCTION PRODUCT RESTRICTIONS GETTING STARTED INSTALLATION LOADING EXTENSION UNINSTALLING ASME FATIGUE APP Background Solution Usage Issues and Limitations REFERENCES APPENDIX A. EXAMPLES APPENDIX B. IMPLEMENTATION APPENDIX C. GENERAL ISSUES AND LIMITATIONS

3 1 Introduction This application has been created using ACT (ANSYS Customization Toolkit), which provides an API (Application Programming Interface) to several ANSYS Workbench modules, including ANSYS Mechanical, ANSYS DesignModeler and ANSYS DesignXplorer. With ACT, the GUI (Graphical User Interface) of ANSYS Mechanical can be extended with new buttons. These buttons have customizable behaviour, which allows the developer to create new features, or re-use existing functionality that previously had to be included via APDL command objects. A few of the advantages with ACT include: Consistent handling of unit systems Manage user inputs Access to the Mechanical database as well as the ANSYS database and results Use Mechanicals graphics library for on-screen representation Shield the user from APDL code Create installable binary files, protecting intellectual property 2 Product Restrictions The ASME Fatigue app described in this document utilize functionality in ANSYS that may or may not be available depending on the available ANSYS license level. The product restrictions are summarized in Table 2-1. Table 2-1: Required ANSYS license level for the ASME Fatigue app ANSYS license level (current) Product code Compatibility [Y/N] DesignSpace caewbpl3 Y Mechanical Pro mech_1 Y Mechanical Premium mech_2 Y Mechanical Enterprise ansys Y ANSYS license level (legacy) Professional NLT prf Y Professional NLS prfnls Y Structural struct Y - 3 -

4 3 Getting Started 3.1 Installation To install the extension, open ANSYS Workbench. On the project page, navigate to ACT Start Page > Manage Extensions and press the + icon to install a new extension (see Figure 3-1). Figure 3-1: Navigating to the Manage Extensions page and installing a new extension In the browsing window that appears, select the binary extension file (.wbex file) downloaded from ANSYS app store (see Figure 3-2). Verify that the correct extension appears in the list in the Extension Manager by going to ACT Start Page > Manage Extensions... (see Figure 3-3)

5 Figure 3-2: Select the.wbex file downloaded from ANSYS app store Figure 3-3 The newly installed extension should appear in the Extension Manager page - 5 -

6 3.2 Loading Extension To use the extension in a project, simply click on the extension on the Extension Manager page. The extension will highlight in green when properly loaded. Mechanical needs to be closed before the loading is effective, so close Mechanical if this is open. Several extensions can be loaded into the same project. Once the project is saved with an extension, it will load automatically with the project, so this procedure only needs to be done once per project. Figure 3-4: Properly loaded extension on the Extension Manager page To unload the extension, open the Extension Manager page and click on the extension again. The extension is unloaded when the green highlighting disappears. 3.3 Uninstalling To uninstall the extension, use the Extension Manager as described in section 3.1 and 0. From the drop-down menu on the bottom right of the extension, select Uninstall

7 Figure 3-5: Uninstalling an extension from the Extension Manager page - 7 -

8 4 ASME Fatigue app Background The fatigue calculation according to ASME 2013 Sec. VIII Div.2 Part 5. Chapter 5.5.3; Fatigue assessment elastic stress analysis and equivalent stress can be done by hand, extracting stress results at nodes for each load case. However, in addition to be a time consuming task with risk of errors, the node location of the maximum damage cannot be known before the actual fatigue damage calculation Solution The Fatigue (ASME VIII Div.2) result object can be used as an efficient post-processing tool to plot the number of cycles to failure, or accumulated damage according to (1) ASME 2013 Sec. VIII Div.2 Part 5 Chapter 5.5.3, for a single, or a combination of, load cases. The fatigue curve data tables are implemented and the fatigue curve is directly built using the material properties of the selected bodies Usage The Fatigue (ASME VIII Div.2) result object can be applied in any Static Structural or Transient Structural analysis. The properties have to be selected or entered regarding how to the results should be calculated. All properties are defined in Table 4-1. The result can be scoped to any type of geometry, but not to mesh entities (directly or through named selections). The user can select to plot the Accumulated Damage, Cycles to Failure and log 10 Cycles to Failure, calculated as described in Appendix B. If the geometry contains shell elements, the selected shell location will be used as a uniform contour through the thickness. The fatigue curve can be the same for all bodies of the geometry selection or body dependent by selecting No for Same Curve for All Bodies. In the case of body dependent fatigue curve, the Fatigue Curve Table has to be filled in. It is not possible to select No if the geometry selection contains a single body. The result can be calculated for a single, or a combination of, load cases by selecting Yes or No for Load Case Combination. In case of a load case combination, the Load Case Table will have to be filled in. See 0 if the table does not pop up. A load case is defined as a range from one load step to another load step in the same analysis. Any analysis sharing the Model cell in Workbench can be used as a load case, but only solved analyses are valid. Start Step and End Step, specified by the user, defines one load cycle, or stress range. A stress range is the two extremes of a cycle and the stress amplitude is one half of the stress range. Thus the simulation must include a full load cycle. Note that the time for a chosen step is the end step time. Step 0 is used to define the initial time 0. An example of property set and result is shown in Figure

9 The fatigue curves used for the calculations are saved in the solver files directory if Yes is selected for Save Fatigue Curve, see Appendix B. It is recommended always to check if the fatigue curve has been calculated as expected. Figure 4-1: Details and graphic view of a Fatigue (ASME VIII Div.2) result object

10 Table 4-1: Summary of properties of the Fatigue (ASME VIII Div.2) result object (grey cells are read-only properties). Scope Geometry Shell Definition Result Temperature Load Case Combination Start Step End Step Number Of Cycles K_f, Fatigue Strength Reduction Factor K_e, Fatigue Penalty Factor Load Case Table Fatigue Curve Same Curve For All Bodies Fatigue Curve (App. 3-F) Fatigue Curve Table (App. 3-F) Save Fatigue Curves Integration Point Results Display Option Information Young s Modulus Table Cycles To Failure Damage Definition Result geometry scope, can be edges, vertices, faces or bodies Specify whether Top, Bottom or Middle results are displayed for shell bodies Specify whether Damage, Cycles To Failure or Logarithm Of Cycles To Failure To Base 10 should be displayed Temperature at which the Young s Modulus is extracted or interpolated for temperature dependent Young s Modulus Specify whether this is a single load case, or a combination of load cases. Any analysis sharing the Model cell in Workbench can be used as a load case, but only solved analyses are valid. Specify the start and end step defining one cycle. The stress component range will be calculated as the stress at end step minus stress at start step. The end time of the step is used. Step 0 corresponds to time step 0 Number of cycles to calculate the damage Specify ASME fatigue strength reduction factor, default factor is 1.0 Specify ASME fatigue penalty factor, default factor is 1.0 Same properties as previously to define load case combination Specify whether the fatigue curve is the same for all selected bodies or not Specify the Appendix 3-F table from which the fatigue coefficients are found Specify the Appendix 3-F table from which the fatigue coefficients are found by body ID (see 0 for body ID description) Specify whether the fatigue curve should be saved to the Solver Files Directory or not Specify whether the result are displayed as Averaged (default) or Unaveraged result Young s Modulus used for the calculation (see 0 for body ID description) Minimum number of cycles to failure Maximum damage

11 By Display Time Result Set Not to be used Not to be used Not to be used Issues and Limitations The Fatigue (ASME VIII Div.2) result object is limited to 3D Static Structural and Transient Structural analyses. If a.csv file is opened or previewed while a result is being evaluated where this file will be overwritten, the evaluation will fail. The file should be closed. Results cannot be displayed by Maximum over Time, or Time of Maximum. If the result object is inserted under an unsolved analysis and the analysis is included to define a load case in a Load Case Table, the Load Case Table will be invalid. Thus, it will not be possible to solve the analysis. The result object will have to be either supressed or deleted before the analysis can be solved. If the scoping method is set to All Bodies, but the geometry contains only one body, Same Curve for All Bodies, will not be set to Yes as read-only at initialisation, but only if the user tries to change it. Error/Warning Messages: - If a solved fatigue result uses an analysis which has be cleared or resolved, the result object will become suppressed or invalid when the user selects it. - If the geometry selection has a plastic behaviour assigned, a warning message will be displayed - If the Young s Modulus is out of range, the evaluation is aborted with an error message, see Appendix B. - If the stress is out of range for the selected fatigue curve table, the evaluation is aborted with an error message, see Appendix B

12 5 References 1. ASME. Section VIII, Division

13 This example shows, step by step, how to use the Fatigue (ASME VIII Div.2) result object, as well as verification of the results. A Static Structural analysis is created and a Duplex Stainless Steel material with elastic behavior is used. The material properties are summarized in Table 5-1. Table 5-1: Material Properties of the Duplex Stainless Steel material. Material Property Value Elastic Modulus [GPa] Poisson s ratio [-] 0.31 The geometry used in this example is a Blind Tee, modeled as a solid multibody part. The previously defined material is assigned to all bodies. The model is subjected to an internal pressure with its corresponding cap force. Further, the outlet surface is fixed in the axial and tangential direction with respect to a local coordinate system as shown in Figure 5-1. For simplicity, symmetry is utilized such that only half of the geometry model is used. Figure 5-1: Loads and boundary conditions for the example model The solved analysis defined the first Load Case and is renamed as Fatigue LC1_BlindT. The Setup cell of Fatigue LC1_BlindT is duplicated on the Project page (RMB in the Setup cell, duplicate), thus sharing the Engineering Data, Geometry and Model cells, as shown in Figure 5-2. This is done in order for the two analysis to share the same mesh, which is a requirement

14 to evaluate the cumulated damage from the two analysis. The second analysis is renamed Fatigue LC2_BlindT. Figure 5-2: Duplicating analysis by duplicating the Setup cell (left) duplicated analysis after renaming (right) For the Fatigue LC2_BlindT analysis, a Remote Force of N is added as shown in Figure 5-3. Figure 5-3: Loads and boundary conditions for the Fatigue (ASME VIII Div.2) example model. To evaluate the accumulated damage in the Blind tee, a Fatigue (ASME VIII Div.2) result object is added from the toolbar and scoped to the body. This object is found in the Results dropdown menu of the extension, as seen in Figure

15 Figure 5-4: Inserting a Fatigue (ASME VIII Div.2) object and Details of Fatigue (ASME VIII Div.2) result object. Load Case Combination is set to Yes. Start Step, End Step and Number Of Cycles fields disappear. Instead, a new field Load Case Table appears as shown in Figure 5-5. By clicking on Tabular Data in the Load Case Table field, a table pops up with properties as shown in Figure 5-6. Refer to Appendix B if the table does not pop up. Figure 5-5: Details of Fatigue (ASME VIII Div.2) result object after setting Load Case Combination to Yes

16 Figure 5-6: Load Case Table after clicking on Tabular Data. Two lines are added to the table by clicking twice on. Then, the table is filled in as shown in Figure 5-7: The analysis without Remote Force (here renamed LC1) is selected with cycles, and the analysis with Remote Force (here renamed LC2) with number of cycles. Figure 5-7: Load Case Table after inserting two lines, and filling with the values. Note that only solved analyses are valid. By clicking Apply in the Material Table Data field, the property becomes valid as shown in Figure 5-8. Note that, exiting by any other way will not save the table

17 Figure 5-8: Details of Fatigue (ASME VIII Div.2) result object after clicking Apply. The Fatigue Curve (App. 3-F) is then specified to 3-F.3. When all properties are filled in, the result object status changes to valid, as shown in Figure 5-9. Figure 5-9: Details of Fatigue (ASME VIII Div.2) result object after selecting the Fatigue Curve. The result object is evaluated. The result plot is shown in Figure Cycles to Failure and Damage Contribution are displayed in the Load Case Table per load case. Note that in this case, both LC1 and LC2 could have been set as 2 steps in the same analysis. Then, the same result can be obtained by selecting the relevant start and end steps, as shown in Figure Figure 5-10: Load Case Table for one analysis with two steps, the same damage result is obtained

18 Figure 5-11: Plot displayed and Load Case Table after evaluation of the result object

19 Verification of the result at the Maximum Accumulated Damage node: To verify the result, the equivalent stresses are extracted at the node of maximum accumulated damage for both analysis, see Figure The local thermal stress is not included in the stress amplitude calculations, thus, the stress amplitude S a can be calculated by Eq and Eq in (1) (K f = 1 and K e,k = 1): S a,lc1 = MPa 2 = MPa ; S a,lc2 = MPa 2 = MPa The number of cycles are then calculated using the Annex 3-F in (1) with the coefficients of Table 3-F.3: N LC1 = cycles ; N LC2 = cycles The accumulated damage is then calculated using equation 5.38 in (1): D = = The ratio obtained by hand calculation is equal to the one obtained with the extension result object Figure Results are verified. Figure 5-12: ANSYS Equivalent Stress at the node of maximum utilization for LC1 and LC

20 1- The fatigue curves are built for the bodies of the geometry selection 1. The fatigue curves are built as specified by the Annex 3-F for a stress range S a varying in the range defined for each table in (1) with a step of 0.2 MPa 2. Note that: - The Young s modulus is retrieved from Engineering Data and used as the modulus of elasticity of the material E T in Eq. 3-F.3 in (1). If E T is temperature dependent, it will be interpolated at the user defined temperature. 3 - The stress amplitude, S a, is calculated by Eq and Eq in (1). The local thermal stress S LT,k in (1) is not included in the stress amplitude calculations. - K f is strength reduction factor accounting for local notch or effect of the weld. This factor is set to 1 by default - K e,k is the fatigue penalty factor. This factor is set to 1 by default. 2- For each load case and each element nodes, the equivalent (von-mises) stress range is calculated for the specified start and end time. The closest superior stress range from the built corresponding fatigue curved is determined which gives the number of cycles. 3- In the case of load combination, the number of cycles to failure for a set of load cases is calculated by Equation 5-1 and the accumulated damage is calculated Eq in (1) load cases 1 N tot = ( 1 ) N i i=1 Equation If a body used a fatigue curve previously built, this step is skipped and, thus, the file is not written to the solver files directory. 2 For Table 3-F.3, a stress range S a maximum of MPa is used instead MPa to avoid singularities. 3 If the specified temperature is outside of the range for which the Young s Modulus has been defined, the Young s Modulus will not been interpolated, instead, the closest value (minimum or maximum) will be selected

21 The specified results are calculated at element nodes. For unaveraged display, results are plotted at element nodes. For averaged results, element nodes result are averaged and plot at nodes, results are averaged across bodies. The result value at midside nodes is the average of the two neighbour corner nodes results. For each fatigue curve, the Young s Modulus has to be close enough to the modulus of elasticity used to establish the design curve E FC to not create singularities or high discontinuities in the fatigue curve. A validity range has been defined for each coefficient, summarized in Table 5-2. If the absolute difference between the Young s Modulus and E FC is higher than 5 %, a warning message will appear to remind the user to check the fatigue curve. If the Young s Modulus is found invalid (i.e.: out of range), an error message will pop up and the evaluation will be aborted. The problematic fatigue curve would still be written to file. Table 5-2: Young s Modulus validity ranges per fatigue curve coefficient table Annex 3-F in (1) Table E FC [GPa] Minimum Young s Modulus [GPa] Maximum Young s Modulus [GPa] 3-F F F F F F F F F

22 One issue regarding using results from another analysis system in load case definition tables: When this is used, and that other analysis system is invalidated/rerun, the result object is not immediately invalidated. Only when the result item is clicked once, the result item is invalidated. Stopping the results evaluation by clicking Stop Solution at the ANSYS Workbench Solution Status pop-up window is not possible. The Display Time is not working correctly in the case that the time specified does not have results stored. To ensure expected results, only select points in time where results are stored. In additions, for some result items the Display Time should not be used at all. This is specified in the Usage chapter for the affected result items. Faces and edges that have been created as Virtual Topology are not selectable as geometry input. Duplicating an evaluated result item results in an un-evaluated result item. The duplicate result item needs to be re-evaluated. Three issues are related to pop-up tables. In the case that Mechanical is open in a display other than the main display, the table may not pop up. In the case that Mechanical is open in the main display, but the Mechanical window is scaled too small, the table may not be visible. The only way to close the table is to click on Cancel or Apply, clicking on the top-right red cross will not close the table. When inserting an item under the Setup level (Initial Conditions, Loads or Supports), and then un-loading the extension, the item is not possible to delete afterwards. The extension needs to be reloaded before the item can be deleted. For result items, the availability to select geometry as mesh elements or nodes is limited. Some load and result objects refer to Body ID. The Body ID can be found by using Selection Information in the main toolbar, as shown in Figure ID (beta) displayed under definition in the detail view of a body, is not the Body ID. Figure 5-13: Selection information table