CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > FLUENT

screens in wind tunnel

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

LinkBack Thread Tools Search this Thread Display Modes
Old   August 22, 2005, 08:12
Default screens in wind tunnel
Posts: n/a
Hi every body,

I am studying on Climatic wind tunnel where i have to design a duct.In this outlet velocity at nozzle end is to be uniform velocity .I have to implement in screens on the duct. At present its 2d base analysis. For screens, an porous jump to be implemented.In 2d ,whether porous jump is to be mention as line or face ( width = thickness)? and also how to calculate the pressure drop calculation for screens.

Regards Ranga
  Reply With Quote

Old   August 22, 2005, 13:55
Default Re: screens in wind tunnel
Posts: n/a
1) Porous jump in 2D is always a LINE and in 3d is a FACE.

2) If you would have been more curious you would have found in Fluent's Documentation a fast, approximate method for calculating the C0 and C1 coefficients you need to input for porous jump boundary condition. The 1st is the inertial resistance of the screen and the 2nd is the viscous resistance. All nice and easy. The only problem is that the method is highly inaccurate (I tried to use it a short time ago and for my soul's peace verified the results using another approach: not even close!!).

So how can you do it? Simple: take a SINGLE hole of your screen and using symmetries all around, construct a test flow domain with a proper mesh (it is better if you can obtain y+=1, results will be more accurate) and simulate flow conditions for several velocities beyond minimum and maximum you expect to obtain for the wind tunnel imposing constant static pressure (101325 Pa) downstream and a velocity inlet upstream (if you can consider incompressible flow) or a pressure inlet (for compressible flow). Then calculate the total pressure drop for each case and plot vs. inlet velocity. You shold obtain a parabolic curve. For this curve, construct a interpolation polynome of this form:


a=C0, b=C1. Now there is another problem: as you will notice for the example given in the documenation, C1 coefficient is NEGATIVE!!!, which means the viscous contribution for total resistance of their porous media is NEGATIVE , which is obviously nonsense! I'm not sure they even noticed this, but one thing is true: you definitely cannot input a negative C1 in Fluent, this will always return error! This problem could appear in your case too, but don't be worried, increase the value of C0 just enough to cover C1's missing.

Now you will ask: can I trust this method? I compared the results obtained with experimental data and the agreement was very good.

Tip: if can mesh it with y+=1, use one of the low Reynolds models, not the Enhanced Wall Treatment!

And also don't worry about the time, I did all this in two days, for 4 different types of screens.

Best wishes, Razvan

  Reply With Quote


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
how to consider perforated wind tunnel wall in CFD simulation littlelz CFX 4 June 11, 2009 05:51
Virtual Wind Tunnel in FLUENT ND FLUENT 0 April 7, 2006 07:43
Wind Tunnel Experiment Validation zi FLUENT 1 August 5, 2005 18:19
Wind tunnel modeling Pandu CFX 3 May 19, 2003 21:49
Wind Tunnel Website now online Mike Worthey Main CFD Forum 0 June 6, 2000 02:27

All times are GMT -4. The time now is 06:37.