Convergence in Elastic-Plastic Analysis 2

[Mm.Kaiser]

Hi,
I decided to perform an E-P analysis according to the ASME VIII-2 part5 criteria so i checked 2 ways to assign a characters to the material:

1-Usign a Non-linear material of ANSYS which used bi-linear isotropic hardening and tangent modulus of 1.45Gpa for structural steel. in this situation, the problem converged easily although it pressurized 2.4*design pressure according to ASME.
2-For more accuracy, Calculating Stress-strain data (True curve) according to VIII-2 Annex 3-D and putting those data in Multilinear isotropic hardening properties of a material. in this situation, the problem couldn't converge although i didn't assign a load factor of 2.4 to it!!

What is the root of my problem? i think it's because of the lack of my knowledge about mulitiliear isotropic hardening.
So each advice will be appreciated.
Regards

 

[TGS4]

Please share your miso input, as well as the material young's modulus, engineering yield and engineering ultimate. A no-linear curve is completely inappropriate.

 

[Mm.Kaiser]

Your answer was as brief as it can so i couldn't understand well what do you mean in "A no-linear curve is completely inappropriate."!
You can see material characteristics in the following:

(A694-F65)
bi-linear isotropic hardening:
Sy=450mpa Su=530mpa E=200gpa Tangent modulus=1.45gpa
Multilinear isotropic hardening:
As you can see in attached image according to VIII-2 Annex 3-D and also Ramberg-Osgood formula (True stress-strain curve):

Thanks a lot

 

[TGS4]

The brief response is that I was responding on my phone - and issues with auto-correct.

Your curve looks absolutely nothing like mine when I run the Annex 3-D calculations.

I obtain a true UTS (sigma_uts,y) of 580.241 MPa, which is where your curve should truncate, and become perfectly-plastic (the coincident true plastic strain is 0.09057, and the coincident true total strain is 0.09347).

sigma_uts,t=sigma_uts*e^m2.

In your case, m2=0.6(1-R), where R=sigma_ys/sigma_uts=450/530=0.849, and therefore, m2=0.091. Furthermore, your curve appears to veer from the elastic slope MUCH too early. I calculate a proportional limit (based on a plastic strain of 1e-6) at 344MPa. Yours starts to deviate around 250MPa.

Are you actually implementing the Annex 3-D calculation?

What I meant to say in my first response is that a bi-linear curve is completely inappropriate, because it doesn't truncate at the true ultimate stress/strain and become perfectly plastic. That is not permitted - see

When using this material model, the hardening behavior shall be included up to the true ultimate stress and perfect plasticity behavior (i.e. the slope of the stress-strain curves is zero) beyond this limit.

This likely has nothing to do with how you implemented the miso curve, and everything to do with how you calculated the curve itself. Re-do the calc ad bring it back here for checking.verification.

 

[Mm.Kaiser]

Finally i could
Thanks a lot TGS4 for your complete answer.
I found the problem in my formulations and now, i can reach exactly to your mentioned value which you can find in the excell attached file.
you are always a troubleshooter for me.

Just one vital question remains to close this document:
According to VIII-2 5.2.4 (E-P analysis), I have generated my FE model with mesh refinement in discontinuities and fillets, adding mulitilinear characteristics of material, Loading according to load cases, and turning on the large deformation. all-over? if the solution converged, it means that the part can tolerate the loads? no need to perform an elastic analysis with stress linearization?

Kind Regards

 

[TGS4]

The answer to your question is found in 5.2.4.4, Step 5

Perform an elastic-plastic analysis for each of the load cases defined in Step 4. If convergence is achieved, the component is stable under the applied loads for this load case. Otherwise, the component configuration (i.e. thickness) shall be modified or applied loads reduced and the analysis repeated. Note that if the applied loading results in a compressive stress field within the component, buckling may occur, and an evaluation in accordance with paragraph 5.4 may be required.

There is absolutely no need to do an elastic analysis - an elastic-plastic analysis is supposed to be better. HOWEVER, remember to check the other failure modes.

Your curves look OK. Just remember that, when you input them into your FEA program, that you have a perfectly plastic tail on the end.

 

[Mm.Kaiser]

That's OK. I god it.
Ansys automaticaly after σ_uts,t point, cheange the curve to the perfectly plastic mode with tangent modulus=0.