
[Sponsors] 
January 25, 2015, 03:56 
Convection as boundary condition.

#1 
Senior Member
Seyyed Ali H.M.
Join Date: Nov 2009
Location: Utah
Posts: 107
Rep Power: 14 
Hello
I am trying to solve heat diffusion in a solid with convection as one of the boundary conditions. Can someone tell me which boundary condition does the convective cooling? h*(T_s  T_inf) where h and T_inf are defined as the boundary condition. I know this not fixed gradient, but don't know which other boundary conditions can define this equation. Thanks.
__________________
SAHM 

January 25, 2015, 08:48 

#2  
Senior Member
Mohammad Shakil Ahmmed
Join Date: Oct 2012
Location: AUS
Posts: 136
Rep Power: 12 
Quote:
The boundary condition you explained is the Robin Boundary condition. You can easily impose that boundary condition using groovyBC (https://openfoamwiki.net/index.php/Contrib/groovyBC). The pdf file here, http://www.modlab.lv/docs/2011/OpenF...Vilums_pdf.pdf, explains how to use it. I guess, now you can solve your problem easily. Cheers shakil 

January 25, 2015, 10:38 

#3 
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 19 
Hello,
Even though what Mohammad says is true, OF actually has a BC for convective heat flux defined out of the box. This BC is called externalWallHeatFluxTemperature. You can find more info about this BC HERE. 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! 

January 26, 2015, 17:02 
Any other form of this boundary condition?

#4 
Senior Member
Seyyed Ali H.M.
Join Date: Nov 2009
Location: Utah
Posts: 107
Rep Power: 14 
Hi
I checked the externalWallHeatFluxTemperature boundary condition and it is what I want, but there's a problem with my case: I defined a solver that models solidgas reaction inside a solid porous medium. I defined temperature and pressure fields independent of OpenFOAM's thermophysical models, therefore I can not use externalWallHeatFluxTemperature and I need a simpler solution. I have groovyBC installed, so maybe that would help with my solver, or I have to define a simple external convection boundary condition for my own solver. Thanks for help.
__________________
SAHM 

February 11, 2015, 20:56 
First try:

#5 
Senior Member
Seyyed Ali H.M.
Join Date: Nov 2009
Location: Utah
Posts: 107
Rep Power: 14 
HeLlO FOAMers.
I checked the solution Mohammed mentioned and unfortunately there's a problem with my case and that solution. In his solution we have to define K (thermal conductivity) within the groovyBC boundary condition that we define. However in my code K is variable and changes with reaction progress. Therefore I couldn't use groovyBC. But I tried to make a boundary condition based on this solution. I defined a convectiveHeatFlux boundary condition as a separate library and it compiles, but when I try to run the case (even though I included the library in my controlDict file) I get this error: Code:
> FOAM FATAL IO ERROR: Unknown patchField type convectiveHeatFlux for patch type patch Valid patchField types are : ... I would appreciate if anyone could help me to resolve the error with this boundary condition. This might be the last step I have to solve to use this solver for my SolidGas Reactor solver. Ali.
__________________
SAHM 

February 12, 2015, 07:09 

#6 
Senior Member
Seyyed Ali H.M.
Join Date: Nov 2009
Location: Utah
Posts: 107
Rep Power: 14 
I forgot to mention, I tried using this boundary condition as static next to my solver and still got the same error message. I also tried to use generic patch fields lib in the controlDict file, but that gave another error message.
__________________
SAHM 

February 12, 2015, 09:38 

#7 
Senior Member
Seyyed Ali H.M.
Join Date: Nov 2009
Location: Utah
Posts: 107
Rep Power: 14 
This is the full error message:
/**\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 1.7.0   \\ / A nd  Web: www.OpenFOAM.com   \\/ M anipulation   \**/ Build : 1.7.05773603db906 Exec : SGReactFOAM Date : Feb 12 2015 Time : 06:54:00 Host : cmtl.mie.uic.edu PID : 21801 Case : /home/sahm/My/ConvectionTest nProcs : 1 SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Reading Reactor Properties Reading field P Reading field T > FOAM FATAL IO ERROR: Unknown patchField type convectiveHeatFlux for patch type patch Valid patchField types are : 41 ( advective buoyantPressure calculated cyclic directMapped directionMixed empty fan fixedFluxPressure fixedGradient fixedInternalValue fixedPressureCompressibleDensity fixedValue freestream freestreamPressure inletOutlet inletOutletTotalTemperature mixed oscillatingFixedValue outletInlet partialSlip processor rotatingTotalPressure sliced slip symmetryPlane syringePressure timeVaryingMappedFixedValue timeVaryingMappedTotalPressure timeVaryingTotalPressure timeVaryingUniformFixedValue timeVaryingUniformInletOutlet totalPressure totalTemperature turbulentInlet turbulentIntensityKineticEnergyInlet uniformDensityHydrostaticPressure uniformFixedValue waveTransmissive wedge zeroGradient ) file: /home/sahm/My/ConvectionTest/0/T::boundaryField::ConvectionWall from line 38 to line 41. From function fvPatchField<Type>::New(const fvPatch&, const DimensionedField<Type, volMesh>&, const dictionary&) in file /home/sahm/OpenFOAM/OpenFOAM1.7.0/src/finiteVolume/lnInclude/newFvPatchField.C at line 110. FOAM exiting
__________________
SAHM 

February 12, 2015, 10:42 

#8 
Senior Member

Hi,
You do not need template class cause your BC is only applicable to scalars. If you try to: 1. Uncomment Code:
#ifdef NoRepository # include "convectiveHeatFluxFvPatchField.C" #endif You'll see that compiler is VERY unhappy about your desire to divide by tensor. So make simple convectiveHeatFluxScalarFvPatchField instead of template. Also if you look at makePatchFields macro, you'll see why patch classes end with FvPatchField. Last edited by alexeym; February 12, 2015 at 13:03. Reason: typo 

February 12, 2015, 11:45 

#9 
Senior Member
Seyyed Ali H.M.
Join Date: Nov 2009
Location: Utah
Posts: 107
Rep Power: 14 
Thanks Alexey.
1 What is that section for? Can you give a short description or a link to a page that describes it. (I'm not good at programming) 2 I tried to make this BC again from inletoutletTotalTemperatureFvPatchScalarField (because it was only scalar) and it worked. Then I changed the constructors and subroutines from my old files. It is working now, but I have to verify and make sure it works properly. When I wasn't addressing convectiveHeatFluxFvPatchFields.C file in my Make/files, is the #include "addToRunTimeSelectionTable.H" the reason that it wasn't recognizing my BC? Thanks for telling me about the makePatchFields macro. I don't know about it, but surely I will take a look at it.
__________________
SAHM 

February 12, 2015, 13:01 

#10 
New Member
ziad khan
Join Date: Feb 2015
Posts: 9
Rep Power: 8 
hifi talk is on...
.... this reminds me of my fluid mechanics instructor raising his brows on me and giving a strange embarrasing look on his face at me when during his lecture i suddenly stopped and asked him " sir what does CONTINUITY mean ?" 

March 26, 2015, 04:57 

#11 
Member
Naresh Yathuru
Join Date: Feb 2015
Posts: 66
Rep Power: 8 
Hi Foamers,
thanks every one for the explanation. and sorry for restarting the thread again. I have read some threads regarding convection boundary conditions. but still could not catch it exactly. i have some basic question i might sound silly .I have a room assume one side of the room(right wall) is expossed to environment t= 260k .so in this case can I had to use a boundary condition that is similaar to convective boundary condition in fluent. that is it considers the wall thickness and temperature of outside and thermal conductivity of the solid. so my question 1. should i to use chtmultiregionFoam solver as i have thermal conductivity? 2. can i use the groovyBC suggested in any heat transfer solver? I really appriciate any tipps on this. Thank you Regards, Naresh Yathuru 

March 27, 2015, 03:28 

#12 
Senior Member
Seyyed Ali H.M.
Join Date: Nov 2009
Location: Utah
Posts: 107
Rep Power: 14 
Hi Naresh
I think you can use groovyBC. If you combine the conduction resistance with the convection resistance and get a total heat transfer coefficient (U) for each wall, the boundary condition will be in the form of q"=U(TsTo)which is similar to pure convection and you can define it in groovyBC as ahmmedshakil mentioned it. SAHM.
__________________
SAHM 

March 27, 2015, 09:07 

#13  
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 19 
Hi Naresh!
Quote:
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 27, 2015, 10:25 

#14  
Member
Naresh Yathuru
Join Date: Feb 2015
Posts: 66
Rep Power: 8 
Quote:
I tried with the groovey boundary condition. i m a newbie so i m not sure if i specified every thing correct. could someone please have a loook at it. Code:
{ type groovyBC; variables "htot=1.5625;Tout=273;heatflux=htot*(Tout  T);"; // lambda(thermal conductivity of a brick) gradientExpression "heatflux"; // 1/hout =1/25=0.04 valueExpression "Tout"; // htot=1.0/(0.04 + (thickness/lambda));lambda=0.5;thickness= 0.5; fractionExpression "0" } 

March 27, 2015, 10:58 

#15  
Member
Naresh Yathuru
Join Date: Feb 2015
Posts: 66
Rep Power: 8 
Hi Alex,
Quote:
if so could you please help me what are the changes is should to implement it for incompressible case. But one small clarification, i have a room with one wall(assume right wall) exposed to environment. and i m interested in the convection inside the room. I want to simulate the room taking into accout the environment temperature(Toutside), convective heat transfer coeff of the environment, and thermal condictivity and thickness of the wall. so i impose a heatflux B.C on the right wall. q=(1/(1/hout)+(d/lambda))*(ToutTsurface) hout heat transfer coeffiecient of the environment fluid lambda thermal conductivity of the wall d thickness of the wall according to this i have set my groovyB.C. i m a newbie to groovyB.C . i have posted my groovyB.C above. i followed this thread. http://www.cfdonline.com/Forums/ope...acianfoam.html sorry for the long text Thank you once again. Regards Naresh 

August 28, 2017, 15:31 

#16 
Senior Member
Seyyed Ali H.M.
Join Date: Nov 2009
Location: Utah
Posts: 107
Rep Power: 14 
Salam Mohammed,
I have a question regarding defining convection as a boundary condition. Thanks to you guys, I have been able to make a convective boundary condition for my solver and it has been working properly since. However my problem became more complicated. I have to change the thermal diffusion equation in my problem to become anisotropic (orthotropic) and because of that, I need to change the way boundary condition works. Now the boundary condition equation is more like: (K.n).∇T + h(TT_inf) = 0. Or probably it's like: (K.∇T).n + h(TT_inf) = 0. (To be honest I'm not sure yet.) K is thermal conductivity tensor, n is vector normal to boundary, h is convective heat transfer coefficient. Now, how can I make this in OpenFOAM Using mixedFVPatchField, since the fraction constant can't be derived like before. Can I define the gradient of T in mixedFVPatchField? Reminder, I can't use GroovyBC because my K and h change over time. Thanks.
__________________
SAHM 

Tags 
boundary condition, coefficient, convection, diffusion 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
An error has occurred in cfx5solve:  volo87  CFX  5  June 14, 2013 18:44 
Low Mixing time Problem  Mavier  CFX  5  April 29, 2013 01:00 
Convection Boundary condition  tomcatbobby  FLUENT  2  April 30, 2012 14:50 
asking for Boundary condition in FLUENT  Destry  FLUENT  0  July 27, 2010 01:55 
RPM in Wind Turbine  Pankaj  CFX  9  November 23, 2009 05:05 