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

Buoyancy issue in free and forced convection problem

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 3, 2015, 05:52
Default Buoyancy issue in free and forced convection problem
  #1
New Member
 
Join Date: Apr 2010
Location: Athens, Greece
Posts: 15
Rep Power: 13
sosat1012 is on a distinguished road
Hello,
i am trying to solve a problem in CFX regarding the temperature distribution inside a greenhouse protected by a solid windbreak. There is a heating source at the floor of the greenhouse (input as constant temperature or heat flux, see picture 1)
results no buoy.jpg

Log law wind velocity profile at inlet (roughness z=0.05) with a velocity at 10m high equal to 1m/s and wind temperature of 10C. This means that at greenhouse level velocity is equal to 0.5-0.6. The point is to have low velocities in order to examine the free convection heating contribution inside the greenhouse. For higher wind velocities forced convection dominates.
Other inputs:
-->Air ideal Gas
-->k-e turbulence model
--> solving the Total Energy

When i solve the problem without buoyancy results seem to be ok (i have solved similar problems). In the first attached picture pressure contours, velocity vectors and boundary conditions and distances are provided.

But when i solve the exact same problem problem including buoyancy (DOMAIN/BASIC SETTINGS/BUOYANCY MODEL/ buoyant with g= - 9.81m/s2 at y-axis, ref density 1.2kg/m3) results seem quite odd (Second attached picture, pressure contours and velocity vectors). The only thing i change is the outlet boundary. I have to change from outlet to opening because there is back flow and cfx proposes that it is more suitable to use an opening. In fact i have never solved something including gravity so i am not sure what to really expect. But i think that this result is not correct. Is there a boundary i should change? What could possibly be the problem?
results with buoy.jpg

Convergence goes below 10^(-4) so i dont believe it is a convergence issue. I do not understand why velocity behaves like this (backflow at the top and exit at the lower part of the outlet). Shouldnt velocities exit normal to the outlet, as in the non buoyant case? And pressure stratification seems odd as well.

Thank you in advance
sosat1012 is offline   Reply With Quote

Old   June 3, 2015, 08:31
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,705
Rep Power: 130
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I suspect this is because when you set the outlet to be zero pressure it includes the hydrostatic head in the gravity model. But the boundary condition is using a fixed 1.2kg/m3 for the hydrostatic head, but in reality your density varies. This means you are not applying 0 pressure relative to hydrostatic and will create spurious flows (like what you see).

It might be better to specify the inlet and outlet to be velocity boundary conditions to avoid this. You will need a pressure boundary somewhere, so make the top sky condition a fixed pressure - it has no vertical component so avoids the problem.
ghorrocks is offline   Reply With Quote

Old   June 3, 2015, 08:59
Default
  #3
Senior Member
 
JuPa's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 361
Rep Power: 11
JuPa is on a distinguished road
A few things:

- You should be using the thermal energy equation and not the total energy equation (only use total energy if compressiblilty is an issue, i.e. flows with speed Ma>0.3)

- You're using air ideal gas, which uses the relationship PV=nRT to determine the change in gas properties. Under applications where there are large pressure variations this works fine. However I believe pressure everywhere is largely atmospheric with little to no hydrostatic contribution (since it's a gas).

Essentially this means you're using the density difference model to simulate buoyancy. I bet if you use the Boussinesq model you'll have far superior results and will see the effects you need to see.

To use Boussinesq use constant properties air as the material, such as Air at 25 C, and set a reference temperature and location (instead of a reference density and location).

[Further reading: the Boussinesq approximation actually is derived from an ideal gas law approximation. Only when you use it in CFD, you're removing the constraint that bouyancy needs to be a function of density (density difference model) and are now saying it's a function of temperature (Boussinesq model). This is fantastic when you have small fluctuations in pressure, but large fluctuations in temperature.]
JuPa is offline   Reply With Quote

Old   June 4, 2015, 06:03
Default
  #4
New Member
 
Join Date: Apr 2010
Location: Athens, Greece
Posts: 15
Rep Power: 13
sosat1012 is on a distinguished road
Thank you very much for your quick answers. They have been both helpful.

Especially your advice RicochetJ helped a lot. The simulation runs smoothly now and i get totally different (no backflow or odd pressure distributions) and much better results. Thanks again.
sosat1012 is offline   Reply With Quote

Old   June 4, 2015, 11:12
Default
  #5
Senior Member
 
JuPa's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 361
Rep Power: 11
JuPa is on a distinguished road
Happy to help.

Just make sure your buoyancy reference temperature is the average of the expected temperature range in your system, to ensure the Boussinesq approximation remains true.

For example if your maximum temperature in your system is approximately 50 degrees c, and your minimum is approximately 0 degrees c, then make the buoyancy reference temperature equal to 25 degrees c. It doesn't need to be exact - just a rough value.
JuPa 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
Free convection from vertical cylinder Mariusz FLUENT 1 February 2, 2017 13:36
forced and free convection over a hot sphere the new one Main CFD Forum 0 October 16, 2013 04:32
Free and forced convection in fluent? pilli FLUENT 4 June 10, 2007 14:59
turbulent scales of forced vortex and free vortex lcw Main CFD Forum 3 September 1, 2005 13:40
mixed convection raj calay Main CFD Forum 6 April 21, 1999 22:33


All times are GMT -4. The time now is 22:35.