validating simulation results 1

[akpalican]

I have read a couple of articles where it advises to validate the FEA results by creating a finer and finer mesh to see if the stress increases. However, those articles didn't specify the magnitude of a stress increase that would indicate that the stress is "false" (i.e. caused by a discontinuity). So, my questions are 1.) is this a good approach for validating FEA results - other than hand calculations 2.) if so, what is the increase in magnitude of stress to look for?
Thanks in advance!

 

[testing]

I generally think of verification and validation of two similar, but distinct checks. Verification would be your usual mesh convergence, comparison between different codes sort of thing. Basically, is the answer I'm getting the answer I expect to get based on best practices and other simulations or hand calcs. Validation in my mind is whether the answer matches to what it should physically, ie, to experimental data.

For mesh convergence, this seems to be a good overview:

http://knowledge.autodesk.com/suppo...ow-to-Perform-a-Mesh-Convergence-Study-s.html

 

[TheTick]

Singularities are more likely if the mesh is too coarse.

As mentioned above, auto-refinement goes a long way to getting an accurate result. Ultimately, you need to keep refining until the results stabilize.

 

[academix]

Hello:

Typically, for establishing convergence in stresses, the mesh refinement between two runs can be compared, at the same location (not the legend value). If the value of the stresses under study, differ by less than 2%, at the same location, then the results can be taken as converged.

Alternately, the plot of the Strain Energy Error Norm would give you a normalized plot between element centroidal stress and nodal averaged stress. A monochromatic plot would reflect convergence. Remember, the error norm plot is NOT a measure of error in FE computations.

If you are looking at real-world validation, then the measured data should have a minimum of atleast 8 data points for the same location. Remember, FEA is a deterministic approach, while measurements are leaning towards probabilistic approach (each measurement using the same apparatus, loading, boundary conditions on the same sample gives different result, right?) with a requirement to understand the nature and mechanism of variation as evident in Nature.

Best regards
Nat


Natarajan Ramamoorthy
Design Engineering Consultant

http://www.egsindia.com

 

[lmrg5387]

Hello,

I am analysis the stresses on this component. How can I interpret the high concentration in the fillet? How would be a good explanation of why it happens?

 

[mmar2087]

lmrg5387:
First you need to understand if it is "real" stress or singularity. Convergence methods are given above.
If it is "real" stress, it converges, you just have to consider if it is a problem or not in your design.

Do this stress peak go beyond yield in your simulation? Then if you do a simple static linear analysis you know that the values presented in SW are not correct.
To get a more accurate result you need non-linear simulation where you have the S-S curve of the material.
You will then find that the stress in this area is much lower. Probably somewhere between yield and UTS.

In reality you will have local yielding. That means that the stiffness in this highly localised area is reduced.
Force follow stiffness, so the flow of force will be relocated around this less stiff area and increase the load in the surrounding area.
And thats it. Nothing more happens. If you are below UTS.

However, if you have a cycling loadcase, this area could fail from fatigue, so in that case you should consider to redesign to reduce stress below yield.