Trouble Transferring Temperatures from a Thermal Solutions

markhollymarkholly
This is my first time running a thermal mechanical analysis. I run lots of conventional stress analysis. Model is a stack of a complex structural inner skin, lots of insulation then a thin external skin. I ran a thermal steady state model and got an excellent temperature distribution that makes intuitive sense as I interrogate the data. Now I want to run the thermally induced stress analysis. When I try to "Transfer temperatures from solution" or try a work around by creating a Table with node temperatures and the apply those as "node temperatures" I get the same error . . . "Some node numbers are not in the mesh"

I compared the number of nodes in the temperature table to those in the input deck via spreadsheet. Identical.

Any thoughts appreciated.

PS I did look at discussions in the Forum to see if there were any issues similar to this. Many thanks.

Comments

  • disladisla
    edited January 2022
    Hi,

    You probably have some shell or beam element in your model.
    If yes, add a modify Keyword *NODE FILE --->OUTPUT 2D.

    Then proceed as normal. I have tried with creating a table, copy into notepad to remove the spaces, and paste it back to mecway. Worked fine.

    NOTE: Ccx expand shells and beams to solids creating new nodes. There are more in the solution than in the model. With Output 2D you calculate the solution on the model nodes.

    EDIT: Transfer temperatures from solution also works straight through. I didn't know this option . Nice

  • prop_designprop_design
    one note about output=2d though. the stress is not useful to gauge safety. it's far from what you get doing something more accurate. the problem with ccx is you are forced to use output=2d sometimes. due to the node expansion. it's a real headache from a user perspective. this is just how ccx was designed. until the author does something different, you may be out of luck for certain analyses.
  • markhollymarkholly
    Thanks, I will look into that. There shouldn't be any shells in the final model but I did start out with shells which were extruded into solids. There might be some strays embedded.
  • disladisla
    You could also use the Deleted unused nodes in Mesh tools.
  • markhollymarkholly
    So I have gone through the input deck trying to hunt down any shells. None were there. I then tried the *NODE FILE modification. This did not do it.

    Then I had been playing with the ability to group the constraints so thermals & mechanicals could be separately suppressed or activated in one shot. AFTER SUPPRESSING THE MECHANICALS, I COULD TRANSFER NODE TEMPERATURES FROM A SOLUTION. So sorry, I did not realize the support constraints for stress analysis interfered with the thermal analysis, maybe this will help someone else.

    The Groups are a really neat feature.

    Thanks to the FORUM!
  • VictorVictor
    Mechanical constraints shouldn't interfere with a thermal analysis. But some of them, such as node-surface coupling and pre-tension section generate extra nodes which would cause that node count mismatch problem.

    Could you tell me what mechanical constraints you have in case there's an unknown bug here?
  • markhollymarkholly
    I guess it was the node-surface coupling.

    Thanks
Sign In or Register to comment.

Howdy, Stranger!

It looks like you're new here. If you want to get involved, click one of these buttons!

Sign In Register