Mechanica versus real life results

[AntonyRobinson]

Does anyone know of a website where I can details of real life objects being stressed?

I would like to remodel them in ProE and compare the results from Mechanica, just to build up some confidence.

 

[corus]

The simplest way is to compare results with analytical solutions, such as those given in Roark & Young - Formulas fro stress and strain. I have seen a comparison of ProMechnica with other FE software

http://www.ddicad.com/Products/Analysis/FEATools-AnalysisDocument.pdf

and the results aren't that brilliant from what I can see.

corus

 

[prost]

The document FEATools-AnalysisDocument.pdf was certainly interesting and very informative. Four FEA tools were investigated: COSMOSWorks, ANSYS, NEI/NASTRAN and Pro/Mechanica (interesting choice, the last one, since my readings on eng-tips and other places indicates to me that they have almost stopped developing this software. Much better choice would have been StressCheck, IMO). Could someone who uses one or all of the first 3 (all h-element FEA codes) tell me exactly what the phrase "...were converged over multiple iterations" means? If you download this PDF, this snippet is in the Plastic Toy example. As I am not a user of these first 3 codes, I am left at guessing what kind of iterating is occurring, and why. Is an 'iteration' in this context a variation in the mesh (say mesh refinement)? Or is it an iteration because of material nonlinearities? My last guess is that is it an iteration because the stiffness matrix is so large and sparse that the solver needs to iterate on the inversion process to arrive at a stable, converged solution. Does someone care to tackle this one?

 

[corus]

Cosmosworks uses an iterative solver, however as it's plastic I guess it might be material non-linearity.

corus

 

[prost]

The problem was "Plastic Gun" though I don't think there was enough information to determine whether the material constitutive relationship was elastic plastic or something else. The author indicated the E and PR, but nothing about yield, suggesting that though the name of the structure is "Plastic Gun" that this is not modeled with a plastic constitutive relation. The E and PR might be ok for a polymer that is small strain/small displacement, that is, Hooke's Law applies.

If the Plastic Gun is modeled as a linear elastic (Hooke's Law that is) material, and the term "iteration" just means the iterative solver needed to invert the really large, sparse matrix, then IMO the author is using the wrong metric to determine how good a particular FEA tool is relative to the other FEA tools.

The author computes the average max displacement (or some other engineering quantity) computed for all 4 FEA codes. This is his metric--the FEA tool that gave him a computed max. displacement closest to this average max. displacement for all 4 codes is what he calls 'the best'.

He has not indicated that he has obtained proper numerical convergence of each of the models (the extension process for FEA is well established; by extension I mean start with a sparse mesh with few degrees of freedom (DOFs), compute the solution, increase the DOFs dramatically, compute another solution, compute a 3rd solution with a really large number of DOFs; compare these 3 solutions and check for convergence with an extrapolation technique such as Richardson's). Because he has not indicated this, the reader is left to assume that he has not obtained numerical convergence; therefore it is impossible to say that any of these FEA solutions means anything; how can you trust any of these solutions if the analyst hasn't obtained numerical convergence? How does the reader of this analyses know that this is the best solution that can be obtained with each FEA tool? For instance, what if the COSMOSWorks, ANSYS and NEI/NASTRAN solutions are numerically converged by chance (the analyst just overdid the number of elements in each model, so that there are say 10 times as many elements as needed), BUT did not have enough elements and DOFs in the Pro/MECHANICA solution to make certain it was numerically converged? Then this would be an unfair comparison of Pro/MECHANICA to the other FEA tools. But there is no indication of DOFs or elements or polynomial level in the elements, so it is impossible to tell even that the comparisons are fair.

Until the analyst/author obtains numerical convergence with each of the 4 FEA tools, then the comparison between the 4 tools is meaningless. If the analyst did obtain numerical convergence using each FEA tool, and the 4 FEA tools don't produce results within say 1% of each other, than there may be problems with the analyses themselves. If the structural geometry, loads and boundary constraints are the same, then the results should not be mesh dependent (or for that matter, FEA tool dependent).

 

[corus]

The author does say that in some cases large displacement was used with contact. In both these cases an iterative solution is required, except for the case of ProMechanica with contact which doesn't update the solution. The author does say that exatly the same boundary conditions and geometry were used (presumably a comparatively similar, and reasonably fine, mesh density). To be fair he does conclude that an engineer would have come to the same conclusion with all 4 codes.

corus

 

[corus]

Revisiting the site, and looking at some of the mesh plots in the pictures it does appear that the fe mesh is more than adequate for the results that were obtained.

corus

 

[prost]

The mesh may appear to be more than adequate, but how do you know unless you check numerical convergence by extension of the degrees of freedom from a "low" number to a "high" number? Have you had a prior experience in which a mesh looked good but gave you poor results? If you have, then why aren't you routinely checking numerical convergence every time, in every model?

 

[corus]

You can't extend the degrees of freedom, there are only 3 dof in a 3D solid structural model. You can improve the mesh density, if that's what you mean, to improve the results. In most cases you don't need to check the convergence with mesh density as experience will tell you if the results are reasonably correct. In some cases verification of the results can be obtained by using simple hand calcs. If there is a particular area I'm concerned about then I'd use sub-modelling to improve the accuracy there. Experience tells me that the mesh they've used looks very good for the analyses they've carried out.
To get back to the subject, in real life you'd have a good model if the results are within 10% of measured results, better for thermal analyses. In part that can be due to the modelling assumptions made, or the accuracy of the measurements. Rarely can the error be attributable to the density of the mesh used, unless you've used a groasely coarse mesh.

corus

 

[AntonyRobinson]

Thanks for your replies but I feel that most of you are going off on tangents.

I know the limitations of mechanica & know that there is better software out there. I havn't looked at Roarks for a number of years now, am I correct in assuming that it will only really contains simple closed form examples?

What I'm interested in is actual test on proper parts that I could have a go at modelling and then analyse in Mechanica.

I teach Pro/E & mechanica to customers and it would be nice to back up what I say to them about their results with more confidence. I think it would be useful for the students aswell.

I normally explain to them that Mechanica is best used as part of the design process, earlier the better, before the models get too complicated.

Most of our customers are not really interested in what happens to their materials in the plastic region.

 

[prost]

The problem is then of understanding the phrase "extension
of the degrees of freedom" which has nothing to do with
increasing the number of possible degrees of freedom at
a particular node. Extending the degrees of freedom means
increasing the number of elements to h-element FE code users; it means increasing the polynomial degree to p=element
FE code users.

 

[corus]

I'd look at Roark and perhaps Peterson's book on Stress Concentration factors. Roark contains some complicated examples and, if my memory serves me well, solutions that were obtained from measurement.

Measured results are always open to interpretation, even in simple cases. People have posted questions on this site regarding results they've obtained from just bending a beam which they can't get to agree with analytical solutions, for various reasons.

corus

 

[JacobL]

Having used MSC/NASTRAN and other MSC products, I'm very disappointed to see that they aren't included in the test.
For genral testing for collision, simple stress tests with isotropic materials and using basic constraints, you can use COSMOS, ProMechanica and other cad-integrated software.
For using anything more serious - contact, springs, non isotropic materials, composites and so forth, a dedicated piece of software has to be used.
Every problem has it's own software - for instance, for contact non linear solutions, there is MSC/MARC, and it does things that NASTRAN can't, as well as DYTRAN (for high velocity high displacement).

So, in general, if you want to compare to real life results, check that the software you are using is the right one, see the the problem is well defined, and in most cases, you'll get the close-to-reality results, more likely to be on the conservative side.

The only exception is CFD - here it's totaly dependant on the code, and you can VERY easily get "garbage-in garbage-out", so be careful.

Jake.