Convergence results analysis

Hello everyone.

I have the simple model with weld seam. So, my goal is to know the max stress in the place of concentration.

I use convergence to figure out how small mesh should be to get accurate result of the stress in that place.

I have set 5 % allowable change and 10 refinement loops. After 10 loops i got the following results.

The maximum stres incrised significantly from 557 MPa to 9800 MPa and allowable change of 5% hasn't reached yet.

How can this results might be assesed?

Is it possible that the Ansys can't calculate the mesh properly to get 5% change?


  • Gary_SGary_S Forum Coordinator

    Results for derived quantities (Equivalent Stress) are very difficult to converge on. The automatic mesh refinement tools are not always practical in this case.

    We have many good discussions about this already on the forum. Search for "convergence refinement riser".

  • peteroznewmanpeteroznewman Member
    edited September 25


    Remove the automatic mesh refinement from the model.

    Consider converting this model to a 2D Plane Strain model, that way, you can get a lot of small elements around the "crack tip" using a Sphere of Influence Mesh Sizing control.

    Add Plasticity to the material model. The simplest one to add is Bilinear Kinematic Hardening. Enter the Yield Strength and set the Tangent Modulus to 0. Check that the Units for Yield Strength are correct when you type in the value.

    Now the highest stress in the model will be limited to the Yield Stress.

    The interesting output is how much of the weld bead has gone plastic and what is the Maximum value of Total Equivalent Strain which includes plastic strain.

    Elongation at Break is a material property, like Yield Strength or UTS. Elongation at Break is compared with the Total Equivalent Strain to decide if the material has failed at that point in the model.

  • Thank you Peter. I will try to do it.

Sign In or Register to comment.