Problem in solving Openfoam with Calculix

Official adapters and tutorials
,
7

I am trying to run your case using run.sh inside fluid-openfoam (using OpenFOAM 10).
Comparing your files to the elastic-tube-3d tutorial, I see that you are calling blockMesh, but you don’t provide a system/blockMeshDict.

I see that there is already a directory constant/polyMesh, so the I am skipping the blockMesh and directly running pimpleFoam. With that, I get:

--> FOAM FATAL ERROR: 
Solution convergence criteria specified in PIMPLE.residualControl must be given as single values. Corrector loop convergence criteria, if appropriate, are specified as dictionaries in PIMPLE.<loopName>ResidualControl.

    From function bool Foam::singleRegionConvergenceControl::readResidualControls()
    in file cfdTools/general/solutionControl/convergenceControl/singleRegionConvergenceControl/singleRegionConvergenceControl.C at line 73.

FOAM exiting

Removing the PIMPLE.residualControl from your system/fvSolution (this probably needs to be adjusted to OpenFOAM 10 syntax), I get to the next error:

---[precice] ERROR:  Data with name "DisplacementData" is not defined on mesh "Fluid-Mesh-Nodes". Please add <use-data name="DisplacementData"/> under <mesh name="Fluid-Mesh-Nodes"/>.

This is a typo: In system/preciceDict, it seems like you have changed the following:

    readData
    (
-      DisplacementDelta
+      DisplacementData
    );

You also have another typo further down:

  Interface2
  {
    mesh              Fluid-Mesh-Faces;
-    patches           (interface);
+    patches           (inteface);

With these changes, the case seems to be running for a while, till I get the following error in CalculiX:

 average force= 0.000027
 time avg. forc= 0.000014
 largest residual force= 0.000000 in node 4 and dof 3
 largest increment of disp= 0.000000e+00
 largest correction to disp= 0.000000e+00

 convergence

Adapter writing coupling data...
Adapter calling advance()...
---[precice] ERROR:  advance() cannot be called with a timestep size of 0.

This error sounds familiar: OpenFOAM-CalculiX: Timestep Error - #5 by mattfrei Please take it from here and update this thread with your findings.

There are also further changes in the CalculiX case, which I cannot evaluate.

Further notes:

  • In system/fvSolution, you have set PIMPLE.nOuterCorrecters 50;. This seems like an arbitrary choice for now (it should probably be nOuterCorrectors, not nOuterCorrecters), which could make the simulation quite slower. I suggest removing it.
  • You have also changed in the system/controlDict:
    - writeControl timeStep;
+ writeControl runTime;
- writeInterval 10;
+ writeInterval 0.10;
    I think you intended to get more frequent results, but this leads to no results for me till at least 0.01s simulation time, when CalculiX fails.
  • What I did, was to use meld to compare your case with the elastic-tube-3d tutorial. This tool may be useful for you as well.
1 Like