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

chtMultiRegionFoam - different mesh on the 2 sides of a coupled boundary

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

Like Tree3Likes
  • 1 Post By turbulencious
  • 1 Post By thomasnwalshiii
  • 1 Post By dhruv

Reply
 
LinkBack Thread Tools Display Modes
Old   September 25, 2012, 09:37
Default chtMultiRegionFoam - different mesh on the 2 sides of a coupled boundary
  #1
New Member
 
Join Date: Jul 2012
Posts: 21
Rep Power: 4
turbulencious is on a distinguished road
solver: chtMultiRegionFoam
version: 2.1-1
BC: compressible::turbulentTemperatureCoupledBaffleMix ed

dear FOAMers,

I hope everything is fine on your side.

I am using chtMultiRegionFoam and expectedly, I would like to have a more densed mesh in the fluid and a less densed mesh in the solid.

Is it possible? and if yes, have anybody already achieved it and can give me some guidelines?

thanks a lot
anothr_acc likes this.
turbulencious is offline   Reply With Quote

Old   September 27, 2012, 09:41
Default coinciding mesh
  #2
New Member
 
Thomas Walsh
Join Date: Nov 2010
Posts: 17
Rep Power: 6
thomasnwalshiii is on a distinguished road
I believe that for the default cht... solver you need coinciding surface meshes in order to transfer the energy between the different regions. You'd have to edit the boundary conditions to incorporate a ggi interface. I remember one of the presentation from the 2011 workshop at Penn State was on a multi-physics solver (conjugatedFsiFoam maybe) and the presenter went through the steps needed to implement this.

Here is the link to the powerpoint slides, http://www.personal.psu.edu/dab143/O...ven_slides.pdf. They only briefly mention how to implement it towards the end. Has anyone in this forum accomplish such a feat?
anothr_acc likes this.
thomasnwalshiii is offline   Reply With Quote

Old   September 28, 2012, 04:50
Default
  #3
New Member
 
Join Date: Jul 2012
Posts: 21
Rep Power: 4
turbulencious is on a distinguished road
thanks Thomas
turbulencious is offline   Reply With Quote

Old   October 12, 2012, 07:46
Default Any Solutions??
  #4
Member
 
supercommandodhruv
Join Date: Sep 2011
Posts: 57
Rep Power: 5
dhruv is on a distinguished road
Hi,

Were you able to solve this problem? Did you implement AMI/GGI on the patches? I have the same kind of problem, but I am not able to figure out how to use AMI in chtMultiRegionFoam.

Any help is greatly appreciated.

Thanks,
Dhruv.

Quote:
Originally Posted by turbulencious View Post
solver: chtMultiRegionFoam
version: 2.1-1
BC: compressible::turbulentTemperatureCoupledBaffleMix ed

dear FOAMers,

I hope everything is fine on your side.

I am using chtMultiRegionFoam and expectedly, I would like to have a more densed mesh in the fluid and a less densed mesh in the solid.

Is it possible? and if yes, have anybody already achieved it and can give me some guidelines?

thanks a lot
anothr_acc likes this.
dhruv is offline   Reply With Quote

Old   July 18, 2014, 15:43
Default
  #5
Member
 
ms
Join Date: Mar 2009
Location: West London
Posts: 43
Rep Power: 8
anothr_acc is on a distinguished road
Hey everyone! I now also need this functionality. Does anybody know if CHT and AMI can be used at the same time, on the same boundary in OF2.3.0 ?

Please say yes!

Best regards,

Mark.
anothr_acc is offline   Reply With Quote

Old   July 24, 2014, 05:58
Default
  #6
Member
 
ms
Join Date: Mar 2009
Location: West London
Posts: 43
Rep Power: 8
anothr_acc is on a distinguished road
Quote:
Originally Posted by anothr_acc View Post
Hey everyone! I now also need this functionality. Does anybody know if CHT and AMI can be used at the same time, on the same boundary in OF2.3.0 ?

Please say yes!

Best regards,

Mark.
Answered my own question. In short, yes! Try it:

in constant/copper/polyMesh/blockMeshDict:

Code:
boundary {
   copper_to_iron { sampleRegion iron; samplePatch iron_to_copper;
    type mappedWall;

    sampleMode nearestPatchFaceAMI;
    //sampleMode nearestPatchFace;

    offsetMode uniform; offset (0 0 0);
    faces ( (2 6 5 1) ) ; } // anti-clock looking in.
    }

in constant/iron/polyMesh/blockMeshDict:

Code:
boundary {
   iron_to_copper { sampleRegion copper; samplePatch copper_to_iron;
    type mappedWall;

    sampleMode nearestPatchFaceAMI;
    //sampleMode nearestPatchFace;

    offsetMode uniform; offset (0 0 0);
    faces ( ( 3 0 4 7 ) ) ; }
    }
And as long as there are no cells on the interface plane with no coupling to a boundary condition, this runs and provides better matching for power into the system and power out of the system for slightly different sized of differently meshed regions than the nearestPatchFace sampleMode.

Best regards,

Mark.
anothr_acc 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
How to let the mesh motion solver just solve a small region near a moving boundary? zhajingjing OpenFOAM 8 April 7, 2014 11:10
Difficulty in calculating angular velocity of Savonius turbine simulation alfaruk CFX 8 December 3, 2013 17:51
snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Native Meshers: snappyHexMesh and Others 2 March 27, 2011 21:11
conjugateHeatFoam: Should solid and fluid have the same mesh at the coupled boundary? awacs OpenFOAM Running, Solving & CFD 6 September 22, 2009 22:58
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10


All times are GMT -4. The time now is 00:26.