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

HEX flow in air-side

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 1, 1999, 04:12
Default HEX flow in air-side
  #1
Chetan Kumar
Guest
 
Posts: n/a
Hi all I intend to simulate flow in an HEX. There are a large number (240) of tubes through which the flue gas flows. The aim of the study is to find the pressure variation in the inlet and out ducts for air. I am using PHOENICS.

Now, as the number of tubes is large and defining tubes with circular cross-section is difficult I want to define the volume containing the tubes as a porous region. This seems to be a good idea to me. I need comments on this. Also, sensible values of porosity values can be suggested by people on this forum who know these things.

Thanks in advance Chetan
  Reply With Quote

Old   May 2, 1999, 01:36
Default Re: HEX flow in air-side
  #2
Duane Baker
Guest
 
Posts: n/a
Hello Chetan,

there are a great number of simulations which have been done with "distributed resistance" (or porous or volume averaged) models and you should do a literature search on these topics. However, the scope of such work is often more of an industrial redesign and some of the nitty gritty details are often absent.

1. A good paper to start with is:

"Computer analysis of the three dimensional flow and heat transfer in a steam generator" by Patankar and Spalding 1978, Forschung im Ingenieurwesen, vol 44, p47.

Also reprinted in:

Spalding, D. B. (Dudley Brian), 1923- "Numerical prediction of flow, heat transfer, turbulence, and combustion : selected works of Professor D. Brian Spalding" edited by Suhas V. Patankar.

2. The porosity must be determined from a drawing of the cross-section of the tube section and will probably vary with position as you move from one region to another. The porosity is likely to be in the range of 40-60% and therefore a large component is from the inertial terms in the sinks of momentum (see below).

3. Most of the models for momemtum sinks that you find will be of the form of Morgan's Law:

for i'th component of momentum:

S''' = -(mu/alpha +rho*|V|/beta) V_i

where the first term is an imperical law for the volume averaged viscous interactions which occur over the surfaces that we have neglected and the second is the for the inertial forces which we have integrated over. The coeficients alpha and beta will be anisotropic for a tube bank and a function of the porosity, pitch of tubes, diameter of tubes, etc. Some corelations are given in the paper that I mentioned.

4. Make sure you do a simple geometry test case with the model and compare to experimental data of the paper you get the correlation from to as a verification step!

5. You will probably also have to solve the energy equation...it is a heat exchanger after all and therefore source/sink terms will be required as well.

good luck.......................................Duane
  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
Simulation of air flow inside valve - FSI? Help! farianka Main CFD Forum 0 April 17, 2011 16:30
Blockmesh error - 2D scramjet - please help ishaninair OpenFOAM Native Meshers: blockMesh 7 March 18, 2011 01:14
Increasing air flow using fans jim sanders FLUENT 0 January 10, 2002 10:24
Question on 3D potential flow Adrin Gharakhani Main CFD Forum 13 June 21, 1999 05:18
computation about flow around a yawed cone Tylor Xie Main CFD Forum 0 June 9, 1999 07:33


All times are GMT -4. The time now is 04:33.