[Ohlzen-Wendy]

Hi everybody,

I am searching for a solution for a calclation of the Scenario showing in the attachment.
we have following Situation:
a small Region produces heat and the heat is transfered into a fluid in a chamber (air without any velocity). a other part of the heat is transfered through different solid materials (e.g. aluminum and steel) into a cooling element. the cooling element is positioned in a Kind of pipe where air is flowing with a given Temperature and Speed.

I think this should be possible to solve with the solver chtMultiRegionFoam but I have several Problems:

The geometry is far more complex then shown. I want to use the program ANSA for creating the mesh of the Case. But how can I create a case with several regions like I Need for chtMultiRegionFoam?
- create every part on its own and merge them afterwards?

If I create the mesh in one case, how can I create the regians afterwards?

Is chtMultiRegionFoam the correct solver for my Problem. I think so but I am not sure.

Has anyone had a similar Problem before? I would be glad if I could get some help.


Best wishes

Andreas

[laurentD]

Hi Andreas,

i often work with the 'chtMutiRegionFoam' utility, but i don't use ANSA for the mesh.
Otherwise, i think the method is the same.
First i do a complete mesh with my meshing tool. Then for all materials i add boundaries (skins) and labels. OpenFOAM is able to read these labels.
Secondly i transfer the mesh files to OpenFOAM separately.
For example in a model with fluid and solid, i transfer the fluid files, i build the directory related to this fluid (constant/fluid/polymesh, system/fluid, 0/fluid) and after that, i do the same with the solid mesh.
I hope this can help you, it is not simple to explain.

Have a good day,
Laurent

[Ohlzen-Wendy]

Hi Laurent,

so I create a mesh in e.g. ANSA. Export the mesh, boundaries etc. of each submesh seperately and copy them manualy with the case structure as shown in the attachment?

do I have to run some other utilities like setSet etc. afterwards?
maybe you can upload something like the allrun script You usaly use?

best wishes and thank you so far

Andreas

[laurentD]

My allrun is useless because i use another mesh utility so i have to use others tools to convert the mesh to OpenFOAM.
But i have read looked for informations related to ANSA and it seems that ANSA can directly provide the polymesh directory.
So if you have the polymesh directory for each 'materials' (like in your tree) it should work.
To verify each part of the mesh, move the polymesh of a material uner constant/ and do the checkMesh command from the work directory (the root one). After this verification think to move again the polymesh directory to put it on the right place.
Laurent

[Ohlzen-Wendy]

hi everybody,

had some other Projects to work on but spent the last day on openFOAM.
So far I managed to Export the whole mesh from ansa and using the "splitMeshRegions -cellZones -overwrite" command to create my regions for fluids and solids.
I modified also the regions setting and solvers. But I still have some questions.

what Kind of BCs do I have to use on the patches between the regions. if it is a fluid to a wall i use the common wall BCs to pressure and velocity etc. but if i have a patch between 2 solids?
splitMeshRegions also created patches for "both sides" ("wall1_to_wall2" and "wall2_to_wall1"). do I have to use the some bcs on each side?

baffles:
What are they for? I want to have a constant heat flux (W/m³ or total W) from one solid. how can I include this? I Need the baffles for this or?

I know a lot of questions but somehow I have not found any satisfying Information.

best wishes


Andy

[zfaraday]

Hello!

Quick answer.

As for the coupling between regions for temperature, take a look at these BC's:

• turbulentTemperatureCoupledBaffleMixed
• turbulentTemperatureRadCoupledMixed

Regarding the volumetric heeat generation, take a look at this thread:
how-i-can-introduce-my-power-heat-w-chtmultiregionfoam.html

Hope it helps.

Best regards,

Alex

[Ohlzen-Wendy]

Hi everybody,

I make some progress regarding my calculation. therefore I set up a small test case. (
This one is running but I still have some questions I am not totally sure about.

If i introduce a heat transfer with a fixed power or flux on a patch between a fluid and a solid or a solid and a other solid - do i have to set the bc on both patches?

while chtMultiRegionFoam is running after some time the time step is decreased to something like 1e-13s. is there a way to track the maximum magnitude speed of the whole domain while the simulation is running?

best wishes

Andy

[BClarke352]

Hi,

I'm also having trouble with some boundary conditions - I have a pipe with fluid in that has a velocity of 1 metre per second, inside a steel block. I've set the fluid and solid regions using topoSet but I'm having trouble with my temperature, velocity and pressure fields. For some reason, velocity and pressure aren't restricted to the fluid region. Does anyone know why this might be happening? Should there be something that I change in changeDictionaryDict to prevent this from happening. Also, I'm trying to make one of the faces of the steel block hotter so it causes the pipe to heat unevenly. However, it doesn't appear to be having any effect despite paraFoam clearly showing me one face that is hotter than the rest.

Any help anyone can give me would be much appreciated!

[vabishek]

Originally Posted by BClarke352

Hi,

I'm also having trouble with some boundary conditions - I have a pipe with fluid in that has a velocity of 1 metre per second, inside a steel block. I've set the fluid and solid regions using topoSet but I'm having trouble with my temperature, velocity and pressure fields. For some reason, velocity and pressure aren't restricted to the fluid region. Does anyone know why this might be happening? Should there be something that I change in changeDictionaryDict to prevent this from happening. Also, I'm trying to make one of the faces of the steel block hotter so it causes the pipe to heat unevenly. However, it doesn't appear to be having any effect despite paraFoam clearly showing me one face that is hotter than the rest.

Any help anyone can give me would be much appreciated!

Hello Bruce,

It is hard to say what could be going wrong in your case without taking a look at the case files. It would make it a lot easier if you could attach a test case.

Based on the info you have provided, I think the issue might be with the "regionProperties" file in the constant/ directory. If the regions are not specified correctly in that file, it could lead to a situation where the fluid equations are solved in the solid region and vice versa. Check that file to make sure everything is correct.

I hope that helps!

[Ohlzen-Wendy]

Originally Posted by Ohlzen-Wendy

Hi everybody,

I make some progress regarding my calculation. therefore I set up a small test case. (
This one is running but I still have some questions I am not totally sure about.

If i introduce a heat transfer with a fixed power or flux on a patch between a fluid and a solid or a solid and a other solid - do i have to set the bc on both patches?

while chtMultiRegionFoam is running after some time the time step is decreased to something like 1e-13s. is there a way to track the maximum magnitude speed of the whole domain while the simulation is running?

best wishes

Andy

The case files for the OF-Case you find here:
https://drive.google.com/file/d/0B_I...ew?usp=sharing

[elham usefi]

Hi everybody. I am simulating a heat transfer problem with the modified chtMultiRegionSimpleFoam solver in which the fluid region is incompressible with force convection (modified) and the solid region is the same as original chtMRSF. When I simulate the fluid region alone with a fixed value or fixed gradient B.C. for temperature with buoyant bousinesqBoussinesqSimpleFoam I get sensible results with all the residuals under e-8. And the same goes for solid region only. But when I solve fluid and solid together with my modified solver and a “turbulent temperature coupled baffle mixed” B.C for temperature in the solid-fluid interface, energy residuals for fluid and solid cannot decrease less than e-4 and e-3, but still the results look sensible! I have tried different schemes and solvers and iteration numbers, but no progress. I guess the thing is with “turbulent temperature coupled baffle mixed” B.C but I can’t understand it well!
Another thing that I’ve found out is that when I increase the solid conductivity or decrease the fluid conductivity, the energy residuals for fluid decreases to e-6! but nothing happens for energy residuals for solid region! On the other hand, when I use an unsteady version of my solver, energy residuals decrease to e-5! Then the problem should be with laplacian term in fluid energy equation but I have tried every scheme! And I need to use the transient solver.

[vangelis]

Hi there
Just to mention that the latest ANSA v18.1.x supports the output of CHT openfoam cases. The user must create different Material and assign it to the corresponding volume properties. In this way ANSA will now how to output mesh for each fluid or solid zone.

Then the user should also set mappedwall boundary conditions on the surfaces between the different materials

[Fluid Tool]

Originally Posted by zfaraday

Hello!

Quick answer.

As for the coupling between regions for temperature, take a look at these BC's:

• turbulentTemperatureCoupledBaffleMixed
• turbulentTemperatureRadCoupledMixed

Regarding the volumetric heeat generation, take a look at this thread:
how-i-can-introduce-my-power-heat-w-chtmultiregionfoam.html

Hope it helps.

Best regards,

Alex

Hi Alex,

It was old topic but I want ask problem at heat flux on baffle between fluid and solid. I want to set heat flux on this face but it will not couple 2 volumes. is there way to set heat flux on coupling between regions?

Thanks

[JuRe09]

Originally Posted by vangelis

Hi there
Just to mention that the latest ANSA v18.1.x supports the output of CHT openfoam cases. The user must create different Material and assign it to the corresponding volume properties. In this way ANSA will now how to output mesh for each fluid or solid zone.

Then the user should also set mappedwall boundary conditions on the surfaces between the different materials

Thank you for this advise! Unfortunately in my case it is not working I have to volumes (mold and fluid) each with a different mat id (solid/fluid). Between the mold and melt lies a shell mesh (property: mappedWall)... Ansa just creates case files for a single region...


Do you have any suggestion what could be wrong. There is another thing i do not unterstand. Do I need for each region a surface mesh between the regions even though it would be exactly the same shape and surface? E.g. mappedWall: moldMelt and mappedWall: meltMold???


Thank you for your support. Iam a total newby in openFOAM...


Greetings
Julian