Heat Transfer problem between solid body and shell box

[nvvvnoliveira]

Hello

I am new to ABAQUS and I have to do a thermal simulation script in Python to observe the heat flux between a solid element and a shell box. I defined this case with a bodyheatflux assigned to the solid element and a surface film condition assigned to both solid and shell elements to account for convection within the system.

I am sending my python code attached.

I am getting errors/doubts and I would appreciate any help with it:

1) In mesh and I don't understand them because, from what I know, DS4 and DS3 mesh elements are assigned to shell parts. Anyway I was able to correct it using ABAQUS GUI but in code the error keeps on appearing.

2) Running the simulation, I can't observe heat flux along the shell box.

- Do you think that film conditions are well assigned for convection?
- Should I assign surface heat flux instead of body heat flux?
- Is it necessary to assign a predefined field to assign initial temperature?


The main objective here is to observe heat flux along the shell box and my problem is to assign interaction properties to the system in order to account for the heat flux from the solid body to the shell.

Thank you very much for your time

 

[FEA way]

The error that you get says that there are elements without temperature DOF in your heat transfer analysis. And that’s right because you have S4R and S3 elements in your model (you can check this easily using Query —> Mesh ok the assembly level).

It seems that this model has overlapping part instances and no connection between the inner box and outer shell walls.

 

[nvvvnoliveira]

Thank you again for your help.

I’ll review the code for mesh elements.

Regarding connection, if I define a tie constraint between shell box and solid element would it become the solution to have heat flux along shell walls?

Thank you

 

[FEA way]

You should still model the medium between those two parts since they are too far away from each other to use tie constraint or thermal contact. Unless you want to account for the surface to surface radiation but, from what you said before, it's not the case here.

 

[nvvvnoliveira]

Yes, that’s my problem. On how to model the medium between the two parts.

I’m really clueless about that, I searched for tutorials on how to do it but wasn’t able to find one.

Is it defined on the interactions module?

 

[FEA way]

As I've mentioned in the previous topic, you can model an additional solid part meshed with continuum diffusion heat transfer elements (DC3D) to represent the air or other fluid inside the box. This will account for conduction in stationary fluid.

 

[nvvvnoliveira]

So that could be a new shell box between the already defined shell box and the solid element? Does it have to be in a specific form?

Thank you for your help.

 

[FEA way]

Not shell, solid. In the shape of the space between the existing parts.

 

[nvvvnoliveira]

hello again,

I made changes in the model. Basically I have defined the whole volume inside the shell as a solid of the same dimensions of the shell and I have assigned a bodyheat flux to the solid.

How do I assign thermal contact between shell faces and the solid? it is a surface to surface condition?

Thank you again and sorry to bother again with this

 

[FEA way]

You can use either tie constraint (full heat flow without resistance) or thermal contact (possibility to define resistance but with very large value you will get non-obscured heat flow like with tie constraint). Both are defined in the Interaction module but the first one is a constraint type while the latter is defined as contact interaction with thermal contact property assigned. It would be best if you tried them on a simple test model first.

 

[nvvvnoliveira]

I did it with tie constraints and it seems better.

Can you please run my code attached to this comment please?

- Does the results for the last increment shown on the odb make sense to you? Do you think that heat is flowing along shell thickness?

- Do you think that a finer mesh will help with convergence of results?

Thank you very much again

 

[FEA way]

There are still overlapping and unmeshed parts in this model. The analysis doesn’t converge.

Before scripting this you should model it manually first and make sure that it works fine.

 

[nvvvnoliveira]

I have achieved convergence of the model. I deleted all unmeshed instances, added an offset to shell to avoid overlap and increased the number of increments for the transient thermal analysis.

It worked with tie constraints as you said.

Thank you very much for your help.