Fatigue Process Manager (FPM) using S-N (Stress - Life) Method

OptiStruct uses the S-N approach for calculating the fatigue life. The S-N approach is suitable for high cycle fatigue, where the material is subject to cyclical stresses that are predominantly within the elastic range. Structures under such stress ranges should typically survive more than 1000 cycles.

The S-N approach is based on elastic cyclic loading, inferring that the S-N curve should be confined to numbers greater than 1000 cycles. This ensures that no significant plasticity is occurring. This is commonly referred to as high-cycle fatigue.

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

Figure 2. Two segment S-N Curve

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

In this tutorial, you will be able to evaluate fatigue life with the S-N method through process manager step by step.

Launch HyperMesh and Process Manager

  1. Launch HyperMesh.
    The User Profile dialog opens.
  2. Select OptiStruct and click OK.
  3. Click Tools > Fatigue Process > Create New.
  4. For New Session Name, enter <my_session_name>.
  5. For Working Folder, select your working folder.
  6. Click Create.
    This creates a new file to save the instance of the currently loaded fatigue process template.

    Figure 3.

Import the Model

  1. Make sure the task Import File is selected in the Fatigue Analysis tree.
  2. For the Model file type, select OptiStruct.
  3. Click the Open model file icon files_panel.
    A Select File browser window opens.
  4. Select the ctrlarm.fem file you saved to your working directory from the optistruct.zip file and click Open.
  5. Click Import.
    This loads the control arm model. It includes a whole definition of two static subcases, elements sets, and material static properties, etc.
  6. Click Apply.
    This guides you to the next task Fatigue Subcase of the Fatigue Analysis tree.

    Figure 4. Import a Finite Element Model file

Set Up the Model

Create a Fatigue Subcase

  1. Make sure the task Fatigue Subcase is selected in the Fatigue Analysis tree.
  2. In the Create new fatigue subcase field, enter fatsub_fpmtut.
  3. Click Create.
  4. For the Select existing fatigue subcase field, select the newly created fatigue subcase fatsub_fpmtut.
    fatsub_fpmtut is selected as the active fatigue subcase. Definitions in the following processes (analysis parameters, fatigue elements and properties, loading sequences, etc.) will be for this subcase.
  5. Click Apply.
    This saves the current definitions and guides you to the next task Analysis Parameters of the Fatigue Analysis tree.


    Figure 5. Create and Select Active Fatigue Subcase to Process

Apply Fatigue Analysis Parameters

  1. Make sure the task Analysis Parameters is selected in the Fatigue Analysis tree.
  2. Select the following options:
    Analysis type
    Stress combination method
    Signed von Mises
    FEA model unit
    Mean stress correction
    Rainflow type
  3. Enter the following values:
    Certainty of survivial
  4. Click Apply.
    This saves the current definitions and guides you to the next task Elements and Materials of the Fatigue Analysis tree. For details, consult the Altair Simulation 2022 help.

    Figure 6. Fatigue Analysis Parameters Definition

Add Fatigue Elements and Materials

  1. Make sure the task Elements and Materials is selected in the Fatigue Analysis tree.
  2. Click Add Material.
    A Material Data window opens.

    Figure 7. Material Data Definition
  3. For Material name, select Aluminum.
  4. Make sure Stress unit is set to MPA.
  5. For Ultimate tensile strength (UTS), enter 600.
  6. Click SN Curve Material Properties.
    An SN Curve Material Properties dialog opens.

    Figure 8.
  7. For Input method of defining S-N curve, select Estimate From UTS.
  8. Click the Show SN curve definition icon 05_sn_curve.
    An SN method description window introducing how to generate the SN material parameter opens.
  9. Click Close.
  10. For Material type, select Aluminum Alloys and click Estimate.
    All the data for SN curve definition are automatically estimated.
  11. Click OK.
  12. Click Plot SN Curve at the bottom of the window to show the SN curve.

    Figure 9.
  13. Close the SN Curve plot window.
  14. Click Add Property.
    A Property Data dialog opens.

    Figure 10.
  15. For Property Type, select Property - PSHELL.
  16. For Property, select shell.
    This is the skin coating the solid control arm.
  17. Click Create to create create PFAT property.
  18. For LAYER, select TOP.
  19. For FINISH, select NONE.
  20. For TREATMENT, select NONE.
  21. Leave the field after KF (Fatigue strength reduction factor) set at 1.0.
  22. Click Close to save the definition of the SN data for the selected property.
  23. Click Close in the Property Data dialog to save the fatigue definition.
    This saves the current definitions and guides you to the next task Load-Time History of the Fatigue Analysis tree.

    Figure 11. Elements and Material Definition

Apply Load-Time History

  1. Make sure the task Load-Time History is selected in the Fatigue Analysis tree.
  2. Click Add by File.
    A Load Time History window opens.
  3. For Load-time history name, enter LTH1.
  4. For Load-time history type, select CSV.
  5. Click the Open load-time file icon files_panel.
    An Open file browser window opens.
  6. Browse for load1.csv.
  7. Click Open > Import.

    Figure 12. Import Load-Time History
  8. Click Save to write the new load-time history into HyperMesh database.
  9. Click Plot L-T to show the load-time history.
  10. Close the Load Time History window.
  11. Click Apply.
    This saves the current definitions and guides you to the next task Loading Sequences of the Fatigue Analysis tree.

    Figure 13. Load-Time History Definition
    Note: The RPC/RSP and DAC file formats are now supported in fpm. Make sure to use HyperMesh Desktop application for this.

Load Sequences

In this step, one event consisting of two load time history is created; in other words, the linear superposition of the stress caused by the two load time history is requested during analysis. Using this event, one load sequence is constructed.
  1. Make sure the task Loading Sequences is selected in the Fatigue Analysis tree.
  2. Click Add.
    A Load Mapping window opens.
  3. For Channels, select LTH1 and LTH2.
  4. For Subcase, select SUBCASE1 and SUBCASE2.
  5. Activate the radio button Auto and leave the event creation method set to default Single Event.
  6. Click + to create a single event with two subcases and two channels.

    Figure 14. Load Mapping to associate load-time history with static subcase
  7. Click Save to close the window and create the fatique event using selected subcases and channels.

    Figure 15. Loading Sequences Definition

Submit the Job

  1. Make sure the task Submit Analysis is selected in the Fatigue Analysis tree.
  2. Click the Save .fem file icon files_panel.
    A Save As browser window opens.
  3. Set the directory in which to save the file, and for File name, enter ctrlarm_fpmtut.fem.
  4. Click Save to close the window.
  5. Click Save to save the OptiStruct model file.
  6. For Run Option, select analysis.
  7. Click Submit.
    This launches OptiStruct 2022 to run the fatigue analysis. If the job is successful, the new results files should be in the directory from which ctrlarm_fpmtut.fem was selected.
    The default files written to the directory are:
    ctrlarm_fpmtut.0.3.fat An ASCII format file which contains fatigue results of each fatigue subcase in iteration step.
    ctrlarm_fpmtut.h3d Hyper 3D binary results file, with both static analysis results and fatigue analysis results.
    ctrlarm_fpmtut.out OptiStruct output file containing specific information on the file set up, the set up of your fatigue problem, compute time information, etc. Review this file for warnings and errors.
    ctrlarm_fpmtut.stat Summary of analysis process, providing CPU information for each step during analysis process.
    Note: The filename.#.fat is created for each fatigue subcase at the first and last iterations only if a fatigue optimization is performed.

    Figure 16. Submit Fatigue Analysis

    Figure 17.

Post-process the Analysis

  1. Make sure the task Post-processing is selected in the Fatigue Analysis tree.
    When fatigue analysis has completed successfully after the previous submit, it will automatically go into this task.
  2. For Fatigue subcase, make sure Select Subcase is selected.
  3. For Result Type and Data Component, select the required data you want to contour from the drop-down menu.
  4. Click Load H3D Results (HV).
    This launches HyperView and loads the ctrlarm_fpmtut.h3d results file. It applies the result contour for selected result type and component. You can use HyperView for more detailed results.
  5. Click Exit to unload Fatigue Process Manager.

    Figure 18. Post-Processing

    Figure 19. Damage Contour in HyperView