CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

 Logan Page August 16, 2013 08:36

5 Attachment(s)
Hi All

I am trying to solve a very simple radiation case in order to validate OpenFoam's radiation model/s, so far with little success.

The case I'm trying to solve is a 2D square enclosure (1m x 1m):
• left wall: uniform T at 100K (black body - emission)
• right, top and bottom walls: uniform T at 0 K (black body - absorption)
• no convection or conduction (vacuum)
The analytical results for this are quite easy to calculate and are as follows:
• Qr from the left wall: 5.67 W/m2
• Qr into right wall: 2.3474 W/m2
• 5.67 * ViewFactor = 5.67 * 0.414
• Qr into top wall: 1.661 W/m2
• 5.67 * ViewFactor = 5.67 * 0.293
• Qr into bottom wall: 1.661 W/m2
• 5.67 * ViewFactor = 5.67 * 0.293
For this I have tried the P1 and fvDOM radiation models, I have tried using the buoyanySimpleFoam solver as well as a custom solver I created and all give me more or less the same incorrect solution.

I have attached the following:

Qr on the leftWall should be uniform across the whole surface equal to 5.67, which I am able to get with the custom solver, but not with the buoyantSimpleFoam solver (for some reason the thermal conductivity in the energy equation has an effect on Qr).
Qr on the rightWall should give a area-weighted sum of 2.3474, in paraFoam I get an area-weighted sum of 0.6103. I am unable to get the correct Qr for the right, top and bottom surfaces.

I hoping that this is the case of me missing something fundamental so any comments / advice would be useful :D

 Logan Page August 19, 2013 06:59

Can someone please explain to me how and where these coefficients (in the radiationProperties file) play a role in the radiation models:

Code:

```absorptionEmissionModel constantAbsorptionEmission; constantAbsorptionEmissionCoeffs {   absorptivity    absorptivity    [ 0 -1 0 0 0 0 0 ]  0;   emissivity      emissivity      [ 0 -1 0 0 0 0 0 ]  0;   E              E              [ 1 -1 -3 0 0 0 0 ] 0; }```
Because if I change the absorptivity and emissivity to 0 (as shown above) i get the exact analytical solution for this test case.

 Zeppo September 7, 2013 13:23

Quote:
 Originally Posted by Logan Page (Post 446604) Because if I change the absorptivity and emissivity to 0 (as shown above) i get the exact analytical solution for this test case.
Have you tried out ViewFactors radiation model?

 ARTem September 30, 2013 02:31

Hello, Logan Page.
The spherical harmonic approx. method (P1) gives me 8.47 [W/m2] and 2.79 [W/m2] for q_left and q_right correspondingly.
The discrete ordinates method gives me 5.67 [W/m2] and 2.31 [W/m2] for q_left and q_right correspondingly. This result is very close to theoretical one.
I haven't used viewFactors model yet.

If you're still interesting in this stuff, I can share test case here.

 olivierG September 30, 2013 03:52

hello,

You can not use P1 model with an empty cavity, since P1 model is for optical thick media (a*l >1), with a= absorptivity and l = carac. length
DO and viewfactor method should work however.

regards,
olivier

 Logan Page September 30, 2013 06:33

1 Attachment(s)
Hi

Thanks for the feedback.

I was able to get the theoretical results using the DO method by setting "absorptionEmissionModel" to "none" in the "radiationProperties" file.

I was also able to figure out the theory and 90% of the implementation thereof in OpenFOAM for the DO method through the use of the book by M. Modest (Radiative Heat Transfer, 3rd Edition)

However for the life of me I cannot figure out why there is an additional source radiation term implemented for the DO method in OpenFoam.
For a participating, non-scattering, medium the governing RTE is given by:
http://www.cfd-online.com/Forums/att...1&d=1380536642

However in OpenFOAM there is an additional source term that has been added:
Code:

```            IiEq =             (                 fvm::div(Ji, ILambda_[lambdaI], "div(Ji,Ii_h)")  //<-- first term               + fvm::Sp(k*omega_, ILambda_[lambdaI])              //<-- second term             ==                 1.0/constant::mathematical::pi*omega_               * (                     k*blackBody_.bLambda(lambdaI)                //<-- third term                   + absorptionEmission_.ECont(lambdaI)/4          //<-- additional source ??                 )             );```
The first 3 terms implemented in OpenFOAM are 100% correct according to the theory, however I cannot find any theory / literature as to why there would be an additional source term in the RTE.

For a "constantAbsorptionEmission" model "ECont(lambdaI)" is simply the "E" value specified by the user in the "radiationProperties" file. For a "greyMeanAbsorptionEmission" model "ECont(lambdaI)" is "EhrrCoeff * dQ" where again "EhrrCoeff" is specified by the user in the "radiationProperties" file.

 wc34071209 February 18, 2014 14:13

Quote:
 Originally Posted by ARTem (Post 454193) Hello, Logan Page. The spherical harmonic approx. method (P1) gives me 8.47 [W/m2] and 2.79 [W/m2] for q_left and q_right correspondingly. The discrete ordinates method gives me 5.67 [W/m2] and 2.31 [W/m2] for q_left and q_right correspondingly. This result is very close to theoretical one. I haven't used viewFactors model yet. If you're still interesting in this stuff, I can share test case here.
Hello,

could you kindly share your test case ? I am facing the same problem and I want to learn a little about how to set up radiation from your case.

thank you very much.

 scintilla March 10, 2014 19:05

Quote:
 Originally Posted by Logan Page (Post 454232) Hi Thanks for the feedback. I was able to get the theoretical results using the DO method by setting "absorptionEmissionModel" to "none" in the "radiationProperties" file. I was also able to figure out the theory and 90% of the implementation thereof in OpenFOAM for the DO method through the use of the book by M. Modest (Radiative Heat Transfer, 3rd Edition) However for the life of me I cannot figure out why there is an additional source radiation term implemented for the DO method in OpenFoam. For a participating, non-scattering, medium the governing RTE is given by: http://www.cfd-online.com/Forums/att...1&d=1380536642 However in OpenFOAM there is an additional source term that has been added: Code: ```            IiEq =             (                 fvm::div(Ji, ILambda_[lambdaI], "div(Ji,Ii_h)")  //<-- first term               + fvm::Sp(k*omega_, ILambda_[lambdaI])              //<-- second term             ==                 1.0/constant::mathematical::pi*omega_               * (                     k*blackBody_.bLambda(lambdaI)                //<-- third term                   + absorptionEmission_.ECont(lambdaI)/4          //<-- additional source ??                 )             );``` The first 3 terms implemented in OpenFOAM are 100% correct according to the theory, however I cannot find any theory / literature as to why there would be an additional source term in the RTE. For a "constantAbsorptionEmission" model "ECont(lambdaI)" is simply the "E" value specified by the user in the "radiationProperties" file. For a "greyMeanAbsorptionEmission" model "ECont(lambdaI)" is "EhrrCoeff * dQ" where again "EhrrCoeff" is specified by the user in the "radiationProperties" file.
Hi Logan,

I was a bit confused by this when I first saw it too -- as you correctly say, only the first three terms appear in the theoretical RTE. However this is a numerical implementation and I believe the reason for the E parameter in the absorptionEmissionModel is to allow the user the choice of defining the emissive power of the gas directly (W/m3), rather than via the gray gas relation (emissivity * planck function). This would be useful if one wanted to apply a radiative source term that does not vary in proportion to the Planck function.

S

 Majed March 10, 2014 21:32

I Need Help

1 Attachment(s)
Hello all,

I am new to this forum. I really need your help to solve my problems in running openfoam. attached is my geometry. There are 5 rows of vanes in front of an intake channel. I have produced my geometry, but I think it is not correct. Does any body know, how I can define the water surface in my geometry? I want to consider it as rigid lid. Then my flow in the channel in turbulent, and I want to use k-epsilon turbulent model for the simulations.

Any help is really appreciated.

 jrsilvio_ver October 11, 2014 16:28

Dear Friends,
In the example of validation discussed, as you would to include the ViewFactor model? What files should include?
I appreciate everyone's attention.

 wc34071209 October 13, 2014 04:49

Quote:
 Originally Posted by jrsilvio_ver (Post 513906) Dear Friends, In the example of validation discussed, as you would to include the ViewFactor model? What files should include? I appreciate everyone's attention.
Hi,

I am eager to know as well.

 Amit-1911 March 2, 2015 06:37

Dear Logan page,

I am new to the OpenFOAM and hence may sound stupid!
Could you pls tell me how did you manage to set up your problem with no convection and conduction ( Conduction i can understand as no solid body present).
and if I want to consider convection with radiation what necessary changes i have to make??

Regards,
Amit Dhage

 Astrodan May 22, 2015 08:03

Quote:
 Originally Posted by Amit-1911 (Post 533971) Could you pls tell me how did you manage to set up your problem with no convection and conduction ( Conduction i can understand as no solid body present).
I assume you can prevent convection by setting an initial velocity field of 0, and deactivating any graviational effects, so that the fluid should have no reason at all o move.
However, I'm not sure conduction really is deactivated, since the thermophysicalProperties values give mu and Pr, which I assume are used für thermal conductivity. Anyway, this should be quite small and probably has little influence on the solution (maybe the reason vor ARTems deviation from the exact soluton).

Quote:
 Originally Posted by Logan Page (Post 454232) However for the life of me I cannot figure out why there is an additional source radiation term implemented for the DO method in OpenFoam. For a participating, non-scattering, medium the governing RTE is given by: http://www.cfd-online.com/Forums/att...1&d=1380536642 However in OpenFOAM there is an additional source term that has been added: Code: ```            IiEq =             (                 fvm::div(Ji, ILambda_[lambdaI], "div(Ji,Ii_h)")  //<-- first term               + fvm::Sp(k*omega_, ILambda_[lambdaI])              //<-- second term             ==                 1.0/constant::mathematical::pi*omega_               * (                     k*blackBody_.bLambda(lambdaI)                //<-- third term                   + absorptionEmission_.ECont(lambdaI)/4          //<-- additional source ??                 )             );```
After we disscused the fourth term in the equation, I'd like to figure out why there is the omega/pi term present? This seems to be some weighting dependend on the solid angle, but I would expect it to be omega/(4*pi), i.e. the fraction of the complete solid angle that this ray covers. Can anyone explain to me what I'm missing? I also have the book by Modest (2nd Ed.), but I can't find the factor there either.

 chriss85 May 26, 2015 10:39

Quote:
 Originally Posted by Astrodan (Post 547319) I assume you can prevent convection by setting an initial velocity field of 0, and deactivating any graviational effects, so that the fluid should have no reason at all o move. However, I'm not sure conduction really is deactivated, since the thermophysicalProperties values give mu and Pr, which I assume are used für thermal conductivity. Anyway, this should be quite small and probably has little influence on the solution (maybe the reason vor ARTems deviation from the exact soluton).
To get a zero velocity field, you should use a very small timestep in a transient solver combined with the conditions you mentioned. In the limit of small times the forces can't accelerate the fluid to meaningful speeds. Another method would be to simply remove the equations from the solver.

 Coris August 4, 2016 04:48

I've also used simple case above to start with radiation and am able to get the analytically expected results with fvDoM (see first post). However, I run into problems when changing the boundary conditions over time.

Any change in BC temperature (which is a fixedValue) is not fully reflected in the radiation model. This concerns me because any transient evolution in boundary temperature will not give correct radiation results.

I have tested this with the square enclosure case, no conduction and no convection. Also, the bottom and top walls are not taking part in the radiation procedure (0 emissivity and absorption), but this should not matter. The left wall starts at 100 K and the right wall at 200 K. After advancing 250s with chtMultiRegionFoam, I get correct results. When I write out these results and change the BC at the right wall to 0K (practically, 0.001 K), the right wall is still radiating to the left wall at 500s.

I have tried various settings of the fvDom solver, but no results. Any thoughts?

Note: The case can be found at https://www.dropbox.com/s/1esjyufcrd...nTest.zip?dl=0, for OF 3. The left and right walls are called Inlet and Outlet in this case. Running sh postProcess.sh shows the radiation balance and input for the relevant surfaces. See the first post for the expected results.

 Coris August 11, 2016 03:21

FYI, I posted the problem above, in a slight modified form, on the OF bug tracker:
http://bugs.openfoam.org/view.php?id=2185

I have also found another fundamental issue with fvDoM when cacheDiv = false:
http://bugs.openfoam.org/view.php?id=2182

 valikang January 25, 2017 04:02

Could you make the case available again?

Quote:
Could you make the case available again. I am looking for a closed enclosure radiation validation case for a conjugate heat transfer problem solved with chtMultiRegionFoam.

-Turo

 wc34071209 April 16, 2017 16:26

Quote:
 Originally Posted by Logan Page (Post 446604) Can someone please explain to me how and where these coefficients (in the radiationProperties file) play a role in the radiation models: Code: ```absorptionEmissionModel constantAbsorptionEmission; constantAbsorptionEmissionCoeffs {   absorptivity    absorptivity    [ 0 -1 0 0 0 0 0 ]  0;   emissivity      emissivity      [ 0 -1 0 0 0 0 0 ]  0;   E              E              [ 1 -1 -3 0 0 0 0 ] 0; }``` Because if I change the absorptivity and emissivity to 0 (as shown above) i get the exact analytical solution for this test case.

Hi,

I think these properties are the properties of air. So if you set all of them zero, then they don't play a role in the radiation and therefore it works like a vacuum and therefore you get exact analytical solutions.

Or you can also do it like this
Code:

`absorptionEmissionModel none;`
I think both ways work the same.

 All times are GMT -4. The time now is 00:01.