Hello Expert, i have two questions, 1) I have two parallel meshes of unequal size, can i define thermal coupling between them, if i can is it a good practice to define thermal coupling between fine mesh and coarse mesh 2) this time i have two perpendicular meshes without shared nodes (as there is no need of thermal coupling if shared node exist), can i define thermal coupling between them, as i read in NX help that thermal coupling is for parallel meshes, if not please suggest me how to proceed for perpendicular meshes without shared nodes please help me, Thank you, Dev.
Yes you can couple meshes of different size and topology. Depending on the accuracy required it's recommended that the mesh size difference does not exceed a factor of 3x or 4x. Even if it is more than 3x or 4x, you can simply make it more accurate by changing the Thermal coupling “resolution” which will affect runtime but can be made very accurate even for mesh size difference higher than 3x or 4x.
The second question relates to Edge Contact capabilities in thermal coupling. The Thermal Coupling dialog has a Magnitude, Type menu. Define the type as Edge Contact for the perpendicular shell meshes example.
If the thermal contact boundary condition is available in the solution using a standard SIM/FEM setup, then it should be available for the same type of solution using a SIM/AFEM setup. You can define boundary conditions that rely on geometry from different AFEM components. For example I've defined surface-surface contact and surface-surface glue for NX Nastran statics and normal modes solutions using AFEM models. This has been the case since the introduction of AFEM.
I'd have to review the specifics of your problem/model to understand why you are having an issue. One item to watch out for is the context of your Selection Scope on the Selection Toolbar. If the Selection Scope is set to Within Work Part Only, then you will be unable to select items contained in the FEM components. When defining your boundary conditions, make sure the Selection Scope is set to Entire Assembly. This confuses people (including myself) once in a while.
It looks like NX doesn't support thermal contact for ANSYS. I tried it in a standard SIM/FEM in NX 8.0.1. There's no option to create a contact when an ANSYS thermal solution is active. It is available with an ANSYS structural solution. I don't know if it would be possible to piece together a thermal input file with a structural input file (containing just the contact definition) and additional deck editing to get the thermal contact in your models. I've not tried this before with ANSYS.
So, I think you have a valid enhancement request here that should be sent to GTAC.
I have filed the request myself, or through Christophe Vandevelde (Belgian CAE representative). I got confused when I read the thread that thermal contact was possible. In the meantime we found two work arounds:
1. Put all parts in one assembly and create one mesh using MMC's
2. Perform the thermal analysis in Nastran environment using .fem and .afem and import the thermal temperatures into the Ansys structural solution.