How to set Boundary in comepute low speed flow

July 9, 2005, 14:25

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?

July 10, 2005, 06:48

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

July 11, 2005, 07:50

thank you very very much , i hope to study more from you ! i will try again according to your hint!

ilkerrior · June 4, 2009, 17:44

Hello,
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)

July 9, 2005, 14:25	How to set Boundary in comepute low speed flow	#1
zuo Guest 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?

July 10, 2005, 06:48	Re: How to set Boundary in comepute low speed flow	#2
Razvan Guest 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

July 11, 2005, 07:50	Re: How to set Boundary in comepute low speed flow	#3
zuo Guest Posts: n/a	thank you very very much , i hope to study more from you ! i will try again according to your hint!

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
CFX does not continue	Shafiul	CFX	10	February 17, 2011 08:57
Boundary conditions low Mach number flow	lost.identity	Main CFD Forum	0	November 28, 2010 05:44
2D Low Speed Airfoil Problem when altering Inlet	mike wilson	CFX	12	August 3, 2010 12:06
RPM in Wind Turbine	Pankaj	CFX	9	November 23, 2009 05:05
Can 'shock waves' occur in viscous fluid flows?	diaw	Main CFD Forum	104	February 16, 2006 06:44

June 4, 2009, 17:44		#4
ilkerrior New Member ilker cakar Join Date: Jun 2009 Posts: 1 Rep Power: 0	Hello, 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)