CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Coupled patches for heat transfer

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree3Likes
  • 1 Post By RaghavendraRohith
  • 2 Post By micpage18

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 7, 2015, 08:04
Default Coupled patches for heat transfer
  #1
Member
 
Rohith
Join Date: Oct 2012
Location: Germany
Posts: 57
Rep Power: 10
RaghavendraRohith is on a distinguished road
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
Attached Images
File Type: jpg coupled patch.jpg (24.1 KB, 146 views)
shohifafitriana likes this.

Last edited by RaghavendraRohith; May 7, 2015 at 09:04.
RaghavendraRohith is offline   Reply With Quote

Old   May 7, 2015, 08:59
Default
  #2
Member
 
Michael Page
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 36
Rep Power: 14
micpage18 is on a distinguished road
Hi,

Does your mesh is identical at the coupled patch?
__________________
Michael Page
michael.page@simu-k.com
Simu-K inc.
www.simu-k.com
micpage18 is offline   Reply With Quote

Old   May 7, 2015, 09:00
Default
  #3
Member
 
Rohith
Join Date: Oct 2012
Location: Germany
Posts: 57
Rep Power: 10
RaghavendraRohith is on a distinguished road
Hi,

Yes, it is identical with the same configuration.

Regards,
RRK
RaghavendraRohith is offline   Reply With Quote

Old   May 7, 2015, 10:35
Default
  #4
Member
 
Michael Page
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 36
Rep Power: 14
micpage18 is on a distinguished road
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,
__________________
Michael Page
michael.page@simu-k.com
Simu-K inc.
www.simu-k.com
micpage18 is offline   Reply With Quote

Old   May 8, 2015, 04:07
Default
  #5
Member
 
Rohith
Join Date: Oct 2012
Location: Germany
Posts: 57
Rep Power: 10
RaghavendraRohith is on a distinguished road
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
RaghavendraRohith is offline   Reply With Quote

Old   May 8, 2015, 08:45
Default
  #6
Member
 
Michael Page
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 36
Rep Power: 14
micpage18 is on a distinguished road
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,
__________________
Michael Page
michael.page@simu-k.com
Simu-K inc.
www.simu-k.com
micpage18 is offline   Reply With Quote

Old   June 3, 2015, 08:16
Default
  #7
Member
 
Rohith
Join Date: Oct 2012
Location: Germany
Posts: 57
Rep Power: 10
RaghavendraRohith is on a distinguished road
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
RaghavendraRohith is offline   Reply With Quote

Old   November 10, 2015, 15:18
Default
  #8
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Germany
Posts: 1,379
Rep Power: 27
akidess will become famous soon enough
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.
akidess is offline   Reply With Quote

Old   November 11, 2015, 03:14
Default
  #9
Member
 
Rohith
Join Date: Oct 2012
Location: Germany
Posts: 57
Rep Power: 10
RaghavendraRohith is on a distinguished road
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
RaghavendraRohith is offline   Reply With Quote

Old   November 13, 2015, 14:22
Default
  #10
Senior Member
 
Zeppo's Avatar
 
Sergei
Join Date: Dec 2009
Posts: 257
Rep Power: 18
Zeppo will become famous soon enough
Quote:
Originally Posted by RaghavendraRohith View Post
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.
So, did turbulentTemperatureCoupledBaffleMixed do the trick?
Zeppo is offline   Reply With Quote

Old   November 17, 2015, 02:35
Default
  #11
Member
 
Rohith
Join Date: Oct 2012
Location: Germany
Posts: 57
Rep Power: 10
RaghavendraRohith is on a distinguished road
Hi,

Sorry for a delayed Reply, Yes it works fine.


Best Regards,
Rohith
RaghavendraRohith is offline   Reply With Quote

Old   April 22, 2021, 11:39
Default
  #12
New Member
 
Shohifa Laili Fitriana
Join Date: Jan 2021
Location: Indonesia
Posts: 2
Rep Power: 0
shohifafitriana is on a distinguished road
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.
shohifafitriana is offline   Reply With Quote

Old   April 22, 2021, 11:41
Default
  #13
New Member
 
Shohifa Laili Fitriana
Join Date: Jan 2021
Location: Indonesia
Posts: 2
Rep Power: 0
shohifafitriana is on a distinguished road
Quote:
Originally Posted by RaghavendraRohith View Post
Hi,

Sorry for a delayed Reply, Yes it works fine.


Best Regards,
Rohith
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.
shohifafitriana is offline   Reply With Quote

Reply

Tags
coupled patches, heat and mass transfer, openfoam 2.2.x

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
problems after decomposing for running alessio.nz OpenFOAM 7 March 5, 2021 04:49
SigFpe when running ANY application in parallel Pj. OpenFOAM Running, Solving & CFD 3 April 23, 2015 14:53
Difficulty In Setting Boundary Conditions Moinul Haque CFX 4 November 25, 2014 17:30
chtMultiregionFoam--unequal temperature at coupled patches zakir hussain OpenFOAM 16 December 29, 2013 16:35
conjugate heat transfer - temperature at coupled patches maHein OpenFOAM Running, Solving & CFD 1 September 6, 2012 06:30


All times are GMT -4. The time now is 02:02.