Learning Forum

[Matthew_1]

Hello everybody!

I have a question regarding the Multilinear Isotropic hardening in Ansys, more specifically the mismatch between the input material stress strain curve and generated curve in Ansys.

I have created a simple 2D model (plane stress), which is supported on the left side (fixed support). Load is added on the right side in a negative Y direction. I used second order hex mesh and applied local sizing to the edge where the stresses are the highest.

[Sean Harvey]

Hello,nPlease watch this video which I created to address the typical issues with mismatch. Further questions, please reply back.nnThank younSeann

[Matthew_1]

Hello Sean,nThank you for the response. I’ve actually watched your video before posting this question and followed you tips (fine mesh, large deflections ON, plotting unaveraged max values, auto time stepping with minimum number of substeps set to 200) but still doesn’t work. I have also added a command ERESX, NO, which copies the integration point results to the nodes.nIf I add more points in the Multilinear Isotropic Hardening table between 0 and 0.0007 plastic strain the result is the same.  But if I chance the table tonit works fine. It seems that the solver can match the curves if the there is a “big” change in the slope between the elastic and the plastic part of stress strain curve. But if the plastic data in the Multilinear Isotropic Hardening is set in a way that the slope in the beginning of strain hardening is similar to the slope of elastic modulus the solver cannot match the curves.nn

[Sean Harvey]

Hello Matthew,nOK thanks for accepting my suggestion to watch the video. I will try out using the material data you provide to try and reproduce and get back. Thank you.nRegards,nSeann

[Sean Harvey]

Hello Matthew,nI ran with your material data and the blue data points are Ansys output and orange are the input curve and it matches exactly. nCan you plot your Ansys results data against the material curve that I am using. I think I see the problem. Seems you are not increasing the elastic strain and keeping as constant from the value of strain at 345 MPa. This is common mistake. You see I have .0032 total strain at 405 and you have something less. The elastic strain does not stop building with increased stress. nElastic strain = true stress/E for this uniaxial test. nnThis video does a great job on the topic and highlights this common mistake.nLet us know how this goes.nThanksnSeann

[Matthew_1]

Hello Sean, nnsorry for late response. You are absolutely correct, I have incorrectly calculated the elastic strain. Like you mentioned, I kept it constant, but in really it is increasing. nWhen I plot the points from Ansys to your table, in which the strains are calculated correctly, both curves match exactly.nnThank you for helping me!nnBest regards,nMatthewn

[Sean Harvey]

Hi Matthew, Awesome. You are welcome!nnRegards,nSeann