OS-T: 6020 Multiaxial Fatigue Analysis (Strain - Life) using E-N Approach

The E-N (Strain - Life) approach should be chosen to predict the fatigue life when plastic strain occurs under the given cyclic loading.

Before you begin, copy the file(s) used in this tutorial to your working directory.
S-N (Stress - Life) approach is not suitable for low-cycle fatigue where plastic strain plays a central role for fatigue behavior. If an S-N analysis indicates a fatigue life less than 10,000 cycles, it is a sign that an E-N approach may be a better choice. The E-N approach, while computationally more expensive than S-N, should give a reasonable estimate for high-cycle fatigue as well.

Figure 1. Low Cycle and High Cycle Regions on the S-N Curve
Since E-N theory deals with uniaxial strain, the strain components need to be resolved into one combined value for each calculation point, at each time step, and then used as equivalent nominal strain applied on the E-N curve (Figure 2).

Figure 2. Strain-Life Curve

In OptiStruct various strain combination types are available with the default being "Absolute maximum principle strain". In general "Absolute maximum principle stain" is recommended for brittle materials, while "Signed von Mises strain" is recommended for ductile material. The sign on the signed parameters is taken from the sign of the Maximum Absolute Principal value.

A flowchart of the fatigue setup in HyperMesh can be described as shown in Figure 3.

Figure 3. Fatigue Analysis Flowchart
The three aspects to the fatigue definition are the fatigue material properties, the fatigue parameters and the loading sequence and event definitions.
Defines the elements and associated fatigue properties that will be used for the fatigue analysis.
Defines the finish, treatment, layer and the fatigue strength reduction factors for the elements.
Defines the material properties for the fatigue analysis. These properties should be obtained from the material's E-N curve (Figure 2). The E-N curve, typically, is obtained from completely reversed bending on mirror polished specimen.
  • Fatigue Parameters

    Figure 4. Mean Stress Correction
    Defines the parameters for the fatigue analysis. These include stress combination method, mean stress correction method (Figure 4), Rainflow parameters, and Stress Units.
  • Fatigue Sequence and Event Definition

    Figure 5. Load Time History
    Defines the loading sequence for the fatigue analysis. This card can refer to another FATSEQ card or a FATEVNT card.
    Defines loading events for the fatigue analysis.
    Defines fatigue loading parameters.
    Defines the y values for each point on the time loading history (Figure 5).

Copy the following model files to your working directory. Refer to Access the Model Files.

ctrlarm_EN.fem, load1.csv and load2.csv


A copy of the model files used in this tutorial are available on <install_directory>/tutorials/hwsolvers/optistruct.

In this tutorial, a control arm loaded by brake force and vertical force is used, as shown in Figure 6. Two load time histories acquired for 2545 seconds with 1 HZ, shown in Figure 7 and Figure 8, are adopted. The material of the control arm is aluminum, whose EN curve is shown in Figure 9. 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.

Figure 6. Control Arm for Fatigue Analysis Model

Figure 7. Load Time History for Vertical Force

Figure 8. Load Time History for Braking Force

Figure 9. EN Curve of Aluminum

Launch HyperMesh and Set the OptiStruct User Profile

The model being used for this exercise is that of a control arm (Figure 6). Loads and boundary conditions and two static loadcases have already been defined on this model.

  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_EN.fem file you saved to your working directory.
  5. Click Open.
  6. Click Import, then click Close to close the Import tab.

Set Up the Model

Define TABFAT Load Collector

The first step in defining the loading sequence is to define the TABFAT curves. This 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 curve 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 curve table2 with TABFAT card image is created.
  14. Exit from the Import TABFAT window.
    Tables appear under Curve 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 curves.
  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 5.0.
  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 5.0.

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 EN.
  5. Set MAXLFAT to Yes for the multiaxial method.
  6. Set STRESSU to MPA (Stress Units).
  8. Set CERTNTY SURVCERT to 0.5.

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 Aluminum material.
    The Entity Editor opens.
  2. In the Entity Editor, set MATFAT to EN.
  3. Set UTS (ultimate tensile stress) to 600.
  4. For the EN curve set (these values should be obtained from the material's EN curve):

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. Select the PTYPE check box and activate PSOLID.
  5. Click <Unspecified> in PID: and select Property collector and then select shell.
  6. Click <Unspecified> in PFATID: and select Loadcol and then select pfat.
  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_EN_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. From the Results Browser (left window pane), toggle Components PSOLID_2 and PSOLID_5 off.
  5. On the Results toolbar, click resultsContour-16 to open the Contour panel.
  6. Set Result type to Life and click on Apply to contour the elements.
  7. Right-click on top of the Contour Plot numeric values (in the graphics window) and select Edit Legend.
  8. Select Interpolation: Log and click OK.
    Figure 10. Elemental Life results indicating ~4500 cycles before the first element fails