[Mondal131211]

Hi Foamer,
I am a newcomer in OpenFOAM family. Last few months I am trying to learn OpenFOAM in details. Still, need to go a long way. As a part of the learning, I was having a problem of reproducing a result. That makes me confidence on OpenFOAM. Actually, I am trying to reproduce a result of another paper but failed several times. I can not understand the mistake.

I want to simulate ''Natural convection flow of air inside an open cavity''. The left wall of this cavity is considered as a hot wall and right side of this cavity is open. Top and bottom walls are insulated. This is a 2D case. I have already set up my simulation in buoyantBoussinesqPimpleFoam (OpenFOAM 3.1.1) based on this paper. But have not got the expected result. The boundary conditions of my simulation as follows,

Velocity:
Hot wall – fixedValue, uniform (0 0 0)
Top and Bottom wall - fixedValue, uniform (0 0 0)
Open boundary – zeroGradient
Default faces-empty

Temperature:
Hot wall – fixedValue, uniform 330
Top and Bottom wall - zeroGradient
Open boundary – inletOutlet, Inletvalue - uniform 300, value- 300
Default faces-empty

P_rgh:
Hot wall – fixedFluxPressure, rho-rhok, uniform 0
Top and Bottom wall- fixedFluxPressure, rho-rhok, uniform 0
Open boundary – fixedValue, uniform 0
Default faces-empty

P:
Hot wall – Calculated (0)
Top and Bottom wall - Calculated (0)
Open boundary – Calculated (0)
Default faces-empty

Others description is in the case file attached here. Please have a look.

Comparing paper link:

https://drive.google.com/file/d/1W7C...ew?usp=sharing

I can not understand what is my mistake. I am sharing my case file with this message. I have spent huge time solving this issue but finally failed to get a good result. All documents attached here in order to provide a good overview of the problem so that I can get a good suggestion from anyone. Please help me to figure it out tell me what was my problem. I am really struggling with this issue.

Need to mention here that, the set up my BC is in dimensional form as OpenFOAM deals with the dimensional equation. All stuff of this paper is in non-dimensional form and I convert it to dimensional form even the time step as well.

[Mondal131211]

Any suggestions, please? I would appreciate any types of help related to this post.

Cheers,
Razon

[Mcesar]

Hello Mondal, I don't know if you already solved your problem, but did you tried the pressureInletOutletVelocity for the open boundary? And I don't understand what was your problem?

[Mondal131211]

Originally Posted by Mcesar

Hello Mondal, I don't know if you already solved your problem, but did you tried the pressureInletOutletVelocity for the open boundary? And I don't understand what was your problem?

Hi Mcesar,

Thank you for your response. Actually, I am not finding the same streamline and isotherm figure. I didn't try by pressureinletoutletvelocity at open boundary. What about temperature BC? is that correct according to this paper BC? I should try by this. I will get back to you tomorrow after getting result by setting up pressureinletoutletvelocity at open boundary.

[Mondal131211]

Resolve this issue.Thanks

[Mcesar]

Originally Posted by Mondal131211

Resolve this issue.Thanks

Great ! What did you do to solve the problem ?

[Mondal131211]

Originally Posted by Mcesar

Great ! What did you do to solve the problem ?

Hi Mcesar,

Just set the ambient temperature (Fixedvalue) at open boundary and set the fixed pressure at this open boundary. Still have the issue with buoyantBoussinesqPimpleFoam. In this solver I haven't got any temperature gradient. Solved it by buoyantPimpleFoam.

[Mondal131211]

Originally Posted by Mondal131211

Hi Mcesar,

Just set the ambient temperature (Fixedvalue) at open boundary and set the fixed pressure at this open boundary. Still have the issue with buoyantBoussinesqPimpleFoam. In this solver I haven't got any temperature gradient. Solved it by buoyantPimpleFoam.

Hi Mcesar,

Oops, after investigating the result carefully, I found the result was wrong. It is not physically correct to set the ambient temperature at an open boundary because some warm fluid should go out through the open aperture. If I set the ambient temperature at open the fluid will go out as cold. That's not correct anymore.

Do you have any idea how to set the pressure at the open boundary? That is the only factor now I have to figure out.

Cheers,
Razon

[Mcesar]

Originally Posted by Mondal131211

Hi Mcesar,

Oops, after investigating the result carefully, I found the result was wrong. It is not physically correct to set the ambient temperature at an open boundary because some warm fluid should go out through the open aperture. If I set the ambient temperature at open the fluid will go out as cold. That's not correct anymore.

Do you have any idea how to set the pressure at the open boundary? That is the only factor now I have to figure out.

Cheers,
Razon

Hi, you can try the pressureInletOutletVelocity for velocity combined with fixedMean or fixedMeanOutletInlet for the pressure, I'm working with this two bc for open domains. Let me know if worked for you!

[Mcesar]

The model of the paper was set with QUICK for advective terms and Crank-Nicholson for time as the schemes of discretization. This could affect your results as well. I don't know if you already tried changing this, maybe it can help.

[Mondal131211]

Originally Posted by Mcesar

Hi, you can try the pressureInletOutletVelocity for velocity combined with fixedMean or fixedMeanOutletInlet for the pressure, I'm working with this two bc for open domains. Let me know if worked for you!

Hi Mcesar,

Please see the attached picture. I set up the BC like this for buoyantPimpleFoam. But fixedMeanOutletInlet, is that compatible with OpenFOAM 3.1.0 version? I am not sure. It is giving me error like an unknown patch field type.

Cheers
Razon

[Mcesar]

The fixedMeanOutletInlet was realeased for OF 6 I guess. Try the fixedMean. And change the discretization schemes.

[Mondal131211]

Hi Mcesar,

Thank you man. Your BC works fine. FixedMean with pressureInletOutletVelocity. You really saved my huge time.

Cheers,
Razon

[Mondal131211]

Originally Posted by Mcesar

The fixedMeanOutletInlet was realeased for OF 6 I guess. Try the fixedMean. And change the discretization schemes.

Hi Mcesar,

Thank you for your help to find suitable open boundary conditions. However, could you please make a comment on my attached case files? This is the same problem of natural convection inside an open cavity. But this time I used buoyantBoussinesqPimpleFoam. The simulation is running fine and reaching up to the last timestep. The problem is that I haven't seen any temperature gradient close to the wall. I am a bit surprised that the temperature gradient only stacks in the first cell. can you give any hints to overcome this situation?
If you get time please try to run this simulation for a while. It won't take too much time.

Natural Convection inside a open Cavity

cheers,
Razon