CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   Heat Transfer (http://www.cfd-online.com/Forums/openfoam/69206-heat-transfer.html)

 ronaldo October 15, 2009 06:28

Heat Transfer

Dear all,

I would like to simulate a heat transfer problem.
- Which solver is adaquat for that?
- Is it possible with rhoSimpleFoam?

I have a fluid (air 200K) and a solid (fin) above that fluid. The top of the solid (Tube) is warmed (350K) and i want to study the convective heat transfert inside the solid .

 LarsPT October 15, 2009 06:47

Hi Ronaldo,

I think the chtMultiRegionFoam solver is adequate for your problem. It solves the energy, navier-stokes and mass conversation equations separately for solid and fluid regions. I did natural convection over a hot plate with this solver. If you use OpenFOAM-1.6 there must be a tutorial case which you can use at sample case.
If you have further problems feel free to ask.

Best regards,
Lars

 ronaldo October 15, 2009 07:01

Thank you very much!

 ronaldo October 15, 2009 08:03

Hi LarsPT,

I use OpenFOAM-1.6. There are two Tutorials case of chtMultiRegionFoam. There appear to be complicated.

- Please could you tell how to set the RegionPropeties?

 LarsPT October 15, 2009 08:22

So, just give me some minutes to prepare my case as a tutorial which is easier to understand because it is 2D and has only tow regions. ;)

Anyway, the folders in the constant folder are needed to set the properties of the fluid regions. Furthermore, a folder for each region in the constant directory is necessary to convert results to VTK afterwards. You will see!

Be a bit patient, please! ;)
Lars

 LarsPT October 15, 2009 09:04

1 Attachment(s)
So, it's done. The problem is quite easy. There's a copper plate heated at the bottom. Over the plate there is air. I decreased mesh resolution because I calculated it on a cluster with 8 CPUs.

Setting the case works like this.
1. Create the whole domain and a mesh with blockMesh
2. Create cell set out of several cells (makeCellSets)
3. Convert cell sets to cell zones
4. Convert cell zones finally to regions (0.001 directory is created automatically)
5. Change the BCs at the intersection of the two regions, e.g. velocity is 0 directly at the plate and so on
6. Remove unnecessary field from both regions, e.g. solid needs no turbulence properties
7. Copy polyMesh data from regions to the constant/region directory, important for post processing
8. Run the solver
9. Convert results to VTK

The creation of the regions is summarized in the mesh.sh script, all the other stuff in the run.sh script. So you might first run mesh.sh and afterwards run.sh to perform a complete simulation.

Hope this helps!

Best regards
Lars

 ronaldo October 15, 2009 15:01

my case

Thank you so much LarsPT!

I would try right now.

 LarsPT October 16, 2009 08:08

It looks like a heat echanger, isn't it? Is the fin supposed to optimize the heat flux from the hot pipes to the air? Furthermore, there is one thing that is not clear to me. Is the air able to flow around the find completely? It seems that the fin is like an obstacle in the channel.

Best Regards
Lars

 ronaldo October 16, 2009 08:34

Quote:
 Originally Posted by LarsPT (Post 232741) Hi Ronaldo, I think the chtMultiRegionFoam solver is adequate for your problem. It solves the energy, navier-stokes and mass conversation equations separately for solid and fluid regions. I did natural convection over a hot plate with this solver. If you use OpenFOAM-1.6 there must be a tutorial case which you can use at sample case. If you have further problems feel free to ask. Best regards, Lars
Quote:
 Originally Posted by LarsPT (Post 232897) It looks like a heat echanger, isn't it? Is the fin supposed to optimize the heat flux from the hot pipes to the air? Furthermore, there is one thing that is not clear to me. Is the air able to flow around the find completely? It seems that the fin is like an obstacle in the channel. Best Regards Lars

It is! I have 4m/s Velocity Inlet. The fin supposed to optimize the heat flux. It looks like "Bild fin" after the Simulation with Fluent. Yes the air able to flow around the find completely.

I would send you another Graphic! Thank you for your Help

 ronaldo October 16, 2009 09:12

Hi LarsLP,

this is the Graphic.

 ronaldo October 19, 2009 04:16

Hi LarsTP,

it donīt work. I tried, but no success.

- I read a Fluent.msh mesh file using fluentMeshToFoam, so i donīt have " blockMeshDict" . I also have following problems:

- How could i set the makeCellSet " (* * *)(* * *)", mesh.sh, file?
- How could i find nFaces and startFace (air_to_plate for example)

have a good Day!

 LarsPT October 19, 2009 08:54

Hi,

first of all I have to confess that I have never worked with fluent so far. So, I can't help at this point, sorry.

The makeCellSets file is necessary to group cells which build a region.
It can be edited to your own purposes by using topoSetSources which can be found in OpenFOAM/OpenFOAM-1.6/applications/mesh/manipulation/cellSet/cellSetDict, e.g. a cylinder or a sphere.

I am not sure with the last point you mentioned. In my cases I don't need to know the start faces. A further boundary file is created somewhere in the 0/regionName directory after splitting up the mesh and creating the regions. There you should find the values for both parameters.

Best regards
Lars

 ronaldo October 19, 2009 09:19

The only problem i have is to simulate using Openfoam (not Fluent)!
please could i post my case here? Maybe you could find out what happend.

 LarsPT October 19, 2009 09:37

Yes, of course you can post your case and I'll have a look at it. But make sure that you post no information protected by any copyright laws! ;)
As university courses start today I can't say when I have time to look at it, but I'll try as soon as possible.

 ronaldo October 20, 2009 05:39

1 Attachment(s)
Quote:
 Originally Posted by LarsPT (Post 233230) Yes, of course you can post your case and I'll have a look at it. But make sure that you post no information protected by any copyright laws! ;) As university courses start today I can't say when I have time to look at it, but I'll try as soon as possible.

Hi LarsTp,

this is my case. I have tried, but i still have problems. I post only " Boundary" in the PolyMesh folder. It is ok?

 ronaldo October 20, 2009 10:01

Hi LarsTP,

i run only "splitMeshRegions -cellZones" and 0.001 directory is created automatically.
I also got 4 region ( 3 for air and ane for solid).
For every Region under 0.001, i got automatically a folder polyMesh and cp,.......U file.
I am on the right way or not?

 LarsPT October 20, 2009 12:09

I didn't have the time to look in your case yet, but the way you described sounds very good. It has to be this way!

 ronaldo October 20, 2009 17:33

Thank you LarsTP!

i would try to ameliorate my case tonigth and post it tomorrow here.

 ronaldo October 22, 2009 02:25

Quote:
 Originally Posted by LarsPT (Post 233410) I didn't have the time to look in your case yet, but the way you described sounds very good. It has to be this way!

Hi LarsTP,

i have only one Problem now. How to set my makeCellSets file.
I did it but i became the following error:

Cell 0 with centre (0.024 0.000155 8.003e-05) is multiple zones. This is not allowed. It is in zone c1 and c2.
I donīt know if i could send you the geometry to Email thereby you set this makeCellSets for me.

sorry but i have tried

 LarsPT October 22, 2009 04:42

Hi Ronaldo,

the mentioned problem can be solved easily. As it simply says there is a cell which is part of two zones. If a cell is part of a particular zone depends on the position of the centre of the specific cell.
The fact that a cell is part of two different zones often appears when a mesh with a odd number of cells is divided in two zones, or something similar.
Being brief it means that the boundary of a zone/region is not allowed to cut a cell. Check your and look for this kind of problem.

Hope this helps, good luck!

Best Regards
Lars

All times are GMT -4. The time now is 09:57.