Non-linear analysis-Permenant Deformation 6

[elogesh]

Hai,

I have a doubt regarding non-linear analysis.

When I started to work in FEM, I begined with linear static structural analysis.Then I understood the concerns about stress singularity in the sharp re-entrant corners due to the absence of filleted regions,mainly for simplifying the geometry.This simplification resulted in better overall economy.

After getting confidence in linear analysis, I started working on non-linear analysis.I use ANSYS-Multiphysics, General purpose finite element package for both the linear as well as non-linear analysis.The package has good material constitutive model for representing the non-linear materials.

I have taken simple structure with fillets removed subjected to pressure load(Bending problem). Then used material models with following properties to define both linear as well as non-linear region(Elasto-plastic analysis).The linear region is defined by young's modulus and poisson's ratio. The non-linear region defined by Tangent modulus and yield strength. I have used Iso-tropic hardening(Without bauschinger effect).The material is steel.

Applied pressure load, stress the few regions beyond the yield strength and the stiffnes in those regions changed to tangent modulus.But the issue is there are few regions in structure having stress singularity. Therefore those singularity regions reachs the stress values above the yield strength and hence Modulus changes from E to Et.But in realistic the stresses at the singularity regions may be less due to the presence of fillets.
I have few ideas running in mind to tackle this singularity, meanwhile I want to know,how usualy people used to deal with material non-linearity(Elasto-plastic) with stress singularity? Can you share your experiences in this regard?

The objective in this analysis is to findout the permeanent deformation after the removal of load.

Looking forward for your comments/suggestions/feed backs.

If there is anything technically wrong,please correct me.

Thanks for spending your time in reading this thread.

With advanced Thanks and Regards,
Logesh.E

 

[idly123]

Greetings

I have limited idea . I belive this would work.

Alternative 1)

AT renterant corners u need to adpatively refine your mesh either follow a h-refinement or a p-refinement so thatu reach a reasonably corect solution for stress. since wwe cannot find the error in computed solution at stress sigular regions we go in to define the "Norm " of computed error in displecemnts or "energy Norm" of the computed errror in stresses . and the H- refinement /p-refinemnt is dependent on these norm values obtained for each element.
Ansys has the capability of computing the energy norm and therey by u can have a plot of variation of error with h or pre finement (plotted ona log scale)..this would be a piece wise linear curve indiacting the rate of convergence of your solution at stress singular regions,
For more details refer to ansys user manual. Refer to Zeinkiwcz and ZHu FE book Vol1 chapter 13. or FE procedures by BAThe.

Alternative 2)
STress singulaity can occur at a crack tip in an isotrpoic material or due to delamination in a layered composite . IN such cases we can also go in for a "singularity Element" ( like an 8 noded iso rectangle) and position the midside nodes and write the shape functions such that at some point along the element edge at midside node u get asingular value.MAy be iam not very clear in writing it ( More of this is very clearly given in The book by RD Cook and others).

Hope this helps in a general understanding although the answer is not specific to your question.
regards
Raj

 

[idly123]

Please see the following thread on "corner stresses"
thread727-46576
It might help you.
regds Raj

 

[brad]

In general stress singularity is not as big of an issue when you have nonlinear material.

Further, if your main goal is to determine amount of permanent deformation, this displacement should converge fairly readily with increasing mesh size (even though the peak stress does not), although in the case of pure plasticity this may be more difficult.

It's a fairly elaborate explanation as to why this is; I would encourage you to try this on your model and confirm my statement.

BTW--Dr. Raj--P-element is irrelevant for this problem, as p-element formulation is limited to linear elasticity.

Brad

 

[corus]

Stress concentrations in a structure are unlikely to cause permanent deformation but only localised yielding. Using elastic-plastic properties to capture the post yield beahviour at these points isn't really worth it unless you are actually modelling the correct geometry as the results will be meaningless. Depending on the size of the irregularity the results away from that region will remain unaffected by that feature and you can use sub-modelling to capture the true plastic strain there if you want. The effect of a fillet will be to stiffen up the corner and remove the singularity of the corner. This could, in some instances, affect the overall displacement of the structure if the fillet is big enough. You would then have to refine your mesh towards the fillet region.

 

[EdR]

elogesh:

First...I assume by stress singularity you mean the stresses are becomming very large....certainly larger than the yield value...If this is true then your problem lies in one of two areas:

1. Material model is incorrectly defined or is not computing correct values.

2. Load step is too large.

My guess is #2...You have applied such a large load step that the material model is unable to correct itself...

In any case you should not see stresses that are (significantly) larger than the yield stress if the model is working correctly....and they should tend toward the yield values...

Hope this helps

Ed.R.

P.S. Using this type of model may give significantly different values for the permanent deformation than you would get from a plasticity model that uses a flow rule....

 

[elogesh]

Hai,

Thanks to bradh,corus,Edr and raj.

Bradh:
I will try your suggestion of increasing mesh size and its effect on displacement converegnce. If I get encouraging results, I will definitely share those in this forum.

Regards,
Logesh.E

 

[paitoon]

To elogesh
i think you shoud control the boundary condition because the right boudary condition will lead you to the right solution. you should also think about geometry nonlinear and material nonlinear.And the convergence relate to mesh size and quality of mesh.
best regard
paitoon

 

[elogesh]

Hai,

Bradh: -

You are correct.Displacements converged fairly well with increasing mesh size.

Recently I read an article about stress singularity .Few quotes of it I had it below,

"You can avoid stress singularity by using different material model,for example elasto-plastic model instead of linear elastic material. The elastic-plastic material model will put a upper bound on stress,and instead of producing meaningless high stress, a plasticity zone would be formed".

Regards,
Logesh.E

 

[idly123]

If u are using an Hierarchial estimator u can go in for p refinement
raj

Raj

 

[jetmaker]

elogesh,

Here is a suggestion. If the reentrant corner is not one that will affect your overall deformation behaviour, then switch the properties of the elements around there back to linear-elastic properties. This way, once the load comes off, they return to zero stress. If the region is important for the results, then suggest adding in the detail of the fillet to obtain proper behaviour.

Model simplification is great if you have limited resources, but keep in mind that any simplification you conduct must not alter the actual behaviour of the model.

Good hunting.