CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

Boundary conditions for free convection in open domains

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 19, 2020, 10:28
Default Boundary conditions for free convection in open domains
  #1
New Member
 
Nicholas
Join Date: Nov 2015
Location: Modena, Italy
Posts: 20
Rep Power: 10
Cobra is on a distinguished road
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.
Attached Images
File Type: png Geom.PNG (8.4 KB, 31 views)
Cobra is offline   Reply With Quote

Old   February 19, 2020, 10:59
Default Setup
  #2
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 36
vinerm will become famous soon enough
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.
vinerm is offline   Reply With Quote

Old   January 19, 2021, 10:23
Default
  #3
New Member
 
Nicholas
Join Date: Nov 2015
Location: Modena, Italy
Posts: 20
Rep Power: 10
Cobra is on a distinguished road
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?
Cobra is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 02:31.