A question about FSI and CHT modules

[Beholder]

Hello!

I saw in the tutorial that multiple modules can be used simultaneously, so I started CHT and FSI simultaneously to solve the problem of cylinder flow. I hope to generate deformation while also heating the walls with gas.The fluid solver uses OpenFOAMv2206, the solid solver uses calculixV2.2.0, and the precision version is 2.5.0

I referred to the tutorials “flow-over-heated-plate” and “perpendicular-flap” and made changes to the corresponding coupling files. It can perform calculations, but I set up a monitoring point and found that the heat flux density is always 0, and displacement can be seen at the monitoring point in the solid domain, but there is no change in the fluid domain. I hope someone can help me answer this question.

Is this because of the issue with setting the file after both CHT and FSI are enabled? Here are the changed configuration files and monitoring point data

perciceDict

preciceConfig "../precice-config.xml";

participant Fluid;

modules (FSI CHT);

interfaces
{
  Interface1
  {
    mesh              Fluid-FSI;
    patches           (cylinder);
    locations         faceCenters;
    
    readData
    (
      Displacement 
    );
    
    writeData
    (
      Force 
    );
  };
/**/ 
  Interface2
  {
    mesh              Fluid-CHT;
    patches           (cylinder);
    locations         faceCenters;
    
    readData
    (
      Heat-Flux
    );
    
    writeData
    ( 
      Temperature
    );
  };

};
}

config.yml

participants:

    Solid:
        interfaces:
        - nodes-mesh: Solid-FSI
          patch: cylinder
          read-data: [Force]
          write-data: [Displacement]
          read-data: [Temperature]
        - faces-mesh: Solid-CHTFlux
          patch: flux_interface
          write-data: [Heat-Flux]
          
          
precice-config-file: ../precice-config.xml

The remaining files are too long. I will attach them here as an attachment:
precice-config.xml (6.2 KB)
precice-Fluid-watchpoint-force.log (327.1 KB)precice-Fluid-watchpoint-heat.log (234.5 KB)
precice-Solid-watchpoint-flux.log (190.0 KB)precice-Solid-watchpoint-force.log (377.4 KB)

[Makis]

@Beholder

It can perform calculations, but I set up a monitoring point and found that the heat flux density is always 0, and displacement can be seen at the monitoring point in the solid domain, but there is no change in the fluid domain.

Indeed. Both are fields that are written by the Solid participant. Are you sure that the patches you define are correct and that preCICE does get values for these fields on those meshes?

Try exporting and visualizing the coupling meshes: Export configuration | preCICE - The Coupling Library

Here is a visualization of your config file:

Even though rather complex (potentially you could merge the CHT and FSI meshes and interfaces), it looks complete.

[Beholder]

Thank you for your reply

I tried to output the coupled mesh in vtk format and the results were the same as reported by the checkpoint.

During this time, I tried to encrypt the wall, that is, the boundary of the deformation, narrowing the order of magnitude between the near-wall mesh height and the shape variable. I found that the deformation can be generated normally, but the heat flux and temperature still can not transfer normally

Re-comparing the two examples, I notice a few differences in the Calculix input file.inp:

In the flow-over-heated plate example

*STEP, INC=2000
*HEAT TRANSFER, DIRECT
0.01, 1.0

In the Vertical-FLAP example

*STEP, INC=10000
*DYNAMIC, ALPHA=0.0, DIRECT
1.E-2, 5.0

Looking through the Calculix manual I found that these are different solution Settings, and when I put the two together something interesting happened:

If the HEAT TRANSFER is behind, only the heat flux and temperature exchange can be carried out smoothly

average flux= 0.000000
time avg. flux= 0.010000
largest residual flux= 0.000000 in node 1188 and dof 0
largest increment of temp= 8.786373e-14
largest correction to temp= 8.786373e-14 in node 7 and dof 0

And if DYNAMIC is behind then there will be only displacement and force exchange

average force= 0.036999
time avg.forc = 0.027279
largest residual force= 0.000000 in node 1259 and dof 1
largest increment of disp= 9.616884e-06
largest correction to disp= 6.185882e-21 in node 86 and dof 1

It should be that there is code coverage, does this mean that the problem is on the solid solver? May I ask how to set Calculix to enable the calculation of accepting force and heat flux at the same time?

thank you

[SarahDi]

Hey,
I also started to couple FSI and CHT simultaneously with OpenFOAM and CalculiX in the last days for a simple plate geometry, although it is not yet working for some other reason.
I was also facing this issue with CalculiX in the beginning and as I understand it, there are two possible steps in CalculiX for a coupled thermo-mechanical analysis:

*COUPLED TEMPERATURE-DISPLACEMENT 

(documentation) and

*UNCOUPLED TEMPERATURE-DISPLACEMENT

where in the first procedure temperatures and displacements are solved simultaneously while in the second type of solution procedure in each increment the thermal analysis is performed first and then used as boundary field for the mechanical analysis.

If you are performing a Dynamic step and a heat-transfer step separately they should be performed in serial (e.g. if you take the flow-over-heated-plate example step and then the vertical-flap step: first heat-transfer for one second and then a dynamic analysis for 5 seconds). That is probably not what you want to do.

Hope that helps

[Beholder]

I’m very sorry that I only saw your reply today. I tried *COUPLED TEMPERATURE-DISPLACEMENT , which can smoothly perform heat transfer and load calculation work, confirming that my CHT and FSI problems lie in the solution settings of calculix!

Really helpful, thank you again!