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 .
Thanks in advance
Help please!

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

Thank you very much!

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?
- What about this bottomAir and topAir Directories in the "Constant" 'Directory

Please Help me!

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

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

my case
 

Thank you so much LarsPT!

I would try right now.
Please here is my case (just for give you more information about my case). It is very important for me!

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

Hi LarsLP,

this is the Graphic.

Hi LarsTP,

it don´t work. I tried, but no success.

- I read a Fluent.msh mesh file using fluentMeshToFoam, so i don´t 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!

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

Thank you for your Reply! I would try now

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.

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?

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?

tell me please!

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!

Thank you LarsTP!

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

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 don´t know if i could send you the geometry to Email thereby you set this makeCellSets for me.

sorry but i have tried

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

Thanks LarsTP,

cellSet plate new boxCell (0 0 0 )(0.01 0.1 0.02)!
How to find this point (your case)? That is my problem now!

Thanks in advance

Hi LarsTP,

i first run splitMeshRegion and i have automatically 0.001 folder, but no sets folder in Constant/polymesh. It is ok or i must have it?

Thanks

The point in my case simply results from the geometrie. My domain is of dimension 0.01x0.1x0.1m (x y z). The plate should have the dimensions
0.01x0.1x0.02m (x y z).
So boxToCell (x0 y0 z0) (x1 y1 z1) defines a vector from (x0 y0 z0) to (x1 y1 z1) which creates the box.

Make sure that you remove the sets folder before you start a new mesh generation!

Hi LasrTP,

I am very happy today!
I made somthing different! Let me know if my way is right.

1. fluentMeshToFoam [case] -writeSets -writeZones -scale 0.001
(the directory sets " constant/polymesh" is created automatically)
2. setsToZones
3. splitMeshRegions -cellZones
(the directory 0.001 is created automatically)

. I just need the chanDictionaryDict to run the Simulation! It´s right?
. must i run it in parallel? (what do you suggest?)

I have 4 folder in the 0.001 directory! It´s possible to run only one of them?
Thank you in advance!

Hi Ronaldo,

that's right. You can set the BCs at the region interfaces either manually or define them in the changeDictionary file.
If you have the abilities to run the case in parallel, I would recommend to do so in order to save time or get a better quality solution.

Best regards
Lars

Hello,

do you know how chtMultiRegionFoam should be modified to be able to solve heat transfer between solid and liquid? As far as I know it applies only to solid-gas heat transfer. I guess it depends on the thermophysical model that the solver applies but I don't know which thermophysical model to use and how to modify the solver properly.

I'd appreciate if you could help me with this.

Regards,

Petri Sulasalmi

Hi petSul,

it should help you to solve your problem!

http://www.tfd.chalmers.se/~hani/kur...08/chtFoam.pdf " (2/4 most important for you)

http://www.opencfd.co.uk/openfoam/th...calModels.html "at the end of the page"

Hope this helps, good luck!

Best Regards
Ronaldo

Thank you very much! I'll check on it.

Regards,

Petri

I'm afraid that the material you gave concernes only solid-gas cases. It basically just explains the solver as it is. If I've understood correctly the default thermophysical stuff available for the solver doesn't apply for solid-liquid cases. So I should somehow modify the solver.

But thanks anyway!

Regards,

Petri

Yes, that's right. I'm sorry that I didn't mention this explicitly. I'm just looking for a solution of that problem myself. There is one thread in this forum where the use of liquids is discussed but I'm not sure if there is a proper solution right now, is there?
In my case (Rayleigh-Bénard convection) I used similarity theory to scale the domain and the temperature difference to reach identical Ra numbers as in the experiment which I use as reference.

Best regards
Lars

Hey guys,
after a short break, I wanna start working with the chtMultiRegion-Solver, I ve already analyzed the different folders and files. But a few things I still dont understand. E.g. I noticed that (in the example case) there are thermophysical properties for air but I'm not really able to find the propertiesfiles for the solidparts. If there isnt any declarationfile where can I find the settings for the heat conductance value?
Now i want to creat my own case with simple case with 3rd party meshing-files, has anyone already tried it, or just using blockmesh?

Best regards.

Hi suitup,

the properties for solid regions are defined in the time directories. K (capital letter) is the thermal conductivity, cp the specific heat capacity and rho is the density.
With these values the thermal diffusity can be calculated easily a=K/(rho*cp)
That's everything needed to calculate heat conduction in solid parts.

Best regards
Lars

Ah great, thank you, lars. Yes I was a little bit confused about the different folder partitions.

Hm the next step would be creating an own case with selfdesigned cad and meshfile. So I would import from e.g. salome my meshfile.

So how can I declare the different regions, I checked the Allrunscript and there a few different kinds of utils for creating the regions(correct me if I write something wrong).

• setset
• setsToZones
• splitMeshRegions
• changeDictionary
• reconstructPar

Ok now my question, setSet, setsToZones and splitMeshegion seems to be the ultis to creat different regions ind the FOAM-Mesh but how to use it/them for complex meshes, for easy blockMesh I understand (seems to be) how get the right coords. With other expression:Have i always to look into the meshfile also for really complex meshes and search the correct coords for the the different zonesettings? Is there a easy way to get right possition?


Best regards.

Hey guys I've still another question, you always use temperature as boundary-condition, is it possible using heat energy (q) instead?

Best regards.

Yes, I think it is possible. As q depends on the temperature gradient you can set a fixedGradient BC for the temperature T.

Best regards
Lars