Learning Forum

[Sebastien Klein]

Hello,

I want to perform a thermomechanical analysis on a model with shell elements. The heat transfer analysis is doing well, I have activated the beta option with thermal variation in the shells. Then I go to the mechanical analysis, I use the import load feature to import the temperature from the heat transfer, but the import does not work, and temperatures applied make no sense (like 1e308 degrees applied on all nodes). 

I use ansys v2020 R2. Should any option be activated when temperature variation is accounted for in the shells ?

Thank you for your answers.

[Chandra Sekaran]

As you point out layered thermal shell is a beta feature. The main issue is that when you have only have one layer TEMP is the dof name. When you have more than one layer (shell131/132) the DOF names change to TBOT, TE1, TE2,..,TTOP. Mapping these DOFs to the corresponding layers in a structural analysis as temperature load is not supported yet.  

[mjmiddle]

 

There is a way to map temperatures to the structural analysis if you accept a linear temperature gradient across the thickness. If the mesh is the same in the thermal and structural analysis (Model cells linked) you can use LDREAD in a command snippet. Or use User Defined Results (UDR) in the thermal system for TBOT and TTOP, and export the data. Then use an “External Data” system to import that data, and you can select top and bottom separately for the two imported temperature loads. Note that beta options must be on as well as the Mechanical beta option “Allow thermal variation along shell thickness.”

 

[Sebastien Klein]

Hello all,

thank you very much for your replies. Indeed it works with the ldread command. I also found out that it works if I use the "Painted shell option". Do you know what is the difference between "Painted shell linear variation" and "linear variation" options ?

Now I also have another issue: in my model I have tubes modelled with shell131. On the outer face of the tubes I would like to account for radiation with ambient, and on the inner face of the tube I have surface to surface radation. But Ansys does not allow to have two different radiation load on the same shell element. Do you know a solution for that issue ?