Continue to Site

Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

Pro/Mechanica Material Nonlinear Analysis

John_Leahey

New member
Pro/Mechanica Material Nonlinear Analysis - Forcing with Restarts


A colleague is interested in attempting a material nonlinear analysis in Pro/Mechanica. Since there isn't currently the ability to perform this analysis in Pro/Mechanica, his idea was to force the analysis by editing a Prestress Static analysis. Currently, Pro/Mechanica allows a user to run a static analysis and use the results as a starting point for a second static analysis (i.e. prestiffened structure has a new set of loads applied in the "Prestress Static" analysis). My colleague's idea is to somehow edit the results of the Prestress Static analysis and make Pro/Mechanica think it is actually the results of a static analysis thus allowing for multiple iterations of a prestress static analysis.


Has anyone been able to force a material nonlinear analysis in Pro/Mechanica with restarting an edited Prestress Static analysis? Are there any other ideas for accomplishing a material non-linear analysis in Pro/Mechanica?


Thanks for the help.


Regards,


John Leahey
 
I think you are wasting your time. Invest in some non-linear software like Ansys if you are interested in such analyses. How can you guarantee your results will be accurate? Non-linear methods often take thousands if not millions of calculation steps to achieve the results. In any case I'm not sure that you would be able to store all the data by manually using the results of one analysis as the start conditions for another.


Phil
 
John,

I have used the "Secant Modulus" to perform some approximate/ballpark Nonlinear Material Analyses in Mechanica:

PROCESS

A. Run Mechanica to determine the Strain
B. Determine the new Secant Modulus from the Strain results
C. Re-run Mechanica with the new Secant Modulus
D. Repeat until results converge

DETAILS ON HOW TO AUTOMATE CONVERGENCE

1. In Excel, create a spreadsheet of Stress VS Strain data of the material
2. Create a column for Secant Modulus (i.e. Stress / Strain)
3. Use the LOOKUP(X,Y) functionality in Excel so you can input a Strain and Excel will "Lookup" the corresponding Secant Modulus
4. In Mechanica, create a Measure to calculate strain in the characteristic direction that will dictate the behavior of the structure (e.g. STRAIN_XX)
5. In Pro/E, create a real number Parameter (e.g. FEA_STRAIN_GUESS) and assign it any temporary value (e.g. 1)
6. In Pro/E, create a Excel Analysis Feature that will use Pro/E Parameter FEA_STRAIN_GUESS and output a Parameter FEA_MODULUS_EXCEL
7. In Mechanica, create a Material Definition using the Parameter FEA_MODULUS_EXCEL as Young's Modulus of Elasticity
8. In Pro/E, create a Mechanica Analysis Feature that creates a Parameter MECHANICA_STRAIN_XX from Mechanica Measure STRAIN_XX
9. In Pro/E, create a Relation that sets FEA_STRAIN_GUESS equal to MECHANICA_STRAIN_XX
10. In Pro/E, create a few columns in the Model Tree to monitor the values of the Parameters
11. In Pro/E, hit Regenerate a few times until the Parameters converge

Thanks,
Ray Miya.
 
The "non-linear" analysis that is advertised in the link that was provided by "muadib3d" is not "material" non-linearity. It lists "geometric" non-linearity - this must not be confused with material non-linearity. This capability will model things like fishing poles under load which produce a very large deformation globally, but not locally. Mechanica does not yet have any material non-linaearity capability. Currently Mechanica handles contact non-linearity and geometric non-linearity.


Kaz Z06
 
so Kaz - taking advantage of Your knowledge - in which cases this capabilities(Adv Pro\M) is usefull?
 

Sponsor

Articles From 3DCAD World

Back
Top