Applying temperature gradient on structural solid 2

[bojun2]

Hi,
I am trying to apply a temperature gradient on a structural solid. Is this possible? It appears that you can only apply a temperature gradient with a thermal solid.

I am trying to apply 10 degrees at the top surface, with a linear temperature gradient with 0 degrees at the bottom surface.

What is the best way to do this?
thank you

 

[vikiso]

You have to perform your thermal analysis first with the thermal solid (by switching your structural solid to a thermal solid). Once the steady state analysis is complete, switch your solid back to a structural element. Then, to apply the thermal gradient to your structural element, you use the LDREAD command to read in the thermal gradient from the thermal results. The thermal analysis results are written to a .rst file or .rth file in your working directory; so, you would for example type in LDREAD,temp,,,,thermal,rth to read in the temperature results applied as a body load in the structural model. From there, you restrain your model and perform a static analysis.

 

[bojun2]

Hi,
Thank you for responding. I am still having one problem. When I run the thermal analysis as a thermal solid, how do I restrain the beam? The options to restrain the DOF is not available for a thermal solid. When I try to run the analysis for a thermal solid, it refuses to run because the beam is not restrained.

Also, if I want to apply just a temperature gradient with ten degrees on the top and zero degrees on the bottom, do I use a heat flux? convection?

thanks

 

[elogesh]

Hai,

I need few information for answering your questions.

Whether you want to carryout the deformation analysis of structures based on the

1) temperature input specified in the structural analysis

or

2) Solving the thermal domain in order to obtain the temperature distribution.Later using these temperature as loading values in structural analysis.

I am assuming that your proceeding with step2.In that case for no need to specify the displacement boundary condition for thermal analysis. The boundary conditions specified for thermal analysis are not enough to solve the thermal problem.You relook at your thermal boundary condition values.Eventhough the problem is with thermal B.C, the error appears indicating problem in displacement.

E.Logesh

 

[bojun2]

I think I am trying to do your choice number 1.

I am trying to carry out the deformation analysis based on the temperature input. However, I need to do deformation analysis based on temperature only, but eventually I need to apply structural loads on the beam as well.

I need to find out what the deformation of the beam is from applying a temperature gradient (linear) with 10 degrees at the top and 0 degrees at the bottom. However when I try to use the temperature gradient, it doesn't seem compatible with the structural analysis to do deformation analysis.

I hope this makes sense.
thanks

 

[vikiso]

When you are completing a thermal analysis in the thermal solver, your boundary conditions are the temperatures at the surface, i.e., you should apply->temperature->on nodes (or areas) at the two ends of your model, 0 at one end and the other temperature at the other end. These temps will be your thermal "restraints". Then solve the steady-state analysis (linear). From the solution, you do as I mentioned in my previous reply by using the LDREAD command. When you run the static analysis in the structural model, remember to switch your elements back to structural solid and to restrain your structural boundary condtions.

 

[elogesh]

Hai,

For your problem,it is better to follow number 2.

Vikiso has already better explained the procedure.You have mentioned that you want to apply a temperature gradient in structural analysis.But in structural analysis for thermal loading you need temperature for each and every element.You specified the tempearure at the two ends.But in structural analysis,you wouldn't get the temperature distribution.You have to carryout thermal analysis to determine the temperature distribution.

If throughout the structure if you want to apply the same temperature,then straightaway you can proceed with structural analysis.

Regards,
Logesh.E

 

[bojun2]

Thank You very much. Your responses have helped me greatly, I have finally figured it out. Thank you, I would not have figured it out if it wasn't for your responses. Reading the .rth file from the thermal analysis into the structural analysis worked.
Thank You