Predefined Field in Shells vs. Solids issue

[Alexander Koss]

Hello

Recently I have encountered a big issue with predefining a temperature field in my Model. I am working on a coupled temp-displacement simulation, with an already meshed model (orphan mesh). As it seems, whenever I create a predefined temperature field for the model, the solids act normally, the temperature is transferred from the initial to the thermal step. But with shells, they seem to always try and go back to temperature 0, causing significant strain in the model. What could be the issue here?

 

[FEA way]

Check msg and dat files for warnings. Which type of shell elements do you use and are there any boundary conditions applied to these shells ?

 

[Alexander Koss]

I looked into the msg and dat files, one thing in the dat file that seems suspicious is the following line:

*shellsection, elset=ASSEMBLY_ShellPart, temperature=2, material="HC340XD"
*solidsection, elset=ASSEMBLY_SolidPart, material="AlSi12Cu1"

This temperature=2, I never set any boundary condition regarding that. There is just 1 boundary condition, which fixes both shell and solid in place, and the predefined temperature field of T=10. Do you know by any chance where this "temperature=2" could come from? Keep in mind, this mesh was inherited from another model.

 

[FEA way]

This parameter indicates the number of equally spaced points through the thickness at which the initial temperature is defined.

Try defining initial temperature for shells this way:
- in the shell section editor leave default integration "During analysis" and temperature variation "Linear through thickness"
- in predefined field editor select "Direct specification" and "Constant through region"

 

[Alexander Koss]

Currently, that was my setting for the shells. Nevertheless, this issue remains.

 

[FEA way]

Could you attach the input file ? You can simplify it first leaving only the shells.

 

[Alexander Koss]

When I set the temperature to be 10, the solids keep it the way it is supposed to be. In the shells the temperature drops almost instantaneously, and settles at 0.8333 degrees. If I set it to -10, it settles at -0.8333. I can't really see the issue in the model definition though, it is the first time something like this happened.

 

[Alexander Koss]

Yeah, I will surely do that, thanks!

 

[FEA way]

What is the value of temperature for shells in 0 frame ? If it’s 10 and drops in subsequent frames then probably some kind of BC/interaction is unintentionally applied to the shells. If it’s lower than 10 in 0 frame already then something is wrong with the definition of initial conditions.

 

[Alexander Koss]

Sadly, I am not able to upload the input, since it contains some internal data. Do you have any other possible explanations for this issue?

 

[Alexander Koss]

In the 0 Frame all the temperatures are 10. Right after that it drops in the shells..

 

[FEA way]

Are there any interactions (like convection/radiation) defined in this model ?

 

[Alexander Koss]

For the sake of finding this issue, I tried deactivating all interactions. The weird behavior of shell elements remains the same, even when there are no interactions in the model. At the same time, solids would have probably had a similar issue, if interactions were to blame for the issue

 

[FEA way]

Can you paste just the *Initial conditions keyword here (with all parameters and data lines) ?

Try refining the mesh and increasing the number of integration points through thickness for shells.

 

[Mustaine3]

Instead of going back and forth it would make sense, that you reproduce the issue on a dummy model and attach that here.

 

[Alexander Koss]

I have changed the number of integration points. All that's changed is the temperature the shells sink to, now it's at around 0.4 degrees.
Here are the Initial conditions:

** Name: T0 Type: Temperature
*Initial Conditions, type=TEMPERATURE
TestSetAll, 10.

The set includes all Nodes in the solid and shell

 

[FEA way]

Try changing this keyword so that the value is specified for all integration points through thickness. For example if you have 5 points use:

*Initial Conditions, type=TEMPERATURE
TestSetAll, 10, 10, 10, 10, 10