Weak Thermal-Mechanical Coupling

[gcassianno]

Hi,

I’m working with a quadratic mesh imported from Workbench into PyMAPDL using mapdl.input(). My goal is to perform a weakly coupled thermal-structural simulation. Here's my current approach:

Thermal step

1. Run the thermal simulation with the quadratic mesh.

2. Before solving, I remove midside nodes using:

   mapdl.esel('all')
   mapdl.modmsh('DETACH')
   mapdl.emid('REMOVE','all')

3. I solve the thermal step and save the results to a .rth file.

Structural step

1. Clear the database and reload the original input file (with contact definitions) using mapdl.input().

2. Change all element types to structural with mapdl.etchg, apply structural boundary conditions, and read the thermal results via:

   mapdl.ldread('TEMP', '', '', '', '', '', '', 'rth')

However, while the thermal results look fine, the displacement field from the structural simulation doesn't match the results in Workbench. I suspect the issue may be due to the contact definitions not being properly reestablished when the input file is loaded.

So I have a few specific questions:

• Is it possible to perform weak thermal-structural coupling in PyMAPDL starting from a Workbench-generated input file? Are there any recommended best practices for this approach?

• I also tried creating contact in MAPDL using GCGEN and GCDEF to build general contact definitions. However, is it necessary to explicitly reset the contact element KEYOPTs using the KEYOPT command when changing the simulation type? Or do the elements automatically adopt the correct settings when using mapdl.etchg?

• I'm a bit unclear about the purpose of the RMODIF and R commands. What parameters can these commands modify, and how do they interact with previously defined real constant sets?

Thank you in advance!

[germa89]

Hi @gcassianno

Regarding your questions:

1. As PyMAPDL just wraps MAPDL commands before send them to an MAPDL instance, it should be possible, since MAPDL is the solver behind Ansys Mechanical (Workbench).
2. From my understanding the configuration of the type of simulation (done with mapdl.antype) is independent of the type of elements (mapdl.et). Meaning that changing one or the other, does not change the other. However, the different elements in different simulation types gives different result types. Eg. some elements do not support harmonic analysis, etc.
3. R are like a set of constants used to help defining something else, for instance an element type or contact condition. In CONTACT174 it is used to set the contact control parameters. I would say that out of contact definition, it is not much used.

Regarding your issue about the displacements.

Which elements types are you using for both, structural and thermal analysis?

[gcassianno]

Hi @germa89, thanks for your reply.

I'm using element 90 for the thermal simulation, and with the mapdl.etchg command I get element 186, which I believe is consistent with the body load applied by ldread.

[germa89]

My guess is the forces stored are not applied to the model as expected. Have you tried to use KIMG = 1 in LDREAD so the forces are applied to the nodes as D?

[mikerife]

@germa89 no, reading temperatures from a rth file into a structural mesh will apply the temperatures as a body load. We don't want to apply them via D as temperature is not a degree of freedom in a (purely) structural mesh.

[germa89]

Ohh.. I see. Thank you Mike! :)

[mikerife]

Hi @gcassianno the ETCHG command only changes the element type and not any keyopts (or real constant, section definition etc) of the element. So you need to change the contact element keyopt so that the degrees-of-freedom are correct. I.E. after etchg of the thermal model the contact elements still have temp as a DOF. And so we need to change keyopt 1 to make them structural contact elements.
mike

[mikerife]

Hi @gcassianno removing the midside node with emid only removes them from the element definition (its connectivity). It does not remove the nodes from the model. You should either delete them (the 'free' midside nodes) or unselect them prior to solving.

[mikerife]

@gcassianno what R can define, and so RMODIF can chage, depends on the element type. Each element type has its own specific set of real constant(s), if any, and you can find out what they are in the MAPDL Element Guide (of the Help).

[gcassianno]

Hi @mikerife

Thank you for the additional information. I’ll try making some changes to my example based on your comments, and I’ll come back with the results I get.

Also, is there a command to select only midiside nodes?

[mikerife]

Hi @gcassianno (prior to using the emid,remove) there is an option on NSLE to select the mid-side nodes. After using emid,remove you can select them in other ways. For example nsle,u will leave you with the set of nodes not used to define the current set of elements.

[gcassianno]

Thank you very much @mikerife and @germa89.

It worked!