Conjugate Heat transfer- Heat generating cylinder & natural convection
 

Hi to All OpenFoam Users,
I have setup case where it involves conjugate heat transfer with heat generation inside solid cylinder, which exchanges heat with fluid through natural convection. Whole set up can be found in attached tar file.

Problem with the results files is - centreline temperature of cylinder shows minimum temperature whereas it should be maximum. Temperature distribution is shown in given picture. I am not sure,where I am going wrong. It is kind request to you all, please help me in this regard .

Thanks.

Hello sandymech!

I cant tell exactly what could be the problem.

The simulation I attached works and is similar to yours.

- Allrun_Pre to generate the mesh.

- Allrun_CD to make the changing dictionaries.

- chtMultiRegionSimpleFoam is used as in your simulation

You are able to compare between the two simulations.

Tell me I it works and where is the mistake if you find it, let me be informed please :)

Regards

Peter

PS: I was not able to execute your simulation. please send a description how to do it!

PS2: the skewness of the fluid elements at the top and the bottom of the solid is very high in your simulation. I would not do it this way!

@PeterHess
 

Hi Peterhess
Thanks for your suggestions!

I could run your test case and it is working fine. I had simulated same case where rectangular domain as heat source. But I am facing problem when I replace rectangular domain to cylindrical domain as heat source. I will give you procedure to run my case after untar of files. I am attaching new tar files.

1. I have divided whole case into fluid and solid. Domain is of 3 dimensional cylindrical shape. Solid region is having heat generating source. I am not using symmetrical boundary conditions due to nature of the problem.
2. Heat generation source value can be changed at system/solid/fvOptions
3. Allrun script simulate whole case.
4. Allclean will clear all files which generated in simulation.

Now we will discuss about boundary conditions,
zeroGradient at boundary in fluid region (top,bottom,lateral) is not a problem for me. As it signifies, temperature will never reach steady state. I am ok with that.

Problem regarding the case- I am attaching snapshot of result file herewith, where it can be seen that centreline temperature is minimum, which should be maximum.


Let me know, if you have questions regarding running simulation.

Thanks once again.

Regards
Sandeep

Hello sandymech,

After some attempts I could successfully able to start your Simulation.

And I got the same results.

Increasing the relaxationFactors from 0.7 to 1 for h in system/solid/fvSolution fixes the problem you are trying to solve.

I dont understand why you put fvOptions in system/solid... this file belongs to constant/solid folder!

Let me stay informed please.

Regards

Peter

@PeterHess
 

Hi Peter
Sorry for late reply. I was trying to get access of cfdonline forum, but due to certain technical issue, I could not .Though I tried with forgot password, it didnt work. I had to make different account itself.

Anyway, thanks for your suggestion. I increased relaxation factor from 0.7 to 1 and also I changed path of fvOptions file to constant/solid from system/solid. It is working.

Thank you once again for your reply.

need help .
 

Hi !
I am working on exactly same kind of problem.


I have defined two regions: air and source.


But i also need: Inlet;Outlet; Side_wall.


The problem: while importing .stl files for snappyHexMesh, how do i combine the inlet, outlet, side_wall patches into "air region" ? I dont know how to club them so that their properties are similar to that of air.

Hello Aero!

Well, I am not sure if I understand your topic right way.

The bounding boundaries (inlet, outlet and other faces)are defined during blockMesh step.

After generating the mesh by snappyHexMesh you need to type:

splitMeshRegions -cellZones -overwrite

to separate the mesh generated by snappyHexMesh into the different regions.

And here you are getting the boundaries defined!

The boundaries defined during blockMesh (inlet, outlet and wall) are then imported automatically and named as in blockMesh.

The boundaries where the different regions are interact are then generated and named automatically by using splitMeshRegions.

Run the Test case I attached above by running:

Allrun_Pre

step by step to see the effect.

Anyway, the topoSet and then createPatch utilities could also be used to patch the patches manually if needed...

Regards

Peter