# Trying to perform test validity of Fluent with simulation of 2D airfoil

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

 April 26, 2011, 20:54 #21 Senior Member   Martin Hegedus Join Date: Feb 2011 Posts: 476 Rep Power: 11 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.

April 26, 2011, 21:07
#22
Member

Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 7
Quote:
 Originally Posted by Martin Hegedus 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~~

 April 26, 2011, 21:13 #23 Senior Member   Martin Hegedus Join Date: Feb 2011 Posts: 476 Rep Power: 11 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.

April 27, 2011, 03:30
#24
Member

Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 7
Quote:
 Originally Posted by Martin Hegedus 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

 April 27, 2011, 06:51 #25 Senior Member   Raashid Baig Join Date: Mar 2010 Location: Bangalore, India Posts: 136 Rep Power: 8 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 ?

April 27, 2011, 08:36
#26
Member

Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 7
Quote:
 Originally Posted by cfd_newbie 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.

 April 27, 2011, 20:15 #27 New Member   Hamidreza Join Date: Apr 2011 Posts: 6 Rep Power: 7 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,

April 27, 2011, 20:44
#28
Member

Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 7
Quote:
 Originally Posted by compeng 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.

 April 27, 2011, 21:36 #29 New Member   Hamidreza Join Date: Apr 2011 Posts: 6 Rep Power: 7 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,

 April 27, 2011, 21:59 #30 Senior Member   Martin Hegedus Join Date: Feb 2011 Posts: 476 Rep Power: 11 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.

April 27, 2011, 23:02
#31
Member

Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 7
Quote:
 Originally Posted by Martin Hegedus 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.

April 28, 2011, 01:42
#32
Senior Member

Raashid Baig
Join Date: Mar 2010
Location: Bangalore, India
Posts: 136
Rep Power: 8
Quote:
 Originally Posted by Martin Hegedus 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.

April 28, 2011, 02:00
#33
Member

Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 7
Quote:
 Originally Posted by cfd_newbie 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.

April 28, 2011, 15:37
#34
Senior Member

Martin Hegedus
Join Date: Feb 2011
Posts: 476
Rep Power: 11
Quote:
 Originally Posted by cfd_newbie 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.

April 29, 2011, 13:36
#35
Senior Member

Martin Hegedus
Join Date: Feb 2011
Posts: 476
Rep Power: 11
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
 cl_vs_y.png (4.2 KB, 44 views) dist_a.jpg (98.1 KB, 55 views) dist_b.jpg (57.7 KB, 52 views) v.jpg (51.4 KB, 47 views) vel_mag.jpg (68.4 KB, 46 views)

April 29, 2011, 13:37
#36
Senior Member

Martin Hegedus
Join Date: Feb 2011
Posts: 476
Rep Power: 11
There seems to be a limit of 5 attachments, so here is the last image.
Attached Images
 vel_04_iso.jpg (54.6 KB, 39 views)

 July 30, 2011, 13:28 #37 New Member   Rambod Mojgani Join Date: Jun 2010 Posts: 9 Rep Power: 8 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,

March 3, 2013, 20:09
can you me for create airfoil geometry
#38
New Member

murali
Join Date: Feb 2013
Location: pondicherry
Posts: 10
Rep Power: 5
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
 air.jpg (89.5 KB, 21 views)

 March 8, 2013, 22:04 #39 New Member   Wheeler Join Date: Jan 2013 Posts: 24 Rep Power: 5 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.

 December 5, 2015, 14:31 #40 Member   mechiebud Join Date: Jan 2015 Posts: 47 Rep Power: 3 Hello everyone, I have generated hyperbolic grid around an airfoil by writing my own code. Can please someone guide me as to how can I check the quality of my grid?

 Tags airfoil, pressure-far-field, structured

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post shereez234 OpenFOAM Running, Solving & CFD 1 November 3, 2015 04:54 Cocorito90 OpenFOAM Running, Solving & CFD 11 October 27, 2015 16:04 robyTKD SU2 Shape Design 21 May 29, 2013 09:26 Maxime31850 FLUENT 2 May 1, 2013 11:15 RajeshAero Main CFD Forum 1 February 8, 2011 05:50

All times are GMT -4. The time now is 05:45.