[condensatoalcioccolato]

I am working on CHT tutorial with the radiation view factor model.
I am trying to what differences there are in terms of temperature inside the fluid, but the results are equal.
It seems that radiation is not seen by the fluid.

could you help me?

[peterhess]

Hello!
the viewFactor model calculate the radiation exchange between the surfaces.
The rays that are passing the fluid does not affect the fluid, cause it suppose "vacuum" inside the fluid!
If the fluid to be affected by the radiation, then you need to use the DoM (Discrate Ordinate Method).

More information could be found here:

Adding Radiations in chtMultiRegionSimpleFoam

Regards

Peter

[condensatoalcioccolato]

firstly, thank you for your answer.
fvDom need other things with the radiation properties? Because I tested fvDom, but the results are equal, without variation.
I the discussion that you linked to me I saw the relaxation factor, but it doesn't affect the result.

[peterhess]

Well, if you have a fixed wall temperatures, then the radiation will not affect the wall temperatures but the total heat flux through the surface (wall).

Like that the fluid has always the same walls temperatures if radiation is turned on or not.

which boundary conditions are you using. Or simply post the case.

Regards

Peter

[condensatoalcioccolato]

Originally Posted by peterhess

Well, if you have a fixed wall temperatures, then the radiation will not affect the wall temperatures but the total heat flux through the surface (wall).

Like that the fluid has always the same walls temperatures if radiation is turned on or not.

which boundary conditions are you using. Or simply post the case.

Regards

Peter

These are the files. I set up the plane2d tutorial file and I am trying to modify it.


https://polimi365-my.sharepoint.com/...SB2CA?e=CwjUsj

[peterhess]

I will check up the case and give you later a feedback.

Anyway, the qr for topAir and bottomAir is:

greyDiffusiveRadiationViewFactor

it must be:

greyDiffusiveRadiation

cause the radiation model is DoM!

Regards

Peter

[condensatoalcioccolato]

thank you for your feedback. now I lunch another simulation with the correction

[peterhess]

Hello!

I made many changes in the case and I am not able to list those changes, cause they are many as I said.

The case after making the changes is uploaded here.

See the case attached.

The case has been made for OF7.0!

If you are using an older version, then you need to replace radiationProperties in the case with the originals in yours to make it work, cause the syntex of the code has been changed in OF7.0!

If there are any questions, then please post it.

If you are not able to run the case, then please tell me the version of OF you are using.

Regards

Peter

PS: I am not sure that DoM is applicable if there is a symmetry BC

[condensatoalcioccolato]

thank you very much.
I saw the common surface between regions have a different type of BC and a different description. Also, radiation properties have different coefficients

I am running now the simulations

Thank you again

[condensatoalcioccolato]

ok, I tried to run a simulation but it takes a very long time, so I still waiting.

My starting questions are:

1) you add in control dict maxDi and the adjustment of time step. What is maxDi and why i need to adjust my time step? Is that the reason for the huge time taken?

2) is not possible solving fos Simple instead of Pimple?

[peterhess]

Originally Posted by condensatoalcioccolato

1) you add in control dict maxDi and the adjustment of time step. What is maxDi and why i need to adjust my time step? Is that the reason for the huge time taken?

maxDi is the maximum diffusivity!

If the simulation is transient, you could need it to limite the diffusivity.

That helps if you have difficulties covergence...

You can delete it...

You adjust the time step to keep the maxDi and maxCo under there limite!

If you turn it off, then the time step will not modified by need (to keep maxDi and maxCo under there values).

Originally Posted by condensatoalcioccolato

2) is not possible solving fos Simple instead of Pimple?

As I know chtMultiRegionFoam just work with PIMPLE. I could be wrong here...

To make the simulation steadyState just replace ddt from Euler to steadyState for all regions in fvSchemes.

Anyway, if you want to use SIMPLE, then you need to use an older Version with chtMultiRegionSimpleFoam.

But making SteadyState with PIMPLE delivers good results.

The simulation (steady state) run fast. See residuals.

Regards

Peter

[condensatoalcioccolato]

Thank you! I switched it in SIMPLE in order to reduce the time.
Now it took all yesterday to solve.

But I still have qr and qin equal to 0. Is that normal? I think they must be different from zero if I wanna have radiative heat flux. It is correct?

[peterhess]

Well, in the last simulation I uploaded, the simulation converges in 2 minutes on 4 cores processor.

And the residuals are very pretty...

The qin and qr are none zeros!

Upload your actual case please to take a look.

By the way, I made many changes in the boundaries in the cases I uploaded compared with the one you posted earlier.

Especially at the outlets I replaced zeroGradient with inletOutlet.

Regards

Peter

PS Which OF version are you using?

[condensatoalcioccolato]

I am using version 5, but with your question, I switch on version 7 and now it seems to work. It takes more than 2 minutes (now is running from 20 minutes and it is still to 100). with 4 cores.

[peterhess]

The last simulation I uploaded is convergating in about 300 iteration and needs about 335 seconds (less than 6 minutes)!

Actually the 0,0001 residuals is reached in about 150 iterations and running the simulation further is just to be sure that nothing wrong happends later...

Regards

Peter

[condensatoalcioccolato]

I downloaded your last simulation, extracted and lunched.
it is still going.

I attached the picture and the file that I am running. I really don't know why.

[peterhess]

Well, the timeStep in the simulation I uploaded is 0.1!

That means u need to calculate just 30 seconds or 300 itterations as I mentioned before...

And the execution time is still less than 6 minutes!

In the image you uploaded you already calculated 3000 timeSteps!

That why you need 10 times more calculation time

Just copy the file I attach here in the case and run:

gnuplot Plot.txt

In a new terminal to see the residuals progress..

Regards

Peter

PS: after installing gnuplot!!!