|
[Sponsors] |
Comparison the airfoil 0012 experimental result and simulation result |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
November 12, 2009, 01:49 |
try LES
|
#21 |
Member
Ivan
Join Date: May 2009
Posts: 85
Rep Power: 17 |
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. |
|
November 12, 2009, 04:28 |
|
#22 |
Senior Member
Jouke de Baar
Join Date: Oct 2009
Posts: 127
Rep Power: 16 |
@ 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. |
|
November 12, 2009, 11:46 |
|
#23 |
Member
ANIL
Join Date: Apr 2009
Posts: 35
Rep Power: 17 |
@ jack1980
Thnx... |
|
November 16, 2009, 00:25 |
What is this?
|
#24 |
New Member
Yang
Join Date: Oct 2009
Posts: 15
Rep Power: 16 |
"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? |
|
November 16, 2009, 07:33 |
|
#25 |
Senior Member
Jouke de Baar
Join Date: Oct 2009
Posts: 127
Rep Power: 16 |
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! |
|
November 18, 2009, 05:09 |
error...
|
#26 |
New Member
Yang
Join Date: Oct 2009
Posts: 15
Rep Power: 16 |
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 |
|
November 19, 2009, 11:37 |
Inflow Boundary
|
#27 |
Member
Andy Robertson
Join Date: Mar 2009
Location: Long Island NY
Posts: 46
Rep Power: 17 |
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 |
|
December 9, 2010, 10:50 |
|
#28 |
New Member
Join Date: Jun 2009
Posts: 6
Rep Power: 17 |
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 |
|
December 9, 2010, 11:46 |
|
#29 |
Senior Member
Jouke de Baar
Join Date: Oct 2009
Posts: 127
Rep Power: 16 |
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! |
|
June 24, 2011, 03:06 |
|
#30 |
Senior Member
Join Date: Mar 2011
Location: Germany
Posts: 552
Rep Power: 20 |
hey all of you try k-w turbulence model. This works best for airfoils
|
|
August 29, 2013, 10:27 |
|
#31 |
New Member
Alexandre Felipe Medina Correa
Join Date: Aug 2013
Posts: 4
Rep Power: 13 |
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. |
|
Tags |
airfoil, experimental data, fluent, naca 0012, naca 4415 |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
About probe result of Wave simulation | shiw | FLOW-3D | 3 | March 13, 2009 09:15 |
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 16:41 |