Life results issue in fatigue analysis

[Anonymous]

Hi everyone,

I'm having some issues calculating life cycles in fatigue analysis. First of all, i've followed step by step the example of "Autodesk University Guide: Don´t get tired of fatigue". It says that: "The Life Contour result is a minimum of 61940 seconds", but when I run the analysis with the same instructions, the Life Contour minimum is 17533,195 seconds. I find that is a big difference and I don't know what's wrong. It would be helpful if there were some pictures in the Autodesk Guide. I'm inserting some pictures of the model and the parameters, maybe someone finds the mistake!

In addition, I've been testing other parts and models, with diferents types of loads, like axial load, but every Life results seems to be wrong comparing it with the hand calculations (I've followed in every case the Goodman modified method, using the book [Shigley] as reference). Between the hand calculations and the simulations Life I've found differences of 1000000 seconds. I'm starting to think that there is some issue in the configuration, but I don't know if I can change something. Any help would be appreciated!! 

Thank you, 

Ines

[John_Holtz]

Hi @Anonymous 

There are three things going on with that example:

1. The fatigue document from Autodesk University (AU) was created with In-CAD version 2017. That version of In-CAD output the fatigue results using the stress at the center of the elements, so it was difficult to compare the fatigue life with the stress shown (which by default is from the corner nodes). In version 2018, the fatigue life was changed to show the result based on the stress at the corner nodes. In the case of the shaft, the stress at the corner nodes is higher than the stress at the center of the element, so the fatigue life is lower.
2. The other difference is that the hand calculation is based only on the bending stress. The In-CAD result is based on the von Mises stress which includes the bending and shear stresses. Therefore, the von Mises stress is a little higher than the hand-calculated bending stress, and this leads to a lower fatigue life.
3. There are a few other subtle differences between the hand calculation and the simulation that I did not realize when I created the AU class. The main difference is the stress concentration factor used in the reference book was 1.55. (The reference was using a reduction in the stress concentration factor because "some materials are not fully sensitive to the presence of notches".) With the fillet modeled in the analysis, the stress concentration factor is closer to 1.69. This different results is a large difference in the calculated stress which results in a large difference in the fatigue life.

It was an unfortunate coincidence that the results from In-CAD 2017 "matched" the hand calculations as well as they did. Had I known recognized all of those subtleties at the time, I would have changed the hand calculations to be a better comparison to the analysis. @wasim_younis is re-writing the fatigue example for his book "Up and Running with Autodesk Inventor Nastran". Perhaps he can share what the "correct" hand calculation result is. 

With all of that in mind, the hand calculations will match the simulation results. As in this case, it is sometimes not so easy to make the analysis duplicate the hand calculations! (Or stated another way, the hand calculation of the fatigue life using the simulation stress results will match the simulation stress result.) 

[Anonymous]

Thank you so much for your fully explained answer @John_Holtz !

I still have some doubts about the S-N curve, let me know if I'm mistaken:

- B is the slope of the curve and the equation is: B=(log(Su)-log(Se)) / (log(Ne)-log(No))

If my No is 1000 and Ne is 1E+06, why the XY plot shows that the  Fatigue limit is reached at 3442 cycles  instead of 1E+06? (see picture)

- Su is the Ultimate tensile strength? or is it the Ultimate tensile strength corrected with the fatigue strength fraction?

- KF is the stress concentration factor but we don't use it because it's already "included" in the FEA analysis

-Se is the corrected endurance limit without the stress concentration factor as the Guide says? or is it the polished endurance limit?

If someone could attach to this post a solved model by fatigue analysis I would be grateful, because I'm still having trouble trying to figure out how to make the simulation results similar to the calculations and maybe I'm doing something wrong...

Thank you in advance!

Ines

[John_Holtz]

Hi @Anonymous 

• You are correct: the XY Plot of the fatigue material properties is incorrect.
• "Su" is the stress corresponding to the number of cycles No. Therefore, the input should be f*Su (where f is the fatigue strength fraction).
• Kf is left as 1 because the stress risers are included in the model.
• Se is the corrected endurance limit, not the polished endurance limit.

You have a solved example (the rotating shaft), but you did not provide the second most important thing in your original post: what was the calculated stress? If you use that stress value in the equation given in the hand calculation example (N=N0*(Su/Sa0)^(1/b)), how many cycles do you get? It should be close to the number of cycles obtained by In-CAD. (The published max principal stress is 374 MPa=Sa0. With N0=1000, Su=582, and b=0.1308, the life should be close to 29000 cycles. If you are getting different results, please attach your model and remind me what version of In-CAD you are using.)

The final reason that the hand calculation may not match In-CAD exactly is because In-CAD may be calculating the life due to each element attached to the node, and then displaying the average of all of those individual calculations. The hand calculation is using the average of all of the stresses in each element at the node, and calculating one life. The two methods are not the same mathematically but approach each other when the mesh is fine enough and the stress from one element to the adjacent element approach the same value.

[Anonymous]

Thank you for all your help @John_Holtz !!

I found out that I had selected the Maximum Principal method in the Fatigue Setup, but the Von Mises method fits better with my hand calculations, so the Life results provided by Nastran are much more similar now to the Life expected. The max principal stress I use is 334MPa, with Su=621MPa and B=0.168 it turns out to be N=4.01E4 cycles and my Nastran result is N=3.2E4 cycles. I'm using Nastran In-CAD 2019.

However, I have modelled another part to try applying multiple forces to the same Part, and if I apply 2 moments simultaneously (flexing and torsional) in the same section, it happens that the Life cycles are always 1E+10, and it doesn't matter the magnitud of the moments. I have appplied 441 N·m of flexing moment and 780 N·m of torsional moment and it is supposed to fail at 1.6E4 cycles. Maybe I'm applying the moments incorrectly, but i don't find any information about fatigue with moments applied. 

Sorry for having such a big amount of doubts, and thank you!

Ines

[John_Holtz]

What is the calculated stress (in your analysis) due to the moment loads?

[Anonymous]

In my hand calculations it should be: Sa=305,06 MPa and Sm=275,3 MPa but in the simulation there are no stresses (see picture).

I don't really know where I should apply the moments, I've applied them in the edge of the work plane, because i want them to be in the middle of the shaft.

[John_Holtz · Accepted solution]

According to the help documentation, you cannot apply a moment to an edge. You can only apply moments to a face of a solid. Therefore, you model has no load, so it has no stress, and the life with 0 stress is infinity.

You need to find an alternate way to apply the moment loads. I suggest using a linear static analysis to get the stresses to work before trying the fatigue analysis.

[Anonymous]

Thank you for all your advice @John_Holtz !!

After trying multiple configurations I found that the torsional moment only works with a Fixed constraint, so I split the shaft into halves and I applied a flexing moment to the surface of the shaft half near the constraint and the torsional moment to the surface of the free shaft half. 

Now I get a calculated life of 2,45E4 cycles and the Life result of the simulation is 1,759E4 cycles... I think that it's close enough. 

I would suggest to create more tutorials on how to use Nastran In-CAD for multi-axial fatigue, because in my opinion there is not enough documentation...

Thank you!

[Anonymous]

Why does the fatigue calculation only work with this ridiculous S-N curve then?