Calculation of Safety Factor using Von Mises Failure Criterion

Anonymous

Calculation of Safety Factor using Von Mises Failure Criterion

Anonymous
Not applicable

I am currently running into an issue where the maximum Von Mises stress and the resulting safety factor at the same node do not match. I have read several forums where it is explained that the material yield stress is used for calculating safety factor, in my case I have set both the ultimate tensile and yield to 44ksi, as well as the failure theory to Von Mises under material properties. I am currently getting results of 16.9ksi as my maximum stress at a node, and the corresponding safety factor is 3.034. By calculating SF=(S_yield)/(S_max), I would expect a SF of 2.6.

Note that these results were obtained through a Linear Static analysis.

 

I additionally read that the safety factor is calculated as the average of the resultant safety factors of that node, however this seems like a considerable deviation form the expected value.

 

Any light you can shed on this would be greatly appreciated. 

0 Likes
Reply
Accepted solutions (1)
3,491 Views
3 Replies
Replies (3)

Roelof.Feijen
Advisor
Advisor

I can imagine that you are surprised about this. I honestly think that for now we have to deal with it. What you can do is vote for the idea of changing it. See link below
https://forums.autodesk.com/t5/nastran-in-cad-ideas/safety-factor-based-on-average-stress/idi-p/8232...

Roelof Feijen

If my post answers your question, please click the "Accept Solution" button. This helps everyone find answers more quickly!

John_Holtz
Autodesk Support
Autodesk Support
Accepted solution

Hi @Anonymous 

 

Your explanation is correct: the factor of safety (FOS) shown by In-CAD/Inventor Nastran is the average of the individual FOS calculated at each node in each element. A 15% difference (3.0/2.6) is not that significant in a simulation unless you have performed a mesh convergence study and gotten the stress results to a highly accurate result.

 

The stress is calculated at each node in each element based on the displacement of the nodes. Therefore, each node has multiple stress results, each calculated independently. In-CAD/Inventor Nastran shows the average stress at the nodes and does not have the feature to show the non-averaged results at the nodes. Simulation Mechanical does have the capability to show the non-averaged results, so I used Simulation Mechanical to create these figures. (The averaged stress and FOS results shown by In-CAD match the results of Sim Mech.)

stress - smooth.pngFigure 1: Averaged stress result = 5513 at node.

 

FOS - smooth.pngFigure 2: With an allowable of 10,000 the FOS (Factor of Safety) is expected to be 1.814 (=10000/5513), not 2.090. Where does 2.09 come from?


stress - unsmooth.png

Figure 3: The individual stress results when not averaged. Note the difference of maximum/minimum is a factor of 3.3!


FOS - unsmooth.png

Figure 4: The individual FOS results when not averaged. Each value is 10,000 divided by the individual stress results (and sorted). The average of 1.030, 1.645, 1.814, 1.954, 2.663, 3.436 is 2.090, and this matches the value shown by the software.

 

What type of elements are you using? It appears that shell elements use a different calculation. The FOS is based on the stress at the center of the elements instead of using the stress at the nodes. 

 

 

 

 

 



John Holtz, P.E.

Global Product Support
Autodesk, Inc.


If not provided already, be sure to indicate the version of Inventor Nastran you are using!

"The knowledge you seek is at knowledge.autodesk.com" - Confucius 😉

Anonymous
Not applicable

That is a really great explanation. Hopefully someone else can find this now and benefit, I spent several hours looking for this kind of info, to no avail. 

Thanks John!

 

 

0 Likes