Fatigue using E-N (Strain

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.

rd2070_SN_curve

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).

rd2080a_strainlife_curve

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.

A flowchart of the fatigue setup in HyperMesh can be described as shown in the image below.

rd2070_fatique_flowchart

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.

The fatigue parameters

rd2070_mean_stress_corr

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.

The fatigue sequence and event definition

rd2070_load_time_history

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).

The following files found in the optistruct.zip file are needed to perform this tutorial. Refer to Accessing the Model Files.

ctrlarm.fem, load1.csv and load2.csv

Exercise

In this tutorial, a control arm loaded by brake force and vertical force is used, as shown in Figure 6. Two load time histories acquired for 2545 seconds with 1 HZ, shown in Figure 7(a) and 7(b), are adopted. The material of the control arm is aluminum, whose E-N curve is shown in Figure 8. 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.

rd2070a_control_arm

Figure 6: Model of the control arm for fatigue analysis

rd2070a_load_time

(a)

rd2070a_vertical_force

(b)

Figure 7: Load time history (a) for vertical force (b) for braking force

rd2080a_EN_curve

Figure 8: EN curve of Aluminum

Step 1: Load and review the model

The model being used for this exercise is that of a control arm as shown in Figure 6. Loads and boundary conditions and two static loadcases have already been defined on this model.

1.	Launch HyperMesh.

2.	Change the User Profiles to OptiStruct.

3.	Import the ctrlarm.fem file you saved to your working directory from the optistruct.zip file. Refer to Accessing the Model Files.

Step 2: Define TABFAT cards

The first step in defining the loading sequence is to define the TABFAT cards. This card represents the loading history.

1.	Click View > Browsers > HyperMesh > Utility.

2.	In the Tools section, click on TABLE Create.

3.	Set Options: to Import table.

4.	Set Tables: to TABFAT.

5.	Click Next.

6.	Browse for the loading file.

7.	In the Open the XY data File dialog box, set the Files of type filter to CSV (*.csv).

8.	Open the file load1.csv.

9.	Create New Table with Name: table1.

10.	Click Apply to save the table. The load collector “table1” with TABFAT card image is created.

11.	Browse for a second loading file named load2.csv.

12.	Create New Table with Name: table2.

13.	Click Apply to save the table. The load collector “table2” with TABFAT card image is created.

14.	Exit from the Import TABFAT window. In the Model browser, tables appear under Load Collector.

Note:

A file in DAC format can very easily be imported in Altair HyperGraph and converted to CSV format to be read in HyperMesh.

Step 3: Defining FATLOAD cards

1.	In the Model browser, right-click and select Create > Load Collector.

2.	For Name, enter FATLOAD1.

3.	Click Color and select a color from the color palette.

4.	For Card Image, select FATLOAD from the drop-down menu.

5.	For TID (table ID), select table1 from the list of load collectors.

6.	For LCID (load case ID), select SUBCASE1 from the list of load steps.

7.	Set LDM (load magnitude) to 1.

8.	Set Scale to 5.0.

9.	Repeat the process to create another load collector named FATLOAD2 with FATLOAD card image and pointing to table2 and SUBCASE2.

10.	Set LDM to 1 and Scale to 5.0.

Step 4: Defining FATEVNT card

1.	In the Model browser, right-click and select Create > Load Collector.

2.	For Name, enter FATEVENT,.

3.	For Card Image, select FATEVNT.

4.	Set FATEVNT_NUM_FLOAD to 2.

5.	Click on the Table icon next to the Data and select FATLOAD1 for FLOAD(1) and FATLOAD2 for FLOAD(2) in the pop-out window.

Step 5: Defining the FATSEQ card

1.	In the Model browser, right-click and select Create > Load Collector.

2.	For Name, enter FATSEQ.

3.	For Card Image, select FATSEQ.

4.	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.

Step 6: Defining the Fatigue parameters

1.	In the Model browser, right-click and select Create > Load Collector.

2.	For Name, enter fatparam,.

3.	For Card Image, select FATPARM.

4.	Make sure TYPE is set to EN.

5.	Set STRESS COMBINE to SGVON (Signed von Mises).

6.	Set STRESS CORRECTION to SWT.

7.	Set STRESSU to MPA (Stress Units).

8.	Set PLASTI to NEUBER (plasticity correction).

9.	Set RAINFLOW RTYPE to STRESS.

10.	Set CERTNTY [SURVCERT] to 0.5.

Step 7: Defining the 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 as EN from the list.

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).

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

Step 8: Defining the PFAT card

1.	In the Model browser, right-click and select Create > Load Collector.

2.	For Name, enter pfat.

3.	Set the Card Image to PFAT.

4.	Set LAYER to TOP.

5.	Set FINISH to NONE.

6.	Set TRTMENT to NONE.

Step 9: Defining the FATDEF card

1.	In the Model browser, right-click and select Create > Load Collector.

2.	For Name, enter fatdef.

3.	Set the Card Image to FATDEF.

4.	Activate PSHELL in the Entity Editor.

5.	Click the Data:PID, PFATID option to open the dialog.

6.	For PID(1), select shell.

7.	For PFATID(1), select pfat.

Step 10: Defining the fatigue load case

1.	In the Model browser, right-click and select Create > Load Step.

2.	For Name, enter Fatigue.

3.	Set the Analysis type to Fatigue.

4.	For FATDEF, select fatdef.

5.	For FATPARM, select fatparam.

6.	For FATSEQ, select FATSEQ.

Step 11: Submitting the OptiStruct analysis and reviewing the results

1.	From the Analysis page, go to the OptiStruct panel.

2.	Click save as following the input file: field. A Save file browser window opens.

3.	Enter the name ctrlarm_hm.fem in File name field.

4.	Click Save.

5.	Submit the analysis by clicking on OptiStruct.

6.	When the analysis process completes, click HyperView to launch the results.

7.	Go to the Results tab.

8.	Change the Load Case to Subcase 3 – fatigue.

9.	Go to the Contour panel in HyperView.

10.	Set Result type to Damage and click on Apply to contour the elements.

rd2080a_results

Figure 9: Elemental damage results

Fatigue using E-N (Strain - Life) Method

Fatigue using E-N (Strain - Life) Method

Fatigue using E-N (Strain - Life) Method

The fatigue parameters

The fatigue sequence and event definition

Exercise