
[Sponsors] 
How to model transient conduction between two solids? 

LinkBack  Thread Tools  Search this Thread  Display Modes 
August 21, 2014, 18:40 
How to model transient conduction between two solids?

#1 
New Member
Cliff
Join Date: Aug 2014
Posts: 10
Rep Power: 11 
Hello,
I have been trying to learn OpenFOAM on my own for a couple weeks now. As a test case to educate myself, I would like to model the transient case for heat transfer between two different solids. I have gone through the multiRegionHeater tutorial and understand it OK (except that I get poor heat transfer when there is no forced fluid flow, but never mind for now). To better learn heat transport using OpenFOAM I have generated a simple test case. I have successfully used the blockMeshDict and topoSetDict to generate two solid cubes (leftSolid and rightSolid). The leftmost patch has a fixedValue of 300K and the rightmost patch has a fixedValue of 500K. The other boundaries are zeroGradient in temperature and the internal temperature starts at 300K. Should be easy right? Sigh... I have attempted to solve this using chtMultiRegionFoam without success (I can successfully model one solid block using laplacianFoam). If I have no fluids in the regionProperties, I get the following in the chtMultiRegionFoam log: [0] > FOAM FATAL ERROR: [0] fluid not found in table. Valid entries: 1(solid) I would be so grateful for some guidance on how to model transient conduction between two solids. Here is a dropbox link to my files. The OpenFOAM v2.3 code is adapted from the multiRegionHeater where now heater, topAir and bottomWater are not used. https://www.dropbox.com/sh/1fxb42g1b...92kKyZgha?dl=0 cheers, Cliff Last edited by cliffdub; August 23, 2014 at 16:39. Reason: to add a dropbox link to files 

August 24, 2014, 16:38 

#2 
Member
Kumar
Join Date: Jun 2013
Posts: 43
Rep Power: 12 
Hello,
I did a similar problem in a very similar way some time ago with an older version of OF. It ran without problems. If you are interested, I can look up those files. kumar 

August 25, 2014, 22:51 

#3 
New Member
Cliff
Join Date: Aug 2014
Posts: 10
Rep Power: 11 
Thank you Kumar. I have it working now. I needed to leave the fluid list empty instead of deleting it all together. Thanks for offering to help.


September 5, 2014, 21:18 

#4 
New Member
Ahmed
Join Date: Jul 2014
Posts: 4
Rep Power: 11 
hi cliff
I ve the same problem, but when I start to solve the following message appears: no finite volume options present. any ideas? thanks 

September 18, 2014, 05:19 

#5 
New Member
Nithish
Join Date: Sep 2013
Location: Erlangen,Germany
Posts: 20
Rep Power: 12 
I had the same problem. Just ignore it.


May 28, 2015, 06:10 
Transient heat conduction between two solids

#6  
New Member
Camila Braga Vieira
Join Date: Apr 2012
Posts: 9
Rep Power: 13 
Quote:
I am interested in checking you testcase. I am trying to solve a transient heat conduction case in two solids (top solid with internal heat source; bottom solid  without heat source), by using he chtMultiregionFoam. However, I am not familiar with this solver and I am getting difficulty to set up correct the case. May you please help me. Thank you very much, Camila 

May 28, 2015, 06:33 

#7 
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 20 
Hi Camila,
I recomend you to take a look into the following tutorial case that you can find in the tutorials directory within your OpenFOAM installation directory: Code:
$FOAM_TUTORIALS/heatTransfer/chtMultiRegionFoam/multiRegionHeater Once you have done it, if you still have doubts or problems running multiRegion cases (you'll likely still have some doubts), you can come back here and ask them and I will be pleased (if I have the time) to help you! Best regards, Alex
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in! 

May 28, 2015, 10:16 
Transient heat conduction between two solids

#8 
New Member
Camila Braga Vieira
Join Date: Apr 2012
Posts: 9
Rep Power: 13 
Thank you very much.
I have run the planewall2D, but I still have some doubts. In my simulation case, I have to specify an interface between the two solids, so that the temperature and heat flux are the same in that patch. My doubts are mainly concerned the interface treatment and how can I check the heat flux through the interface. So far I have tried to understand the "turbulentTemperatureCoupledBaffleMixed", which should be applied for a temperature and flux continuity boundary condition (BC), as it is in my case, but I could not understand, by looking at the .C file, how the condition of same temperature and heat flux is kept by that BC. Would you know a reference that explains better how an interface patch is treated in OpenFOAM? I will be very grateful to receive your help. Thank you, Camila 

May 28, 2015, 11:11 

#9 
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 20 
Ok, I will give you a little help with this. In OpenFOAM boundary fields are calculated as
where "refValue" and "refGrad" are the value and the gradient taken as reference values. "f" is a fraction that switches the boundary condition between a Dirichlet BC (f=1) and a Neumann BC (f=0). is the center patch face to center cell distance and is the temperature in the cell center. Knowing that theory behind the specification of BC's in OpenFOAM now we have to take a look at the source code to know what they are doing. Below you can see a snipet of the turbulentTemperatureCoupledBaffleMixed BC, namely the lines 241245 Code:
this>refValue() = nbrIntFld(); this>refGrad() = 0.0; this>valueFraction() = nbrKDelta()/(nbrKDelta() + myKDelta()); Code:
if (contactRes_ == 0.0) { nbrIntFld() = nbrField.patchInternalField(); nbrKDelta() = nbrField.kappa(nbrField)*nbrPatch.deltaCoeffs(); } else { nbrIntFld() = nbrField; nbrKDelta() = contactRes_; } mpp.distribute(nbrIntFld()); mpp.distribute(nbrKDelta()); tmp<scalarField> myKDelta = kappa(*this)*patch().deltaCoeffs(); Note that the subscript nbr indicates that values are taken from the neighbouring zone. To the reader concerns the developement of the equations in order to understand how the BC is implemented. Hope it helps, Alex
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in! 

May 28, 2015, 11:26 
Transient heat conduction between two solids

#10 
New Member
Camila Braga Vieira
Join Date: Apr 2012
Posts: 9
Rep Power: 13 
Thank you Alex. It really helped me to better understand how this BC works.


May 28, 2015, 16:33 

#11 
Member
Kumar
Join Date: Jun 2013
Posts: 43
Rep Power: 12 
Hi Camila,
In case you still want this, here is a simple example of a composite slab (no fluid regions present). I was just studying heat conduction with chtMultiRegion solvers  the domain is sliced into two equal halves using topoSet feature, designated solidleft and solidright. The left boundary (of solidleft) is fixed at 600 K and the right boundary (of solidright) is modeled with a groovyBC to simulate the heat loss through mixed convection and radiation. You can as well comment out the groovy and instead use the externalWallHeatFluxTemperature to model only convection. kumar 

June 3, 2015, 05:56 
Transient heat conduction between two solids

#12 
New Member
Camila Braga Vieira
Join Date: Apr 2012
Posts: 9
Rep Power: 13 
Thank you Alex and Kumar for helping me to deal with this problem. I am still trying to set up correctly my simulation case, since I am getting some errors in the check mesh topology (probably because of the interface), but as soon as I advance, I will let you know my progress.


December 14, 2015, 08:29 

#13 
Member

Hi Alex,
Thanks for those details. Can you please tell me what the \lambda stand for ? Also, I have a few questions:  I don't understand the use of the refGrad parameter. How do we set this value ?  You stated Ti as being the value at the centre of the cell, but is not supposed to be the temperature at the interface ? (Meaning, between Tb and Tb', in which case it would be the temperature on the face separating the two baffles)  One last thing, where can we specify the "f" parameter (switch from Dirichlet to Neumann) ? Thank you so much for your help ! 

December 14, 2015, 09:05 

#14  
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 20 
Quote:
I will respond quickly to your questions.
You are welcome. Best regards, Alex PS/tip: in this document you will find the solution for the procedure to solve your main doubts... Again, you are welcome!
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in! 

December 15, 2015, 12:32 

#15 
Member

Hi again Alex,
Sorry for my late reply ! I thank you so much for your very valuable input, I think I've got everything I needed. Your help is very appreciated. Best regards, Fouad 

December 13, 2016, 08:27 

#16  
New Member

Quote:
In boundary conditions turbulenttemperaturecoupledbafflemixed, how can I make the temperature and heat flux keep the same for the conjugate boundaries ? With the utility of wallHeaFlux, I found the heat flux was different for the conjugate boundaries. It confused me. 

Tags 
chtmultiregionfoam, conduction, conjugate heat transfer, heat transfer 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
chtMultiRegionFoam, conduction with a contact resistance between two solids  romain.h  OpenFOAM Running, Solving & CFD  1  October 8, 2013 01:25 
Running transient for turbulence model in FLUENT  phamhoanghuyphuocloi  FLUENT  0  June 9, 2013 21:33 
help on a convective heat transfer transient model  cmbv  FLUENT  0  December 14, 2007 17:16 
conduction between 2 different solids  matt  FLUENT  5  November 9, 2006 08:57 