Boundary conditions for free convection in open domains

Cobra · February 19, 2020, 10:28

Hello,

I'm trying to simulate a very simple 2D case of natural convection on a warm cylindrical surface in the open atmosphere.

The main problem that I'm facing so far is to impose the right boundary conditions to the outer 'environment' borders of my domain.

I've tried to use 'pressure-inlet' for the lower boundary and 'pressure-outlet' for the side and top ones.

I've tried using 'Pressure-Based' and 'Density-Based' solver settings, with either Ideal Gas, Incompressible Ideal Gas and Boussinesq formulation for my gas density, and with Specified Operating Density either on or off.

I haven't been able to obtain a realistic velocity field with none of these settings.

In particular:

-with 'Pressure-Based' and 'Specified Operating Density' active I have a strong velocity field from the bottom to the top of the domain even when the DeltaT between the cylindrical surface and the domain is 0

-with 'Pressure-Based' and 'Specified Operating Density' the above mention problem doesn't exist anymore, but I have a strong recirculation from the top part of the domain to the lower one when the DeltaT is non-zero

-with 'Density-Based' and 'Boussinesq' gas density I still obtain an unrealistic velocity field with a non-zero DeltaT

What I'm I doing wrong? Could someone please try to replicate these simulation and let me know through which settings is it possible to obtain realistic results?

Thanks a lot.

vinerm · February 19, 2020, 10:59

Are you running it as steady-state or transient? With 0 $\Delta T$ , you may get unrealistic velocity field with steady-state solver but transient will return correct field. However, with some $\Delta T$ , you can do the following (and certainly run it as steady-state)

1. Ensure gravity in correct direction
2. If the density variation over the $\Delta T$ is not significant, you can use Boussinesq model, otherwise, use ideal gas law.
3. With Boussinesq, it is very important that the density in the materials panel and that in the Operating Conditions panel is same and is in accordance with the Boussinesq temperature specified in the Operating Conditions panel
4. For ideal gas, Operating Density should be set to 0.
5. If the domain is large, then the location of the reference pressure should be set to the highest point of the domain.
6. You can set all outer boundaries as either pressure-outlet or pressure-inlet. The current conditions are alright as well because you expect flow to go up.
7. Prefer using Coupled Solver with pseudo-transient but SIMPLE(C) will work as well.

No need to use density-based solver.

Cobra · January 19, 2021, 10:23

So I had to solve a problem with free convection again, and I tried to do as suggested.
The Boussinesq Model works great.
The incompressible Ideal Gas model still gives me some headaches though.

What I noticed so far:

-Boundary conditions: pressure-inlet or pressure-outlet work more or less the same

-Operating density: if there are no temperature differences in my domain I can leave it 'unspecified', and the velocity field will be indeed zero as ecpected.
If however I start switching on some Delta T on my boundaries, an irrealistic velocity field starts appearing.
For this case the best solution has been specifying an Operating density equal to the one that the gas has at the pressure outlets (i.e. with that Temperature and Pressure). The irrealistic velocity field goes than back close to 0, but not completely.

How can I get a physically more accurate solution?
Anyone who tried this in Fluent?

February 19, 2020, 10:59	Setup	#2
vinerm Senior Member Vinerm Join Date: Jun 2009 Location: Nederland Posts: 2,946 Blog Entries: 1 Rep Power: 35	Are you running it as steady-state or transient? With 0 $\Delta T$ , you may get unrealistic velocity field with steady-state solver but transient will return correct field. However, with some $\Delta T$ , you can do the following (and certainly run it as steady-state) 1. Ensure gravity in correct direction 2. If the density variation over the $\Delta T$ is not significant, you can use Boussinesq model, otherwise, use ideal gas law. 3. With Boussinesq, it is very important that the density in the materials panel and that in the Operating Conditions panel is same and is in accordance with the Boussinesq temperature specified in the Operating Conditions panel 4. For ideal gas, Operating Density should be set to 0. 5. If the domain is large, then the location of the reference pressure should be set to the highest point of the domain. 6. You can set all outer boundaries as either pressure-outlet or pressure-inlet. The current conditions are alright as well because you expect flow to go up. 7. Prefer using Coupled Solver with pseudo-transient but SIMPLE(C) will work as well. No need to use density-based solver. __________________ Regards, Vinerm PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
polynomial BC	srv537	OpenFOAM Pre-Processing	4	December 3, 2016 09:07
Radiation interface	hinca	CFX	15	January 26, 2014 17:11
Trouble compiling utilities using source-built OpenFOAM	Artur	OpenFOAM Programming & Development	14	October 29, 2013 10:59
Question about heat transfer coefficient setting for CFX	Anna Tian	CFX	1	June 16, 2013 06:28
RPM in Wind Turbine	Pankaj	CFX	9	November 23, 2009 04:05

January 19, 2021, 10:23		#3
Cobra New Member Nicholas Join Date: Nov 2015 Location: Modena, Italy Posts: 20 Rep Power: 10	So I had to solve a problem with free convection again, and I tried to do as suggested. The Boussinesq Model works great. The incompressible Ideal Gas model still gives me some headaches though. What I noticed so far: -Boundary conditions: pressure-inlet or pressure-outlet work more or less the same -Operating density: if there are no temperature differences in my domain I can leave it 'unspecified', and the velocity field will be indeed zero as ecpected. If however I start switching on some Delta T on my boundaries, an irrealistic velocity field starts appearing. For this case the best solution has been specifying an Operating density equal to the one that the gas has at the pressure outlets (i.e. with that Temperature and Pressure). The irrealistic velocity field goes than back close to 0, but not completely. How can I get a physically more accurate solution? Anyone who tried this in Fluent?