Stress Error Plot - What are the units? 2

[stanm]

Can anyone explain to me the basis of the stress error when plotted using the ERR option.

Specifically, is this reporting the error in the energy norm or a more tangible error such as actual "stress" or a percentage error?

I can't find anything in the user manual that explains this.

 

[EngAddict]

It is a percentage, start here:

http://help.solidworks.com/2010/Eng...sisBackground/StaticAnalysis/Stress_Error.htm

 

[stanm]

Thanks EngAddict, that is aan excellent resource. Now, how do we consider the % error in the error norm to calculate possible maximum stresses?

 

[Elabbasi]

This error measure should not be used to calculate maximum stresses but to check if you mesh is fine enough for the results to be reasonable accurate. If the error is high, especially in areas of high stress, then you need to rerun the analysis with a finer mesh and recheck the error.


Nagi Elabbasi

http://www.veryst.com

 

[stanm]

Elabbasi how would you define a 'high' error?

 

[Elabbasi]

I wish there was a simple practical answer! I sometimes use 2% sometimes 10%. It is much better however to rely on a mesh convergence study (solve with different mesh densities) and look at the difference in maximum stress, or any other quantity of interest, between mesh densities. For example, if Mesh 3 is double Mesh 2 which is double Mesh 1, then ideally, the difference between Mesh 3 and Mesh 2 should be small, say 2%, and it should be smaller than the difference between Mesh 2 and Mesh 1.

It is important to remember also that even a mesh convergence study only shows that you are converging to the exact solution of your FE model. If the boundary conditions, loads, material model or properties do not match the physical model then it creates a false sense of confidence in the results!

Nagi Elabbasi

http://www.veryst.com

 

[stanm]

There is always a simple practical answer. I don't subscribe to the notion that design by analysis methods must involve any black art/touchy feely/mumbo jumbo techniques. From what you suggest I think that the ERR option is somewhat redundant. Mesh convergence is the tried and tested method. I am, however, more intrigued by other software that appears to offer lower and upper bound estimates as a result of error estimation.

 

[Elabbasi]

Yes the simple practical answer is to not use ERR to estimate what is the maximum stress, but do mesh refinement instead. It would be intriguing if a software offered good bounds based on an error estimate. However, I doubt that very much.

Here is for example a warning from the Abaqus manual against just that:

"Warning: Error indicator output variables are approximate and do not represent an accurate or conservative estimate of your solution error. The quality of an error indicator can be particularly poor if your mesh is coarse. The error indicator quality improves as you refine the mesh; however, you should never interpret these variables as indicating what the value of a solution variable would be upon further refinement of the mesh"

Here is also a link to a good but older paper about error estimation using ANSYS:

http://www.ansys.com/events/proceedings/2004/PAPERS/54.PDF

There is no black art/touchy feely whatever involved in good error estimation (it is a little subjective though). It's a complex topic that is still the subject of research in academia and commercial simulation software.

Nagi Elabbasi

http://www.veryst.com

 

[EngAddict]

I agree error estimate is not an absolute sign of convergence and it should always be done manually. You can use it to guide your mesh refinement on the fly but there will always be some areas, such as discontinuities and abrupt changes in thickness, that will indicate high errors but don't require further refinement. I always refine my mesh and plot stress, and repeat until the stress converges. If you do it as you go and enter the data into excel, it doesn't actually take any longer to achieve. Plus I like to control where my mesh is fine and where it is coarse instead of use adaptive methods, which also use error principles to refine the mesh, often inaccurately.

 

[stanm]

I think this has drifted slightly off topic. I am not looking to justify single run + error = accurate solution.

If the solution, to the problem on which you are working, is to be compared to a limiting stress then would it not be a reasonable approach to use the error estimation to estimate an upper bound stress value to ensure that the acceptance criteria is still satisfied. In suggesting this I am making the assumption that convergence has been demonstrated, mesh refinement is adequate and that the 'error' is 'low'. The solution will never be 100% accurate. If you have a number of stress categories to which stress limits apply then it seems logical, as a final operation, to quantify the maximum predicted stress. This would be particularly relevant where the predicted stresses are close to the stress limits.

I am also considering other software, such as Ansys, that can report upper bound values.

 

[Elabbasi]

That is a good idea. For a 'good' solution, you compare the limit stress to an upper bound stress obtained from the maximum stress and the error estimate.

Nagi Elabbasi

http://www.veryst.com