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

Help! Could anyone help me on Simulation of 2D airfoil?

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   April 26, 2011, 20:54
Default
  #21
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 467
Rep Power: 9
Martin Hegedus is on a distinguished road
There should be a way to set the Courant (CFL) number. The CFL number is usually constant throughout the domain and the actual time step a cell uses is then based on this number and the cell size. The larger the cell size, the larger the local time step. By decreasing the CFL number I hope you will find that the problem converges. It is the main way to converge a solution. Using the CFL number means that you are looking for a steady state solution and not a time accurate solution (since the actual time step varies across the grid). If you are after a time accurate solution you need to specify a constant physical time step.
Martin Hegedus is offline   Reply With Quote

Old   April 26, 2011, 21:07
Default
  #22
Member
 
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 6
didiean is on a distinguished road
Quote:
Originally Posted by Martin Hegedus View Post
There should be a way to set the Courant (CFL) number. The CFL number is usually constant throughout the domain and the actual time step a cell uses is then based on this number and the cell size. The larger the cell size, the larger the local time step. By decreasing the CFL number I hope you will find that the problem converges. It is the main way to converge a solution. Using the CFL number means that you are looking for a steady state solution and not a time accurate solution (since the actual time step varies across the grid). If you are after a time accurate solution you need to specify a constant physical time step.
Well, for FLUENT, only the density-based solver can activate the set of CFL number~~
didiean is offline   Reply With Quote

Old   April 26, 2011, 21:13
Default
  #23
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 467
Rep Power: 9
Martin Hegedus is on a distinguished road
OK, so I think that is the solver you need to use. I believe there is an explicit (uncoupled) and implicit (coupled) solver. The best bet is probably to go with the implicit solver, at least for now.
Martin Hegedus is offline   Reply With Quote

Old   April 27, 2011, 03:30
Default
  #24
Member
 
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 6
didiean is on a distinguished road
Quote:
Originally Posted by Martin Hegedus View Post
OK, so I think that is the solver you need to use. I believe there is an explicit (uncoupled) and implicit (coupled) solver. The best bet is probably to go with the implicit solver, at least for now.
Well~Coupled scheme for pressure-velocity coupling does seem to work. But the reason still remains not clear. As I know somebody does use normal SIMPLE to get the convergent results~
Thanks a lot~ You are so kind
didiean is offline   Reply With Quote

Old   April 27, 2011, 06:51
Default
  #25
Senior Member
 
Raashid Baig
Join Date: Mar 2010
Location: Bangalore, India
Posts: 136
Rep Power: 7
cfd_newbie is on a distinguished road
Hi Felix,
I am getting into this discussion late, but I want to why are you simulating S809 airfoil, are you planning to go for NREL Phase VI validation ?
cfd_newbie is offline   Reply With Quote

Old   April 27, 2011, 08:36
Default
  #26
Member
 
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 6
didiean is on a distinguished road
Quote:
Originally Posted by cfd_newbie View Post
Hi Felix,
I am getting into this discussion late, but I want to why are you simulating S809 airfoil, are you planning to go for NREL Phase VI validation ?
Thank you~
What I want to investigate is on wind turbine. Just because lots of experimental and simulating data are available for S809. This is easy to compare for my first stage of simulation.
didiean is offline   Reply With Quote

Old   April 27, 2011, 20:15
Default
  #27
New Member
 
Hamidreza
Join Date: Apr 2011
Posts: 6
Rep Power: 6
compeng is on a distinguished road
Dear Didiean,

Do you analyse with respect to time or just steady? If you analyse with time, may you describe what should man do to change it to time dependent?

Cheers,
compeng is offline   Reply With Quote

Old   April 27, 2011, 20:44
Default
  #28
Member
 
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 6
didiean is on a distinguished road
Quote:
Originally Posted by compeng View Post
Dear Didiean,

Do you analyse with respect to time or just steady? If you analyse with time, may you describe what should man do to change it to time dependent?

Cheers,
Currently, I just simulate the steady case.
I don't quite understand what you you mean by "change it to time dependent". If you mean simulating unsteady case, for FLUENT, it includes unsteady solver which could solve this.
didiean is offline   Reply With Quote

Old   April 27, 2011, 21:36
Default
  #29
New Member
 
Hamidreza
Join Date: Apr 2011
Posts: 6
Rep Power: 6
compeng is on a distinguished road
Yeah, I meant for Unsteady. Also for steady you can find 2 tutorials in internet which can help you. for 2D it has no problem.

https://confluence.cornell.edu/displ...+Specification

Cheers,
compeng is offline   Reply With Quote

Old   April 27, 2011, 21:59
Default
  #30
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 467
Rep Power: 9
Martin Hegedus is on a distinguished road
Just for fun I ran Aero Troll CFD (http://www.hegedusaero.com/software.html) on the S809 (Mach=0.10, Re=2e6, fully turbulent SA, characteristic B.C., incoming turb=0.1, C grid, farfield distance=50 times chord) All the runs were steady and all residuals converged. I've also included the CFL number I used.

"alpha" "cl" "cd" "CFL"
0.0 1.280048e-01 1.417824e-02 20
5.0 6.907618e-01 1.618729e-02 20
10.0 1.186345e-00 2.412572e-02 20
12.5 1.319514e-00 3.924694e-02 20
15.0 1.303051e-00 7.187542e-02 20
20.0 1.260819e-00 1.572631e-01 20
22.5 9.683451e-01 2.949351e-01 10
25.0 8.443910e-01 4.430438e-01 10
30.0 8.844666e-01 5.819109e-01 10

The results can be compared to the tripped results from the Delft University data. (http://www.osti.gov/bridge/purl.cove...9/webviewable/) I didn't plot the numbers, but, eyeballing it, before stall, the values seem to compare well. The CFD and WT disagree once stall occurs. From what I read on the net, people seem to attribute this lack of agreement to the turbulence model. Considering that the Delft max stall values seem to be somewhat insensitive to Reynolds number and whether the flow is tripped or not, I'm skeptical. It could be that how the wing stalls at the WT wall has affected the stall characteristics at the position where the data was taken. The ratio of half span to chord is 1.04 and the pressure orifices are not at the center line thus they are closer to one wall than the other. Unfortunately the report does not comment on wall interference effects at stall and I can't get the information I want out of the B&W oil photographs included in the report. Of course, I very well may be wrong on my thoughts about stall.

If someone is interested, they can create a simple 3D model of it by stretching the grid along the span and specify no-slip conditions (or maybe just no-slip in the vicinity of the airfoil, and slip everywhere else to minimize B.L. buildup) at the ends. If I have time, I might do it.
Martin Hegedus is offline   Reply With Quote

Old   April 27, 2011, 23:02
Default
  #31
Member
 
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 6
didiean is on a distinguished road
Quote:
Originally Posted by Martin Hegedus View Post
Just for fun I ran Aero Troll CFD (http://www.hegedusaero.com/software.html) on the S809 (Mach=0.10, Re=2e6, fully turbulent SA, characteristic B.C., incoming turb=0.1, C grid, farfield distance=50 times chord) All the runs were steady and all residuals converged. I've also included the CFL number I used.

"alpha" "cl" "cd" "CFL"
0.0 1.280048e-01 1.417824e-02 20
5.0 6.907618e-01 1.618729e-02 20
10.0 1.186345e-00 2.412572e-02 20
12.5 1.319514e-00 3.924694e-02 20
15.0 1.303051e-00 7.187542e-02 20
20.0 1.260819e-00 1.572631e-01 20
22.5 9.683451e-01 2.949351e-01 10
25.0 8.443910e-01 4.430438e-01 10
30.0 8.844666e-01 5.819109e-01 10

The results can be compared to the tripped results from the Delft University data. (http://www.osti.gov/bridge/purl.cove...9/webviewable/) I didn't plot the numbers, but, eyeballing it, before stall, the values seem to compare well. The CFD and WT disagree once stall occurs. From what I read on the net, people seem to attribute this lack of agreement to the turbulence model. Considering that the Delft max stall values seem to be somewhat insensitive to Reynolds number and whether the flow is tripped or not, I'm skeptical. It could be that how the wing stalls at the WT wall has affected the stall characteristics at the position where the data was taken. The ratio of half span to chord is 1.04 and the pressure orifices are not at the center line thus they are closer to one wall than the other. Unfortunately the report does not comment on wall interference effects at stall and I can't get the information I want out of the B&W oil photographs included in the report. Of course, I very well may be wrong on my thoughts about stall.

If someone is interested, they can create a simple 3D model of it by stretching the grid along the span and specify no-slip conditions (or maybe just no-slip in the vicinity of the airfoil, and slip everywhere else to minimize B.L. buildup) at the ends. If I have time, I might do it.
Thanks a lot~
I have heard some interesting comments that people who doing experiments and CFD never trust what they get. Maybe I expect too much from CFD. As the Cl is 0.1469 at 0 AOA, I just expect results of CFD around it less than 5% error. Sometimes, the trend is more important than the values themselves I think. And different turbulence models are available for different cases. Certain turbulence model can predict the stall angle well but not all of them. For the experimental results of DTU, as the intervals they give are big, the stall angle may not be so clear. Your analyses on the experimental results are very brilliant.
didiean is offline   Reply With Quote

Old   April 28, 2011, 01:42
Default
  #32
Senior Member
 
Raashid Baig
Join Date: Mar 2010
Location: Bangalore, India
Posts: 136
Rep Power: 7
cfd_newbie is on a distinguished road
Quote:
Originally Posted by Martin Hegedus View Post
Just for fun I ran Aero Troll CFD (http://www.hegedusaero.com/software.html) on the S809 (Mach=0.10, Re=2e6, fully turbulent SA, characteristic B.C., incoming turb=0.1, C grid, farfield distance=50 times chord) All the runs were steady and all residuals converged. I've also included the CFL number I used.

"alpha" "cl" "cd" "CFL"
0.0 1.280048e-01 1.417824e-02 20
5.0 6.907618e-01 1.618729e-02 20
10.0 1.186345e-00 2.412572e-02 20
12.5 1.319514e-00 3.924694e-02 20
15.0 1.303051e-00 7.187542e-02 20
20.0 1.260819e-00 1.572631e-01 20
22.5 9.683451e-01 2.949351e-01 10
25.0 8.443910e-01 4.430438e-01 10
30.0 8.844666e-01 5.819109e-01 10

The results can be compared to the tripped results from the Delft University data. (http://www.osti.gov/bridge/purl.cove...9/webviewable/) I didn't plot the numbers, but, eyeballing it, before stall, the values seem to compare well. The CFD and WT disagree once stall occurs. From what I read on the net, people seem to attribute this lack of agreement to the turbulence model. Considering that the Delft max stall values seem to be somewhat insensitive to Reynolds number and whether the flow is tripped or not, I'm skeptical. It could be that how the wing stalls at the WT wall has affected the stall characteristics at the position where the data was taken. The ratio of half span to chord is 1.04 and the pressure orifices are not at the center line thus they are closer to one wall than the other. Unfortunately the report does not comment on wall interference effects at stall and I can't get the information I want out of the B&W oil photographs included in the report. Of course, I very well may be wrong on my thoughts about stall.

If someone is interested, they can create a simple 3D model of it by stretching the grid along the span and specify no-slip conditions (or maybe just no-slip in the vicinity of the airfoil, and slip everywhere else to minimize B.L. buildup) at the ends. If I have time, I might do it.
Hi Martin,
Have you looked into the the following paper by Dr. Menter where he has compared the experimental and CFD results of S809 airfoil ? "Predicting 2D Airfoil and 3D Wind Turbine Rotor Performance using a Transition Model for General CFD Codes",
R. Langtry, J. Gola and F. Menter, ANSYS CFX, Otterfing, Germany, AIAA-2006-0395 44th AIAA Aerospace Sciences Meeting and Exhibit

About the inaccuracy of the experimental results - I think the chances of CFD results being wrong are about 100 times greater than experimental results for this case.
cfd_newbie is offline   Reply With Quote

Old   April 28, 2011, 02:00
Default
  #33
Member
 
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 6
didiean is on a distinguished road
Quote:
Originally Posted by cfd_newbie View Post
Hi Martin,
Have you looked into the the following paper by Dr. Menter where he has compared the experimental and CFD results of S809 airfoil ? "Predicting 2D Airfoil and 3D Wind Turbine Rotor Performance using a Transition Model for General CFD Codes",
R. Langtry, J. Gola and F. Menter, ANSYS CFX, Otterfing, Germany, AIAA-2006-0395 44th AIAA Aerospace Sciences Meeting and Exhibit

About the inaccuracy of the experimental results - I think the chances of CFD results being wrong are about 100 times greater than experimental results for this case.
I read this paper before. It seems that CFD using full turbulence model cannot predict the Cl as well as that using transitional models. I get nearly the same conclusion. But I can't explain it. I used to consider the full turbulence model do predict the Cl very well though large departure for Cd.
didiean is offline   Reply With Quote

Old   April 28, 2011, 15:37
Default
  #34
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 467
Rep Power: 9
Martin Hegedus is on a distinguished road
Quote:
Originally Posted by cfd_newbie View Post
Hi Martin,
Have you looked into the the following paper by Dr. Menter where he has compared the experimental and CFD results of S809 airfoil ? "Predicting 2D Airfoil and 3D Wind Turbine Rotor Performance using a Transition Model for General CFD Codes",
R. Langtry, J. Gola and F. Menter, ANSYS CFX, Otterfing, Germany, AIAA-2006-0395 44th AIAA Aerospace Sciences Meeting and Exhibit

About the inaccuracy of the experimental results - I think the chances of CFD results being wrong are about 100 times greater than experimental results for this case.
Unfortunately I'm not close enough at the moment to the local university to access the paper. And when searching for it, there doesn't seem to be a public version available. When I get a chance I'll pick it up. I am interested in the results.

In regards to the experiment, I don't think it is wrong. For me, personally, I'm not sure I completely understand the data presented. And I like to be cautious. For example, once the separation bubble occurs, and assuming the results are steadyish (which they seem to be) a vortex will be running along the span on the top side of the wing (i.e. 3D airfoil). The ends of the vortex that are at the no slip wall can not go into the wall, therefore they must turn downstream. And from the Delft report it sounds like the end plates are solid (i.e. non porous) So what exists is a horseshoe vortex where the bound leg (i.e. leg parallel to span) is hovering above the wing and the trailing legs (i.e. legs perpendicular to airfoil) go down stream and are next to the WT wall. Those bound legs will create a downwash on the wing, thus reducing the maximum lift. So the question then becomes, how big is this effect? Of course, it is probably best to assume that if the separation bubble is significant, the tailing legs will also be. I doubt viscosity has had much of a chance to reduce their strength. So last night I put together a test case at 15 degrees and am running it. It will take a while to run since I can't dedicate that much CPU time to the problem. Unfortunately the grid is also somewhat coarse.
Martin Hegedus is offline   Reply With Quote

Old   April 29, 2011, 13:36
Default
  #35
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 467
Rep Power: 9
Martin Hegedus is on a distinguished road
Attached are the results for my 3D run of the S809 airfoil.

M=0.1, Re=2.0e6 (based on chord), alpha=15, fully turbulent SA.

My grid is a C grid with 300 cells along chord (I) direction (50 wake, 100 airfoil bottom, 100 airfoil top, 50 wake), 50 cells along span (J) direction, and 100 cells outward (K) direction. I've used symmetry and have only modeled half the span. J=0 is symmetry and J=50 is the wall. To simulate the walls of the Delft WT I set a portion of my C grid (J=50) to a no slip BC, and the rest was slip. I didn't want a boundary layer to build up over the entire J=50 surface. My first grid point is 1.0e-5 off the airfoil and the wall.

The Delft data was taken at 0.2725 (non dim by chord) from the center line. Therefore, I used this span location to calculate my cl and cd.

The Results:
cl = 1.170257
cd = 0.131609

This compare to my 2D results of
cl (2D) = 1.303051e-00
cd (2D) = 7.187542e-02

The cl with wall interference has fallen with respect to the 2D value about 11 percent.

The reason I ran fully turbulent SA is that this is currently the only turbulence model I have coded in Aero Troll CFD and my main intent was to use this example to further test the code. From seeing the results posted by Felix and the Delft data, it is clear that the transitional turbulence model of Fluent compares better for Delft's non fixed data at and below 5 degrees angle of attack. The fully turbulent SA results compare well to Delft's fixed data. At 10 degrees angle of attack the Delft data appears to be influenced by the wall. Therefore, at 10 degrees angle of attack a true 3D CFD model needs to be built and analyzed for any true conclusion to be drawn on the validity of the various turbulence models.

As for pretty pictures,
1) Shows cl vs. span. Y=0 is at the symmetry plane and Y=1.04 is at the wall. The Delft data was taken at about Y=0.2725
2) Shows the airfoil surface and my version of the end plate. For the end plate I used a portion of the C grid.
3) Shows the entire side view of the C grid
4) Shows the v component of the velocity vector. The velocity has been non-dimensionalized by the freestream speed of sound. Planes at the plane of symmetry, trailing edge, and leading edge are shown. This plot indicates qualitatively the size of the vortex at the trailing edge. A small vortex at the leading edge can also be seen.
5) Shows the magnitude of the velocity vector. A slow region can be seen at the trailing edge.
6) Shows the isosurface of mag(velocity)=0.04. This is a qualitative representation of the wall interference.
Attached Images
File Type: png cl_vs_y.png (4.2 KB, 39 views)
File Type: jpg dist_a.jpg (98.1 KB, 50 views)
File Type: jpg dist_b.jpg (57.7 KB, 47 views)
File Type: jpg v.jpg (51.4 KB, 43 views)
File Type: jpg vel_mag.jpg (68.4 KB, 43 views)
Martin Hegedus is offline   Reply With Quote

Old   April 29, 2011, 13:37
Default
  #36
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 467
Rep Power: 9
Martin Hegedus is on a distinguished road
There seems to be a limit of 5 attachments, so here is the last image.
Attached Images
File Type: jpg vel_04_iso.jpg (54.6 KB, 34 views)
Martin Hegedus is offline   Reply With Quote

Old   July 30, 2011, 13:28
Default
  #37
New Member
 
Rambod Mojgani
Join Date: Jun 2010
Posts: 9
Rep Power: 7
rmojgani is on a distinguished road
I lost track of the answers; and I don't know if the debate is yet continued. (constant density may be applied for material)
Pressure far filed is used for compressible flows so its better to use pressure outlet for BC
from the velocity contour it seems that the velocity inlet condition has problems, are you sure you didn't set it normal to boundary by mistake ? i had once such an experience, and changing it to velocity components solved that.
it maybe be a good idea to check transition points you get from the model,
rmojgani is offline   Reply With Quote

Old   March 3, 2013, 20:09
Default can you me for create airfoil geometry
  #38
New Member
 
murali
Join Date: Feb 2013
Location: pondicherry
Posts: 10
Rep Power: 4
murali is on a distinguished road
hello didiean

i am new here to fluent, i am also create the airfoil geomentry as your geometry but i have some while creating the geometry,


rightside top and bottom of rectangular comes in straight line
Attached Images
File Type: jpg air.jpg (89.5 KB, 19 views)
murali is offline   Reply With Quote

Old   March 8, 2013, 22:04
Default
  #39
New Member
 
Wheeler
Join Date: Jan 2013
Posts: 24
Rep Power: 4
shlgzz is on a distinguished road
I'm facing the same problem with you.Could you tell me the values of turbulence viscosity and hydraulic diameter of inlet and outlet? and some information about the chord RE No. and material of fluid? Thank you in advance.
shlgzz is offline   Reply With Quote

Reply

Tags
airfoil, pressure-far-field, structured

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
Domain format problem on airfoil flow simulation andrenonaka CFX 6 December 4, 2014 04:57
Airfoil simulation using moving wall Alejandro NUMECA 9 November 4, 2008 03:00
NO STAGNATION POINT FOR AIRFOIL SIMULATION Rif Main CFD Forum 6 February 4, 2008 08:33
Simulation of transonic flow over NACA0012 airfoil MSc Student CD-adapco 2 August 9, 2006 13:49
Compressible transonic airfoil RAE2822 simulation Stefano CD-adapco 9 June 21, 2006 10:47


All times are GMT -4. The time now is 16:40.