Convection to the ambient air
 

Hi foamers,
i am currently trying to simulate the convection from a solid, heated by its inside, to the ambient air. I don't find the kind of boundary i have to use.
I would like a boundary which let me fix the Temperature at the infinity, so the ambient air temperature, and the h coefficient for the heat transfer between my solid and the air.
Could you help me ?
Thanks.
LD

Hi laurentD,

Which solver are you using? Is your case something like a heated vertical wall in ambient air? Could you give us more details?

Hi Thiago,
a am using a chtMultiRegionFoam solver and the boundary on which i work is a boundary between a solid part and the ambient air, which is not meshed.
I think i have found something.
I will try to use externalWallHeatFluxTemperature with h and Ta.
Do you think it is a good method in my case ?
LD

Hey laurentD,

Now I get it! Once the air region is not meshed, I think it is.

I have a question :), suppose you have a solid region surrounded by a fluid in a laminar flow (chtMultiRegionSimple). Regarding the velocities and pressure BC's, do I need any special boundary condition for the fluid_to_solid patches (as is needed for T, e.g.)?
I'm using the fixedValue (no slip) for velocity and fixedFluxPressure for pressure.

Hello Thiago,

These BC's should do it, I'm using the same ones in my multiRegion cases.

Regards,

Alex

Hi,
the use of externalWallHeatFluxTemperature have not given the good results...
I have fixed :
ta = 293.15 (i think it is the external temperature)
h = 10 (the convection coefficient)
value = 293.15 (the initial value)
But after some timesteps, the value of the temperature on the solid have exploded, with values like 6e+22...
Any ideas ?
Maybe a problem of unity for h ?

Best regards,
Laurent

Hello Laurent,

If you don't give us a better information it's impossible to find out what you are doing wrong. You should post your log file, at least the piece corresponding to the last time steps so that we can see what you are doing wrong. What are your initial conditions? Is your geometry correct?

By the way, the units of h are [W/(m²*K)].

Regards,

Alex

Hi,
i understand.
You can find in attached files a directory with some of the files i have used.
Thank you for your time.
Best regards,
Laurent

And this job has run without any problems with adiabatic conditions on exterior boundaries, so i think the problem is not related to the geometry or anything like it.
I have just added the externalWallHeatFluxTemperature on each solid part.
Best regards

Hello Laurent,

You didn't share much information about your case (like which solver you are using, etc.) so it is difficult to judge the reason for the failure.

Anyways from the solver log file it can be observed that Courant number reaches very high value. Try with lesser "deltaT" value and check

-
Best Luck!

Hi,
thanks to spend part of yor time to help me.
I use the solver chtMultiRegionFoam, and i don't calculate the cinematic field, since it is calculated in a previous run. So in my previous studies, the blocking of the cinematic calculation allowed me to work with Courant number higher.

But this time there is a problem so i had tried to decrease the timestep. I have used dt = 1e-06 instead of 1e-02 and the maximal courant number is now equal to 1. But the problem of divergence of temperature still exits.

To be complete about the Courant number, i have to say that this is calculated on the Fluid part of my job, but this fluid part is inside the solid parts. The convection i am now trying to simulate is on the other side of the solid parts, the parts which are in contact with the ambient air.

I keep fighting to obtain results...
Best regards,
Laurent

Thank you for briefing again

Check your mesh quality? using "checkMesh". May be problem could be with the mesh. I don't know much detail of the solver so can't comment on it. Try with available tutorials: check out Maaike Van Der Tempel's slides, report and case files.

https://openfoamwiki.net/index.php/G..._-_planeWall2D

I hope this will solve your problem

-
Best Luck!

Thank you but i have already read it. I haven't found anything wich can help me.
I have used the checkMesh utility and everything seems ok.
I am currently doing tests on timepsteps and i see strange behaviours.
For example :
- when dt = 7e-03, the explosion came at t = 0,014,
- when dt = 1e-03, the explosion came at t = 0,006.
So my opinion is that problem comes from numerical scheme. If there was an unity problem, the explosion should arrive at the same time, shouldn't it ?
But even if i take dt = 1e-06, the problem si still alive.

Another road to follow maybe :
My geometrical mpdel is built on millimeters, so when i use it on OpenFOAM, i use transformPoints -scale (0,001 ...) and everything was working well before last friday (the day i tried to simulate natural convection on boundaries with exterior). Thanks to the "transformPoints" utility, all my model is in meters. When i look the polymesh/points files, the coordinates are in meters, so there isn't problem here.

Best regards,
Laurent

I have to precise :
i am working with OpenFOAM 2.1.0.
I prefer to say that beacuse maybe the utility i am trying to use weren't able to work with this version. If anybody can have informations on it...
Best regards,
Laurent

Hi guys,
i have more information to help those who want to help me.
Initially the temperature of the solid is around 283 K.
- if i put Ta = 293, h= 10, the job crashes when one cell of the solid boundary has a temperature higher than 293. Suddenly, all the temperature of my model is diverging.
From here, i consider that OF don't like when the order between Ta and Ts is inversed.
- if i put Ta = 280, h= 10, the job crashes during the first iteration.
- if i put Ta = 280, h= -10, the job run well but the results are false. It seems that the heat flux goes by the bad way. The 280 K ambient air doesn't bring freshness to the solid.
- if i put Ta = 380, h = 10, the job run but i don't see effects from the convection.
If you need more informations to have ideas, ask me, i really need help.
Thanks a lot.
Laurent

End of the discussion
 

Hi guys,
i have found the key of my problem.
As i said in a previous post, i am using OF 2.1.0, and i have seen on :

https://github.com/OpenFOAM/OpenFOAM...hScalarField.C

that there is some bugs to correct in files related to externalWallHeatFluxTemperature. Now i have a tool which works well.

Thank you Thiago, Alex and Tushar for your support and for your time.

Have a good day,
see you soon in this forum.

Laurent