OS-T: 6010 Multiaxial Fatigue Analysis (Damage Calculation) using S-N Approach

In Multiaxial Fatigue Analysis, OptiStruct uses the stress tensor directly to calculate damage.

Before you begin, copy the file(s) used in this tutorial to your working directory.

Multiaxial Fatigue Analysis theories are based on assumption that stress is in the plane-stress state. In other words, only free surfaces of structures are of interest in Multiaxial Fatigue Analysis in OptiStruct.

For solid elements, a shell skin is automatically generated by OptiStruct, shell elements are used as-is. Multiaxial Fatigue Analysis features are activated by setting MAXLFAT=YES on the FATPARM Bulk Data Entry.

Further for the S-N approach, the Goodman and the Findley models are used to check the damage caused by the tensile and the shear cracks.

In this tutorial, a control arm loaded by brake force and vertical force is used, as shown in Figure 1. Two load time histories acquired for 2545 seconds with 1 HZ, shown in Figure 2 and Figure 3, are adopted. Because a crack always initiates from the surface, a skin meshed with shell elements is designed to cover the solid elements, which can improve the accuracy of calculation as well.

To incorporate the multiaxial behavior additional parameters are introduced.

rd2070a_control_arm
Figure 1. Control Arm for Fatigue Analysis Model

rd2070a_load_time
Figure 2. Load Time History for Vertical Force

rd2070a_vertical_force
Figure 3. Load Time History for Braking Force

Launch HyperMesh and Set the OptiStruct User Profile

  1. Launch HyperMesh.
    The User Profile dialog opens.
  2. Select OptiStruct and click OK.
    This loads the user profile. It includes the appropriate template, macro menu, and import reader, paring down the functionality of HyperMesh to what is relevant for generating models for OptiStruct.

Import the Model

  1. Click File > Import > Solver Deck.
    An Import tab is added to your tab menu.
  2. For the File type, select OptiStruct.
  3. Select the Files icon files_panel.
    A Select OptiStruct file browser opens.
  4. Select the ctrlarm.fem file you saved to your working directory.
  5. Click Open.
  6. Click Import, then click Close to close the Import tab.
    The outline of the Fatigue Analysis setup to be achieved in the following steps.


    Figure 4. Fatigue Setup – MultiAxial SN

Set Up the Model

Define TABFAT Load Collector

The first step in defining the loading sequence is to define the TABFAT cards. This card represents the loading history.
  1. Make sure the Utility menu is selected in the View menu. Click View > Browsers > HyperMesh > Utility.
  2. Click on the Utility menu beside the Model tab in the browser. In the Tools section, click on TABLE Create.
  3. Set Options to Import table.
  4. Set Tables to TABFAT.
  5. Click Next.
  6. Browse for the loading file.
  7. In the Open the XY Data File dialog box, set the Files of type filter to CSV (*.csv).
  8. Open the load1.csv file you saved to your working directory.
  9. Create New Table with Name table1.
  10. Click Apply to save the table.
    The load collector table1 with TABFAT card image is created.
  11. Browse for a second loading file load2.csv.
  12. Create New Table with Name table2.
  13. Click Apply to save the table.
    The load collector table2 with TABFAT card image is created.
  14. Exit from the Import TABFAT window.
    Tables appear under Load Collector in the Model Browser.
    Note: A file in DAC format can very easily be imported in HyperGraph and converted to CSV format to be read in HyperMesh.

Define FATLOAD Load Collector

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter FATLOAD1.
  3. Click Color and select a color from the color palette.
  4. For Card Image, select FATLOAD.
  5. For TID(table ID), select table1 from the list of load collectors.
  6. For LCID (load case ID), select SUBCASE1 from the list of load steps.
  7. Set LDM (load magnitude) to 1.
  8. Set Scale to 3.0.
  9. Repeat the process to create another load collector named FATLOAD2 with FATLOAD Card Image and pointing to table2 and SUBCASE2.
  10. Set LDM to 1 and Scale to 3.0.

Define FATEVNT Load Collector

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter FATEVENT.
  3. For Card Image, select FATEVNT.
  4. For FATEVNT_NUM_FLOAD, enter 2.
  5. Click on the Table icon table_pencil next to the Data field and select FATLOAD1 for FLOAD(1) and FATLOAD2 for FLOAD(2) in the pop-out window.

Define FATSEQ Load Collector

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter FATSEQ.
  3. For Card Image, select FATSEQ.
  4. For FID (Fatigue Event Definition), select FATEVENT .
    Defining the sequence of events for the fatigue analysis is completed. The Fatigue parameters are defined next.

Define Fatigue Parameters

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter fatparam.
  3. For Card Image, select FATPARM.
  4. Verify TYPE is set to SN.
  5. Set MAXLFAT to Yes for the multiaxial method.
  6. Set STRESSU to MPA (Stress Units).
  7. Set RAINFLOW RTYPE to LOAD.

Define Fatigue Material Properties

The material curve for the fatigue analysis can be defined on the MAT1 card.

  1. In the Model Browser, click on the MAT1 material.
    The Entity Editor opens.
  2. In the Entity Editor, set MATFAT to SN.
  3. Set UTS (ultimate tensile stress) to 600.
  4. For the SN curve set (these values should be obtained from the material's SN curve):
    SRI1
    1903.0
    B1
    -0.123
    NC1
    1e6
    B2
    0.0
    FL
    0.0
    SE
    0.0

Define PFAT Load Collector

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter pfat.
  3. For Card Image, select PFAT.
  4. Set LAYER to TOP.
  5. Set FINISH to NONE.
  6. Set TRTMENT to NONE.
  7. Set Kf to 1.0.

Define FATDEF Load Collector

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter fatdef.
  3. Set the Card Image to FATDEF.
  4. Activate PSOLID in the PTYPE Entity Editor.
  5. Edit FATDEF_PSOLID_NUMIDS to 2. The model contains 2 solid properties defined in the model.
  6. Click on the Table icon table_pencil next to the Data field and select PSOLID_2 for PID(1), pfat for PFATID(1) and PSOLID_5 for PID(2) and pfat for PFATID(1) in the pop-out window.
  7. Click Close.

Define the Fatigue Load Step

  1. In the Model Browser, right-click and select Create > Load Step.
  2. For Name, enter Fatigue.
  3. Set the Analysis type to fatigue.
  4. For FATDEF, select fatdef.
  5. For FATPARM, select fatparam.
  6. For FATSEQ, select fatseq.

Submit the Job

  1. From the Analysis page, enter the OptiStruct panel.
  2. Click save as following the input file field.
    The Save As dialog opens.
  3. For File name, enter the name ctrlarm_fatigue.fem.
  4. Click Save.
  5. Click OptiStruct to submit the analysis.

Review the Results

  1. From the OptiStruct panel, click HyperView.
    HyperView is launched and the results are loaded. A message window appears to inform of the successful model and result files loading into HyperView.
  2. Go to the Results tab.
  3. Change the Load Case to Subcase 3 - fatigue.
  4. On the Results toolbar, click resultsContour-16 to open the Contour panel.
  5. Set Result type to Damage and click on Apply to contour the elements.
  6. Figure 5. Elemental Life results indicating ~4500 cycles before the first element fails