Convergence in Elastic-Plastic Analysis
Convergence in Elastic-Plastic Analysis
(OP)
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
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





RE: Convergence in Elastic-Plastic Analysis
RE: Convergence in Elastic-Plastic Analysis
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
RE: Convergence in Elastic-Plastic Analysis
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
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.
RE: Convergence in Elastic-Plastic Analysis
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
RE: Convergence in Elastic-Plastic Analysis
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.
RE: Convergence in Elastic-Plastic Analysis
Ansys automaticaly after σuts,t point, cheange the curve to the perfectly plastic mode with tangent modulus=0.