Convergence issues (force converges, but moment don't)

[hmsantanna]

Hello sirs,

Maybe I can have some help on this issue...
I'm running na elastoplastic shell model, using large displacement effects.
This analysis is a plastic colapse analysis, so, the loads are magnified according to some API 579 (Fitness for service ) rules.
I have done this kind of analysis before, but now I'm having a problem I never had before: I getting an easy convergence on forces, but not at all moments converge.
I and other colleague have performed some checks, and everything looks ok (units, materials, mesh, etc).
As I told, it is a quadratic shell model (SHELL281), no contacts, internal pressure, self weight and hidrostatic pressure. I'm using an multilinear isotropic hardening material model, and large displacements.
Could anyone have a hint about why this moments are not converging???
Thanks a lot for any help!
Best regards



_______________________________
Hervandil Sant'Anna
Petrobras

 

[cvan42]

Hi Hervandil,
Have you tried the stabilize command? In 14.0+ it is an option in the Nonlinear Controls tab. Earlier versions you need a script STABILIZE, CONSTANT (OR REDUCE) ENERGY,1E-5,ANYTIME. In the results it's a good idea to compare stabilze energy to strain energy to make sure the stabilization is well under 1% of strain energy.

You might want to try an elastic support condition if it's allowed on surface- calculate the area of your scoping, multiply by the max displacement you expect (this give the mm^3), then mulitply by the force you'd want to apply for this condition (few grams, fraction of grams, milligrams,etc) Sometimes very small elastic supports help.

Also might want to figure out the natural frequency, select a time increment half or less of this value, and use transient instead of structural (if you're using staic structural)

Here's a list of the options and some scripting I researched a while back, hope these help.

!UNDER ANALYSIS TYPE BRANCH
STABILIZE,CONSTANT,ENERGY,1E-5,ANYTIME
!NROPT,UNSYM
!SOLCONTROL,1,1,,1E-2
CNCHECK,AUTO,ALL
NLGEOM,ON
PRED,ON
CUTCONTROL,PLSLIMIT,0.8
finish
/config,nres,10000 ! increases results set limit from 1000 to 10000
/solu




1. NLGEOM,ON (ELEMENT LARGE STRAIN ALLOWANCE)

2.CNCHECK,AUTO,ANY (RESETS OPTIMIZED CONTACT SETTINGS FOR ALL PAIRS FOR CONVERGENCE ISSUES)

3. STABILIZE COMMAND: STABILIZE,CONSTANT,ENERGY,1E-5,ANYTIME (MOVE TO 1E-4, 1E-3 ABSOLUTE HIGHEST TOLERANCE)

4. CUTCONTROL,PLSLIMIT,0.2 (NOTE 0.15 IS DEFAULT FOR STRAIN LIMIT)

5. PRED,ON (CONTACT SEARCH TIMESTEP PREDICTOR)

6. SOLCONTROL,1,1,,1.0E-3 (INCREASE VOLUMETRIC TOLERANCE)

7. NROPT,UNSYM (GO TO MORE INTENSIVE RAPHSON SOLVER TO AVOID SINGULARITIES)

8. ARCLEN,ON (RAPHSON REPLACMENT WITH ARC LENGTH METHOD)

 

[hmsantanna]

Dear cvan42,

Thanks for your reply. I had already tried the stabilization option, without any success.
But, while doing my reasearches, I figured out that I was having a numerical issue, named locking. The deformations were so high, that the elemento could not rotate, despite they could deformate. I could solve this by reducing the element polynomial order (to linear one), and improving the mesh in that site.
However, I still couldn't understand why the shell elements could not properly rotate.
Since this is a real industrial problem, I had a schedulle to accomplish, then I could not go really deep in this very interesting problem.
Best regards
Hervandil

_______________________________
Hervandil Sant'Anna
Petrobras

 

[cvan42]

Hervandil,
Thank you for the update. SHELL208 and 209 have only 3 DOF, but with SHELL181 and 281 you should have all 6 DOF. I'm guessing you have the 181 or 281, so it sounds like there is something else going on. My experience using shell to model large structures and frames is very low. My only other guess would be the material model parameters could be encouraging the locking due to all the data used to define it, like poisson's reaching near 0.5. I do remember trying to approximate a PTFE paste model and it would cause the locking until I changed the type of material model. It used shear and bulk modulus terms on top of density, posson's (0.49 was successful) and E. Does anyone else here know why there is locking going on?

 

[hmsantanna]

Hello,

So, as I told you before, the model is a large pressure vessel with a dent in a region, with pressure, hidrostatic pressur, wind and self-weight loads.
I use Workbench 14.5. This version uses by default element SHELL181. The pressure loads are applied through skin elements (SURF154, if I'm not wrong).
I'm using NLGEOM,ON and an multi-linear isotropic hardening steel model (data are based on MPC equations, similar to Ramberg-osgood model).
I'm figuring out if this locking could be related to this skin elements, but I'm almost sure that I'm not sure!!!! I didn't have time to test this model without using these skin elements to check if I'm right or wrong...
Anyway, it is a good problem to academics discover what goes wrong!
Thanks again, and best regards

_______________________________
Hervandil Sant'Anna
Petrobras