[tw463]

Hello,
I am new to this forum, and this is my first post. Please do point out if I am doing anything inappropriate. Thanks.

I am using ANSYS Fluent 18.2, but this problem I believe is not really specific to the software package. It should be more related to my method.

The problem I am having at the moment is the drag coefficient from CFD is not matching wind tunnel experiment data. CFD result is lower than experiment result.

I am trying to reproduce a wind tunnel experiment in CFD so as to better understand the flow field. The wind tunnel is 3D of course, but the setup is uniform in the Z direction so I think I can simplify this into a 2D problem.

The setup is a cylinder subject to free stream, with an airfoil section behind it, aligned with its center line. It is well known that vortex will shed off the trailing edge of a cylinder, thereby introducing drag. We think if obstruction is placed on the center line in an appropriate position downstream, it will impede the motion of the vortex crossing onto another side periodically so there would be less shedding, hence less drag.

The wind tunnel uses a scaled down model because the test section is small. The cylinder of interest is 200mm diameter, and in the experiment the model was 75mm diameter (the airfoil scaled down accordingly). In the CFD model I am using real size.

The wind tunnel runs at ReD=1.1e5, and I will match this in the CFD analysis (by decreasing flow speed). Working fluid is air with density 1.225 and viscosity 1.7885e-5, same for tunnel and CFD.

The wind tunnel data, after correcting for the carriage drag and tunnel blockage, is:

• bare cylinder in free stream, Cd=1.21
• cylinder with airfoil, cylinder Cd=0.91, airfoil Cd=0.02

Please note that the reference area for drag coefficient is frontal area of the cylinder, ie diameter * depth

My computational domain is rectangular, with the following dimensions (from center of cylinder):

• 2.5m upwind (12.5D)
• 5m downwind (25D)
• 2.5m to each side (12.5D)

Cell count is approximately 500k. The cylinder and airfoil surface have surface sizing and inflation of 25 layers. The mesh is fine around the cylinder and airfoil, and getting coarse far away. The most coarse mesh measures 0.02m. Meshing method is all triangle, except in the inflation layer, where the mesh is like rectangular (with curvature). I have attached some screenshots of the mesh. I think my inflation is adequate to resolve for the boundary layer.

Physics setup is as follows:

• model depth is 1m so that reference area is 0.2m^2
• velocity inlet at 8.028m/s (so that ReD=1.1e5)
• pressure outlet at 1 atm ie 0 gauge pressure, because the tunnel is open loop ie discharge into the room
• cylinder and airfoil are walls with no slip BC, roughness is 3e-6m ie 3um (this is estimated from machining quality, and scaling up from 75mm to 200mm so that relative roughness is kept constant)
• the domain boundary is wall with specified shear 0 pascal, because the wind tunnel blockage effects have been corrected for, so I do not need to simulate those walls

Solver setup is as follows: (I believe it should be some of these that is not quite right)

• transient simulation with time step 0.001s (I tried several times and with this time step it converges in like 25 iterations)
• viscous model is transient SST (4 equations)
• Coupled scheme
• Green Gauss Node Based
• Pressure 2nd order
• 2nd order upwind for residuals
• 2nd order implicit for transient
• double precision
• Courant Number = 200 as default
• max 50 iterations per time step

And I go ahead and solve for it. The Cd from CFD is like 0.75 while the wind tunnel result is 0.91 so the match is poor.

Besides my results is oscillatory in the time domain, plot attached.

The wind tunnel cylinder is tapped, and I know the boundary layer separation happens at about 80deg and 280deg (clockwise positive from upstream stagnation point). I have attached a screenshot of my streamlines, and I think the separation behavior is about right. Therefore, I cannot explain why the drag coefficient is so different given that for this bluff body certainly the form drag dominates?

By the way I have tried other viscous models such as the k epsilon model. Problems with these is that the separation point is at 100deg and 260deg, and the Cd is less than 0.55, which is very incorrect. So I need a model that can handle laminar turbulent transition, because I think as soon as the laminar boundary layer detach from the cylinder it will immediately become turbulent given the Reynolds number, and the downstream airfoil will be subject to fully turbulent flow. I have also tried laminar model, and the flow does not make any sense at all, with drag coefficient varying in the time domain from 0.2 to 2 very violently.

If you have any suggestions why my result would be incorrect, I would very much appreciate any help! If you need any further information please reply and I would be happy to supply them.

Thanks

Update 1: By running the model for much longer (for 2 travels), it is observed that the Cd value slowly but steadily rises to a better value of around 0.85 but still not precise enough for my purpose. Besides the airfoil is constantly reporting negative drag. I certainly need to refine the mesh around that region.


Update 2: the results are now running into further problems of mesh dependence after I have did the mesh around the trailing edge of the airfoil better. p.s. the airfoil is supposed to have its trailing edge trimmed off.

[beer]

Your setup seems mostly fine.
However, judging from the fourth picture you resolve each vortex with only 4 time steps, which is probably not enough. The time step should be reduced.

[FMDenaro]

Cell count is approximately 500k. The cylinder and airfoil surface have surface sizing and inflation of 25 layers. The mesh is fine around the cylinder and airfoil, and getting coarse far away. The most coarse mesh measures 0.02m. Meshing method is all triangle, except in the inflation layer, where the mesh is like rectangular (with curvature). I have attached some screenshots of the mesh. I think my inflation is adequate to resolve for the boundary layer.


We could discuss a lot about the validity assumption of your 2D URANS setup and the fact that such formulations is physically debatable.
However, let me first observe that the first thing is to compute the y+ of the firtst cell close to the wall to assess if you are resolving or not the BL. Then, a correct refined mesh should also involve the vortex shedding zone.
I suggest to chech such issues and then try to resolve the 3D case.

[flotus1]

Totally agree. And the mesh near the trailing edge of the airfoil definitely needs some more attention.
Edit: but don't be mistaken: this setup is very challenging if you want simulation results that quantitatively match experimental values.

[tw463]

Originally Posted by beer

Your setup seems mostly fine.
However, judging from the fourth picture you resolve each vortex with only 4 time steps, which is probably not enough. The time step should be reduced.

Hi,
I have just found that this pattern is a result of extrapolating variables. The macroscopic fluctuation is much better resolved.
Thanks for you help.

[-DodgerIsBlack-]

If your wind tunnel is "small" as you mentioned you cannot use the data directly. It is essential to correct your experimental data to account for wake blockage, streamline curvature, and pressure blockage. You can use Pope's old book for reference, or you might want to review this NASA publication:

http://www.dtic.mil/dtic/tr/fulltext/u2/657092.pdf

These corrections change for different objects, such as for buildings or wind turbines.

[tw463]

Originally Posted by -DodgerIsBlack-

If your wind tunnel is "small" as you mentioned you cannot use the data directly. It is essential to correct your experimental data to account for wake blockage, streamline curvature, and pressure blockage. You can use Pope's old book for reference, or you might want to review this NASA publication:

http://www.dtic.mil/dtic/tr/fulltext/u2/657092.pdf

These corrections change for different objects, such as for buildings or wind turbines.

Hi,
thanks for this good read about wind tunnel blockage. I did not do the experiment myself. Those who did it reported a tunnel blockage ratio of 0.11, and data has been processed by the Allen & Vincenti semi empirical correction formula (which seems to me to be specifically designed to assess the flow over cylinders):
Cd=Cd0(1-0.5Cd0*beta-2.5beta^2)
However, I must admit that I am unsure at the moment what correction would be needed for the airfoil on top of that. The block ratio did not take the airfoil into account given that it is completely shielded behind the cylinder.

[LuckyTran]

Originally Posted by tw463

The wind tunnel runs at ReD=1.1e5, and I will match this in the CFD analysis (by decreasing flow speed). Working fluid is air with density 1.225 and viscosity 1.7885e-5, same for tunnel and CFD.

I am curious where is this wind tunnel that has air with these properties? These are air properties at STP. Is your wind tunnel in Antartica?

[tw463]

Originally Posted by LuckyTran

I am curious where is this wind tunnel that has air with these properties? These are air properties at STP. Is your wind tunnel in Antartica?

I believe these are properties of air at psl=1.01325bar and tsl=15degC, according to "thermofluids databook" of Cambridge university engineering department, which I believe the experimenter has referred to.

[mCiFlDk]

Originally Posted by FMDenaro

However, let me first observe that the first thing is to compute the y+ of the firtst cell close to the wall to assess if you are resolving or not the BL. Then, a correct refined mesh should also involve the vortex shedding zone.

Hi FMDenaro,

I was looking for another issue but I couldn't avoid while reading your post to remember a question I had for some time.

If the first layer height is much bigger than y+, does it mean that the BL won't be solved and a wall function will "do the work"? Or the first layer height should be always similar to y+ despite solving it or not?

Thanks a lot

[FMDenaro]

Originally Posted by mCiFlDk

Hi FMDenaro,

I was looking for another issue but I couldn't avoid while reading your post to remember a question I had for some time.

If the first layer height is much bigger than y+, does it mean that the BL won't be solved and a wall function will "do the work"? Or the first layer height should be always similar to y+ despite solving it or not?

Thanks a lot

Be careful, the first layer height produces some y+ numerical value. You should check if this value is enough small to solve the BL or is high and you need to use a wall model. But using a wall model is not panacea! The assumption of a wall model is based on a specific type of turbulent BL over a wall and is not general for all cases.

[mCiFlDk]

Originally Posted by FMDenaro

Be careful, the first layer height produces some y+ numerical value. You should check if this value is enough small to solve the BL or is high and you need to use a wall model. But using a wall model is not panacea! The assumption of a wall model is based on a specific type of turbulent BL over a wall and is not general for all cases.

Thanks for the quick response! I'm aware that the wall functions must be studied and previously adapted, but the thing was that I've never needed to perform an analysis where the wall is resolved. But I got your point and I'll read quite a lot of literature before trying anything.

Only one more issue regarding this topic. Is there any generalization for using or not wall functions? For example, when using air or another fluid, with a certain type of mesh element, with higher or lower pressure gradients... Because I've only found info about models where wall functions can be omitted (i.e. k-omega SST, Spalart Allmaraz)

Thanks a lot

[FMDenaro]

Originally Posted by mCiFlDk

Thanks for the quick response! I'm aware that the wall functions must be studied and previously adapted, but the thing was that I've never needed to perform an analysis where the wall is resolved. But I got your point and I'll read quite a lot of literature before trying anything.

Only one more issue regarding this topic. Is there any generalization for using or not wall functions? For example, when using air or another fluid, with a certain type of mesh element, with higher or lower pressure gradients... Because I've only found info about models where wall functions can be omitted (i.e. k-omega SST, Spalart Allmaraz)

Thanks a lot

In my opinion, a strong theoretical assumption would be only the grid enough refined to resolve the BL (at least 3-4 nodes before y+=1)

[mCiFlDk]

Originally Posted by FMDenaro

In my opinion, a strong theoretical assumption would be only the grid enough refined to resolve the BL (at least 3-4 nodes before y+=1)

Thank you!!