|
[Sponsors] |
May 11, 2010, 06:04 |
conjugateHeatFoam
|
#1 |
New Member
Antonello
Join Date: Apr 2010
Posts: 20
Rep Power: 16 |
hi,
I use openfoam for my thesis. i wish to use conjugateHeatFoam but in the forum no information are present. Can anyone post or direct me on a "how to" use this code? I have been looking arround, hoping to find my way out from the tutorials. Thank you. |
|
May 13, 2010, 15:43 |
|
#2 |
Senior Member
Ben K
Join Date: Feb 2010
Location: Ottawa, Canada
Posts: 140
Rep Power: 19 |
Have you seen this post:
http://www.cfd-online.com/Forums/ope...-openfoam.html There's lots of information there. |
|
May 15, 2010, 05:17 |
|
#3 |
New Member
Antonello
Join Date: Apr 2010
Posts: 20
Rep Power: 16 |
Thanks for the replay Benk
the information in the forum are incomplete! The construction of a case is very difficult for me... |
|
May 15, 2010, 13:24 |
|
#4 |
Senior Member
Ben K
Join Date: Feb 2010
Location: Ottawa, Canada
Posts: 140
Rep Power: 19 |
Ok, the first thing you have to do is make sure that you can run the test case "conjugateHeatFoam" and that it works properly (ie. you don't get any error messages when you compile and run it).
The basics of this solver: 1) This solver is for multiple regions where, for example, you have multiple regions in contact with one another and you have a species (like heat) transferred through each of those regions. Each region is associated with a mesh. You'll have 1 main mesh and other regions are the submeshes (in the test case the main mesh is in the conjugateCavity directory and the submesh is the solid directory which is a link to the heatedBlock directory). You have to make sure you understand the directory structure of meshes and submeshes first. 2) Another important point about the mesh is that in the constant/polyMesh/boundary file, you'll have to manually add the regionCouple information (every time you run the blockMesh command), like: Code:
right { type regionCouple; nFaces 10; startFace 200; shadowRegion solid; shadowPatch left; attached on; } 3) To implement the equations, you use the special coupledFvScalarMatrix object which is written so that each equation is in an array. For the syntax, see solveEnergy.H file in the test case. 4) When creating coupled fields (for example in the createFields.H file), you have to include "attachPatches.H" before creating any fields that are to be coupled and include "detachPatches.H" before creating any fields that are not coupled. The [de|at]tachPatches.H essentially turns on or off the regionCoupling information in your boundaries file since regular solvers don't know what to do with this special boundary. 5) In the time = 0 directory, you must also indicate the coupling on boundaries for each coupled field. For example, if you look at the T (and DT) file for the conjugateHeatFoam case, you'll see: Code:
right { type regionCoupling; value uniform 273; remoteField T; } 6) In your system/fvSolution, you need to indicate which fields are coupled, using: Code:
T+T BiCG { preconditioner { type Cholesky; } minIter 0; maxIter 1000; tolerance 1e-6; relTol 0.0; }; 7) I've found that it's also a good idea to use harmonic averaging in the system/fvSchemes file but not necessary to run a case. For another example case, see http://www.cfd-online.com/Forums/ope...tml#post251473 and all posts within. |
|
May 15, 2010, 13:26 |
|
#5 |
Senior Member
Ben K
Join Date: Feb 2010
Location: Ottawa, Canada
Posts: 140
Rep Power: 19 |
PS. If anybody has run this solver in parallel, I'd like instructions on how to do that!
|
|
June 20, 2011, 05:39 |
|
#6 | |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Quote:
some questions for you:
mad |
||
June 20, 2011, 22:39 |
|
#7 | |||
Senior Member
Ben K
Join Date: Feb 2010
Location: Ottawa, Canada
Posts: 140
Rep Power: 19 |
Quote:
Quote:
Quote:
The solver will just apply the following conditions at the interface between 2 regions (ie. internal boundaries): 1. phi(region 1) = phi(region 2) 2. flux(region 1) = -flux(region 2) |
||||
July 30, 2020, 06:00 |
|
#8 | |
New Member
Hailong
Join Date: Sep 2019
Posts: 8
Rep Power: 7 |
Quote:
If I have multiple solid, and they have different thermal properties, diffusivity, and so on. Besides attachPatches.H file,do I need to modify other files? for example creatSolidField.H |
||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
conjugateHeatFoam, grid spacing and gradient calculation | benk | OpenFOAM | 1 | May 5, 2010 17:06 |
conjugateHeatFoam: Problems adding 3rd region | benk | OpenFOAM | 5 | April 21, 2010 13:46 |
conjugateHeatFOAM: exchange of INFO at INTERFACE?? | dinonettis | OpenFOAM | 7 | March 25, 2010 15:09 |
conjugateHeatFOAM: exchange of INFO at INTERFACE?? | dinonettis | OpenFOAM Programming & Development | 0 | March 19, 2010 13:11 |
conjugateHeatFoam: Should solid and fluid have the same mesh at the coupled boundary? | awacs | OpenFOAM Running, Solving & CFD | 6 | September 22, 2009 23:58 |