conjugateHeatFoam
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. |
Have you seen this post:
http://www.cfd-online.com/Forums/ope...-openfoam.html There's lots of information there. |
Thanks for the replay Benk
the information in the forum are incomplete! The construction of a case is very difficult for me... |
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 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 6) In your system/fvSolution, you need to indicate which fields are coupled, using: Code:
T+T BiCG 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. |
PS. If anybody has run this solver in parallel, I'd like instructions on how to do that!
|
Quote:
some questions for you:
mad |
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) |
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 |
All times are GMT -4. The time now is 15:04. |