In this tutorial, 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 example. The FRF subcase is utilized for the fatigue
calculation, and a TABLED card scaling the same.
Note: The sweep
parameters are currently supported by editing the generated fem deck. This
process is explained in the tutorial.
Figure 1. bracket_frf_EN Model for Fatigue Analysis
The outline of the Fatigue Analysis setup in this tutorial is shown in the Figure 2
block diagram.Figure 2. Fatigue Setup Sine Sweep - EN Damage
Launch HyperMesh
Launch HyperMesh.
In the New Session window, select HyperMesh from the list of tools.
For Profile, select OptiStruct.
Click Create Session.
Figure 3. Create New Session This loads the user profile, including the appropriate template, menus,
and functionalities of HyperMesh relevant for
generating models for OptiStruct.
Import the Model
On the menu bar, select File > Import > Solver Deck.
In the Import File window, navigate to and select
bracket_frf_EN you saved to your
working directory.
Click Open.
In the Solver Import Options dialog, ensure the Reader is
set to OptiStruct.
Figure 4. Import Base Model in HyperMesh
Accept the default settings and click Import.
Set Up the Model
Define TABLED1
In the Model Browser, right-click and select
Create > Curve.
A default Curve editor window opens.
For Name, enter tabled-fat.
Enter the following magnitudes for (x,y):
(x1, y1) = (0.0, 2.5)
(x2, y2) = (10000.0, 2.5)
Close the Curve editor window.
In the Model Browser, under Curves, select
tabled-fat.
For Card Image, select TABLED1 from the drop-down
menu.
Verify the XAXIS and YAXIS interpolation scheme is set to
LINEAR.
Figure 5. TABLED1 Card
Define FATLOAD
In the Model Browser, right-click and select
Create > Load Collector.
For Name, enter fatload-fat.
For Card Image, select FATLOAD from the drop-down
menu.
Select the TID_INTEGER check box.
Set the value of TID as the Curve ID of tabled-fat (in this tutorial,
tabled-fat ID = 6).
For LCID (load case ID), select 03_frf from the list of
load steps.
This is the Frequency Response Analysis load step.
Select the Sweep check box.
Define the sine sweep parameters as:
SR (sweep rate) = 2.0
SRUNIT (sweep rate unit) = HZPS
Figure 6. FATLOAD with LCID and SWEEP Parameters
Click
Close.
Define FATEVNT
Create a random response events for the FATLOAD_RAND created.
In the Model Browser, right-click and select
Create > Load Collector.
For Name, enter fatevent-fat.
For Card Image, select FATEVNT from the drop-down
menu.
Set FATEVNT_NUM_FLOAD to 1.
For FLOAD in the Loadcol field, select
fatload-fat.
Click
Close.
Define FATSEQ
In the Model Browser, right-click and select
Create > Load Collector.
For Name, enter fatseq-fat.
For Card Image, select FATSEQ from the drop-down
menu.
For FATSEQ_NUM, enter 1 as we have 1 FATEVENT
created.
For FID (Fatigue Event Definition), select fatevent-fat
from the list of load collectors.
For N, enter 1.
Figure 7. FATSEQ Showing the fatevent-fat Created
Click
Close.
Define Fatigue Parameters
In the Model Browser, right-click and select
Create > Load Collector.
For Name, enter fatparm-fat.
For Card Image, select FATPARM from the drop-down
menu.
Under STRESS, for COMBINE select VONMISES.
For STRESSU to MPA.
Verify TYPE is set to EN.
Under CERTNTY, for SURVCERT enter 0.9.
Select the SWEEP check box.
Select the NF_OPTION check box and enter
30 in the text box.
Figure 8. FATPARM with SWEEP Parameters
Click
Close.
Define Fatigue Material Properties
The material curve for the fatigue analysis can be defined on the
MAT1 card.
In the Model Browser, click on the
Aluminum material.
The Entity Editor opens.
In the Entity Editor, select the
MATFAT and EN check boxes from
the list.
For UTS (ultimate tensile stress), enter 600.
For the EN curve set, enter the following values (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
In the Model Browser, right-click and select
Create > Load Collector.
For Name, enter pfat-fat.
For Card Image, select PFAT.
For LAYER, select WORST.
For FINISH, select NONE.
For TRTMENT, select NONE.
For Kf, enter 1.0.
Click
Close.
Define FATDEF
In the Model Browser, right-click and select
Create > Load Collector.
For Name, enter fatdef-fat.
For Card Image, select FATDEF.
Select the PTYPE check box.
Select the PSHELL check box.
For FATDEF_PSHELL_NUMIDS, enter 1.
For PID, select new_bracket.
For PFATID, select pfat-fat.
Click
Close.
Define the Fatigue Load Step
In the Model Browser, right-click and select
Create > Load Step.
For Name, enter 04-Fatigue.
For Analysis type, select fatigue.
For FATDEF, select fatdef-fat.
For FATPARM, select fatparm-fat.
For FATSEQ, select fatseq-fat.
Click
Close.
Submit the Job
Run OptiStruct.
From the Analyze ribbon, click Run OptiStruct
Solver.
Figure 9. Select Run OptiStruct Solver
Select the directory where you want to write the OptiStruct model file.
For File name, enter Bracket_frf.
The .fem filename extension is the recommended extension
for Bulk Data Format input decks.
Click Save.
Click Export.
In the Altair Compute Console, click
Run.
If the job is successful, an "ANALYSIS COMPLETED" message appears in the
Compute Console Solver View Message Log. New results
files are in the directory where the model file was written. The
Bracket_frf.out file is a good
place to look for error messages that could help debug the input deck if any
errors are present.
View the Results
When the analysis is finished, click HyperView to
launch the results.
In the Results tab, select Subcase 4 (04-Fatigue) from
the Subcase field.
