Multi-Axial Fatigue Analysis - Life Contour Convergence

[Ruwan.B]

Hi all

I am performing a multi-axial fatigue analysis on a simple (enough) shaft. The specifications I am using are as follows:

Uts = 650 MPa

Yield = 310 MPa

Surface Finish = Machined

Radius = 1.6mm

Applied Load = -8300 N (Y direction)
Kf = 2.146

Kt = 2.20

Su = 553.662 MPa

Se = 217.976 MPa

N0 = 1000 cycles

B (S-N Curve slope) = 0.1349

Stress Bending (Calculated) = 200.627 MPa

Cycles to Fatigue (Calculated) = 1.853e6

When performing the analysis the deflection and von Mises stress match up to what I calculate. The issue is I have noticed that the life contour seems to be extremely sensitive to the mesh density. So much so that a slight change in the element size (0.182 to 0.181) can in effect produce a difference of 3e6 cycles.

This makes it difficult to achieve convergence w.r.t the life contour. If anyone can help me with a solution to achieve convergence on the life contour I would really appreciate it. I have worked through "Durability 101: Don't get tired of Fatigue rev_3" form @John_Holtz to try and see if there is anything regarding convergence but could not find anything.

Using Inventor Nastran 2023

Please see attached files.

[John_Holtz]

Hi @Ruwan.B 

There is no input in the Inventor file for the analysis, so it is hard to know what is going on.  

The question is this: does the stress result converge to a consistent value when you change the mesh? To quantify this better, you need to edit the stress contour plot and set "Contour Options > Contour Type" to "Elemental" and check the box for "No Averaging". If the unsmoothed stresses are changing with the mesh size, then the calculated life will change. (The life is calculated from the unsmoothed stresses, and then the life is smoothed. The average stress may not change much, but the unsmoothed stress can change more. Since the life is based on a log calculation, the smoothed life can change more than the smoothed stress.)

In other word, the shape of the elements can create some "hot spots" in the unsmoothed stress results that may not be apparent in the smoothed stress result. The hot spots become more apparent in the fatigue life.

If you still have questions, please confirm the model includes the Nastran input. Then attach the .ipt file again.

John

[Ruwan.B]

Hi @John_Holtz 

Thank you for reaching out and assisting in my issue.

I have uploaded the model with the Nastran input.

So if I understand this correctly, the life is calculated from the von Mises stress (as my fatigue set-up was set to von Mises) which includes additional effects to that of pure calculated bending stress (differing geometry as so forth).

The singularities or "hotspots" being more apparent in fatigue life makes sense.

I basically just want to make sure I am on the right track with a multi-axial fatigue analysis and knowing when to stop refining the mesh in the fillet to achieve convergence (say after 3-5 iterations)

(Please let me know if my model uploaded correctly with the Nastran inputs. I have also included the custom BS 070M55 normalized material I created for this analysis_.nasmat file)

[John_Holtz · Accepted solution]

Hi @Ruwan.B 

The model came through successfully. Thanks.

I think the variation in stress is the real underlying issue, but the following may be a better way to explain the variation in the life. See the figure below and note the following:

• You would expect the life to be smoother around the circumference than it is.
• The gradient moving away from the peak line is very high. In one direction ("up" in the figure), the life changes from red (shorter life) to blue (infinite life) in one element! In the other direction ("lower left"), the life changes over 1 or 2 elements. If the mesh is slightly different and moved in either direction up or down, the calculate life can be much different due to that high gradient.

It makes sense to do a mesh convergence study for the fatigue life, but I have not encountered the question before. Just based on the variation that I see, it may be better to do some type of manual calculation to get an average value. Either

• Calculate an average life based on N number of nodes in the region of high stress.
• Or, calculate an average stress based on N nodes in the region of high stress, then calculate the fatigue life. (This will probably converge more easily.)

That is, the single point with the minimum life is too sensitive to the position of the node and calculated stress. You want to average the result over a small region to smooth out the single point with the maximum. If you want to do some type of manual calculation, one thing that would help would be to split the fillet so that there is an edge in the CAD model around the circumference along the plane of maximum stress. (Similar to how you split the shaft to apply the load.) That way, there will be nodes at a consistent location x coordinate through the region of max stress (even through the nodes will vary in the circumferential direction which should be less of a factor).

John

[Ruwan.B]

Hi @John_Holtz 

Splitting the fillet and doing average calculations are doing the trick!

Thank you very much