CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

InterDyMFoam for breaking wave simulation

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

Like Tree1Likes
  • 1 Post By egp

Reply
 
LinkBack Thread Tools Display Modes
Old   April 22, 2010, 09:25
Default InterDyMFoam for breaking wave simulation
  #1
New Member
 
yannH
Join Date: Feb 2010
Posts: 26
Rep Power: 7
yannH is on a distinguished road
Hello !

I'm actually trying to run a simulation for a breaking wave in 'deep water'. I've already got some good plunging breakers with interFoam . But when I try to run interDyMFoam, for a ras model, I've got this message that never appears with interFoam :

This mesh contains patches of type empty but is not 1D or 2D
by virtue of the fact that the number of faces of this
empty patch is not divisible by the number of cells.

From function emptyFvPatchField<Type>::updateCoeffs()
in file fields/fvPatchFields/constraint/empty/emptyFvPatchField.C at line 148.

FOAM exiting

I've seen that it could be a multiple declaration for vertices of the mesh but it's not my case, see my blockMeshDict :


convertToMeters 1e-1;
vertices
(
(0 0 0)
(1 0 0)
(1 0.4 0)
(0 0.4 0)
(0 0 0.01)
(1 0 0.01)
(1 0.4 0.01)
(0 0.4 0.01)
);
blocks
(
hex (0 1 2 3 4 5 6 7) (250 100 1) simpleGrading (1 1 1)
);
edges
(
);
patches
(
cyclic leftAndRight
(
(0 4 7 3)
(2 6 5 1)
)
wall lowerWall
(
(1 5 4 0)
)
patch atmosphere
(
(3 7 6 2)
)
empty frontAndBack
(
(0 3 2 1)
(4 5 6 7)
)
);
mergePatchPairs
(
);


Does anyone see what is wrong ?

Yann
yannH is offline   Reply With Quote

Old   April 23, 2010, 05:11
Default
  #2
egp
Senior Member
 
egp's Avatar
 
Eric Paterson
Join Date: Mar 2009
Location: Blacksburg, VA
Posts: 197
Blog Entries: 1
Rep Power: 9
egp is on a distinguished road
You need to provide more information. Your blockMeshDict looks OK (did you run checkMesh to check it?).

What is in your dynamicMeshDict? Which dynamicFvMesh are you trying to use?

Since you have cyclic on leftAndRight, and empty on frontAndBack, what is driving your flow (I presume the motion of your lowerWall is driving the flow?).
egp is offline   Reply With Quote

Old   April 23, 2010, 06:05
Default
  #3
New Member
 
yannH
Join Date: Feb 2010
Posts: 26
Rep Power: 7
yannH is on a distinguished road
Hi Eric,

Thanks for your reply, I want to use interDyMFoam because i'm interested in dynamic meshing... As I said, i work on breaking wave in deep water and for spilling breakers I need very tiny mesh for the crest.

my dynamicMeshDict looks like :

dynamicFvMesh dynamicRefineFvMesh;
dynamicRefineFvMeshCoeffs
{
refineInterval 1;
field alpha1;
lowerRefineLevel 0.001;
upperRefineLevel 0.999;
unrefineLevel 10;
nBufferLayers 1;
maxRefinement 2;
maxCells 200000;
correctFluxes
(
(
phi
U
)
);
dumpLevel true;
}
}

(I've just copied one from damBreak example, so i'm not sure...)

Otherwise about your question my lowerWall doesn't move. I initialize the velocity field with funkySetFields, in order to get an unsteady inital sinusoidale wave, that immediately breaks.

velocityField.jpg

mediumRes_deepWater.jpg
yannH is offline   Reply With Quote

Old   April 23, 2010, 06:15
Default
  #4
egp
Senior Member
 
egp's Avatar
 
Eric Paterson
Join Date: Mar 2009
Location: Blacksburg, VA
Posts: 197
Blog Entries: 1
Rep Power: 9
egp is on a distinguished road
Hmm, dynamicRefineFvMesh for 2D... that's what I figured. Isn't going to work since it only does isotropic refinement (including in the z-direction of your mesh).

If you really need to do the 2D refinement, you'll have to hack the dynamicRefineFvMesh class and create a 2D version. Otherwise, you will have to make your domain truly 3D and periodic in the z-direction, and let the mesh refinement do its work as designed.
mm.abdollahzadeh likes this.
egp is offline   Reply With Quote

Old   April 23, 2010, 07:59
Default
  #5
New Member
 
yannH
Join Date: Feb 2010
Posts: 26
Rep Power: 7
yannH is on a distinguished road
ok, I'll try in 3D with cyclic boundaries for front and back... 3D was my first idea when I began, with an epsilon value into velocity field varying with the width to avoid artificial 3D, but computation time scared me. So it's gonna be the occasion to try it...I'll post screenshots if it works !

thanks Eric,

Yann
yannH is offline   Reply With Quote

Old   June 18, 2010, 09:19
Default
  #6
Senior Member
 
Emanuele
Join Date: Mar 2009
Posts: 110
Rep Power: 8
nuovodna is on a distinguished road
any news on 2D dynamicMeshDict ??? I have a problem settings cyclic instead of empty patches: setFields for alpha1 doesn't work and it returns error.
nuovodna is offline   Reply With Quote

Old   July 13, 2010, 10:06
Default
  #7
New Member
 
yannH
Join Date: Feb 2010
Posts: 26
Rep Power: 7
yannH is on a distinguished road
Is it really useful (or interesting in mechanical terms) to use interDyMFoam instead of interFoam ? I'm asking that because I'm a little lost. My domain doesn't move, only the interface.. What is the interest of dynamic meshing or the situation it is needed ?
yannH is offline   Reply With Quote

Old   July 26, 2010, 08:50
Default
  #8
New Member
 
yannH
Join Date: Feb 2010
Posts: 26
Rep Power: 7
yannH is on a distinguished road
Hi everyone,

I am testing my example of breaking waves with interFoam or interDyMFoam and with different schemes (for divergence terms of the equation). I have not enough knowledge about efficiency or accuracy about it, so I test with those from dambreak tutorial

div(rho*phi,U) Gauss upwind; // or Gauss limitedLinearV 1;
div(phi,alpha) Gauss vanLeer;
div(phirb,alpha) Gauss interfaceCompression;

or sloshing case.

div(rho*phi,U) Gauss vanLeerV;
div(phi,alpha) Gauss vanLeer;
div(phirb,alpha) Gauss vanLeer;

Results are different (especially with upwind).. can someone give me advice or tell me what is the best ? thanks

Regards,

Yann
yannH 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
detonation wave simulation Krish FLUENT 6 October 14, 2010 02:32
I lose some fluid during simulation using InterDyMFoam anmartin OpenFOAM Running, Solving & CFD 0 April 20, 2010 15:19
About probe result of Wave simulation shiw FLOW-3D 3 March 13, 2009 10:15
Two question about Wave simulation shiw FLOW-3D 4 February 20, 2009 12:12
Wave simulation Navin Fogla FLUENT 0 March 6, 2008 10:50


All times are GMT -4. The time now is 14:05.