[ronaldo]

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

[ronaldo]

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

[LarsPT]

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!

[ronaldo]

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!

[LarsPT]

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

[PetSul]

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

[ronaldo]

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

[PetSul]

Originally Posted by ronaldo

Hi petSul,

it should help you to solve your problem!

http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2008/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

[PetSul]

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

[LarsPT]

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

[suitup]

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.

[LarsPT]

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

[suitup]

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.

[suitup]

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

Best regards.

[LarsPT]

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