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

Comparison the airfoil 0012 experimental result and simulation result

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

Like Tree5Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   November 12, 2009, 02:49
Default try LES
  #21
Member
 
Ivan
Join Date: May 2009
Posts: 85
Rep Power: 8
ivanbuz is on a distinguished road
you guys may want to try LES. I did some airfoil flow simulation. though Cl and Cd are not important in my cases, I did simple comparison and they match experimental data pretty well. I guess the reason is that LES deals with the transition from leminar to turbulence pretty well.

But surely the computation cost is much much higher. parallel computation is needed for LES.
ivanbuz is offline   Reply With Quote

Old   November 12, 2009, 05:28
Default
  #22
Senior Member
 
Jouke de Baar
Join Date: Oct 2009
Posts: 122
Rep Power: 7
jack1980 is on a distinguished road
@ Makaero: roughness constant 0.5 is fine for flat plate, would expect to be ok for airfoil. However, it only takes effect when your roughness height is sufficiently large. So just converge your solution for smooth foil (ie rougness height = 0) and then try, say, roughness height of 0.0001 m. Roughness height is the diameter of the roughness grains on your surface.

@ harrislcy: Maybe the following will work? First converge your solution with 1st upwind laminar model. Then (do not initialize) for 1st upwind k-e. Finally (again do not initialize) for 2nd upwind k-e.
jack1980 is offline   Reply With Quote

Old   November 12, 2009, 12:46
Default
  #23
Member
 
ANIL
Join Date: Apr 2009
Posts: 35
Rep Power: 8
makaero is on a distinguished road
@ jack1980

Thnx...
makaero is offline   Reply With Quote

Old   November 16, 2009, 01:25
Default What is this?
  #24
New Member
 
Yang
Join Date: Oct 2009
Posts: 15
Rep Power: 7
harrislcy is on a distinguished road
"turbulent viscosity limited to viscosity ratio of 1.000000e+005 in 2 cells "

What make this happen? Is it the meshing problem? How to solve it?
harrislcy is offline   Reply With Quote

Old   November 16, 2009, 08:33
Default
  #25
Senior Member
 
Jouke de Baar
Join Date: Oct 2009
Posts: 122
Rep Power: 7
jack1980 is on a distinguished road
Sorry, should have told, that happens oftenly.

Before running k-e calcs, do the following:

Solve -> Initialize -> Initialize ...
Do not press Init! Scroll to the box containing Turbulent Kinetic Energy and write down the value. Press Close.

Solve -> Initialize -> Patch ...
Variable = Turbulent Kinetic Energy
Value = value you've written down
Zones to patch = fluid
Press patch

This should help, good luck!
blgypeng likes this.
jack1980 is offline   Reply With Quote

Old   November 18, 2009, 06:09
Default error...
  #26
New Member
 
Yang
Join Date: Oct 2009
Posts: 15
Rep Power: 7
harrislcy is on a distinguished road
Error: divergence detected in AMG solver: temperature

Again, another error opup again when in the K-ep silmulation. This happen after 200 iterations. How to avoid this?Thanks
harrislcy is offline   Reply With Quote

Old   November 19, 2009, 12:37
Default Inflow Boundary
  #27
New Member
 
Andy Robertson
Join Date: Mar 2009
Location: Long Island NY
Posts: 22
Rep Power: 8
AndyR is on a distinguished road
Check your inflow condition.
Make sure that the inflow is a close to laminar conditions as possible. Core flow of wind tunnels is generally turbulent, but at a very small intensity and length scale. This depends on the tunnel of course. Look at what the viscosity ratio is just downstream from the inlet. Except at tunnel walls (if you modeled them). It should be less than 1. A good quiet tunnel might have a turbulent viscosity ration of less than .1

Learned this the hard way myself
- Andy
AndyR is offline   Reply With Quote

Old   December 9, 2010, 11:50
Default
  #28
New Member
 
Join Date: Jun 2009
Posts: 6
Rep Power: 8
ferranpm is on a distinguished road
Hello people!

I want to test the profile NACA 0012 for differents alfa and compare the results with experimental and XFoil graphics. It should be simple, but my results are not satisfactory:

ro= 1,225 Kg/m^3
Mu_air=1,75*10^5 Kg/(m*s)
D=1

with these Data, i obtain the differents velocities (in m/s):

Re=200K -> vs= 2,8
Re=500k -> vs= 7,102
Re=3M -> vs=42,612
Re=6M -> vs=85,224

For alpha= 0°and different viscosity theories:

RE=6M
Spall. Alm. /// K-E Stndrd /// K-w SST Trans.flow /// X-Foil(=Exper.)
cd 3.31*10^(-2) /// 6.2*10^(-2) /// 3.32*10^(-2) /// 5.08*10^(-3)


RE=1M
K-E RNG /// K-E Stand (Ehn. W.T.) /// K-w SST Trs.fl /// X-Foil(=Exper.)
cd 2.1*10^(-3) /// 3.24*10^(-3) /// 1.73*10^(-3) /// 5.4*10^(-3)
RE=200k
Spall. Alm. /// K-E RNG /// K-w SST/// Trs.flow /// X-Foil(=Exper.)
cd 6.4*10^(-5) /// 1.5*10^(-4)/// 3.14*10^(-4) /// 1.02*10^(-2)



For Low-Re I thought that K-omega sst could be better than K-Epsylon, but I don't see a good result...anywhere (the mesh is good, from the profes.)


Thank you for your help!




Ferran
blgypeng likes this.
ferranpm is offline   Reply With Quote

Old   December 9, 2010, 12:46
Default
  #29
Senior Member
 
Jouke de Baar
Join Date: Oct 2009
Posts: 122
Rep Power: 7
jack1980 is on a distinguished road
Hi, you might be having trouble with the transition point. I think there are two approaches:

- Move from xfoil to experimental data with a ' trip wire '. This should fix the transition point near the leading edge. Now you can really use a turbulence model in you entire domain.

- If you want to stick with the xfoil data: try running viscous as well. If the exp. data is somewhere between your viscous and turbulent (for examp. rke) results, you might want to look into fixing the transition point manually. This can be done by splitting your grid in a viscous and a turbulent part.

Good luck!
jack1980 is offline   Reply With Quote

Old   June 24, 2011, 03:06
Default
  #30
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
hey all of you try k-w turbulence model. This works best for airfoils
cfd seeker is offline   Reply With Quote

Old   August 29, 2013, 10:27
Default
  #31
New Member
 
Alexandre Felipe Medina Correa
Join Date: Aug 2013
Posts: 3
Rep Power: 3
LexMedina is on a distinguished road
Hey guys,

I am having the same problem with Fluent here. I am an aeronautical engineering bachelor's student and as part of a research project I am first simulating the flow around a NACA0012 with 0 AoA.

My Reynolds is about 1.0 e4, and my Cd should be around 0.037.
First I tried to use a K-Omega SST, but after reaching 1.0e-7 residuals, my cd is still 0.13. I tried also S-A, and the cd drops to 0.05, but my continuity can't converge to less than 1.0e-4.
Since it is a symmetric airfoil, the Cl should be zero, but now is around 1.0e-5 for S-A and 1.0e-3 for k-W SST.

I used all the standart settings. Also, my Y+ is in the range 1.0 to 1.4.
LexMedina is offline   Reply With Quote

Reply

Tags
airfoil, experimental data, fluent, naca 0012, naca 4415

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
About probe result of Wave simulation shiw FLOW-3D 3 March 13, 2009 10:15
Single phase result file for multiphase simulation Kushagra CFX 2 July 8, 2008 21:14
Airfoil 2D, very weird result Martin FLUENT 4 June 13, 2007 12:21
Airfoil Simulation for Validation Purposes Angela Bong Main CFD Forum 7 September 13, 2006 13:04
how to make sure the simulation result is correct? sham81 CFX 3 March 22, 2004 17:41


All times are GMT -4. The time now is 13:41.