# uniform heating of fluid region

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

 March 31, 2010, 13:09 uniform heating of fluid region #1 Member   santhosh Join Date: Apr 2009 Location: India Posts: 68 Rep Power: 8 Hi, I am using bousinesqBuoyantSimpleFoam to model a heat exchager. I would like to give uniform heating to whole fluid region as a source term (volumetric heating in W/m^3). Can anybody suggest me how to do this in OpenFOAM. Regards Santhosh.

 April 5, 2010, 06:29 Doubt regd TEqn.H #2 Member   santhosh Join Date: Apr 2009 Location: India Posts: 68 Rep Power: 8 I am looking at the TEqn.H in boussinesqBuoyantSimepleFoam. following is snippet copied from the above file. Code: ```fvScalarMatrix TEqn ( fvm::div(phi, T) - fvm::Sp(fvc::div(phi), T) - fvm::laplacian(kappaEff, T) );``` Can anybody tell me what is the need of second term Code: `fvm::Sp(fvc::div(phi), T)` according to following relation Code: `div(sV) = sdiv(V)+V.grad(s)` (s is scalar and V is vector). Combination of first two terms will results in the following, Code: `phi.gradT` Can anybody help me understanding these equations. I am finally trying to find heat source term in the equation so that I can specify uniform heating thoughout the fluid region. Regards Santhosh.

 April 6, 2010, 06:52 #3 Member   santhosh Join Date: Apr 2009 Location: India Posts: 68 Rep Power: 8 I have added the source term in the TEqn.H as below. Code: ```fvScalarMatrix TEqn ( fvm::div(phi, T) - fvm::Sp(fvc::div(phi), T) - fvm::laplacian(kappaEff, T) - Q/(rho0*cp0) );``` I have compiled and run the some simple test case. I have not yet seen the results just run completed successfully. I will post back if there is any other alternative. Regards Santhosh

 April 7, 2010, 11:09 #4 New Member   Oli Join Date: Apr 2009 Posts: 27 Rep Power: 8 That sounds interesting. Please let us know, if you have some results. Regards.

 May 11, 2010, 01:10 #5 Member   santhosh Join Date: Apr 2009 Location: India Posts: 68 Rep Power: 8 Hi Oli, That seems to be working, I am solving very big heat exchanged problem, As for as residuals and priliminary results I am not facing any major problem (Compared to the one without source terms). The only thing I am worried about is Eugene's following post.. http://www.cfd-online.com/Forums/ope...-new-post.html I am also finding many problems with these set of solvers, especially convergence of Temperature is very very slow. forget about second order results (Remember I am a novice user still, and I think I am continue to be novice as long as openfoam does not provide documentation) I am doing lot of parametric study (Thanks to my organization for proving me the infinite compute power on world's faster super computer, EKA) Regards Santhosh

May 11, 2010, 01:50
Sensitivity of Turbulent prandtl number
#6
Member

santhosh
Join Date: Apr 2009
Location: India
Posts: 68
Rep Power: 8
Hi,

Please look at the residual file attached here,

Unknowingly I initially used the turbulent Prandtl number (Prt) equals 5. After reading the documentation I came to know Prt is used as a contribution to production term in turbulent kinetic energy equation. Also for k-e model it has to be aroung 0.85.

So I changed the value of Prt to 0.8 from 5. I observed lot of variation in residue plots.

In the attached plot, sensitivity with viscosity (which I changed matching experimental) and Prt. The results are similar in case of variation of viscosity (although very little change). But with variation of Prt I found completely different residual.

I am using upwind numerical schemes for interpolation.

Please can anybody through a light on the use of Prt. Is it okey to use Prt=5 if not can you suggest chages to get residual down.

I have observed simular variation in residual for other parameteers also.

Thanks
Santhosh
Attached Images
 Prt_sensitivity_residual.jpg (82.1 KB, 90 views)

 June 28, 2010, 10:58 #7 Senior Member     maddalena Join Date: Mar 2009 Posts: 436 Rep Power: 13 Hi Santhos, I am new on heat transfer problems using cfd and I would like to model a constant volume heat generation, following the approach you proposed, since it seems to me that there is no already implemented function to model it in OF. Before starting, I would like to know it you have some results showing that this is a good approach, i.e. cfd matches with experimental results. regards, mad

 June 29, 2010, 06:14 #8 Member   santhosh Join Date: Apr 2009 Location: India Posts: 68 Rep Power: 8 Hi, I have added source term as I have mentioned above. I have even completed one test case with the modified solver. But unfortunately, I have not compared the results with the any benchmark case. Qualitatively It seemed OK to me. If you find any benchmark cases to test it, please let me know, and I am happy to test it for you. Regards, Santhosh

 July 16, 2010, 11:17 #9 Senior Member     maddalena Join Date: Mar 2009 Posts: 436 Rep Power: 13 Hi Santhosh, finally I included the heat source contribution on chtMRFoam, as you suggested above. However, as explained here, the new solver gives acceptable values only if I use a single region. In the case of multiple region, of which only one is heated, the solver does not perform well. I am thinking that this may be due to the coupling between the regions. Have you any experience in that? Any suggestion is welcome. Regards, mad

 July 19, 2010, 10:53 adding term in solidWallMixedTemperatureCoupled #10 Senior Member     maddalena Join Date: Mar 2009 Posts: 436 Rep Power: 13 Hi all, trying to find an explanation on the strange results of my cht simulation including heat source, I ended up with the following: solidWallMixedTemperatureCoupled in OF 1.6.x and 1.7 implements a coupling that differs from OF 1.6 and previous. In OF 1.6 (code): Code: ``` forAll(*this, i) { // if outgoing flux use fixed value. if (normalGradient()[i] < 0.0) { this->refValue()[i] = operator[](i); this->refGrad()[i] = 0.0; // not used this->valueFraction()[i] = 1.0; nFixed++; } else { this->refValue()[i] = 0.0; // not used this->refGrad()[i] = normalGradient()[i]; this->valueFraction()[i] = 0.0; } }``` while in OF 1.7 (code) Code: ``` this->refValue() = nbrIntFld; this->refGrad() = 0.0; this->valueFraction() = nbrKDelta / (nbrKDelta + myKDelta());``` In any case, the two approach gives equal results for chtMultiRegionFoam so that is fine. My doubts raise when applying a heat source. The 1D steady state conduction equation + heat source says that: dT2/dx2 + H/K = 0. Integrating once gives dT/dx - H/K*x = 0. It means that, in the case of an heat source refGrad is not equal to zero, but it is proportional to the heat souce itself. For this reason, I am thinking to modify the solidWallMixedTemperatureCoupled to include this contribution as well. K is already read into solidWallMixedTemperatureCoupled.C, and I can easily modify the solver to read H as well. What I am missing is how to get the size of the cell normally to the coupling interface. Is there anyone that can confirm my approach? anyone that can help me to understand how to get the cell size? thanks in advance from any suggestion I may get. cheers, mad

September 12, 2011, 10:41
#11
Senior Member

Anne Gerdes
Join Date: Aug 2010
Location: Hamburg
Posts: 154
Rep Power: 7
Hey Santhosh,

Quote:
 Originally Posted by santoo_cfd I am looking at the TEqn.H in boussinesqBuoyantSimepleFoam. following is snippet copied from the above file. Code: ```fvScalarMatrix TEqn ( fvm::div(phi, T) - fvm::Sp(fvc::div(phi), T) - fvm::laplacian(kappaEff, T) );``` Can anybody tell me what is the need of second term Code: `fvm::Sp(fvc::div(phi), T)` according to following relation Code: `div(sV) = sdiv(V)+V.grad(s)` (s is scalar and V is vector). Combination of first two terms will results in the following, Code: `phi.gradT` Can anybody help me understanding these equations. I am finally trying to find heat source term in the equation so that I can specify uniform heating thoughout the fluid region. Regards Santhosh.
I think I am now able to answer the question.
Basically we have the term
d/dxj (rho * u_j * T)
which includes the density.
This term goes to
d/dxj (rho * u_j * T) = rho * d/d_xj ( u_j * T) + u_j* T * d rho /dxj
The first term equals to
HTML Code:
`fvm::div(phi, T)`
The second term includes the derivative of the densitiy, rho.
From the continuity equation we know

d/dxj (rho * uj)=0
According to product rule
d/dxj (rho * uj ) = uj * d rho/dxj + rho * duj/dxj =0
and therefore
uj * d rho / dxj = - rho * duj/dxj

Therefore the second term becomes
u_j* T * d rho /dxj = - T * rho * duj/dxj

Which is in OF the term

HTML Code:
`fvm::SuSp(-fvc::div(phi), T)`
as everything is divided by density.
The additional term is zero for incompressible flows.

 September 12, 2011, 23:44 #12 Member   santhosh Join Date: Apr 2009 Location: India Posts: 68 Rep Power: 8 Thanks for your effort in neatly explaining. Actually a while ago, My professor cleared my doubt about post. Sorry I forgot to post it back to forum. The explanation was similar to the one you explained. Thanks again Santhosh

September 18, 2013, 04:02
some error
#13
Member

Himanshu Sharma
Join Date: Jul 2012
Posts: 84
Rep Power: 5
Quote:
 Originally Posted by santoo_cfd I have added the source term in the TEqn.H as below. Code: ```fvScalarMatrix TEqn ( fvm::div(phi, T) - fvm::Sp(fvc::div(phi), T) - fvm::laplacian(kappaEff, T) - Q/(rho0*cp0) );``` I have compiled and run the some simple test case. I have not yet seen the results just run completed successfully. I will post back if there is any other alternative. Regards Santhosh
Hi,

I used user idea for building the source term in my solver and i specify Q as volumetric heat source dimension my solver is compiling properly but when i am using the solver it is giving me some kind of dimension error i am not able to debug it if you can help.

Code:
```Different dimensions for =
dimensions : [0 2 -1 0 0 0 0] = [0 4 -3 0 0 0 0]

From function dimensionSet::operator=(const dimensionSet&) const
in file dimensionSet/dimensionSet.C at line 165.```
Thank you.

 June 5, 2014, 08:18 #14 New Member   ashwin Join Date: Jul 2012 Location: erlangen Posts: 26 Rep Power: 5 Can any of you tell me How to implement the volumetric source term in 'buoyantSimpleFoam'?

 Tags source term

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post sek OpenFOAM Running, Solving & CFD 37 November 28, 2015 14:41 claco OpenFOAM 7 April 20, 2010 04:32 kumar2 OpenFOAM Running, Solving & CFD 8 March 24, 2008 19:38 Lindz FLUENT 0 August 3, 2007 07:34 Harry Dong Main CFD Forum 12 February 4, 2006 01:55

All times are GMT -4. The time now is 08:59.