Fatigue using E-N (Strain - Life) Method

The E-N (Strain - Life) method should be chosen to predict the fatigue life when plastic strain occurs under the given cyclic loading. S-N (Stress - Life) method 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 method may be a better choice. The E-N method, while computationally more expensive than S-N, should give a reasonable estimate for high-cycle fatigue as well.

rd2070_SN_curve
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).

rd2080a_strainlife_curve
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.

rd2070_fatique_flowchart
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.
FATDEF
Defines the elements and associated fatigue properties that will be used for the fatigue analysis.
PFAT
Defines the finish, treatment, layer and the fatigue strength reduction factors for the elements.
MATFAT
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

    rd2070_mean_stress_corr
    Figure 4. Mean Stress Correction
    FATPARM
    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

    rd2070_load_time_history
    Figure 5. Load Time History
    FATSEQ
    Defines the loading sequence for the fatigue analysis. This card can refer to another FATSEQ card or a FATEVNT card.
    FATEVNT
    Defines loading events for the fatigue analysis.
    FATLOAD
    Defines fatigue loading parameters.
    TABLEFAT
    Defines the y values for each point on the time loading history (Figure 5).
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. The material of the control arm is aluminum, whose E-N curve is shown in Figure 4. 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.

rd2070a_control_arm
Figure 6. Model of the Control Arm for Fatigue Analysis

rd2070a_load_time
Figure 7. Load Time History for Vertical Force

rd2070a_vertical_force
Figure 8. Load Time History for Braking Force

rd2080a_en_curve
Figure 9. EN Curve of Aluminum

The model being used for this exercise is that of a control arm as shown in Figure 1. Loads and boundary conditions and two static loadcases have already been defined on this model.

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. Refer to Access the Model Files.
  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 cards. This card represents the loading history.

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter TABFAT.
  3. For Card Image, select TABFAT from the drop-down menu.
  4. For TABLEFAT_NUM, enter 2.
  5. Click on the Table icon table_pencil next to the Data: field, enter 1 in row1 and enter -1 in row2 as the y values.
  6. Click Close.

Define FATLOAD Load Collector

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter .
  3. For Card Image, select FATLOAD.
  4. For TID(table ID), select table1 from the list of load collectors.
  5. For LCID (load case ID), select SUBCASE1 from the list of load steps.
  6. Set LDM (load magnitude) to 1.
  7. Set Scale to 5.0.
  8. Repeat the process to create another load collector named FATLOAD2 with FATLOAD Card Image and pointing to table2 and SUBCASE2.
  9. Set LDM to 1 and Scale to 5.0.

Define TABEVNT 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. Set FATEVNT_NUM_FLOAD to 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 TABSEQ 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 from the list of load collectors.
    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 STRESS COMBINE to SGVON (Signed von Mises).
  6. Set STRESS CORRECTION to SWT.
  7. Set STRESSU to MPA (Stress Units).
  8. Set PLASTI to NEUBER (plasticity correction).
  9. Set RAINFLOW RTYPE to STRESS.

Define the 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 as EN from the list.
  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).
    SF
    1002.000
    B
    -0.095
    C
    -0.690
    EF
    0.350
    NP
    0.110
    KP
    966.000
    NC
    2E+08
    SEE
    0.100
    SEP
    0.100

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.

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 PSHELL in the PTYPE Entity Editor.
  5. Click the Data:PID, PFATID option to open the dialog.
  6. For PID(1), select shell.
  7. For PFATID(1), select pfat.
  8. Click Close.

Define the Fatigue Load Case

  1. In the Model Browser, click on 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, click the OptiStruct panel.

    OS_1000_13_17
    Figure 10. Accessing the OptiStruct Panel
  2. Click save as.
  3. In the Save As dialog, specify location to write the OptiStruct model file and enter for filename.
    For OptiStruct input decks, .fem is the recommended extension.
  4. Click Save.
    The input file field displays the filename and location specified in the Save As dialog.
  5. Set the export options toggle to all.
  6. Set the run options toggle to analysis.
  7. Set the memory options toggle to memory default.
  8. Click OptiStruct to launch the OptiStruct job.
If the job is successful, new results files should be in the directory where the .fem was written. The .out file is a good place to look for error messages that could help debug the input deck if any errors are present.

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 11. Elemental Life results indicating ~4500 cycles before the first element fails