Thermal-Stress Analysis Procedure 1

[grnlan03]

I have been attempting to do a sequentially coupled thermal-stress analysis and I keep running into problems with the thermal data transferring from the thermal analysis to the mechanical analysis. This is procedure I am doing right now.

1. Run heat transfer analysis

2. Copy model and delete heat transfer step and use the same mesh for the stress model. Then create a stress analysis step.

3. Apply the temperature data to the stress analysis model using a predefined field.

Is this the correct way to do this or should I be using some other procedure such as defineing all the steps in one model?
Thanks

 

[corus]

If it's a transient then I make the stress analysis have the same time interval as the thermal analysis, though I believe that's not necessary as the temperatures will be loaded pro-rata. You have to make sure that the initial time step is sufficiently small, however, so that the change in temperature with time is captured and any change in material properties (such as phase change in steel) is also captured. Otherwise it'll just jump to the end of the transient. If it's steady state though, ignore the above.

corus

 

[grnlan03]

The model is set at steady-state. Does the procedure I wrote above seem like the best way to do a sequentially coupled thermal-stress analysis?

 

[corus]

You can't do it in one model as it would mean changing the element type. There might be a way round that but it's not worth the effort. I usually use the same .cae file, redefine the step to static, general, and redefine the loads/displacements etc. to that of a stress run. You can just modify the element type in the mesh module, or redfine the mesh and specify the mesh isn't compatible. It's best to save the temperatures in the output so you can check that the temperatures you've input are those that were shown in the heat transfer analysis as it has happenened that the temperatures have been allocated wrongly. You can usually spot that error though as the stress distribution will be just weird.

corus

 

[kag50]

I've decided to use a sequentially coupled thermal-stress analysis for my model. I was able to successfully replicate the heat transfer analysis part of the model. I'm having a problem when I try to run the stress analysis using the nodal temperatures as a predefined field. Here is what I'm doing:

Using the same model that I used for the heat transfer analysis, I delete the heat transfer step and create a static, general step with the same time increments as the heat transfer model.

I apply the appropriate load and boundary conditions.

For the predefined field, I selected the temperature distribution "from results or output database file". Then I selected the .odb file from the heat transfer analysis. There are other options for Begin Step, Begin increment, End step, End Increment. I left all of these blank because I wasn't sure what to put there.

For the mesh, I keep the same mesh that was used in the heat transfer analysis; however, the element was changed to the one that you used in your report.

I run the analysis using a different job than what was used in the heat transfer analysis and I get an error that says this:

*TEMPERATURE MAY NOT BE USED WITH ELEMENTS THAT POSSESS TEMPERATURE DEGREES OF FREEDOM. USE *BOUNDARY TO PRESCRIBE BOUNDARY CONDITIONS ON TEMPERATURE

I've tried to use temperature boundary conditions and I still get the same error message.

Did you run across anything similar to this when you were developing your model? I really appreciate your help!!

 

[corus]

You might have some elements that you haven't changed to stress elements in one part or another. You can check in the .odb file by using the display group and selecting that element set that is in error.
Check the .sta file for the end increment value. If you only have one step then bstep=1, binc=1, estep=1 and einc will be however many increments it took.

Tata