[sahm]

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.

[ahmmedshakil]

Originally Posted by sahm

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.

Hi Sahm,
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

[zfaraday]

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

[sahm]

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 solid-gas 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]

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:

--> FOAM FATAL IO ERROR: 
Unknown patchField type convectiveHeatFlux for patch type patch

Valid patchField types are : ...

I have attached my solver and boundary condition and a case file test that I am using to check and validate my boundary condition.

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 Solid-Gas Reactor solver.

Ali.

[sahm]

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]

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 : 1.7.0-5773603db906
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/OpenFOAM-1.7.0/src/finiteVolume/lnInclude/newFvPatchField.C at line 110.

FOAM exiting

[alexeym]

Hi,

You do not need template class cause your BC is only applicable to scalars. If you try to:

1. Uncomment

#ifdef NoRepository
#   include "convectiveHeatFluxFvPatchField.C"
#endif

2. Change in Make/files convectiveHeatFluxFvPatchField.C to convectiveHeatFluxFvPatchFields.C

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.

[sahm]

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.

[ziadkhan]

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 ?"

[Naresh yathuru]

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

[sahm]

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(Ts-To)which is similar to pure convection and you can define it in groovyBC as ahmmedshakil mentioned it.

SAHM.

[zfaraday]

Hi Naresh!

Originally Posted by Naresh yathuru

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

You don't need to use chtMultiRegionFoam because as Sahm pointed out you can use groovyBC in order to create a BC that takes into account a solid wall that releases heat to the environment by convection. However, it already exists a BC implemented in OF that does exactly the same, this is the BC, called externalWallHeatFluxTemperature, that allows you to define a convective heat transfer coeff. and an environment temperature and, also, a thickness and a thermal conductivity for an external layer.

Hope it helps.

Best regards,

Alex

[Naresh yathuru]

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(Ts-To)which is similar to pure convection and you can define it in groovyBC as ahmmedshakil mentioned it.

Thanks for the reply sahm and alex.

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.

{
        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"
    }

[Naresh yathuru]

Hi Alex,

You don't need to use chtMultiRegionFoam because as Sahm pointed out you can use groovyBC in order to create a BC that takes into account a solid wall that releases heat to the environment by convection. However, it already exists a BC implemented in OF that does exactly the same, this is the BC, called externalWallHeatFluxTemperature, that allows you to define a convective heat transfer coeff. and an environment temperature and, also, a thickness and a thermal conductivity for an external layer.

Thanks a lot for the suggestion. you are exactly correct. I m using buoyantboussinesqsimpleFoam. I read in some threads that externalwallheatFluxtemperature B.C works for compressible solver as mine is a incompressible case, i didnt use it. or can i use it for incompressible?

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))*(Tout-Tsurface)
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.cfd-online.com/Forums/ope...acianfoam.html

sorry for the long text Thank you once again.

Regards
Naresh

[sahm]

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(T-T_inf) = 0.
Or probably it's like:
(K.∇T).n + h(T-T_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.