
[Sponsors] 
Record Heat Flux using chtMultiRegionFoam and turbulentTemperatureCoupledBaffleMixed 

LinkBack  Thread Tools  Display Modes 
October 2, 2015, 11:03 
Record Heat Flux using chtMultiRegionFoam and turbulentTemperatureCoupledBaffleMixed

#1 
New Member
Join Date: Jun 2015
Posts: 2
Rep Power: 0 
Right now I have a simple simulation with several different solid regions and a 'dummy' fluid region (which has not be developed yet). Right now, I am trying to establish the best way of recording/obtaining the heat flux between regions (namely solidtosolid at the moment).
At all of my interfaces I use turbulentTemperatureCoupledBaffleMixed since it allows for interfacial resistance to be coded in (something I need). My code runs fine, but I would like to be able to record the heat flux across the patches between regions. The most straightforward solution is using the wallHeatFlux utility, but the calculation is simply done using: Code:
surfaceScalarField heatFlux ( fvc::interpolate ( ( turbulence.valid() ? turbulence>alphaEff()() : thermo>alpha() ) )*fvc::snGrad(h) ); My question is, what is the best way to obtain the values calculated by turbulentTemperatureCoupledBaffleMixed? I noticed it creates the fields: Code:
makePatchTypeField ( fvPatchScalarField, turbulentTemperatureCoupledBaffleMixedFvPatchScalarField ); Code:
tmp<scalarField> myKDelta = kappa(*this)*patch().deltaCoeffs(); I'm in a little over my head and its hard to tell what fields are accessible and how to access them. If someone could point me the right direction, I'd be most appreciative. I haven't found the answer despite many different searches on this site. 

December 11, 2015, 09:14 

#2 
Member
Join Date: May 2015
Posts: 68
Rep Power: 4 
Did you find an answer to your question?
If so would you be so kind to share it with me 

December 11, 2015, 12:39 

#3 
New Member
Join Date: Jun 2015
Posts: 2
Rep Power: 0 
Not yet, but its primarily because I haven't been working on this side of my project lately. I'll update this thread if I establish anything.


December 22, 2015, 08:40 

#4  
Senior Member
Join Date: Sep 2013
Posts: 112
Rep Power: 6 
I think I am confused. Please check if I am correct. Let me begin by quoting Hrvoje Jasak from here.
Quote:
The first step is looking up the T field of the other region: nbrField... = ...TnbrName_ Afterwards we set this into the variable nbrIntFld and calculate the value the heat conduction kappa has in the other region and devide it by the celltocell distance which is the deltaCoeffs part. Code:
// Swap to obtain full local values of neighbour internal field tmp<scalarField> nbrIntFld(new scalarField(nbrField.size(), 0.0)); tmp<scalarField> nbrKDelta(new scalarField(nbrField.size(), 0.0)); if (contactRes_ == 0.0) { nbrIntFld() = nbrField.patchInternalField(); nbrKDelta() = nbrField.kappa(nbrField)*nbrPatch.deltaCoeffs(); } else { nbrIntFld() = nbrField; nbrKDelta() = contactRes_; } Code:
tmp<scalarField> myKDelta = kappa(*this)*patch().deltaCoeffs(); Code:
this>refValue() = nbrIntFld(); this>refGrad() = 0.0; this>valueFraction() = nbrKDelta()/(nbrKDelta() + myKDelta()); A few lines later in the debug options it reads Code:
scalar Q = gSum(kappa(*this)*patch().magSf()*snGrad()); You should however be able to extract the values with a codedfunctionobject (). One example of this here: Code:
functions ( pAverage { functionObjectLibs ("libutilityFunctionObjects.so"); type coded; redirectType average; outputControl outputTime; code #{ const volScalarField& p = mesh().lookupObject<volScalarField>("p"); Info<<"p avg:" << average(p) << endl; #}; } ); 

December 22, 2015, 09:50 

#5 
Senior Member
Alex
Join Date: Oct 2013
Posts: 334
Rep Power: 14 
Hi Stephan,
You seem to understand quite good the code behind turbulentTemperatureCoupledBaffleMixed BC, at least what you describe is ok so I don't know exactly what are your hesitations about it. Maybe, you are not totally aware of what refValue, rafGrad and valueFraction mean and how are they used in the calculations. If this is what you don't know, keep in mind that a boundary value is computed in OpenFOAM according to the expression below: Where f is the valueFraction, Tp the value of temperature at the patch and us the inverse value of the deltaCoeffs() function. Ti is the value at the cell center. To get a better understanding about how bounday conditions are specified in OpenFOAM you can take a look at this document, I wrote during my Master Thesis development. After reading it maybe you are able to understand better each variable defined in turbulentTemperatureCoupledBaffleMixed BC. Hope it helps. Besst 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! 

March 22, 2016, 09:36 

#6 
Member
matteo lombardi
Join Date: Apr 2009
Posts: 67
Rep Power: 10 
Dear all,
what I don't get is why the reference gradient is set to zero. I would have set it to nbrField.kappa(nbrField)*nbrField.snGrad() to match the neighbor heat flux Hope someone can help. Matteo 

March 22, 2016, 12:29 

#7 
Senior Member
Alex
Join Date: Oct 2013
Posts: 334
Rep Power: 14 
Hi Matteo,
Maybe the explanation comented out in the source code itself can help you. Below you can see the whole comment: Code:
// Both sides agree on //  temperature : (myKDelta*fld + nbrKDelta*nbrFld)/(myKDelta+nbrKDelta) //  gradient : (temperaturefld)*delta // We've got a degree of freedom in how to implement this in a mixed bc. // (what gradient, what fixedValue and mixing coefficient) // Two reasonable choices: // 1. specify above temperature on one side (preferentially the high side) // and above gradient on the other. So this will switch between pure // fixedvalue and pure fixedgradient // 2. specify gradient and temperature such that the equations are the // same on both sides. This leads to the choice of //  refGradient = zero gradient //  refValue = neighbour value //  mixFraction = nbrKDelta / (nbrKDelta + myKDelta()) Hope it helps. 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! 

March 22, 2016, 13:38 

#8 
Member
matteo lombardi
Join Date: Apr 2009
Posts: 67
Rep Power: 10 
Thank you very much for your quick answer!
the document is indeed very useful. I was trying to understand a bit more into deep the way this b.c. works because in my industrial multi solid case I have one of the solids whose temperature converges very slowly (approx. 5000 iterations, while for the other solids it takes around 1000). Have you experienced anything like this (slow solid temperature convergence)? Is there any trick to speed up solid convergence? I'm running steady simulation. In my case solid heat balance doesn't show any imbalance (residuals go down fairly well). It's just the coupling with the fluid around it that takes ages to converge... Best regards 

March 22, 2016, 13:52 

#9 
Senior Member
Alex
Join Date: Oct 2013
Posts: 334
Rep Power: 14 
The matter of the slow convergence of the chtMR solvers is a well known issue. Take a look at the thread below where some ways to speed up convergence are discussed.
conjugateheattransferslowsolidtemperatureconvergence Btw, as for the issue you mention of only one solid converging slowly, the convergence in solid regions depends on its physical properties too. Is there a big difference on its thermal conduction or density compared to the other solids? 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! 

March 22, 2016, 15:05 

#10 
Member
matteo lombardi
Join Date: Apr 2009
Posts: 67
Rep Power: 10 
Thanks,
Unfortunately i'm already using UR=1 for the solids and 0.95 for the fluid. Also for each iterations solid residuals go down very well so using more non orthogonal correction wouldn't make any difference. Why would you expect solid density to make some difference in a steady state simulation? Regards 

March 22, 2016, 17:12 

#11 
Senior Member
Alex
Join Date: Oct 2013
Posts: 334
Rep Power: 14 
What about the solver tolerances (relTol and tolerance)? Maybe you can lower them after the first iterations so as to get a better convergence (remember that in these kind of cases they should have very low values, somewhere in the forum I read a while ago that the recomended values for tolerance were around 1e10 or even lower!).
I think you are right, I checked the code and density seems not to have any influence on convergence for steady state cases. However, it is important to notice that the values of thermal conductivity (and probably heat capacity too) have a strong influence over the convergence time in this solver. Maybe you could even give a lower value to conductivity for the first time steps and then increase it to its desired value (I don't remember if the relation between conductivity and convergence velocity goes in this direction or in the opposite direction) in order to increase convergence velocity. Best regards
__________________
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! 

March 24, 2016, 09:33 

#12 
Member
matteo lombardi
Join Date: Apr 2009
Posts: 67
Rep Power: 10 
Dear Alex,
can you confirm that refGradient = zero gradient refValue = neighbour value mixFraction = nbrKDelta / (nbrKDelta + myKDelta()) can be derived just in the case of conformal mesh between the two sides? in this case the areas would be the same and so cancel on both sides of heat fluxes equation. In my opinion this relationship is no longer valid in case of non conformal interfaces. What do you think? Regards 

March 24, 2016, 11:30 

#13 
Senior Member
Join Date: Sep 2013
Posts: 112
Rep Power: 6 
Not quite. This is still true for non conformal meshes but the method to compute the values (marked below) needs to change.
Code:
refGradient = zero gradient refValue = neighbour value mixFraction = nbrKDelta / (nbrKDelta + myKDelta()) Code:
sampleMode nearestPatchFace; IMO though you should always make sure that your meshes are identical on coupled patches. Especially coupling patches of different sizes to one another should not be done. Interpolating can drastically reduce accuracy. SnappyHexMesh as well as commercial meshing programs like ansa do have options to make sure this is the case. And should be used! A good way to estimate these loses is to calculate the wallheatflux. A big difference between the two regions can easily be just because of poor interpolation. And your problem with slow convergence is something I had problems with when I started using these solvers. I suppose you have meshed your regions with tetrahedral elements? I experienced much quicker convergence on polyhedral meshes. If you are using ansa just use the convertToPoly button. If your mesh is already fine enough you can not see a difference between the results but convergence is progessing a lot faster from my experience. OpenFoam also offers the polyDualMesh utility to convert a tet mesh to polys. 

March 30, 2016, 15:27 

#14 
Member
matteo lombardi
Join Date: Apr 2009
Posts: 67
Rep Power: 10 
Thanks Bloerb,
I tried and having a conformal interface didn't help the convergence. Would you transform to poly the fluid, the solid region or both? Changing a bit topic: If I put anisotropic conductivity in one of my solid region I get to a converged solution but with non zero heat balance! The values of the heat fluxes at each boundary make sense (I get the same values on the solid and fluid sides). It's just the Total heat flux for the anisotropic solid region that is not zero! Something like 100W for a 1000W imposed heat rate. Changing schemes for sngrad (to corrected) or mesh didn't help. Does anybody have experience with anisotropic conductivities? Thanks a lot 

April 7, 2016, 17:23 

#15 
Senior Member
Join Date: Sep 2013
Posts: 112
Rep Power: 6 
If i understood you correctly your heat fluxes cancel out on coupled patches as they should, but the imposed heat flux on an exterior boundary is much higher than specified?
Please post how you specified your anisotropic conductivity, schemes and solution settings. Or even better upload everything without the mesh and I'll check. 

April 27, 2016, 01:35 

#16 
New Member
Volker
Join Date: Aug 2014
Location: Germany
Posts: 8
Rep Power: 4 
Hi there,
I have a comment/question related to heat conservation in the turbulentTemperatureCoupledBaffleMixed BC used by chtMultiRegionFoam. Possibly this is related to the heat balance problem stated above. Although this BC formally bases on equal heat flows on both sides, meanwhile I think that in practice the BC will not always operate strictly heat conservative. Within each time step, the fluid and solid regions are not solved in a common, big matrix but sequentially region by region. In chtMRF first the loop over all fluid regions is completed, followed by the loop over all solid regions. The first call of this BC is always done from the fluid side. Depending on kappa, mesh dimensions and time step, in the inner iterations of a time step the heat flow from the boundary may not only reach the face cell of the boundary, but also get deeper into the bulk cells of the fluid volume. As a consequence, a certain amount of heat will already be gone into the fluid bulk when the second call for this boundary patch from the solid side is done. The heat balance of the first iteration on the solid side is equal to the heat balance done at the final iteration of the fluid side (it does not look like that the solid side uses the old fluid temperature field from the previous time step for heat balance evaluation, right?). As stated above, this means that the difference between the first and the final iteration of the previous fluid side part of the heat balance will not be taken into account. Because a similar difference may occur on the solid side, too, some kind of compensation may take place so the actual error might be much smaller than the above amount of heat that already went into the bulk. I think the product of kappa (thermal conductivity) and deltaCoeffs() (=inverse distance from face cell center to boundary) should be the decisive quantity for the accuracy of the heat balance by the BC. If this product is equal on both sides, heat conservation will turn out close to perfect; otherwise it might however become poor depending on the difference of the product kappa*deltaCoeffs() on the fluid and the solid side. It would help me a lot if someone could clarify if there is an error in my considerations or if this BC in fact works as I suspect. Regards, Volker
__________________
I am quite new to everything here (OpenFOAM, CFD, C++) but I should have some idea of physics and (old) FORTRAN. 

April 27, 2016, 13:27 

#17 
Senior Member
Join Date: Sep 2013
Posts: 112
Rep Power: 6 
From my interpretation of the code this is correct.


April 29, 2016, 01:46 

#18 
New Member
Volker
Join Date: Aug 2014
Location: Germany
Posts: 8
Rep Power: 4 
Hi Bloerb,
Thanks for your confirmation. My C++ capabilities are growing but are still limited and so I have my doubts. My background to stumble on this issue is that I made a mass transfer BC based on the thermal BC. I used the thermal solver and BC as draft and more or less just replaced thermal conductivity by diffusion and temperature by concentration. Formally physics are quite the same and everything seemed more or less straightforward. As things started to look reasonable, I tried a quantitative mass balance. The quantitative results were less pleasant than the pretty ParaView colour graphs suggested and I tracked my problems through to the above issue. As my solid and fluid diffusivities differ by orders of magnitude this inaccuracy probably came out more obvious than in the original thermal BC. For now it looks like there is no further need to check my mass transfer BC for another programming mistake. Instead my present approach is to force the mass balance by calculating the mass transfer from fluid to solid only once per patch field in the fluid loop before the matrix solution and inner iterations start. The mass transfer from/to the solid neighbour is collected and written into an additional source term field that remains constant during a time step. For the corresponding call from the solid side in the same time step, the same but negative mass transfer from the fluid patch field is written into the opposite face cells of the corresponding source term field for the solid. This way a new mass transfer calculation on the solid side is avoided. The BC on both sides just sets this>valueFraction() = 0 and this>refGrad() = 0, so it practically acts as a "zeroGradient" BC. Consequently everything related to surface mass transfer between the regions is put into the equations via the opposite sign source term fields and therefore the mass balance should come out fine. Well, I think I will find out if it really does. Thanks again! Regards, Volker
__________________
I am quite new to everything here (OpenFOAM, CFD, C++) but I should have some idea of physics and (old) FORTRAN. 

June 18, 2016, 12:27 

#19  
New Member
Stephan Derkohlkopf
Join Date: Feb 2016
Posts: 2
Rep Power: 0 
Hello Matteo,
did you by any chance find out more about the strange behaviour of the tTCBM boundary when one or both sides are anisotropic? Quote:
Code:
thermoType { type heSolidThermo; mixture pureMixture; transport constAnIso; thermo hConst; equationOfState rhoConst; specie specie; energy sensibleEnthalpy; } coordinateSystem{type cartesian; origin (0 0 0); coordinateRotation { type STARCDRotation; rotation (0 0 0); }} mixture { specie { nMoles 1; molWeight 12; } transport { kappa (10 10 10); } thermodynamics { Hf 0; Cp 1000; } equationOfState { rho 3000; } } Thanks, Stephan 

Tags 
chtmultiregionfoam, heat flux, wallheatflux 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
ChtMultiRegionFoam heat flux  grmb7  OpenFOAM Running, Solving & CFD  0  June 24, 2015 21:00 
define new heat transfer coefficient in ChtMultiRegionFoam  tjliang  OpenFOAM Programming & Development  0  May 15, 2015 05:42 
chtMultiRegionFoam connection between solid and fluid region of heat exchanger  ahab  OpenFOAM  0  March 2, 2015 13:19 
Heat Flux boundary conditions with groovyBC for chtMultiRegionFoam with solids only  Kumudu  OpenFOAM PreProcessing  7  August 23, 2014 14:33 
chtMultiRegionFoam heat flux  sailor79  OpenFOAM Running, Solving & CFD  0  September 27, 2013 08:08 