|
[Sponsors] |
January 6, 2014, 15:08 |
convection heat transfer in one region
|
#1 |
Senior Member
|
Dear All,
i want to simulate convection heat transfer for flow exposed to constant wall temperature without including tube thickness. my problem is chtMultiRegionSimpleFoam is used for multiple Regions only. thanks, |
|
January 7, 2014, 06:59 |
|
#2 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 |
Hi,
you are wrong. cht can also used for one Region but is generated for Multi regions (conjugated heat Transfer). If you want to simulate just one Region you can use buoyantSimpleFoam or buoyantBoussinesqSimpleFoam - or the Pimple for transient Solutions. Regards |
|
January 7, 2014, 09:05 |
|
#3 | |
Senior Member
|
Quote:
1- how could i use chtMultiRegionSimpleFoam for one region? 2- i think buoyantSimpleFoam is used for natural convection not forced convection. also, all thermo models available with it are for perfect gases not lequids. thanks, Ahmed |
||
January 7, 2014, 11:35 |
|
#4 | |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 |
Quote:
Hi, you could use cht for one region. You just have to use one region where is the problem? the buoyantSimpleFoam are for natural convection but I think for forced convection you could also do it. PS: you can use water as well - use icoPolynomial functions to describe your fluid. |
||
January 11, 2014, 15:18 |
|
#5 | |
Senior Member
|
Quote:
Hi Tobias, i want to use one fluid region and no solid regions, cht don't accept this. splitMeshRegions doesn't create mesh for only one region. also, cht must read regions to apply suitable equations. thanks, Ahmed |
||
January 12, 2014, 06:20 |
|
#6 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 |
Hi,
you are wrong. Hmmm, you are not very familiar to the software, arent you? I dont want to tell you step by step how to do it (no time) but some hints: 1. why do you need splitMeshRegions? - you need it if you are using sHM with more than one region (--> cellZones) 2. just mesh your solid 3. move the mesh from constant/polyMesh into constant/solid/polyMesh 4. change the "regionProperties" - only solid is available 5. change the boundarys in constant/solid/polyMesh like you need 6. change 0/solid/* files to your application -> start You can simply check it out in the following way: a) buoyantSimpleFoam tutorial -> buoyantCavity b) make the mesh c) move the mesh from buoyantCavity/constant/polyMesh into your cht case -> cht_case/constant/myRegion d) move the files in 0 directory from buoyantCavity/0 into your cht case -> cht_case/0/myRegion e) change the regionProperties so you have only one fluid (myRegion) f) check that you have the fvSchemes and Solutions in system/myRegion -> start Be sure that the fluid files are in the constant/myRegion folder too. Hope it will help you now. PS: have a look at the source code then you will be able to understand how this solver is working Regards Tobi |
|
January 12, 2014, 06:22 |
|
#7 | |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 |
Quote:
It does not matter if you just want to use one region for fluid or solid. Therefor you should use buoyantSimpleFoam: In the energy eqn you find the turbulent term Code:
fvScalarMatrix EEqn ( fvm::div(phi, he) + ( he.name() == "e" ? fvc::div(phi, volScalarField("Ekp", 0.5*magSqr(U) + p/rho)) : fvc::div(phi, volScalarField("K", 0.5*magSqr(U))) ) - fvm::laplacian(turbulence->alphaEff(), he) == radiation->Sh(thermo) + fvOptions(rho, he) ); |
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Heat transfer, natural convection: Heat sink <-> Air | SvenH | OpenFOAM Running, Solving & CFD | 10 | March 11, 2020 04:40 |
convergenceof natural convection prob. in cfx | cpkewat | CFX | 15 | January 31, 2014 06:29 |
Heat Transfer Coefficient For Natural Convection | Nitin Minocha | Main CFD Forum | 0 | April 1, 2013 00:19 |
[Other] StarToFoam error | Kart | OpenFOAM Meshing & Mesh Conversion | 1 | February 4, 2010 04:38 |
free convection heat transfer from a heated horizontal surface through a liquid to a thin cooled fin | Kaushik | FLUENT | 1 | May 8, 2000 06:47 |