Workshop Transient 1-way FSI Load Mapping using ACT Extension 15. 0 Release Solving FSI Applications Using ANSYS Mechanical and ANSYS Fluent 1 2014 ANSYS, Inc.
Workshop Description: This example considers a T junction that is subjected to thermal loads due to the mixing of two fluids with different temperatures, as well as a fluid pressure. Learning Aims: Introduction This workshop shows how to calculate the stresses in the T junction due to thermal and pressure loads using one-way fluid-structure-interaction. An extension is installed to facilitate the communication between Fluent and Mechanical. The workflow for creating and loading necessary files is illustrated. 2 2014 ANSYS, Inc.
The Extension Files To Download the extension files : 1. Navigate to Ansys Customer Portal (https://support.ansys.com/portal/site/ansyscustomerportal) 2. After logging in, under Downloads, click on Extensions Library 3. Scroll down to FSI Transient Load Mapping and download the associated file 4. Unzip the archive 3 2014 ANSYS, Inc.
The Extension Files Once Extracted: 1. Locate the CFX_FSI_IORead.cse and CFX_FSI_IOWrite.cse files :...\ACT_FSI_Transient_R150_v4\CFD Post Macros 2. Copy the above mentioned files to the following folder: Windows: C:\Program Files\ANSYS Inc\v150\CFD-Post\etc\PostReports Linux: /ansys_inc/v150/cfd-post/etc/postreports/ See the next slide if you do not permissions to place the files in these directories 4 2014 ANSYS, Inc.
The Extension Files Local Directory Setup Note: Instead of copying the Macro files to the installation directory, you can follow these steps to use a local directory for the Macro files: 1. Open the directory where you extracted the extension files and locate the FSI_Transient_Export_Surf.cse file in the /ACT_FSI_Transient_R150_v4/CFD Post Macros/ directory 2. Open the FSI_Transient_Export_Surf.cse file in a text editor 3. Find the line :! my $datadir $datadir = $ENV{CUE_LOCAL_DATA_DIR}; 4. Replace $ENV{CUE_LOCAL_DATA_DIR}; with a local directory path, for example: "C:/ACT_FSI_Transient_R150_v4/CFD Post Macros/"; This directory would be different for each user. Note the usage of / instead of \ in the path; this applies to both Windows and Linux. The quotes should be included around the directory path and the semi-colon is required at the end of the line. 5 2014 ANSYS, Inc.
The Extension Files Local Directory Setup 5. In the next line, replace "/PostReports/CFX_FSI_IORead.cse"; with "CFX_FSI_IORead.cse"; 6. Find the line :! $fname = $datadir."/postreports/cfx_fsi_iowrite.cse"; 7. Replace the "/PostReports/CFX_FSI_IOWrite.cse"; with "CFX_FSI_IOWrite.cse"; 8. Save the changes 9. Repeat the same steps for the FSI_Transient_Export_Vol.cse file 6 2014 ANSYS, Inc.
Starting Workbench [1] 1. Start ANSYS Workbench and select File > Restore Archive: a) Select T-Junction_1way_FSI.wbpz b) Save to your working directory (save to a local hard disk, not a USB stick) The fluid flow solution for this exercise has already been completed. Review the solution in Fluent if you wish by editing the Solution (A5) or Results (A6) cells. 2. Drag a Transient Structural system onto the Project Schematic and drop it onto the Geometry cell (A2) of the FLUENT system The link creates a common Geometry. 7 2014 ANSYS, Inc.
Workbench Engineering Data [1] Next you will create a material for use in Mechanical that has the same physical properties as the material used for the calculation in Fluent. 1. Double-click the Engineering Data cell under Transient Structural (B2) 2. Right-click on Structural Steel and select Duplicate Structural Steel 2 is created 3. Rename Structural Steel 2 to Steel by simply selecting the cell and typing 8 2014 ANSYS, Inc.
Workbench Engineering Data [2] 4. Toggle the filter button in the toolbar to display all material properties 5. With Steel selected, enter a Density value of 8030 kg/m 3 6. Enter an Isotropic Thermal Conductivity value of 16.27 W/m⁰C 7. Enter a Specific Heat value of 502.48 J/kg⁰C 8. Close the Engineering Data tab to return to the Project Schematic 9 2014 ANSYS, Inc.
Workbench Install The Extension 1. From the main toolbar in Workbench, select Extensions and then Install Extensions... 2. Navigate to where the extension files were extracted to (or to where the input_files folder is located) :.../Extension/Binary/ FSI_transient_v4.wbex 3. Select OK 4. From the main toolbar in Workbench, select Extensions and then Manage Extensions... 5. Check the box for FSI_Transient and close the Extensions Manager window 10 2014 ANSYS, Inc.
Fluent Setup 1. Double-click on the Fluent Setup Cell (A4) 2. In the pop-up window, make sure Double Precision is checked, press OK This will launch Fluent 3. From the list on the left hand side, click on Calculation Activities 4. Set the Autosave frequency to 1 11 2014 ANSYS, Inc.
Fluent Calculate 1. Click on Run Calculation from the left hand side list and press Calculate 2. Press Yes in the pop-up window to initialize the case Fluent will start calculation. This will take a few minutes. 3. Once the calculation is complete press OK and close Fluent 12 2014 ANSYS, Inc.
CFD-Post Temperature Results 1. Launch CFD-Post by double clicking on the FLUENT Results cell (A6) Inserting a temperature contour : 2. From the main toolbar click on Contour Button 3. Name the new contour temperature in the Insert Contour window 4. In Details of temperature press the Locations browse button and while holding the left Ctrl button, select all the items under Solid part_2 5. Change the variable to Temperature and make sure the range is set to Global 6. Click Apply to view the results 13 2014 ANSYS, Inc.
CFD-Post Pressure Results Inserting a pressure contour : 1. From the main toolbar click on Contour Button 2. Name the new contour pressure in the Insert Contour window 3. In Details of pressure press the Locations browse button and select interface_fluid_side 4. Change the variable to Pressure and make sure the range is set to Global 5. Click Apply to view the results 14 2014 ANSYS, Inc.
CFD-Post Pressure Results Files The extension installed in Workbench requires input files from CFD-Post to run the analysis. Input files are created for both Pressure and Temperature: To export pressure data: 1. Navigate to the Calculators tab 2. Double click on Macro Calculator 3. Click on the Macro browse button and locate the FSI_Transient_Export_Surf.cse file in: [extraction directory]\act_fsi_transient_r150_v4\cfd Post Macros 4. In the exportlocator drop-down list, select interface_fluid_side 5. Set Export Pressure to Yes 6. Press Calculate This will write the pressure data files 15 2014 ANSYS, Inc.
CFD-Post Pressure Results Files 7. Three files will be saved in Workbench Permanent Files* folder: a) XYZ file that contains the x,y,z values of the CFD mesh in 3 columns b) Time file that contains the step end times from the CFD simulation c) Pres file that contains the nodal load values for all time steps. Each time step corresponds to one column. *To change Workbench Permanent Files folder location: 1. In Workbench, from the main toolbar select Tools and then select Options.. 2. The location of the Permanent Files folder is shown under Default Folder for Permanent Files 3. You can change the location by clicking on the browse button and selecting a new location. 16 2014 ANSYS, Inc.
CFD-Post Temperature Results Files To export temperature files: 1. In the Macro Calculator, click on the Macro browse button and select the FSI_Transient_Export_vol.cse file in: [extraction directory]\act_fsi_transient_r150_v4\cfd Post Macros 2. In the exportlocator drop-down list select solid part_2 3. Set Export Temperature to Yes 4. Press Calculate This will write the temperature data files 17 2014 ANSYS, Inc.
CFD-Post Temperature Results Files 5. Three files will be saved in Workbench Permanent Files* folder: a) XYZ file that contains the x,y,z values of the CFD mesh in 3 columns b) Time file that contains the step end times of the CFD simulation c) Temp file that contains the nodal load values for all time steps. Each time step corresponds to one column 6. Close CFD-Post *Refer to slide 15 for instructions on how to change the Permanent Files folder 18 2014 ANSYS, Inc.
Structural Setup Materials 1. Launch the Transient Structural Model by double clicking on the Model cell (B4) 2. In the model tree, expand Geometry 3. Right-click on fluid and select Suppress Body 3. Select NutsBolts then in the Details view change the Assignment to Steel 4. Select solid and change the Assignment to Steel 5. Expand the solid object under Geometry 6. Highlight all the parts under solid and right click and select Create Named Selection 7. Type Solid 19 2014 ANSYS, Inc.
Structural Setup Mesh 1. Highlight Mesh in the Outline tree 2. In the Details view, expand Sizing and set Relevance Center to Medium 3. In the Outline tree right-click on Mesh and select Insert > Method 4. In the Graphics view, right-click and pick Select All 5. Click Apply in the Details view 6. Change the Method to Tetrahedrons 7. Right-click Mesh and select Generate Mesh 20 2014 ANSYS, Inc.
Structural Pressure Load 1. Click on the Pressure button from the new FSI toolbar This will create a Import Pressure object in the transient model and a Imported Pressure object in the results. 2. Click on the Import Pressure object from the outline tree to view its details 3. Expand the list for Scoping Method and select Named Selection 4. Expand the list for Named Selection and select interface_solid_side 5. Click on the yellow field for XYZ_Data and locate CSV_TRN_2D_NXYZ.sfe from the Workbench permanent files folder* *Refer to slide 15 for instructions on how to find Workbench permanent files folder 21 2014 ANSYS, Inc.
Structural Pressure Load 6. Similarly, load the CSV_TRN_2D_PRES.sfe and CSV_TRN_2D_TIME.sfe files for the next two fields 7. Set Create Time Steps to Yes 8. Right-click on the Imported Pressure item in the Outline tree and click on Generate to import the loads Once imported, you can view the pressure from the last time step 9. Click on Imported Pressure under the Solution 10. Set Scoping Method to Named Selection and select interface_solid_side from the list 22 2014 ANSYS, Inc.
Structural Temperature Load 1. Click on the Temperature button from the new FSI toolbar This will create Import Temperature object in the transient model and Imported Temperature object in the results 2. Click on the Import Temperature object from the outline tree to view its details 3. Expand the list for Scoping Method and select Named Selection 4. Expand the list for Named Selection and select solid 5. Click on the yellow field for XYZ_Data and locate CSV_TRN_3D_NXYZ.sfe from the Workbench permanent files folder 23 2014 ANSYS, Inc.
Structural Temperature Load 6. Similarly, load the CSV_TRN_3D_TEMP.sfe and CSV_TRN_3D_TIME.sfe files for the next two fields 7. Set Create Time Steps to Yes 8. Right-click on the Import Temperature item in the Outline tree and click on Generate to import the loads Once imported, you can view the Temperature from the last time step 24 2014 ANSYS, Inc.
Structural Importing Loads Note : 1. Scoping is restricted to Bodies for importing temperature load and to Surfaces for importing pressure load 2. One must be careful when selecting bodies and surfaces for writing files in CFD- Post and importing them in Mechanical. In order to have a working model, the surfaces and bodies overlap. 25 2014 ANSYS, Inc.
Structural Analysis settings 1. Select Analysis Settings Notice that 5 steps have been automatically created, one for each set of CFD results. The Step End Time for each step has also been set to the corresponding CFD results. 26 2014 ANSYS, Inc.
Structural Setup Support and Solve 1. In the Outline tree right-click Transient (B5) and select Insert > Fixed Support 2. Select the three surfaces shown to the right (in green) and click Apply in the Geometry field 3. Right-click Solution (B6) and Solve 1 3 2 27 2014 ANSYS, Inc.
Structural Results 1. Right-click Solution (C6) and select Insert > Deformation > Total 2. Right-click Solution (C6) and Insert > Stress > Equivalent (von-mises) 3. Right-click Solution (C6) and Evaluate All Results 4. Examine the Deformation, Stress, Imported Pressure and Imported Temperature results. For each result the Display Time can be set to any of the step end time points to view the transient results. 5. After examining the results close Mechanical, return to the Project Schematic and save the project 28 2014 ANSYS, Inc.