|
[Sponsors] |
March 17, 2009, 03:58 |
interTrackFoam diffusivity distortionEnergy
|
#1 |
Member
Virginie Ehrlacher
Join Date: Mar 2009
Posts: 52
Rep Power: 17 |
Hello Foamers,
I had a problem with interTrackFoam when I tried to use it with the diffusivity option distortionEnergy. The simulation runs fine during one time step and then aborts with the following error message: Time = 4e-05 include readInterfaceSIMPLEControls.H: done Courant Number mean: 4.56289e-06 max: 0.000340596 velocity magnitude: 0.0325762 include CourantNo.H: done interface.updateDisplacementDirections(): done CG: Solving for motionUx, Initial residual = 0.282994, Final residual = 9.8461e-10, No Iterations 73 CG: Solving for motionUy, Initial residual = 0.285915, Final residual = 7.86543e-10, No Iterations 74 CG: Solving for motionUx, Initial residual = 2.17566e-08, Final residual = 4.42034e-10, No Iterations 1 CG: Solving for motionUy, Initial residual = 0.000535407, Final residual = 7.8184e-10, No Iterations 22 Different dimensions for += dimensions : [0 1 0 0 0 0 0] = [0 1 1 0 0 0 0] From function dimensionSet:perator+=(const dimensionSet& ds) const in file dimensionSet/dimensionSet.C at line 157. I suppose that the dimension of a field is inadvertently changed during the first iteration... Does anyone know how to fix that? Thank you a lot. Virginie |
|
April 4, 2012, 12:03 |
|
#2 |
Member
Wolfgang W.
Join Date: Nov 2009
Location: Switzerland
Posts: 57
Rep Power: 16 |
Hi Virginie,
I know that this post dates back quite a while ... but did you find any solution to your problem? I'm encountering the exact same issue when using either diffusivity option distortionEnergy or deformationEnergy in bubbleInterTrackFoam. Some kind of dimension mismatch occurs ... curiously, when running another solver like icoFsiFoam the same settings work quite fine. Do you or has anybody else any hints on how to solve this problem? Cheers, Wolfgang |
|
May 9, 2012, 21:18 |
|
#3 |
Senior Member
Kyle Mooney
Join Date: Jul 2009
Location: San Francisco, CA USA
Posts: 323
Rep Power: 17 |
A good place to start might be running it again in debug and getting a stack trace on the error.
|
|
May 10, 2012, 05:32 |
|
#4 |
Member
Wolfgang W.
Join Date: Nov 2009
Location: Switzerland
Posts: 57
Rep Power: 16 |
Hi Kyle,
Thanks for your reply! I actually got it sorted out ... it seems that in some tutorial cases (namely surfaceTracking/interTrackFoam/hydrofoil & ramp) the dimension of motionU is set incorrectly to [ 0 1 0 0 0 0 0 ] (distance) while it should certainly be [ 0 1 -1 0 0 0 0 ] (velocity). This tiny flaw usually doesn't show up because apparently only the .value() is read, but seemingly, the distortionEnergy and deformationEnergy options in dynamicMeshDict trigger a check for dimensions. Cheers, Wolfgang P.S.: Be aware that moreover the dimension of surfaceTension (constant/freeSurfaceProperties) in all interTrackFoam cases should be [ 1 0 -2 0 0 0 0 ] instead of [ 1 -2 0 0 0 0 0 ]. |
|
May 10, 2012, 10:18 |
|
#5 |
Senior Member
Kyle Mooney
Join Date: Jul 2009
Location: San Francisco, CA USA
Posts: 323
Rep Power: 17 |
Good find! You might want to consider posting this as a bug, it would be good to have the mesh motion solvers consistently do dimension checks regardless of the formulation.
Kyle |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
InterTrackFoam any information | rajon | OpenFOAM Running, Solving & CFD | 30 | January 1, 2016 16:27 |
Wall contact in interTrackFoam | virginie_e | OpenFOAM Running, Solving & CFD | 2 | November 8, 2011 11:52 |
SIMPLE loop in interTrackFoam | virginie_e | OpenFOAM Running, Solving & CFD | 3 | March 17, 2009 05:40 |
Pressure divergence with interTrackFoam | virginie_e | OpenFOAM Running, Solving & CFD | 8 | March 4, 2009 05:07 |
InterTrackFoam error | kester | OpenFOAM Running, Solving & CFD | 10 | November 8, 2007 02:55 |