XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''"> Fatigue Preprocessing
MSC.Fatigue has the following preprocessing modules:
• Set Fatigue Environmental Variables
• Low Damage Removal
• Calculate Stress Gradient
Low Damage Removal
The Low Damage Removal utility is designed to extract areas of the model that are likely to sustain high damage. These areas are then grouped based on User selection of existing User created groups or automatically extracted material groups resident in the Patran database. In the example shown on the right, the User may select all or pick one or more of the automatically extracted material groups. The Von mises stress or strain results from all selected loadcases are scanned and for each material group, a group is created that contains the top User selectable percentage of loaded entities in that group. The solution sequences that utilize stress or strain results can benefit from this extraction. The only exception to this is Seam weld, and although this utility can be used to identify the critical areas, users will have to exercise caution in using the extracted groups as the Seam weld module performs an extraction of the seam off the weld group and it is possible that the weld may not be a part of the extracted group.
For the force-based Spotweld solution sequence, critical Spot weld elements are extracted based on the magnitudes of the translational and rotational components. Either the material group associated with the Spot weld elements or a group containing only the Spot weld elements (recommended) is used for the extraction.
The groups extracted by this utility may then be used in a subsequent fatigue analysis for a quick assessment of the high damage areas of the model.
Note: | This extraction performed by this Utility does not take into account the phasing from Superpositioning of the results for multiple channel loading. FASTAN should be used in this case as proper account of the phasing is taken into account to extract high damage areas. |
This Low Damage Removal utility can be accessed by selecting the option from the Fatigue Preprocessing pull-down menu under Tools | MSC.Fatigue (for Patran) or under Tools | Fatigue Utilities (for Pre & Post).
From the low damage removal form:
1. Select the Type (either Group or Material).
2. Select either the material names or group names that are of interest.
3. Select the loadcases.
4. Select the percentage of loaded entities desired. The default value is 10 but you can select a value anywhere from 1 to 20. (i.e., If you select 15 then the top 15 percent of damaged entities will be added to the new group)
5. Hit Apply. The results data for each selected material name or group name is processed and the top requested percent of elements with the worst damage are put into a group using the following naming convention: HD_material name or HD_group name. (ie. If you selected mat1.1 and mat1.2 then two new groups would be created. One called HD_mat1.1 and the other called HD_mat1.2)
6. These new groups can then be used in the Materials Information form to quickly identify the “Fatigue hot-spots” in the Model.
Calculate Stress Gradients
If fatigue calculations are made based on either local elastic stresses calculated from FE, or based on nominal stresses and Kt values, over conservative life predictions may result. This is particularly a problem with many engine and powertrain components where combinations of sharp stress concentrations, small fillet radii and notch-insensitive cast materials can lead to the effect being quite large. The stress gradient correction adopted in MSC.Fatigue is based on a method described in the FKM Guideline "Analytical Strength Assessment of Components in Mechanical Engineering" 5th edition, 2003, English version, Tr. E. Haibach published by VDMA, Frankfurt. ISBN 3-8163-0425-7. This method, which considers only normal cases, shear cases, and positive stress gradients, is an endurance limit approach. It does not allow corrections at shorter lifetimes or specify how it might be applied to a general multiaxial case.
In MSC.Fatigue we are effectively applying the same factor to the strength at all lifetimes. This means predictions at shorter lifetimes may still be somewhat conservative, but not as conservative as predictions made with no stress gradient correction.With the application targeted for such components, the stress gradient correction has only been implemented for solid element FE models and users should not use this for shell element models.
As an example, we will here calculate the stress gradients on a cantilever beam, imported from the Nastran results output file, chex.op2 (located in the mscfatigue_files/examples folder under the MSC.Fatigue Installation directory).
Open a new database and import the results from the chex.op2 file (Analysis>access results> read output2>both).
From Tools>MSC.Fatigue>Fatigue Pre-Processing> Calculate Stress Gradients, bring up the interface for calculating gradients
Pick the default_group, click on Select All LoadCases, and Hit Apply. A SG_Default_group_skin and 2 results load cases corresponding to the selected load cases are created. The results load cases are labeled SG_Bend, Static Subcase and SG_Pull, Static Subase. Click on Cancel to exit this interface.
The create group function has created 2 results load cases on group, SG_default_group_skin This group consists of surface skin elements on which the surface stresses and the calculated gradients can be displayed. The plots of the Von Mises surface stresses and Gradients for SG_Bend case on the SG_default_group_skin are shown below.
Plotting the stress gradients and the surface stresses is useful in ensuring that the calculated gradients (since this is a regular results load case, all components may be viewed separately) and the surface stresses make sense. It can also help isolate problematic areas in the model (e.g. abrupt gradient changes) and help the analyst understand load paths in the structure.
On the MSC.Fatigue Main Interface, set:
Analysis to S-N
Ensure Res. Units are set to PSI
Enter gradient_vv as Jobname
Press the Solution Params button to open the Solution Parameters form.
Set Mean Stress Correction to None
Select Use Stress Gradient
Gradient Res. Units should show inches - if not, select inches
Click OK to close the form
Press the Loading Info button to open the Loading Information form.
Select the cell under Load Case ID
Click the Get/Filter Results button
Select the All Results Cases toggle
Click Apply.
Select the SG_BEND loadcase, from the list box
Select the cell under Time History
Select SINE01.DAC from the "Select a Time History" spreadsheet
Click OK.
Click the Material Info button to open the Material Information form. On the form:
Select the cell under Material
Select 2014_HV_0 from the Select a Material list box
Select SG_Default_group_skin for Region
Ensure layer 2 is filled in the layer cell
Accept Defaults for the remaining cells
Click OK.
Click the Job Control button to open the Job Control form.
Set Action to Full Analysis and click Apply
Set Action to Monitor Job and click Apply to check the status of the job. When the job is complete, click Cancel to close down the Job Control form
Press the Import Fatigue Results button to open the Results form.
Click Apply (Ignore any warning message).
Click Cancel to close the MSC.Fatigue Results form.
Go to the Main menu bar and select the "Results" toggle switch. On the form that appears:
Set Action to Create
Set Object to Quick Plot
Select Total Life, gradient_vvfef from the "Select Result Cases" list box
Select Damage from the "Select Fringe Results" list box
Click Apply. The maximum damage should be 1.08-05 at Node 1
Close Results and return to the Main MSC.Fatigue form.
Note: If the same fatigue job is run without stress gradients, a 29% over conservative estimate of the damage is obtained at the critical location (Node 1).
