Problem 5: Transient Results

Fatigue User’s Guide > Validation Problems > Problem 5: Transient Results

XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">

Problem Description

In this example, we investigate the use of transient FE results in a MSC.Fatigue job. This example is broken up into two separate examples, one using external results files, and the other using transient results from MSC.Patran FEA. The first has no specific geometry associated with it while the second is the familiar keyhole model. In both cases, we investigate the difference between the transient approach and the normal pseudo-static method in which a load time history is associated with each static loading case. All things being equal, the two should produce the same results.

Simple Transient Comparison

Objectives

1. To show how to set up a MSC.Fatigue job using external transient results files.

2. To compare this method with results from the pseudo-static method.

Step 1: Geometry and FEA Results

In this particular example, there is no geometry and we have synthesized some results to simulate a transient analysis that may have come from any analysis code which the MSC.Patran system supports.

During the job setup stage, we will create a single node to which we will associate these stress results. There are nine time steps which reside in nine separate files called transN.gps where N corresponds to the time step number. These file can be found in the examples directory delivered with your MSC.Fatigue system.

<install_dir>/mscfatigue_files/examples

For comparison purposes, we will also use the stresses from the first of these files (trans1.gps) with an equivalent load time history to run a pseudo-static fatigue calculation to compare with fatigue life from the transient analysis. This is possible due to the simplicity of this example.

Step 2: Material Characterization

The material chosen is the MANTEN steel alloy with a polished surface finish and no surface treatment. The material already resides in the materials database.

Step 3: Loading Histories

The loading time history is defined by the transient analysis and therefore it is not necessary to create one. However, we also wish to run a fatigue analysis from pseudo-static results for comparison purposes.

The time history will be created by scaling the stress results from the first time step by the ratio relative to the other time steps. These happen to be -2, 2, -1, 0.5, -0.5, 1.5, 1, and 2. In other words the stresses from the second time step are twice (negative) that of the first time step, the third are twice the first, the forth are negative the first, the fifth are half the first, etc. Figure 14‑11 shows the actual load history. The following PTIME keystrokes will reproduce this time history using the X-Y point option. This exercise assumes you are starting in a clean, empty directory.


Operation	Comments
ptime	Invoke PTIME either from the system prompt or from the MSC.Fatigue Loading Information form.
Enter X-Y points	Choose the X-Y point creation option to create the other time history.
Filename: TRANSIENT	Give it a filename called TRANSIENT.
Description 1: Transient example	Give it a description. Accept the defaults for all other fields. Press OK when done.
0 / 1 / -2 / 2 / -1 / 0.5 / -0.5 / 1.5 / 1 / 2 / 0	Enter these values and use the RETURN key each time.
End	Press the End button when done defining the X-Y points.
Plot an entry	Select the Plot option and accept the default. Close the graphics when done.
File / Exit / eXit	Close the graphical display by selecting Exit under the File menu and then select the Exit option to leave PTIME.

Figure 14‑11 Transient Example Time History Equivalent

Step 4: Setup MSC.Fatigue Job

Enter MSC.Patran and use the following keystrokes to set up both jobs. Accept all defaults unless otherwise specified.


Operation	Comments
patran	Invoke MSC.Patran (or MSC.Fatigue Pre & Post) if you have not already done so.
File / New...	Open a new database from the File pull -down menu. Call it “transient.” Set the analysis preference to MSC.Nastran if asked. Ignore any warning messages.
Finite Elements	Open the Finite Elements application from the main form of MSC.Patran.
Action: Create Object: Node Method: Edit	Set the Action, Object, and Method accordingly.
Node Location List: [0,0,0]	Input “[0,0,0]” as the location of a node to be created and click the Apply button. If the Associate with Geometry toggle is ON, set it to OFF before clicking Apply. If you are using MSC.Fatigue Pre & Post you can create the node by typing in the command window: STRING create_nodes[VIRTUAL] fem_create_nodes(“Coord 0”,”Coord 0”,TRUE,”1”,”[0,0,0]”,create_nodes)
Tools / FATIGUE... (Analysis)	Invoke MSC.Patran’s FATIGUE interface by selecting it from under the Tools pull-down menu (or the Analysis application switch in MSC.Fatigue Pre & Post).
General Setup Parameters:
Analysis: Initiation	Set the analysis type to Crack Initiation on the main form.
Jobname: Transient	Give the job a name. Use transient.
Title: Transient Example	Give the job a title.
Solution Parameters Form: Accept all defaults.
Materials Information Form:
Material: MANTEN	Place the cursor in the cell under the word Material and click on the mouse. A listbox will appear. Select the material MANTEN from this listbox.
Finish: Polished	Select Polished from the option menu that appears. The word polished appears in the Finish cell. The SAE specimen was a polished specimen with no surface treatment.
Treatment: No Treatment	Select No Treatment from the option menu that appears.
Region: default_group	Select the default group as the region. This contains the node we created at the beginning of this exercise. The Materials Information form can be closed down now by clicking the OK button.
Loading Information Form:
Results Type: Transient	FE results are from a Transient analysis.
Results From: External	The results are from an external MSC.Patran results file.
Surface: Top	This parameter is not applicable for this example.
External File Names: trans#.gps Columns: 1,2,3,4,5,6	Input the trans#.gps file name. Also indicate which columns the component stresses can be found in the files. Each time step comprises one file where the wildcard (#) will be replaced by the time step number.
Scale Factor: 1	Leave this at unity.
No. of Time Steps: 9	The number of time steps is 9. There are nine external stress results files in your local directory. Press OK.
Job Control Form:
Full Analysis	Set the action to Full Analysis and click the Apply button. Let this job run and set up the static analysis for which we will compare against.
General Setup Parameters:
Jobname: static	Change the jobname on the main form to static.
Title: Static Example	Give the job a different title.
Loading Information Form:
Results Type: Static	Change the FE results from Transient to Static.
Results From: External	This should stay the same.
External File Names: trans#.gps Columns: 1,2,3,4,5,6	This stays the same.
Load Case ID: 1	Place the cursor in this cell and press RETURN to accept load case one from the displayed databox.
Time History: TRANSIENT	Select the TRANSIENT time history from the spreadsheet that appears when this cell is active.
Load Magnitude: 1.0	Accept the default for this cell. Make sure you press RETURN in the databox to accept the value in the cell.
Job Control Form:
Full Analysis	Set the action to Full Analysis and press the Apply button.
Monitor	Monitor the job if you wish.

The following notes are made about the job setup:

1. Notice that when setting up the transient job, no time history and/or load case data was requested. This makes the setup much easier and quicker.

2. When specifying the time history files you are required to indicate the number of time steps. In this case there were nine. The program then looks for files called trans1.gps, trans2.gps, ..., trans9.gps. The # wild card is substituted for the time step numbers. For transient cases, these must be sequential starting as 1.

3. For static cases, the load case ID is substituted for the # wild card. It does not have to be sequential. For instance, we could have indicated trans5.gps to be the only load case by specifying the load case id as 5. In this case only trans1.gps was used and was scaled according to the externally defined time history transient.dac.

Step 5: Evaluate Results

The last portion of this exercise is to simply look at the results and see that they are the same between the two different fatigue jobs (~550 repeats).


Operation	Comments
Results Form:
List Results	Set the Action to List Results. The separate MSC.Fatigue module PFPOST will be spawned. Press the Apply button.
OK	Press OK twice when the PFPOST form comes up to accept the default jobname (static).
Most Damaged Nodes	Select the first option to view the most damaged elements. Press OK when done.
Cancel	Press the Cancel button to page up to the initial form.
Jobname: transient	Input the transient jobname.
Most Damaged Nodes / OK / eXit	Repeat the operations above to look at the transient results and then exit.

MSC Nastran Transient Results

Objectives

1. To show how to set up a MSC Fatigue job using MSC Nastran static and transient results.

2. To compare this method with results from the pseudo-static method as done in the previous example.

Step 1: Geometry and FEA Results

The geometry is the keyhole model that you have used in some of the previous problems. However, you will need to use a different neutral file that has been set up specifically for a modal transient analysis. The geometry and results are in the key_stat.op2 and key_tran.op2 files which can be found in the examples directory delivered with your MSC.Fatigue system.

<install_dir>/mscfatigue_files/examples

Unlike previous examples you will need to import these results into the database.

Enter MSC.Patran or MSC.Fatigue Pre & Post and use the following keystrokes:


Operation	Comments
patran	Invoke MSC.Patran (or MSC.Fatigue Pre & Post) if you have not already done so.
File / New...	Open a new database from the File pull down menu. Call it “keyhole.” Set the analysis preference to MSC.Nastran if asked. Ignore any warning messages.
Analysis / Import	Open the Analysis application from the main form of MSC.Patran or the Import application in MSC.Fatigue Pre & Post.
Action: Read Output2 Object: Both Method: Translate	Set the Action, Object, and Method accordingly.
Select Results File...	Select the result file key_stat.op2. Click the Apply button to import the model and static results.
Action: Read Output2 Object: Result Entities Method: Translate	Set the Action, Object, and Method accordingly.
Select Results File...	Select the result file key_tran.op2. Click the Apply button to import th transient results.
Tools / FATIGUE... (Analysis)	Invoke MSC.Patran’s FATIGUE interface by selecting it from under the Tools pull-down menu (or the Analysis application switch in MSC.Fatigue Pre & Post).

The static load case results were determined using a 30 Newton loading at the same point of application as the original keyhole problem, the results from which, when scaled by the load time history should give roughly equivalent stress time histories for all nodes as does the modal transient analysis. This of course does not take into account any dynamic effects that the mass distribution may have on the dynamic behavior and resulting stress results, however with this simple model and a very evenly distributed mass, there should not be a large difference. The previous example we expected to obtain exactly the same answer between the pseudo-static and transient examples. This will not be the case for this problem but the answers should be statistically equivalent.

Step 2: Material Characterization

The material chosen is the MANTEN steel alloy with a polished surface finish and no surface treatment. The material already resides in the materials database.

Step 3: Loading Histories

The loading time history is defined by the transient analysis and therefore, is not necessary to create one. However, we also wish to run a fatigue analysis from pseudo-static results for comparison purposes.

The time history will be created by reading in an ASCII version of this time history that is equivalent to the force time history used in the transient analysis. This file can be found in the examples directory delivered with your MSC.Fatigue system and is called key_tran.asc. The following PTIME keystrokes will accomplish this for you assuming you started in a clean, empty directory.


Operation	Comments
Loading Information Form:
ptime	Invoke PTIME either from the system prompt or from the MSC.Fatigue Loading form by pressing the Time History Manager button.
Add an entry / ASCII convert + load	Select the ASCII load option.
ASCII Filename: key_tran.asc	Enter the name of the file.
OK	Accept this form.
Description 1	You must enter at least one descriptive title. Accept the defaults for the rest of the fields and click the OK button.
Plot an entry...	Select the Plot a time history option to plot the new time histories. Use the List button to select one for viewing. Repeat this operation as many times as you wish to view the time histories.
File / Exit / eXit	Close the graphical display by selecting Exit under the File menu and then select the Exit option to leave PTIME.

Step 4: Setup MSC.Fatigue Job

Re-enter MSC.Patran (if you left) and issue these commands to set up the fatigue analyses using both the transient and the static results from the MSC.Fatigue main form accepting all defaults unless otherwise specified.


Operation	Comments
General Setup Parameters:
Analysis: Initiation	Set the analysis type to Crack Initiation on the main form.
Jobname: key_tran	Give the job a name. Use “key_tran.”
Title: Transient Example	Give the job a title.
Solution Parameters Form: Accept all defaults.
Materials Information Form:
Material: MANTEN	Place the cursor in the cell under the word Material and click on the mouse. A listbox will appear. Select the material MANTEN from this listbox.
Finish: Polished	Select Polished from the option menu that appears. The word polished appears in the Finish cell. The SAE specimen was a polished specimen with no surface treatment.
Treatment: No Treatment	Select No Treatment from the option menu that appears.
Region: default_group	Select the default group as the region. This contains all nodes in the model. The Materials Information form can be closed down now by clicking the OK button.
Loading Information Form:
Results Type: Transient	FE results are from a Transient analysis.
Get/Filter Results...	Open this form from the Loading Information form. Select the only Result Case that appears in this top of this form. It may already be selected for you (LOAD_CASE.1, 131 subcases).
Filter Method:Global Variable - Variable:Time	Turn this option menu to Global Variable and set the Variable to Time. This may already be the default settings.
Filter/Add/Close	Press the Filter button. This will filter only subcases with time step information from the Result Case. Remember there is a static load case in these also. Click the Apply button. This will load all the time steps into the listbox on the Loading Information form which will be used in the analysis.
Results Time Steps / Select a Stress/Strain Tensor / Select a Layer	Select one of the time steps in the first listbox. Since there are only stresses and the top layer is the default this is all you need to do. Everything else is automatically selected. All the time steps in the list box will be used in the analysis. Click OK to accept the Loading form.
Job Control Form:
Full Analysis	Set the action to Full Analysis and click the Apply button. Let this job run and set up the static analysis for which we will compare against.
General Setup Parameters:
Analysis: Initiation	Set the analysis type to Crack Initiation on the main form.
Jobname: key_stat	Give the job a name. Use “key_stat.”
Title: Static Example	Give the job a title.
Solution Parameters Form: Accept all defaults.
Materials Information Form: This remains the same.
Loading Information Form:
Results Type: Static	Change the FE results from Transient to Static.
Load Case ID:	Place the cursor in this cell and click the mouse to reveal the database result listboxes.
Get/Filter Results...	Open this form from the Loading Information form.
Select All Results Cases	Turn this toggle on and click the Apply button. This will fill the listbox with available results from time step analyses.
Results Time Steps / Select a Stress/Strain Tensor / Select a Layer	Select the only “Static Subcase” in the first listbox (the time steps from the transient analysis also appear but don’t select any of them). Since there are only stresses and the top layer is the default this is all you need to do. Everything else is automatically selected.
Fill Cell	Press the Fill Cell button to fill the Load Case ID cell with the internal Result Case IDs of the selected static results.
Time History: KEY_TRAN	Select the KEY_TRAN time history from the spreadsheet that appears when this cell is active.
Load Magnitude: 1.0	Accept the default for this cell. Make sure you press RETURN in the databox to accept the value in the cell.
Job Control Form:
Full Analysis	Set the action to Full Analysis and click the Apply button.
Monitor	Monitor the job if you wish after reopening the forms.

Step 5: Evaluate Results

The last portion of this exercise is to simply look at the results and see that they are approximately the same between the two different fatigue jobs (~2400 repeats). There is a difference between the two which is most likely due to the fact that the modal transient takes into account the dynamic effects of the mass distribution whereas the pseudo-static does not, as mentioned earlier.


Operation	Comments
Results Form:
List Results	Set the Action to List Results. The separate MSC.Fatigue module PFPOST will be spawned. Press the Apply button.
OK	Press OK twice when the PFPOST form comes up to accept the default jobname (“key_stat”).
Most Damaged Nodes	Select the first option to view the most damaged elements.
OK	Clear the summary page.
Cancel	Press the Cancel button to page up to the initial form. Repeat this for the “key_tran” job.