[hend]

Dear all,
I'm trying to solve an heat transfer issue with buoyantSimpleFoam. I reduced the geometry to a smooth channel with quadratic cross section, using 10*Dh to get a fully developed velocity profile. The geometry is shown in the figure below.

Attachment 63152
Selection_008.png

The problem is: wallHeatFlux doesn't correspond to dm/dt * cP * deltaT, whereas deltaT is determined via patchIntegrate and inlet temperature. The deviation is around 20% - 40%!
The problem arises using laminar as well as turbulent flow conditions. For turbulent flow I tried Low Re with y+<1 and wallFunction models with y+>30 using kOmegaSST and kEpsilon turbulence models.
In the simplified laminar case I tried first and second order discretization schemes and reduced the solvers tolerance for h equation to a magnitude of 1e-12. So convergence should be okay.
I tried lots of different BCs, which all didn't result in proper energy balance. In thermophysicalProperties I set rhoConst or perfectGas at equationOfState.
The simulation was also run with different meshes.
My OpenFoam version is 4.1.

Are there any ideas, what can be done to get correct results in terms of energy balance?

[hend]

Perhaps it might help to add the case. So here it is.
caseHeatTransfer-Re1000.zip
The mesh is removed due to data size. It's 30x30x400 cells, with homogeneous cell sizes.

I would be really pleased, if someone had an idea!

[piu58]

The buoyant solvers are finicking, especially in a combination of free convection and buoyancy. Do you have buoyancy effects in your problem? If not, try the combination of simpleFoam and scalarTransportFoam.

[hend]

Thanks for your reply!
As you suggested, I tried the combination simpleFoam and scalarTransportFoam. The disbalance concerning energy remains in a comparable order of magnitude, unfortunately.

[calf.Z]

Originally Posted by hend

Are there any ideas, what can be done to get correct results in terms of energy balance?

I also encounter the energy balance problem in buoyantSimpleFoam. Do you use a constant heat flux BC? The result of (h*phi)out-(h*phi)in is bigger than q*s. I have no idea about it.

[hend]

Originally Posted by calf.Z

I also encounter the energy balance problem in buoyantSimpleFoam. Do you use a constant heat flux BC? The result of (h*phi)out-(h*phi)in is bigger than q*s. I have no idea about it.

I used a fixedValue (temperature) BC for the hot section. But it doesn't make a difference, if you use constant heat flux.

What helped me to get rid of the energy balance problem, was adding an outlet section behind the section with hot walls to the simulations. I don't no why, but with this the energy balance is satisfied with around 2% deviation.

[calf.Z]

Originally Posted by hend

I used a fixedValue (temperature) BC for the hot section. But it doesn't make a difference, if you use constant heat flux.

What helped me to get rid of the energy balance problem, was adding an outlet section behind the section with hot walls to the simulations. I don't no why, but with this the energy balance is satisfied with around 2% deviation.

Thank you for giving the information.

You said you used fixedValue BC, does it mean an isothermo BC?

In my simulation, there is an isothermo wall behind the constant heat flux wall, so I think it is what you suggested? But the energy balance is still not satisfied.

[hend]

yes fixedValue means that the temperature is constant.

[arvindpj]

Just curious, when specifying constant heat flux bc for the wall, does the wall temperature vary with Y+ values.

I ran a similar simulation and noticed that for LowRe simulation, I had to use a Y+<<1 eg., Y+=0.02 to get mesh converged wall temperature results. For regular wall function approach, Y+>30, the wall temperatures always varied with Y+ values.

For alpha wall function, I used the alphajayatilleke. Any insight is much appreciated.

Cheers,
arvind

[calf.Z]

Originally Posted by arvindpj

Just curious, when specifying constant heat flux bc for the wall, does the wall temperature vary with Y+ values.

I ran a similar simulation and noticed that for LowRe simulation, I had to use a Y+<<1 eg., Y+=0.02 to get mesh converged wall temperature results. For regular wall function approach, Y+>30, the wall temperatures always varied with Y+ values.

For alpha wall function, I used the alphajayatilleke. Any insight is much appreciated.

Cheers,
arvind

Did you use the externalWallHeatFluxTemperature BC for giving constant heat flux? With this BC, the checking result of heat flux by wallHeatFlux is not the same as the setting one. the min and max are different. I do not know why.

And what do you mean mesh converged wall temperature? Thank you.

[julieng]

Hello,


I have the same problem of energy balance non respected with chtMutiRegionSimpleFoam (Openfoam v5). I use komegaSST without wall functions.
My y+ is 0.15, I reproduction your test case with inlet duct length = 10xD, heating zone duct length = 10xD, and outlet duct length = 5xD.


With rho = const, I have 5% of error between input power and output power, but with rho = perfectGas I have 30% of deviation!! with the same mesh and parameters (the simulation is converged residual < 10-5).
I have also a strange flow profile close to the outlet whatever i try, every-time some local high velocity close to the outlet...
See the posts:

chtMultiRegionSimpleFoam alphat



Maybe I can decrease y+ < 0.02.

Arvind, when you talk about lowRe, is it with komegaSST or with another turbulence model?

Someone has tried lowRe turbulence model like LaunderSharmaKE? I don't find inlet and outlet BC example for internal flows. Can someone share some experience with it ?


Best regards


Julien

[arvindpj]

Yes, I had used the externalWallHeatFluxTemperature BC. My objective is to estimate the wall temperature and/or temperature gradient at the wall. As that would determine whether I had to use the wall boiling model or not. (If Twall > Tsat).

I could get converged wall temp/gradient only at Y+ < 0.01.

Cheers,
Jay

[arvindpj]

Julien,

I am using kOmegaSST without wall functions. I am yet to try out LaunderSharmaKE.

Cheers,
-Jay

[julieng]

Thank you for your quick answer.

Can you share your 0/ files and system files please? (if possible)
I have inlet outlet, walls, there is a lot of possibility and advices on the forum for the lowRe BC.

Concerning the LaunderSharmaKE, do you mean that you try to work with it now?

Best regards

Julien

[hend]

Originally Posted by hend

I used a fixedValue (temperature) BC for the hot section. But it doesn't make a difference, if you use constant heat flux.

What helped me to get rid of the energy balance problem, was adding an outlet section behind the section with hot walls to the simulations. I don't no why, but with this the energy balance is satisfied with around 2% deviation.

If I remember correctly, I also studied laminar testcases with similar problems (unsatisfied energy balance). So trying different turbulence models will probably not help.



In my case adding an outlet section with adiabatic walls, was the only solution. For that section a certain length was necessary, which I determined parametically. If someone will find the reason why that helps, I would be interested to hear.


Cheers,
Hendrik

[julieng]

Hello hend,

What is the duct outlet lenght that you choose: duct diameter x how many ?

And how many was your y+ to see the Energy balance satisfied ?

Do you achieve to have good Energy balance with turbulent duct compressible flows with your additionnal duct at the outlet ? If yes can you tell your y+ and details about your BC? Thank you very much.

Best regards

[calf.Z]

Originally Posted by arvindpj

Yes, I had used the externalWallHeatFluxTemperature BC. My objective is to estimate the wall temperature and/or temperature gradient at the wall. As that would determine whether I had to use the wall boiling model or not. (If Twall > Tsat).

I could get converged wall temp/gradient only at Y+ < 0.01.

Cheers,
Jay

I used externalWallHeatFluxTemperature BC and the temperature field seems normal. But when I check q by wallHeatFlux. It gives min/max values and they are different with the setting q in the BC.As usual, min=max=setting q. I don't know if it is related to Y+. Thank you.

[julieng]

There is plenty of example of non balanced energy heat transfer cases on the forum.



Is there someone for sharing a very basic case of a (turbulent if possible) duct flow with appropriate mesh, appropriate BC, appropriate fvSolution and Scheme to see a satisfied thermal balance ?



It would be very helpful for a lot of people on the forum, I think.


Thank you.


Julien


PS: I reduce the y+ value of my mesh to 0.008, it doesn't improve the energy balance...

[hend]

Originally Posted by julieng

Hello hend,

What is the duct outlet lenght that you choose: duct diameter x how many ?

And how many was your y+ to see the Energy balance satisfied ?

Do you achieve to have good Energy balance with turbulent duct compressible flows with your additionnal duct at the outlet ? If yes can you tell your y+ and details about your BC? Thank you very much.

Best regards

The outlet length was 40 x d!


The y+ was for example 0.06 0.5 0.4 (min max average). I ran many different cases. The relative error of energy balance was 1.5 % in that case. Hope that helps!

[julieng]

Hello,
Can you post your BC please?
Do you have try turbulent flow?
How do you have mesh your case ? I suspect salome mesh to add some issue close to the output, i dont know how and why, but blockmesh give my better results with the same mesh. I need to try snappyhexmesh but i have to learn how to use it first.

Best regards