[mCiFlDk]

Dear foamers,


As I'm aware that this module is not widely used, I'll explain the issue the best I can but straight to the point.

There are 2 operation modes provided by this module: singleRun (to calculate sensitivity maps, similar to U or p surface maps) and steadyOptimisation (to modify the mesh based on those maps). The differences between their setup are mainly 2:

• The constant/dynamicMeshDict/ is not needed for the singleRun
• The system/optimisationDict/ has to omit some lines if singleRun since it's simpler, without further issues

In my case, any singleRun sim works perfectly, but when I try to imitate the tutorial provided,

$FOAM_TUTORIALS/incompressible/adjointOptimisationFoam/shapeOptimisation/motorBike

the following error shows up when the first mesh morphing will be carried out (just after the 2nd cycle starts):

( ... ) # First cycle worked

* * * * * * * * * * * * * * * * *
Optimisation cycle 2
* * * * * * * * * * * * * * * * *

Adjoint solver adjSolver1
lift : 0.395253
Weighted objective : 0.395253

Using steepest descent for the first iteration
maxAllowedDisplacement/maxDisplacement of boundary	0.05/2.267379
Setting eta value to 0.0220519

[0] [2]
[2]
[2] --> FOAM FATAL ERROR: (openfoam-2012[3]
[3]
[3] --> FOAM FATAL ERROR: (openfoam-2012)
[3] Attempting to replace controlPointsMovement with a set of different size
[1]
[1]
[1] --> FOAM FATAL ERROR: (openfoam-2012)
[1] Attempting to replace controlPointsMovement with a set of different size
[1]
[1]
[0]
[0] --> FOAM FATAL ERROR: (openfoam-2012)
[0] Attempting to replace controlPointsMovement with a set of different size
[0]
[0]     From void Foam::volumetricBSplinesMotionSolver::setControlPointsMovement(const vectorField&)
[0]     in file )
[2] Attempting to replace controlPointsMovement with a set of different size
[2]
[2]     From void Foam::volumetricBSplinesMotionSolver::setControlPointsMovement(const vectorField&)
[2]     in file dynamicMesh/motionSolver/volumetricBSplinesMotionSolver/volumetricBSplinesMotionSolver.C at line 136.
[2]
FOAM parallel run exiting
[2]

 ( ... ) # Error keeps on going saying the same

I truly believe the error, after several trials, is caused by the setup of dynamicMeshDict. What confuses me is that it's just made up by a single control box, which is NOT in contact with any boundary (just in case you thought the issue was that).

I hope any of you have faced this similar issue, since I'm a bit desperate with it. I attach the optimisationDict and the dynamicMeshDict in case you find them useful.


Thanks in advance

[mCiFlDk]

SOLVED:

Originally Posted by mCiFlDk

Dear foamers,

( ... )

Hi,

For future adjointOptimisationFoam users I want to explain how I solved the issue.

If you download the two dicts I uploaded, you'll see that under "sensitivities" section in the optimisationDict, I was using "surfacePoints" to calculate the sensitivities. At the same time, I was using the "volumetricBSplines" option under dynamicMeshDict to morph the mesh.

It seems that, when you want to morph the mesh, you have to keep coherence between the options since there are incompatibilities between them. To solve it, I just changed the option under "sensitivities" section in the optimisationDict from "surfacePoints" to "volumetricBSplines", and that solved the issue.

Hope it helps!

[rohi1989]

Thank you for explanation