Comments

• Victor

  March 26

  Yes, beam elements work with thermal stress.
  
  Your screenshot shows analysis type is thermal, so change it to static which has displacement DOFs. That's also why many of the boundary conditions are shown in red, which means error (displacement constraints aren't valid for thermal analysis type).
• Sandrailstudent

  March 26

  Thank you for the response, Victor.
  
  I rebuilt the model out of shells, in case they are able to behave differently. I could not get the temperatures to drive displacements, which would then drive reaction forces. I exported the temperatures on all nodes, but it still did not produce displacements.
  
  Please advise if shells are able to produce thermal displacements, then please let me know. The model screenshot attached did not produce displacements.
  
  
  
  
  

  Screenshot 2026-03-25 231342.png 68.7K
• Victor

  March 26

  Yes, shells can too. Could you post the .liml file and I can identify all the problems.
  
  I notice there's no thermal stress item in Loads & Constraints. You need to include that when you do the static solve.
• Victor

  March 26

  I should also add that items displayed in red text in the outline tree have errors. To see what it is, right click it and pick What's wrong? Items with orange text are warnings which are also worth looking at if something's not working right.
• Tibor

  March 26

  Cool, Mecway for piping stress.. I need to try it 😀
• Sandrailstudent

  March 26

  Thanks Victor,
  
  I cannot get anything beyond temperature, heat flux, and contact from the thermal steady state solver. The model and some screen shots are attached.
  
  Thanks again in advance.
  
  
  
  
  
  
  Chris

  Crossover Shells.liml 22M
• Sergio

  March 26 edited March 26

  Change your analysis type to static 3d, unsuppress the frictionless suports, add a thermal stress bc, in the solution branch request displacements, stresses and reactions forces and solve again. Could you please upload/share the beam model and the reference results maybe?
  
  
  
  
  
  Bes regards
  
• Victor

  March 26

  I made 4 changes:
  - Set the analysis type to Static 3D.
  - Unsuppressed the mechanical constraints.
  - Added a thermal stress item. I chose 0°C as the Reference temperature so you might have to change that.
  - Added displacement and reaction force to the solution using the same menus you showed in your last post. They are no longer disabled since analysis type has been set to Static 3D where they're valid.
  
  
  
• Sandrailstudent

  March 26

  Sergio and Victor,
  
  THANK YOU BOTH SO MUCH FOR WEIGHING IN AND MAKING IT WORK!!!!!
  
  Per your request, the line model is attached. I have messed with this model quite a bit trying to get it to do what i wanted it to.
  
  The other thing that would seem to be really useful if i continue to use Mecway for pipe stress would be the ability to add a gap to a restraint. I could always figure out which way the node moves and force the elimination of the gap through a displacement, but it seems like a rough way to go for every guide. Thermal displacements on the shells obliviously worked, but line elements cannot do that.
  
  At some point i will probably get Ceasar II or similar pipe stress software, but so far i am really pleased with what Mecway is able to do, even with the corners that i had to cut like forced displacements on cold pipe (which added its own inaccuracies).
  
  Thanks again,
  
  Chris

  Inlet Terminal Guide Load Study_w_Crossover_simple displacements+restraint.liml 29K
• Victor

  March 29

  For the beam model, just add a thermal stress item and unsuppress the temperatures.
• Sandrailstudent

  April 7

  Thanks Victor. Those 2 little steps did it for me for the beam model.