CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   View factor radiation model. Symmetry boundaries verification.. (http://www.cfd-online.com/Forums/openfoam-solving/104665-view-factor-radiation-model-symmetry-boundaries-verification.html)

Dimoon July 12, 2012 11:02

View factor radiation model. Symmetry boundaries verification..
 
3 Attachment(s)
Hello everybody!

I simulated radiation transfer in a cylindrical chamber with 4 heaters symmetrically placed inside. For this I used a domain representing 1/4 of a model with symmetry boundary conditions. Cylinder and heater emissivity is 1. Temperatures 300 and 2500 K respectively.

I expected to get something like this Attachment 14398. It is the result of simulation with commercial software which seems to be reasonable. Color on the side wall represents heat flux.

When I run similar problem with OpenFoam I get this Attachment 14400. Most area of cold wall have negative flux, which is unrealistic.

At the same time I performed simulation with walls having zero emissivity instead of symmetry boundaries. Under this conditions the result obtained with OpenFOAM is correct and very similar to the result of another software Attachment 14401. This make me think that the problem is connected with treatment of symmetry boundary conditions in view factor radiation model.

I set symmetry condition for radiation by usual way as "type symmetryPlane;". Probably there is a special procedure to set symmetry for this case, does anybody know?

gschaider July 15, 2012 17:26

Hello Dmitry!
Quote:

Originally Posted by Dimoon (Post 371145)
This make me think that the problem is connected with treatment of symmetry boundary conditions in view factor radiation model.

I set symmetry condition for radiation by usual way as "type symmetryPlane;". Probably there is a special procedure to set symmetry for this case, does anybody know?

I'm afraid that the sad truth is that the view factor model does not support symmetry-BCs at all. At least does a quick glance at the code not show any consideration towards symmetry. And I think it should (according to my limited understanding of the model)

But may I suggest that you ask such questions next time in the "Running, Solving & CFD"-forum as it is better suited for questions on case-setup

Bernhard

cliffoi February 19, 2013 19:39

I know this discussion is probably dead by now but I thought I'd add my two cents worth since I have been dealing with this exact issue recently. Dmitry, the problem you are probably encountering is that your view factors have not been calculated for a full enclosure, in which case energy is not necessarily conserved. OpenFOAM does not take symmetry boundaries into account when solving for view factor radiation. It simply takes the view factors you provide and calculates the net heat flux based on these. To fix this you need to compute view factors that include the symmetry effects. The approach I would use for your model is:
  • Copy and rotate your mesh (N faces) to obtain a full 3D model with 4N surfaces
  • Calculate the 4Nx4N view factors using this set of surfaces
  • Apply the rules of composition and distribution for view factors to combine the symmetric faces to obtain a NxN view factor matrix that includes the symmetry effects
Depending on what utilities you are using this could take a bit of effort but I guarantee that it does work.

Regards
Ivor

eddi0907 March 26, 2013 11:14

2 Attachment(s)
Hello,

I want to use the viewfactor radiation with chtmultiregionfoam.

I found very strange results for the model attached (due to size limitation I had to remove the mesh. Is there another possibillity to upload the complete model (1,2 Mb?)):


It's a "simple" test case, a solid sphere within a rectangular air domain surrounding, where the temperature at the outer air walls is fixed to 1000 K while the initial solid sphere and the inner air domain temperature is 300 K.

Running the case the temperature on the solid sphere becomes not physical at all. inhomogeneous distributed with local temperature drops to 226 K!!!!!
(Please see attached picture)

There should never be a temperature below 300K!

I tried OF version 2.1.1 and 2.2.0.

Any help is more than welcome.

Kind Regards.

Edmund

eddi0907 March 27, 2013 05:59

2 Attachment(s)
I changed the geometry.

Using a cube instead of a sphere it seems to work.

Except for low solid thermal conductivity it crashes initially:

--> FOAM FATAL ERROR:
Maximum number of iterations exceeded

From function specieThermo<Thermo>::T(scalar f, scalar T0, scalar (specieThermo<Thermo>::*F)(const scalar) const, scalar (specieThermo<Thermo>::*dFdT)(const scalar) const) const
in file /usr/local/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 69.

I tried changing featureAngle to 0.001 and nFacesInCoarsestLevel to 10000 in viewFactorsDict without success.

How to make a complex surface work in a radiation viewFactor model?

Or is it impossible actually even with OF 2.2.0 because of this bug: ID 656 http://www.openfoam.org/bugs/ ?

MangoMango March 26, 2014 10:36

@eddi0907

..can you post your casefile in this thread? I would be really glad, because I can't find a proper viewFactor Tutorial case (the rectangle one).

Thanks in advance

Best regards,

Alex

eddi0907 March 31, 2014 01:48

Hi Alex,

you can try viewfacctorgen_sphere_bug.tar.gz

on http://www.openfoam.org/mantisbt/view.php?id=656

Regards

Edmund

MangoMango March 31, 2014 11:41

Hi Edmund,

thank you very much. I will give it a shot :)

regards

Alex

MangoMango March 31, 2014 12:50

1 Attachment(s)
Hi Edmund,

not sure and correct me if i'm wrong, but shouldn't be the 5th of the Allrun-skript line "faceAgglomerate -dict constant/viewFactorsDict" instead of "faceAgglomerate -dict constant/viewFactorsDict"

The viewFactorDict file is inconsistent too. { <- too much.

If I correct both - there is still something odd. I have too run Allrun twice and then there is only F00: 1.02709 shown... (using of-2.3.0)

Maybe my corrections are wrong. Because..

This errormsg pops up too:
Determining initial surface intersections
-----------------------------------------



--> FOAM FATAL ERROR:
Number of cells in mesh:8000 does not equal size of cellLevel:15844
This might be because of a restart with inconsistent cellLevel.

From function hexRef8::getLevel0EdgeLength() const
in file polyTopoChange/polyTopoChange/hexRef8.C at line 358.

FOAM aborting

#0 Foam::error::printStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 Foam::hexRef8::getLevel0EdgeLength() const at ??:?
#3 Foam::hexRef8::hexRef8(Foam::polyMesh const&, bool) at ??:?
#4 Foam::meshRefinement::meshRefinement(Foam::fvMesh& , double, bool, Foam::refinementSurfaces const&, Foam::refinementFeatures const&, Foam::shellSurfaces const&) at ??:?
#5
at ??:?
#6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7
at ??:?
Aborted (core dumped)


Please don't get me wrong. I don't want to play the smartypants...I only got stuck and need help. As a newbee its tough to see through this type of thermophysicalmodel :confused:

It would be really glad of you if you could help me on this :D

Best regards
Alex

p.s.: I ran this case on two machines to crosscheck if there are any compiler/build errors (but both gcc and icc versions are showing the same behaviour)

Dimoon April 29, 2014 02:12

Quote:

Originally Posted by MangoMango (Post 482218)
@eddi0907

..can you post your casefile in this thread? I would be really glad, because I can't find a proper viewFactor Tutorial case (the rectangle one).

Thanks in advance

Best regards,

Alex

Hi Alex! I can not find it. But you can use standard tutorial: /tutorials/heatTransfer/chtMultiRegionSimpleFoam/multiRegionHeaterRadiation

I used it to prepare that case.

best regards,
Dmitry


All times are GMT -4. The time now is 14:48.