[qtruong]

Hi,

Since chtMultiRegionSimpleFoam was removed in OpenFOAM 6, I tried running a steady state case with chtMultiRegionFoam, with a residualcontrol (shown below). But it does not stop when converged. Has anyone tested if residualcontrol works in the new chtMultiRegionFoam?

PIMPLE
{
     residualcontrol
     {
          U     1e-4;
     }
}

[Robin.Kamenicky]

Hi qtruong,

could you try

residualControl

instead of

residualcontrol

Kind regards,
Robin

[qtruong]

Originally Posted by Robin.Kamenicky

Hi qtruong,

could you try

residualControl

instead of

residualcontrol

Kind regards,
Robin

thank you for the response.

Sorry, it was my typo while writing the post. It was actually "residualControl" in the code, and it's confirmed by the log file:

PIMPLE: Region gas
PIMPLE: Convergence criteria found
             U:    tolerance  0.0001

Otherwise, with lower "c", there would be "no convergence criteria found".

Nonetheless, the convergence is reached, but chtMultiRegionFoam keeps running until my endTime.

[Robin.Kamenicky]

Hi qtruong,

Originally Posted by qtruong

Nonetheless, the convergence is reached, but chtMultiRegionFoam keeps running until my endTime.

the chtMultiRegionFoam should run till the endTime. It is transient solver not steady-state as chtMultiRegionSimpleFoam.

The residualControl allows to exit PIMPLE outer loops when the residual criteria are fulfilled. Then it continues with next time step.

Kind regards,
Robin

[qtruong]

Originally Posted by Robin.Kamenicky

Hi qtruong,


the chtMultiRegionFoam should run till the endTime. It is transient solver not steady-state as chtMultiRegionSimpleFoam.

The residualControl allows to exit PIMPLE outer loops when the residual criteria are fulfilled. Then it continues with next time step.

Kind regards,
Robin

Is there then a way to solve steady state conjugate heat transfer in OpenFoam 6 ?

[Robin.Kamenicky]

Hi qtruong,

Originally Posted by qtruong

Is there then a way to solve steady state conjugate heat transfer in OpenFoam 6 ?

There is no solver for steady state conjugated heat transfer in OpenFoam6. However, if your problem is steady state problem, the transient solver will converge to steady state.

Eventually you can try to use local time stepping (localEuler time derivative approximation).

Another possibility is to use OpenFoam5 and chtMultiRegionSimpleFoam. If I understand right, the difference between OpenFoam5 and OpenFoam6 is only in usability for conjugated heat transfer solvers.

Hope it helps,
Robin

[julieng]

Hello,


I try to result a CHT steady state case with openfoam 6 and chtMultiRegionFoam. I am not able to solve it, it crashes after few time steps.

chtMultiRegionSimpleFoam done the job with Openfoam 5, I obtained good accuracy with analytical solutions.



I read your post Robin.Kamenicky, you wrote :

There is no solver for steady state conjugated heat transfer in  OpenFoam6. However, if your problem is steady state problem, the  transient solver will converge to steady state.

What is the reason to have give up the steady state solver in openfoam 6 ?


Best regards

[Robin.Kamenicky]

Hi julieng,

Actually, I have been mistaken. The official documentation of OF6 for chtMultiRegionFoam tells:

Solver for steady or transient fluid flow and solid heat conduction, with
     conjugate heat transfer between regions, buoyancy effects, turbulence,
     reactions and radiation modelling.

What was the error?

Kind regrads,
Robin

[Robin.Kamenicky]

Hi julieng,

according to tutorials. You can setup scheme for time derivative to

steadyState

Kind Regards,
Robin

[julieng]

Hello Robin,

Yes it works for stationary cases, I have test it. I have same results than openfoam v5.

I try the new functionnality
"wallHeatTransferCoeff"

I read on the Openfoam 6 release:
Data Processing: function objects for individual regions in a multi-region simulation [ commit a5a034 ]; wallHeatTransferCoeff function object to calculate the wall heat transfer coefficient [ commit 99841e ]; in wallHeatFlux, improved efficiency of heat flux calculation [ commit 6584fa ] and corrected contribution of radiative heat flux [ commit 396259 ].

But I see that it works only for incompressible fluids… cht is for compressible fluids. Maybe someone knows how to modify the file.


I see the post of bloerb
https://www.cfd-online.com/Forums/op...ing-print.html

But I Don't know how to do. I am a total beginner in function object.

Best regards

[hokhay]

Originally Posted by julieng

Hello Robin,

Yes it works for stationary cases, I have test it. I have same results than openfoam v5.

I try the new functionnality
"wallHeatTransferCoeff"

I read on the Openfoam 6 release:
Data Processing: function objects for individual regions in a multi-region simulation [ commit a5a034 ]; wallHeatTransferCoeff function object to calculate the wall heat transfer coefficient [ commit 99841e ]; in wallHeatFlux, improved efficiency of heat flux calculation [ commit 6584fa ] and corrected contribution of radiative heat flux [ commit 396259 ].

But I see that it works only for incompressible fluids… cht is for compressible fluids. Maybe someone knows how to modify the file.


I see the post of bloerb
https://www.cfd-online.com/Forums/op...ing-print.html

But I Don't know how to do. I am a total beginner in function object.

Best regards

Do you need to change the anything in fvSolution and controlDict too? Such as relaxationFactors or Courant number.

Thank you