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

How to set Boundary in comepute low speed flow

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

LinkBack Thread Tools Search this Thread Display Modes
Old   July 9, 2005, 13:25
Default How to set Boundary in comepute low speed flow
Posts: n/a
hi all

when i will use fluent to compute the low speed(Ma=0.2, alpha =18 degree) flow around the air-plane, i make icem to meshing hex grids ,I'd like to know whether i use couple or segerate , and what Y+ value is best(mine Y+ is 30-200)? how to set inlet or outlet?

when i used SA tublence model , the Cd was about double of the winner tunnel's values , so i think it is too large , and Cl is also larger. would you tell me how can i do it better?
  Reply With Quote

Old   July 10, 2005, 05:48
Default Re: How to set Boundary in comepute low speed flow
Posts: n/a
1. You must surely use segregated solver because your flow is dominated by low velocities.

2. If you succedeed in making a structured grid around the airplane with orthogonal boundary layer, there is not so much concerning about Y+, but it must not exceed 100 if you're using Ymin>30, and the medium value is best around 40-50.

3. Your velocity is pretty low, but the compressibility is not negligible, especially if you want to calculate more precisely Cl and Cd (taking into account that these values are oftenly obtained with errors of 10 to 25 percent!!, even with the most complicated turbulence models) so I advise you to try compressible approach.

4. The flow domain could be made in two ways:

-try to simulate the windtunnel environement and in this case you have to use a pressure-inlet+pressure-outlet pair (but it would be a lot more convenient to use a incompressible approach with a velocity-inlet+pressure-outlet pair), which should give you results closer to the tunnel measurements

-use an external domain with a pressure-far-field boundary placed at (at least!!)10 lengths of airplane, that should give results closer to real life situations

5. Your angle of attack is quite high, so the flow over the airplane's wings could be partially separated, which will strongly influence Cl and Cd values. In this case, you better try a k-w model (not sst-kw), but be very careful what turbulence specification method you choose (better try a turb.intensity+lenght-scale pair, these values are easy to calculate in windtunnel environement, or turb.intensity<0.5%>-turb.viscosity-ratio<1> for external flow). The best solution is of course RSM, but it is hard to work with.

Hope this will help you.

Best wishes, Razvan
  Reply With Quote

Old   July 11, 2005, 06:50
Default Re: How to set Boundary in comepute low speed flow
Posts: n/a
thank you very very much , i hope to study more from you ! i will try again according to your hint!
  Reply With Quote

Old   June 4, 2009, 16:44
New Member
ilker cakar
Join Date: Jun 2009
Posts: 1
Rep Power: 0
ilkerrior is on a distinguished road
i know the topic is old but i need to try my chance

firstly ur informations helped me a lot, i found some ways to calculate the intensity and the lenght scale;

I=0,16.Re^(-1/8) and L=0,07.Dh

I: Intensity
Re: Reynolds number
L: Lenght scale
Dh: Hydraulic diameter

i wonder if these equations are useful for a wind tunnel flow,
(i am analysing a car model in a wind tunnel)
ilkerrior is offline   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
CFX does not continue Shafiul CFX 10 February 17, 2011 07:57
Boundary conditions low Mach number flow lost.identity Main CFD Forum 0 November 28, 2010 04:44
2D Low Speed Airfoil Problem when altering Inlet mike wilson CFX 12 August 3, 2010 11:06
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 04:05
Can 'shock waves' occur in viscous fluid flows? diaw Main CFD Forum 104 February 16, 2006 05:44

All times are GMT -4. The time now is 13:10.