[LIYAFEI]

Dear CFDer


I'm trying to use openfoamV11 (foundation edition) to simulate PVD reactor,


The highest temperature in the case is around 2000 degree. So I need to use the radiation model. Now I use the fvDOM method to simulate the radiation.


But for the solid material, I have nontransparent graphite and transparent quartz.


So I want to know how to set these two material?


The default setting for the solid is as following




radiation on;

radiationModel opaqueSolid;

absorptionEmissionModel constant;

absorptivity absorptivity [0 -1 0 0 0 0 0] 0.01;

emissivity emissivity [0 -1 0 0 0 0 0] 0.2;

E E [1 -1 -3 0 0 0 0] 0;

scatterModel none;

sootModel none;


Should I also set the radiationProperties of the transparent quartz the same with air?


thank you



LI

[Alczem]

Hey!


Transparent medium is not implemented currently, only transparent boundaries.


I tried several workarounds to achieve the same thing you are doing, but the main issue is that the radiative fields are not communicating between two regions of a CHT case.


Good luck to you, and if you do manage to find a solution, please share it, it is a feature I would love to see implemented!

[LIYAFEI]

Thank you for your reply.
The following are the boundary conditions I set.

type greyDiffusiveRadiation;
value uniform 0;
emissivityMode solidRadiation;
emissivity uniform 1;



So, as you said, the emissivity of the gas-solid interface (transparent solid) is 0, and the emissivity of the gas-solid interface (completely opaque) is 1, is that right?

Originally Posted by Alczem

Hey!


Transparent medium is not implemented currently, only transparent boundaries.


I tried several workarounds to achieve the same thing you are doing, but the main issue is that the radiative fields are not communicating between two regions of a CHT case.


Good luck to you, and if you do manage to find a solution, please share it, it is a feature I would love to see implemented!

[Alczem]

Originally Posted by LIYAFEI

Thank you for your reply.

So, as you said, the emissivity of the gas-solid interface (transparent solid) is 0, and the emissivity of the gas-solid interface (completely opaque) is 1, is that right?

Yep, but OpenFOAM does not compute a radiative field inside solid regions, so whatever you set at the boundary, the radiation will be converted to heat conduction inside the solids.


I tried to use a fluid region with frozen flow on, but there is not only one radiative field, each region has its own. Meaning that an incident ray from region 1 will hit the interface between region 1 and region 2, and its angle of incidence won't matter when region 2 will compute radiation, the radiation from region 1 will be re-computed according to the boundary properties for region 2, if that makes sense...

[LIYAFEI]

Thank you


But Can I use fvDOM model for solids?

[giorgianig]

Originally Posted by Alczem

Yep, but OpenFOAM does not compute a radiative field inside solid regions, so whatever you set at the boundary, the radiation will be converted to heat conduction inside the solids.


I tried to use a fluid region with frozen flow on, but there is not only one radiative field, each region has its own. Meaning that an incident ray from region 1 will hit the interface between region 1 and region 2, and its angle of incidence won't matter when region 2 will compute radiation, the radiation from region 1 will be re-computed according to the boundary properties for region 2, if that makes sense...

Hello Alczem,

I am trying to compute radiation through a transparent solid, is this limitation still there? Did manage to find a workaround?
Thanks in advance.

[Alczem]

Originally Posted by giorgianig

Hello Alczem,

I am trying to compute radiation through a transparent solid, is this limitation still there? Did manage to find a workaround?
Thanks in advance.

Hey,


As far as I am aware, it is not implemented yet, and I have not figured out a way around, sorry!

[giorgianig]

Originally Posted by Alczem

Hey,


As far as I am aware, it is not implemented yet, and I have not figured out a way around, sorry!

Thanks. Did you manage to "freeze" the fluid then? If yes, how did you do it?

[Alczem]

Hey,


You can use the frozenFlow entry set to yes in fvSolution, for the region of your choice.

[giorgianig]

Originally Posted by Alczem

Hey,


You can use the frozenFlow entry set to yes in fvSolution, for the region of your choice.

Thanks, I didn't know this parameter. I think I managed to do more or less the same lowering a lot the mu transport coefficient of the fluid and reducing the number of iteration of the p_rgh.

[giorgianig]

Originally Posted by Alczem

Hey,


You can use the frozenFlow entry set to yes in fvSolution, for the region of your choice.

Hey Alczem, maybe you can help me with a radiation case I cannot set up properly. Can you take a look to this post?
Radiation boundary condition with the viewFactor model