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.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).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.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
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
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.Figure 6. Model of the Control Arm for Fatigue Analysis Figure 7. Load Time History for Vertical Force Figure 8. Load Time History for Braking Force 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
Launch HyperMesh.
The User Profile dialog opens.
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
Click File > Import > Solver Deck.
An Import tab is added to your tab menu.
For the File type, select OptiStruct.
Select the Files icon .
A Select OptiStruct file browser
opens.
Select the ctrlarm.fem file you saved
to your working directory.
Click Open.
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 curves. This represents
the loading history.
Make sure the Utility menu is selected in the View
menu. Click View > Browsers > HyperMesh > Utility.
Click on the Utility menu beside the Model tab in the
browser. In the Tools section, click on TABLE
Create.
Set Options to Import table.
Set Tables to TABFAT.
Click Next.
Browse for the loading file.
In the Open the XY Data File dialog box, set the Files of
type filter to CSV (*.csv).
Open the load1.csv file you saved to your working directory.
Create New Table with Name table1.
Click Apply to save the table.
The curve table1 with
TABFAT card image is created.
Browse for a second loading file load2.csv.
Create New Table with Name table2.
Click Apply to save the table.
The curvetable2 with TABFAT card image is
created.
Exit from the Import TABFAT window.
Tables appear under Curve in the Model Browser.
Note: A file in DAC format can very
easily be imported in HyperGraph and converted
to CSV format to be read in HyperMesh.
Define FATLOAD Load Collector
In the Model Browser, right-click and select Create > Load Collector.
For Name, enter FATLOAD1.
Click Color and select a color from the color
palette.
For Card Image, select FATLOAD.
For TID(table ID), select table1 from the list
of curves.
For LCID (load case ID), select SUBCASE1 from the
list of load steps.
Set LDM (load magnitude) to 1.
Set Scale to 5.0.
Repeat the process to create another load collector named
FATLOAD2 with FATLOAD Card
Image and pointing to table2 and
SUBCASE2.
Set LDM to 1 and Scale to 5.0.
Define TABEVNT Load Collector
In the Model Browser, right-click and
select Create > Load Collector.
For Name, enter FATEVENT.
For Card Image, select FATEVNT.
Set FATEVNT_NUM_FLOAD to 2.
Click on the Table icon 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
In the Model Browser, right-click and select Create > Load Collector.
For Name, enter FATSEQ.
For Card Image, select FATSEQ.
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
In the Model Browser, right-click and select Create > Load Collector.
For Name, enter fatparam.
For Card Image, select FATPARM.
Verify TYPE is set to EN.
Set STRESS COMBINE to SGVON
(Signed von Mises).
Set STRESS CORRECTION to SWT.
Set STRESSU to MPA (Stress Units).
Set PLASTI to NEUBER (plasticity correction).
Set RAINFLOW RTYPE to STRESS.
Define the 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, set MATFAT
as EN from the list.
Set UTS (ultimate tensile stress) to 600.
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
In the Model Browser, right-click and select Create > Load Collector.
For Name, enter pfat.
For Card Image, select PFAT.
Set LAYER to TOP.
Set FINISH to NONE.
Set TRTMENT to NONE.
Define FATDEF Load Collector
In the Model Browser, right-click and select Create > Load Collector.
For Name, enter fatdef.
Set the Card Image to FATDEF.
Activate PTYPE and PSHELL in
the PTYPE Entity Editor.
Click the PID, PFATID option to open the dialog.
For PID, select shell.
For PFATID, select pfat.
Click Close.
Define the Fatigue Load Case
In the Model Browser, click on Create > Load Step
For Name, enter Fatigue.
Set the Analysis type to Fatigue.
For FATDEF, select fatdef.
For FATPARM, select fatparam.
For FATSEQ, select FATSEQ.
Submit the Job
From the Analysis page, click the OptiStruct
panel.
Figure 10. Accessing the OptiStruct Panel
Click save as.
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.
Click Save.
The input file field displays the filename and location specified in the
Save As dialog.
Set the export options toggle to all.
Set the run options toggle to analysis.
Set the memory options toggle to memory default.
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
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.
Go to the Results tab.
Change the Load Case to Subcase 3 - fatigue.
On the Results toolbar, click to open the
Contour panel.
Set Result type to Damage and click on
Apply to contour the elements.
Figure 11. Elemental Life results indicating ~4500 cycles before the first
element fails