CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Phoenics

How to simulate plenum space?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 11, 2003, 09:57
Default How to simulate plenum space?
  #1
Song
Guest
 
Posts: n/a
Hello,

Does anybody have experience in simulating plenum space together with a room space? For example, there is a room, on the ceiling there is plenum, which is connected to the true inlet of this system. On the ceiling, there is diffuser, thru which air is pressurized from the plenum into the room. The room also has outlet on the side wall.

My problem is to simulate the diffuser. What type of boundary should I use (I already set plenum inlet as inlet type)? What should I do if I want to simulate the airflow coming out the diffuser at some angles from the normal direction of the diffuser? Many thanks,

Song
  Reply With Quote

Old   April 13, 2003, 19:41
Default Re: How to simulate plenum space?
  #2
Leon Mills
Guest
 
Posts: n/a
Song,

For the ceiling plenum, I tend to use a plate or thin plate to seperate the plenum from the room to simulate the ceiling tiles / plastre board. This sysem is good as you can define the porosity of the material a simulate air leakage in this way.

Diffusers I handle in two ways, firstly is using a plate with a poristy set to give the equivelant free area. Sencond is to building accurately in PHOENICE or some CAD platform and import the geomerty. Then use fine grid volume around the difussers or over the entire lining seperating the room from the plenum.

From experience it takes a fair number of cells to simulate the air moving out of a difuser at an angle and fine grid volumes (using built in grid techniques) are the best way of handling this interface. Also look at adjust the powers in the meshing so that more cells are in the area of interest and not over the whole space.

Hope this helps.

Leon Mills

  Reply With Quote

Old   April 14, 2003, 23:17
Default Re: How to simulate plenum space?
  #3
Song
Guest
 
Posts: n/a
Leon,

Really appreciate your quick response. It definitely points me to the right direction.

I did try to simulate the diffuser using porous plate and found it's difficult to get converged result. Then when I put fine grids there, the computation time doubled and the result just didn't converge. Is this normal? How should I solve it? Since I didn't use fine grids before, I am not quite sure whether I am doing the right thing.

In addition, you mentioned that using Phoenics to input the detail structure of diffuser. How to do that since the diffuser is so irregular? Should I use plate to make a diffuser?

Many thanks,

Song
  Reply With Quote

Old   April 14, 2003, 23:33
Default Re: How to simulate plenum space?
  #4
Leon Mills
Guest
 
Posts: n/a
Song,

The best way to build the diffuser is in a 3d drawing package and import the information over. If you need to buid it in VR-Editor look at insresting wedges and the like, and rotatinging them. If doing this turn on partial solids treatment.

I have found that this sort of problem - for me- did take a while to converge and I needed o pay around with the relaxation parameters - particular the velocity terms.

Have you selected and appropriate turbulence model, and is where you are looking at for convergence an approporaite spot.

When I do this sort of problem I normally set the inlet velocity to 1m/s and porosity to 100% (commpletely open) and size the make up air (natural or by fans) accordingly. My first stab is usally just an opening 1m high for the entire width of the space.

Ocen i get this solution to converge I set the porosity to 50% close for most diffusers, then set the pressure drop based on tech data 5-20 Pa. Get this solution to converge.

Then I set up the make up air by natural openings or by supply/exhaust air fans. Sometimes not providing enough make up air can cause this kind of problem not to converge.

Fine Grid volumes - irst try setting the grids to 2 in each of the planes. I would suggest to try to keep the grids approximately square in this region.

Hope this helps.

Leon Mills

  Reply With Quote

Old   April 14, 2003, 23:44
Default Re: How to simulate plenum space?
  #5
Song
Guest
 
Posts: n/a
Wah! Such a detailed response in such a short time. I'm totally surprised. Seems like it will be of great help to me.

Before I try this out, can you be specific about what you mean by inlet velocity and make up air? Does inlet velocity mean the inlet flow to the plenum system? What's make up air for? My understanding is that make up air is only used when exhaust flow is larger than inlet flow. Many thanks,

Song
  Reply With Quote

Old   April 15, 2003, 00:25
Default Re: How to simulate plenum space?
  #6
Leon Mills
Guest
 
Posts: n/a
Inlet air into the plenum is the amount of air entering the plenum.

Make up air / Relief opening is for the room to alow for the air entering the room from the plenum. In normal air conditrioing this is return air or spill air. You need somewhere for the air to go.

Hope this helps.

Leon Mills

  Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
space conservation law Dorain CD-adapco 1 February 22, 2005 09:11
mesh space Hannah liang CFX 3 August 27, 2002 11:53
Out of Environment Space Guillermo Solano Phoenics 2 April 5, 2002 08:13
RAM and Swap Space and HD space Anindya CD-adapco 1 March 9, 2001 04:07
HD Space for LES ANINDYA Main CFD Forum 4 February 16, 2001 12:56


All times are GMT -4. The time now is 13:38.