Mismatch between the input material stress strain curve and generated curve in Ansys.

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.

For elastic material properties I have defined Young’s Modulus (160 000 MPa) and Poisson's Ration (0.33).  Yield point of the material is 410 MPa, at 0.002 plastic strain (determined with the offset method). The elastic limit is set at 345 MPa. For plasticity I have defined Multilinear Isotropic Hardening, where the first point in the table is the elastic limit at zero plastic strain. All points in the table taken from the true stress strain curve. Auto time stepping is turned ON (min 200 substeps), as well as large deflection.

With the load of 300 N, stresses in the magnified corner exceed the yield point. 

I have created a Named Selection on the node in the proximity of max stress and plotted max unaveraged Von-Mises stress versus max unaveraged total strain to create a stress-strain curve.  As you can see from the right graph, the stress strain curve from Ansys is not completely aligned with the material curve. In the elastic part (up to 345 MPa) the curves are completely aligned, but there is a deviation as soon as the plastic strain occurs. 

Eventually the curves realign, and if the stresses are well beyond yield this mismatch is not a problem. But I am interested in the region just below the yield, therefore this deviation is not acceptable, as the difference in stress, for example at 0.003 total strain, is around 20 MPa.

Can anybody help me how to resolve this issue?

Comments

  • sharveysharvey San Diego, CAMember

    Hello,

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


    Thank you

    Sean

  • Hello Sean,

    Thank 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.

    If 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 to

    it 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.

  • sharveysharvey San Diego, CAMember

    Hello Matthew,

    OK 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.

    Regards,

    Sean

  • sharveysharvey San Diego, CAMember

    Hello Matthew,

    I ran with your material data and the blue data points are Ansys output and orange are the input curve and it matches exactly.

    Can 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.

    Elastic strain = true stress/E for this uniaxial test.


    This video does a great job on the topic and highlights this common mistake.

    Let us know how this goes.

    Thanks

    Sean

  • Hello Sean, 


    sorry 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. 

    When I plot the points from Ansys to your table, in which the strains are calculated correctly, both curves match exactly.


    Thank you for helping me!


    Best regards,

    Matthew

  • sharveysharvey San Diego, CAMember

    Hi Matthew, Awesome. You are welcome!


    Regards,

    Sean

Sign In or Register to comment.