Fatigue Vibration with Fe-Safe

In summary, the student is trying to use Fe-Safe to fatigue analyse harmonic and PSD vibrations. They need to create two files with Modal participation factors and a steady state dynamic analysis. They also need to be sure that the modal participation factors for each node are matched to steps in Abaqus, plus the frequency interval for which output is requested for each step is identical.f
  • #1
Hello everybody ,

I am student in mechanical enginnering. I have to evaluate the solution Fe-Safe.
i am working on two subjects: Harmonic and PSD Vibrations.

The modal analysis are done in Abaqus. I would like to understand how Fe-Safe computes Life Fatigue in case of harmonic analysis. What Fe-Safe needs to calculate the life cycle.
i would like to have some tutorials in vibration analysis(harmonic/PSD). i can't find anything about Fe-Safe on the internet.

I will be grateful for any help you can provide.


Last edited by a moderator:
  • #2
I am currently interested in this subject as well. I will possibly using FE Safe in conjunction with the Abaqus CAE solver in the near future. I understand that the standard method to solve random vibration in the FEA world would be by using Miners rule and the cumulative damage model in order to sum the effects of the vibration. FE safe is using the power spectral density function in order to solve the random vibration in frequency domain. I am yet to completely understand exactly how this works but I do have a few resources that I am working through. Once I gain an understanding I may share.

If you can find SAE paper 14m-0324 it is on random vibration fatigue. I have a file but I cannot find it on the net. You may have to buy it. See video below.

  • #3

I started working in Harmonic analysis using Fe-Safe. my FE model (abaqus) contains 4 steps :
  1. the first contains modal step to compute the natural frequencies
  2. the 2,3,4 step; it is a steady state dynamics steps (harmonic)
From Fe-Safe Documentation, to perfom a fatigue analysis for Harmonic and PSD analysis, we use PSD analysis, and fot that you need 3 files:

.odb file with natural frequencies
.odb file with Modal Participation factors
.psd the PSD matrix.

so i run firstly the modal step,then afte, I make a restart to compute the steady state dynamics response from the modal results. to obtain two files .odb
-Modal.odb : Natural frequencies
-Harmo.odb=GU: Generalized displacements and GPU Phase angle of generalized displacements for all modes.


Please, can you help me to create the second file .odb which contains only the Modal participation factors (GU, GPU)?

Thanks in advance.


Error Messages:




  • upload_2015-1-6_11-43-57.png
    57.8 KB · Views: 710
  • #4

I have the exact same problem. I also dont't know how to make Steady State Analysis correctly for import for fe-safe PSD Fatigue analysis. When I try to open all required files, I always get ".odb has an invalid extension (it should be mcf)" Have you made any progress since? If you have, could you please tell me how to create second odb. file?

Thanks in advance.
  • #5
Here is an e-seminar for fe-safe's PSD capability. I do not think it will help with the specific problem ou are experiencing, but it may be of interest:


Looking at the help manual for fe-safe 6.15-02, two .odb files are required.

1. Modal stresses need to be calculated using a natural frequency extraction analysis. The Abaqus specific modal participation factors should be created.
2. Once 1 is complete you need to run a steady state dynamic analysis to generate a set of displacement related results.

The manual warns to be sure that modal participation factor for each node are matched to steps in Abaqus, plus the frequency interval for which output is requested for each step is identical.
  • #6
...talking to someone more familiar with the PSD analysis, it sounds like Nesho and salwacheg are both in situations where they are using Abaqus (odb) but fe-safe is expecting ANSYS. You need to play around in the PSD Open Model Dialog to be sure that the filetype is set to "odb".
  • #7
I had a little breaktrough today... for the second ODB file, you have to make "Steady-State Dynamics, Modal" analysis, and under "History Output Request" you have to add "GU, Generalized Displacements" and "GPU, Phase Angle of generalized displacements". Then fe-safe recognizes second ODB file correctly and and it doesn't show "...odb has an invalid extension (it should be mcf)" anymore.

Thanks for the suggestions anyway
  • Like
Likes nikaa

Suggested for: Fatigue Vibration with Fe-Safe