OS-T: 6090 Sine Sweep Fatigue Analysis (EN Damage)

This tutorial provides an overview of fatigue life of structures under Sinusoidal Loading.

Before you begin, copy the file(s) used in this tutorial to your working directory.
A bracket tested for frequency response analysis is utilized to perform the Sine Sweep Fatigue Analysis. The model is already setup for the FRF analysis, an additional loadstep for EN-Fatigue Calculation, with Aluminum as the material, is created in this tutorial. The FRF subcase will be utilized for the fatigue calculation, and a TABLED card scaling the same.
Note: The sweep parameters are currently supported by editing the .fem deck generated, which is explained in this tutorial.
Figure 1. bracket_frf_EN Model for Fatigue Analysis

Launch HyperMesh and Set the OptiStruct User Profile

The model being used for this exercise is that of bracket_frf_EN (Figure 1). Three loadsteps have already been defined on this model, each of which represent Static Analysis, Normal Modes Analysis and Frequency Response excited at the loading point.

  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 bracket_frf_EN.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 2. Fatigue Setup Sine Sweep – EN Damage

Set Up the Model

Create TABLED1 Curve

For Sine Sweep Fatigue Analysis, the TABLED1 card is used.

  1. In the Model Browser, right-click and select Create > Curve.
  2. For Name, enter tabled-fat.
  3. Enter the following magnitudes for (x,y).

    In the x1 field, enter 0.0

    In the y1 field, enter 2.5

    In the x2 field, enter 10000.0

    In the y2 field, enter 2.5

  4. Close the Curve Editor window.
  5. In the Model Browser under Curves, select tabled-fat.
  6. For Card Image, select TABLED1 from the drop-down menu.
  7. Set XAXIS and YAXIS interpolation scheme to LINEAR.
    Figure 3. TABLED1 Curve

  8. Click Close.
    The load collector TABLED1 that defines the time history of the loading has been created.

Define FATLOAD Load Collector

The model has a Frequency Response loadstep defined, which is used to define the FATLOAD.

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter fatload_fat.
  3. For Card Image, select FATLOAD.
  4. Select the option for TID INTEGER.
  5. Set the TID value as the curve ID of tabled-fat (8 in this tutorial).
  6. For LCID(load case ID), select 03_frf from the list of load steps.
    Note: TABFAT and scaling parameters are not required for this calculation.
  7. Select the Option for SWEEP and define the sine sweep parameters via SR (sweep rate) and SRUNIT (sweep rate unit) fields.
    Figure 4. FATLOAD with LCID and SWEEP Parameters

Define FATEVNT Load Collector

Create a random response event for the FATLOAD_RAND created.

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter fatevent-fat.
  3. For Card Image, select FATEVNT.
  4. For FATEVNT_NUM_FLOAD, enter 1.
  5. Select fatload-fat for FLOAD in the Loadcol field.

Define FATSEQ Load Collector

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter fatseq-fat.
  3. For Card Image, select FATSEQ.
  4. For FATSEQ_NUM enter 1, as 1 FATEVENT has been created.
  5. For FID (Fatigue Event Definition), select fatevent-fat and N as 1.
    Figure 5. FATSEQ showing fatevent-fat created

    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 fatparm-fat.
  3. For Card Image, select FATPARM.
  4. Verify TYPE is set to EN.
  6. Set STRESSU to MPA (Stress Units).
  7. Set CERTNTY SURVCERT to 0.9.
  8. Select the SWEEP option and define NF=30.
    Figure 6. FATPARM with SWEEP Parameters

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-fat.
  3. For Card Image, select PFAT.
  4. Set LAYER to WORST.
  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-fat.
  3. Set the Card Image to FATDEF.
  4. Activate PTYPE and PSOLID in the PTYPE Entity Editor.
  6. Select new_bracket for PID and pfat-fat for PFATID.

Define the Fatigue Load Step

  1. In the Model Browser, right-click and select Create > Load Step.
  2. For Name, enter 04-Fatigue.
  3. Set the Analysis type to fatigue.
  4. For FATDEF, select fatdef-fat.
  5. For FATPARM, select fatparm-fat.
  6. For FATSEQ, select fatseq-fat.

Save and Edit the .fem File

  1. Click File > Save As > Model.
  2. Select the bracket-fatigue.hm file from your working directory.
  3. Click Save.
  4. Click Export Solver Deck.
  5. Verify the working directory path and select the bracket-fatigue.fem file.
  6. Click Export.
  7. Open bracket-fatigue.fem in a textpad/notepad.
  8. For FATLOAD, enter TABLED ID = 8
    Figure 7.

  9. For FATPARM, enter:
    Figure 8.

  10. Click Save to save the bracket-fatigue.fem deck.

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 bracket-frf.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. In the Results tab, select Subcase 4 (04-Fatigue) from the subcase field.
  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.
    Figure 9. Damage Contour Plot