CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Bugs

interTrackFoam diffusivity distortionEnergy

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   March 17, 2009, 04:58
Default interTrackFoam diffusivity distortionEnergy
  #1
Member
 
Virginie Ehrlacher
Join Date: Mar 2009
Posts: 52
Rep Power: 8
virginie_e is on a distinguished road
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
virginie_e is offline   Reply With Quote

Old   April 4, 2012, 12:03
Default
  #2
Member
 
Wolfgang W.
Join Date: Nov 2009
Location: Switzerland
Posts: 57
Rep Power: 7
WiWo is on a distinguished road
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
WiWo is offline   Reply With Quote

Old   May 9, 2012, 21:18
Default
  #3
Senior Member
 
kmooney's Avatar
 
Kyle Mooney
Join Date: Jul 2009
Location: Amherst, MA USA - San Diego, CA USA
Posts: 278
Rep Power: 9
kmooney is on a distinguished road
A good place to start might be running it again in debug and getting a stack trace on the error.
kmooney is offline   Reply With Quote

Old   May 10, 2012, 05:32
Default
  #4
Member
 
Wolfgang W.
Join Date: Nov 2009
Location: Switzerland
Posts: 57
Rep Power: 7
WiWo is on a distinguished road
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 ].
WiWo is offline   Reply With Quote

Old   May 10, 2012, 10:18
Default
  #5
Senior Member
 
kmooney's Avatar
 
Kyle Mooney
Join Date: Jul 2009
Location: Amherst, MA USA - San Diego, CA USA
Posts: 278
Rep Power: 9
kmooney is on a distinguished road
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
kmooney is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
InterTrackFoam any information rajon OpenFOAM Running, Solving & CFD 29 January 17, 2012 16:50
Wall contact in interTrackFoam virginie_e OpenFOAM Running, Solving & CFD 2 November 8, 2011 12:52
SIMPLE loop in interTrackFoam virginie_e OpenFOAM Running, Solving & CFD 3 March 17, 2009 06:40
Pressure divergence with interTrackFoam virginie_e OpenFOAM Running, Solving & CFD 8 March 4, 2009 06:07
InterTrackFoam error kester OpenFOAM Running, Solving & CFD 10 November 8, 2007 03:55


All times are GMT -4. The time now is 14:49.