General Mechanical

General Mechanical

Thermoelastic analysis of 2D plane strain cylinder

    • Md Ahad
      Subscriber

      I made a plane strain 2D cylinder model where i applied internal pressure but when i applied temperature at the internal edge then i got error. But i want to get the thermoelastic characteristics results. Here I am giving a snapshot and attaching my file too.

    • Sandeep Medikonda
      Ansys Employee

      Ahad,


        Can you click on 'Show Errors' button at the top and see what it says? Also, can you show the details of the temperature you have input?


      Regards,
      Sandeep


       

    • Md Ahad
      Subscriber

      Hi Sandeep,


      I have attached the archive file sothat you can see what is the problem. Ok i am gonna reply you with the details of the error. I had applied 1100 deg cel at the point A and 100 deg cel at the point B.


      Regards

    • Md Ahad
      Subscriber

      Sandeep


      please check the attached archive file.

    • Sandeep Medikonda
      Ansys Employee

      Ahad, I am not allowed to view ansys generated files hence the request for the pictures. If you can, please post pictures. If not, maybe peter or someone else from the community can help.

    • Md Ahad
      Subscriber

    • peteroznewman
      Subscriber

      Sandeep,


      I noticed that in a Steady State Thermal model of 2D geometry, Mechanical will not allow a Temperature BC to be applied to 2D Plane Strain Geometry, but it will allow a Temperature BC to be applied to 2D Plane Stress Geometry.  This is the "error" that is troubling Md Ahad, the ? on the Temperature BC. I don't know why Mechanical would allow one but not the other, perhaps you can explain it.


      If the temperature solution is to be used in a downstream Plane Strain model, the link must only be the SS Thermal Solution to the Static Structural Setup cell in order to have the freedom to have the SS Thermal model be Plane Stress while the Static Structural is configured to be Plane Strain. You can't have the Model cell link from Thermal to Structural because then you can't do a Plane Strain Static Structural solution. See the first few posts in this discussion.


      Regards,
      Peter


       

    • Sandeep Medikonda
      Ansys Employee

      Hi Peter, 


        Indeed, it is given in the manual that we only support plane stress and axi-symmetric behaviors only for 2D


        I can't think of a reason why this has to be limited though. I will talk to my colleagues and file an enhancement request with development as needed. 


      Regards,
      Sandeep

    • peteroznewman
      Subscriber

      Hi Sandeep,


      I think the reason you can't have a SS Thermal model with a 2D Plane Strain model is because in Plane Strain, the surface bodies have no thickness property, the depth is infinite, while in Plane Stress, the surface bodies do have a thickness property.


      In SS Thermal, you can apply a Heat Flux and a Heat Flow boundary condition. While Heat Flux is in the units of W/mm^2, the units of Heat Flow is W.  How many Watts does it take to heat an infinitely large area?  That is the problem and the reason why you are not permitted to have 2D Plane Strain in SS Thermal.


      Regards,
      Peter

    • Sandeep Medikonda
      Ansys Employee

      Hi Peter,


        Indeed, that is what I've been able to find out as well and was about to update here and then saw your post :-)


        Anyway, thanks for that.


      Regards,
      Sandeep

Viewing 9 reply threads
  • You must be logged in to reply to this topic.