Spot Weld Fatigue (FPM) using S-N Method

Spot weld fatigue can only be applied to spot welds between two shells. The spot weld location is defined by three attributes, sheet 1, sheet 2, and the nugget. The sheets are defined by shell elements, and the nugget is defined by CWELD, CBAR, CBEAM, or CHEXA elements. The nugget can be directly connected to the shells or RBE2/RBE3 elements can be used to connect the nugget to the shells.

The following file found in the file is needed to perform this tutorial. Refer to Access the Model Files.


A frame is experiencing frontal and rear torsional loads in addition to vertical bending. Welds are modeled between the sections forming the frame.

Figure 1. Spot Welds Modeled between Two Frame Sections
You will be able to calculate the damage that occurs at the spot weld locations. The solver deck setup is done using process manager. In brief, the following contents are covered:
  • Launch Fatigue Process Manager
  • Import a model
  • Create fatigue subcase
  • Define fatigue analysis parameters
  • Define fatigue elements and S-N properties
  • Define load-time history and loading sequence
  • Submit the job
  • View results summary and launch HyperView for post-processing

Launch HyperMesh and Set the OptiStruct User Profile

The model being used for this exercise is that of an automotive frame (Figure 1). The input file consists of 3 static loadsteps to which the frame is subjected to – Frontal torsion, Rear torsion and the Vertical bending.

  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 Spotweld_CharNugget.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.
    The outline of the Fatigue Analysis setup to be achieved in the following steps.

    Figure 2. Fatigue Setup – Spot Welds

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 Fatigue-SpotWeld-Analysis.
  3. Click Create.
  4. For the Select existing fatigue subcase field, select the newly created fatigue subcase Fatigue-SpotWeld-Analysis.
    Fatigue-SpotWeld-Analysis 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 3. Create and Select Active Fatigue Subcase to Process

Define Fatigue Parameters

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter Fat-Parameter.
  3. For Card Image, select FATPARM.
  4. Verify TYPE is set to SN.
  5. Set STRESS COMBINE to SGVON (Signed von Mises).
  6. Set STRESSU to MPA (Stress Units).
  8. Set GATEREL to 0.0.
  9. Set CERTNTY SURVCERT to 0.5.
  10. Check the box beside SPWLD and select the following options:



    SURVCERT = 0.9


    NANGLE = 20

  11. Click Apply.

Add Fatigue Elements and Materials

Make sure the task Elements and Materials is selected in the Fatigue Analysis tree.

  1. Click Add Material.
    A Material Data window opens.

    Figure 4. Material Data Definition
  2. For Material name, select Steel.
  3. Make sure Stress unit is set to MPA.
  4. For Ultimate tensile strength (UTS), enter 1000.
  5. Activate Spot Weld Material Properties, then click Spot Weld Material Properties.
  6. Enter the values for Mean Stress Sensitivity, MSS2, Structural SN Curve along with bending and membrane SN curve material values, as shown below.

    Figure 5. Spot Weld Material Properties dialog
  7. Click OK.
  8. Click Save.
  9. Click Add Property.

    Figure 6. Property Data dialog
  10. For Property Type, select Property - PBARL.
  11. For Property Name, select PBARL_4.
  12. Click Close to save the definition of the SN data for the selected property.

Define PFATSPW Property

  1. In the Model Browser, right-click and select Create > Property.
  2. For Name, enter PFATSPW.
  3. For Card Image, select PFATSPW.
  4. Set SPTFAIL to All.
  5. Set ALPHA to 3.5.
  6. Set TREF to 1.0.
  7. Set TREF_N to 0.2.
  8. Set SF to 1.0.
  9. Click Close.

Define FATDEF Load Collector

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter FATDEF1.
  3. Set the Card Image to FATDEF.
  4. Activate PTYPE, PBARL and PFATSPWID in the PTYPE Entity Editor.
  5. For FATDEF_PBARL_NUMIDS, enter 1.
  6. Select PBARL_4 for PID and PFATSPW for PFATSPW.

    Figure 7. Fatigue Definition showing the combination of Weld Element Properties
  7. Click Close.

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 8. 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 9. 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. Activate the radio button Manual and leave the event creation method set to default Single Event.
  4. Click + button to create a single event with three subcases and two channels.
  5. Drag and drop the three subcases (Front Torsional Stiffness, Rear Torsional Stiffness and Vertical Bending Stiffness) under Subcases of the newly created event.
  6. Drag and drop the two channels (LTH1 and LTH2) to the three subcases to create loading sequence, as shown below.
  7. Drop LTH1 for the first subcase (Front Torsional Stiffness) and LTH2 for the other two subcases (Rear Torsional Stiffness and Vertical Bending Stiffness).
  8. Set LDM to 0.1 and Scale to 3.0 for all three cases.

    Figure 10. Load Mapping to associate load-time history with static subcase
  9. Click Save to close the window and create the fatique event using selected subcases and channels.

    Figure 11. Loading Sequences Definition

Submit the Job

Make sure the task Submit Analysis is selected in the Fatigue Analysis tree.

  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 SpotWeld_Cbar_Nugget_fat.fem.
  4. Click Save twice.
  5. For Run Option, select analysis.
  6. Click Submit.
    This launches OptiStruct to run the fatigue analysis.
    If the job was successful, new results files can be seen in the directory where the OptiStruct model file was written. The default files written to your directory are:
    Hyper 3D binary results file, with both static analysis results and fatigue analysis results.
    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.
    Summary of analysis process, providing CPU information for each step during analysis process.

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 SpotWeld_Cbar_Nugget_fat.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 12. Post-Processing

    Figure 13. Damage Contour in HyperView