Transient Thermal and Residual (transient structural) Analysis of Dental Model.

Hi everyone!

I get a problem with finding the residual stress after doing transient thermal analysis of the dental model. Transient thermal analysis is okey but residual stress analysis (transient structural) that depends on transient thermal analysis has errors. The model was converted on Ansys APDL ( converted .cdb format). The external model was applied in Ansys mechanical and geometry was defined. Mesh was attached on the model in ansys apdl so that I cant repair it on ansys mechanical. The program has given some errors and warnings during finding the residual stresses. How can I find the residual stresses on the model?


  • @SercanKumru

    I recommend you connect the Transient Thermal to a Static Structural. You don't need Transient Structural because the inertia forces will be insignificant.

    In Static Structural, you must add a support or it will not solve. You could use a Remote Displacement and pick the the face on the inside of the crown. In the properties of the Remote Displacement, set all six constraints to 0, three displacements and three rotations. Most importantly, you must set the Behavior to Deformable. You must not leave the Behavior set to Rigid because that will add stiffness to the model that you do not want.

  • The model exists two part, the first is porcelain veneer and the other one is Ni-Cr metallic veneer. Which can I carry it out on model's face?

  • Thank you so much mr.peter

    I achived the residual stresses on the model. But I think some problems are exist. The maximum and minimum stress values between the model are so much. Are there some problems about mechanical properties of the model? Is it possible? But I think that I entered the correct values to the system.

  • @SercanKumru

    The mesh used was very coarse. You should do a mesh refinement study where you reduce the element size and plot how the maximum stress changes as the elements get smaller.

    It's possible to build geometry that has a sharp interior corner. The theoretical value of stress at that corner is infinity. This is called a singularity. A real corner has a small radius so the stress is finite. It is possible your geometry has a sharp corner and as you make the elements smaller and smaller, the stress will go higher and higher without limit. You would then need to edit the geometry to add a small radius.

    I suggest you build a very simple geometric model with two bodies that use these two materials. One idea is two spherical shells. Cut through the sphere on 3 planes of symmetry to hold 1/8 of the sphere using Symmetry boundary conditions. Apply a temperature load in a Static Structural analysis to see the stress from the thermal expansion. In this example, there are no stress concentrations, no singularities. You can do a mesh refinement study on this simple model to see how element size affects stress.

    If you clear the mesh from your model and save a Project Archive .wbpz file, then put that in a zip file and attach it to your reply, I will do this with your materials.

  • Hi Mr. Peter,

    first of all thank you so much for your interest. we tried u model by using it and the same mistakes have occured. but I realized that the stress values are closer each other when the time is changed on Analysis settings in static structural analysis. for example, the stress is about 60 Mpa at 20th s but at 5000th s, it is about 13000 Mpa. I didnt understand why it happens. And also we want to see that the stress values depend on the time. I guess It is not possible in static structural analysis so we wanted to try it in transient structural analysis.

    As you said, we wanted to changed mesh type (mesh refinement) but the file doesnt allow to us to reorganise. I will send you the analysis files if you accept it.

  • peteroznewmanpeteroznewman Member
    edited December 2020


    Thank you for the files. It is better to use File, Archive to put them into a single file, but I was able to open what you sent.

    You can read about a suggestion I made to @muge who is working with you on this in the other thread.

    I see why your model has unrealistically high values of stress, your Coefficient of Thermal Expansion is about 1 million times too big! Here is one reference for Ni-Cr.

    From that reference, the values of CTE are between 9e-6 and 16e-6 /degree C. You have used values between 13.7 to 17. Change that to 13.7e-6 and 17e-6 /C. Once the CTE is set to the correct values, your stress will be greatly reduced.

    Another observation is that in the Transient Thermal, you have added Convection, but chosen 2 Bodies. That doesn't seem right because not every face on each body can convect heat to the air, the outer face of the porcelain is in contact with the inner face of the Ni-Cr crown, so they can only conduct heat between them. I think you should only select faces that touch air.

  • Hello Mr. @peteroznewman

    You are right. We overlooked the CTE values. We adjusted the CTE values. We want to do a transient structural analysis to see the stress that corresponds to every 10 seconds. While we have reached correct results in static structural analysis, we have not reached correct results in transient structural analysis yet. Why might we not find the same results?

    And we want the part to cool in the suspended structure. Since we could not intervene in the meshes, we could not select a point, we defined it with remote displacement. When we select the remote displacement under the part or on the inner surface, we encounter stress values ​​in different regions. On which surface should we apply remote displacement?

    Best Regards,


  • @muge @SercanKumru

    I recommend picking a small face that is not near the high stress area. Maybe on the inside?

Sign In or Register to comment.