|
[Sponsors] |
May 7, 2015, 09:04 |
Coupled patches for heat transfer
|
#1 |
Member
Rohith
Join Date: Oct 2012
Location: Germany
Posts: 57
Rep Power: 14 |
Hi All,
Does someone have an idea of defining heat transfer boundary or B.C on a coupled patch in contact with an other mesh. I have gone through the Cht multiregion foam it didnot help me. I basically want to define a heat transfer boundary condition using something like baffle which i have used. What would be a relevant b.C for a coupled patch ? baffle or something else? I have also gone through some solvers with fluid and solid heat transfer but the results are still not satisfactory. The temperature increases non physically. thanks in advance RRK Last edited by RaghavendraRohith; May 7, 2015 at 10:04. |
|
May 7, 2015, 09:59 |
|
#2 |
Member
Michael Page
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 36
Rep Power: 17 |
Hi,
Does your mesh is identical at the coupled patch? |
|
May 7, 2015, 10:00 |
|
#3 |
Member
Rohith
Join Date: Oct 2012
Location: Germany
Posts: 57
Rep Power: 14 |
Hi,
Yes, it is identical with the same configuration. Regards, RRK |
|
May 7, 2015, 11:35 |
|
#4 |
Member
Michael Page
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 36
Rep Power: 17 |
In this case, standard settings from tutorials must work:
1- Create or import your meshes; 2- Use splitMeshRegions -cellZones -overwrite to define the regions; 3- Modify the polymesh/boundary file of each region to use type mappedWall at mesh connexions 4- For temperature boundary conditions, use type compressible::turbulentTemperatureCoupledBaffleMix ed I have used these settings with chtMultiRegionSimpleFoam for a heat exchanger and I got a good agreement with experimental values. Best regards, |
|
May 8, 2015, 05:07 |
|
#5 |
Member
Rohith
Join Date: Oct 2012
Location: Germany
Posts: 57
Rep Power: 14 |
Hi Micheal,
First of all thanks for your detailed info. But! My problem is a little complex than chtMultiRegionFoam, despite being familiar with multiple mesh techniques, i have found myself in a pot hole as, the thing i would need is exactly a heat transfer or patch boundary in order to enhance the diffusion of heat into the mesh2 from mesh1. This may be also possible with chtMultiRegionfoam but the major problem would the mesh refinement. If in case, i want to refine the inner region (mesh1), it would be a strenuous or an impossible task. Best Regards, RRK |
|
May 8, 2015, 09:45 |
|
#6 |
Member
Michael Page
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 36
Rep Power: 17 |
If I understand your problem, you want both sides coupled with different meshes. If this is the case, you can use the sampleMode nearestPatchFaceAMI. Here's a discussion about that:
chtmultiregionfoam-different-mesh-2-sides-coupled-boundary If not, can you give more explanation of your problem? Best regards, |
|
June 3, 2015, 09:16 |
|
#7 |
Member
Rohith
Join Date: Oct 2012
Location: Germany
Posts: 57
Rep Power: 14 |
Hi Micheal,
Let me put you this on a very simple note. My Mesh 1 is solid in the beginning but changes its state to liquid due to the heat input from mesh 2 from the coupled patch. Both mesh1 and mesh2 have incompressible fluids, so the B.C. compressible::turbulentTemperatureCoupledBaffleMix ed; is not valid in my case. I cant use the chtMultiRegionFoam because my solid in mesh1 temperature equation is very different from the original. On a straight hit, I may need a heat transfer patch B.C. for an incompressible which allows heat transfer between two meshes which just works like compressible::turbulentTemperatureCoupledBaffleMix ed;. newton law of cooling (fvOptions.H) may not work because the overlapping area is 0. between the meshes. Thanks in Advance, Best Regards, RRK |
|
November 10, 2015, 16:18 |
|
#8 |
Senior Member
Anton Kidess
Join Date: May 2009
Location: Germany
Posts: 1,377
Rep Power: 30 |
RaghavendraRohith, perhaps you already know this by now, but nothing in compressible::turbulentTemperatureCoupledBaffleMix ed is specifically tuned to compressible or turbulent flows.
__________________
*On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer. |
|
November 11, 2015, 04:14 |
|
#9 |
Member
Rohith
Join Date: Oct 2012
Location: Germany
Posts: 57
Rep Power: 14 |
Hi Anton,
Thank you for your reply. Ya, i have found it, i have done it using compressible and incompressible coupling which worked fine. I have managed somehow to get it right. Thank you once again. BR, Rohith |
|
November 13, 2015, 15:22 |
|
#10 |
Senior Member
Sergei
Join Date: Dec 2009
Posts: 261
Rep Power: 21 |
||
November 17, 2015, 03:35 |
|
#11 |
Member
Rohith
Join Date: Oct 2012
Location: Germany
Posts: 57
Rep Power: 14 |
Hi,
Sorry for a delayed Reply, Yes it works fine. Best Regards, Rohith |
|
April 22, 2021, 12:39 |
|
#12 |
New Member
Shohifa Laili Fitriana
Join Date: Jan 2021
Location: Indonesia
Posts: 2
Rep Power: 0 |
RaghavendraRohith. so do you stick to the "compressible :: turbulentTemperatureCoupledBaffleMix" type for your incompressible simulation?
I have the same simulated case as you . I am use OF 8. |
|
April 22, 2021, 12:41 |
|
#13 | |
New Member
Shohifa Laili Fitriana
Join Date: Jan 2021
Location: Indonesia
Posts: 2
Rep Power: 0 |
Quote:
I have the same simulated case as you . I am use OF 8. |
||
August 30, 2021, 09:24 |
|
#14 | |
New Member
Join Date: Aug 2020
Posts: 7
Rep Power: 6 |
Quote:
Hi I too have the same doubt. Hope you might have solved your doubt by now. If so, pls shed light. Thanks in advance |
||
Tags |
coupled patches, heat and mass transfer, openfoam 2.2.x |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
problems after decomposing for running | alessio.nz | OpenFOAM | 7 | March 5, 2021 05:49 |
SigFpe when running ANY application in parallel | Pj. | OpenFOAM Running, Solving & CFD | 3 | April 23, 2015 15:53 |
Difficulty In Setting Boundary Conditions | Moinul Haque | CFX | 4 | November 25, 2014 18:30 |
chtMultiregionFoam--unequal temperature at coupled patches | zakir hussain | OpenFOAM | 16 | December 29, 2013 17:35 |
conjugate heat transfer - temperature at coupled patches | maHein | OpenFOAM Running, Solving & CFD | 1 | September 6, 2012 07:30 |