What are the points in simulating 2D airfoil??
 

Hi, guys,

I would like to calculate the aerodynamic dimensionless factors, Cl, Cd, Cm of the airfoils under any situation since I have to develop an unmanned helicopter.

So, for the first step, I have been trying to simulate the 2D airfoil of NACA 0012 with Fluent so far.

But, unfortunately I couldn't derive the reasonable values of the factors, yet. I compared them with the chart of NACA0012 characteristics on 'Helicopter Performance, Stability and Control by Raymond W. Prouty' which I attached here.

The conditions of the first case was 4 degree of the angle of attack with Mach 0.8 using the solvers, SA, RSM and k and epsilon.
But, all of them were failed.
(I could not upload the the case & data file I tried due to the file size.)

Could you give me some advises what's the point to set up the boundary conditions and/or the modeling for simulating 2D airfoil?

Especially, I'm confused with the relation of the near-wall function with the mesh near the airfoil surface.
According to ANSYS help, the mesh should be fine without the wall functions, while it may be coarse if I choose one of the wall functions.
So, do I have to make the mesh coarse if I use RSM or k and epsilon model? Also what is the suitable functions for this case among the wall functions?

Thanks,
Have a good day!

ps) If you have additional tips for the rotor blade which is generally considered its own rotation, could you please let me know them?

Hi, please post a picture of your mesh and the value of Y+ that you get. For a RANS simulation please remember that y+ shall not exceed 300. If you are willing to get precise numerical results I recommande a y+ around 10.

Generally you have to get closer results for 2d airfoil cases... can you check which boundaries you are using to integrate pressure/skin friction to get total cl, cd, cm...you have to use only airfoil boundary for intgration, not the farfield boundary... are you doing proper axes transformations when converting from cx, cy, cmy to cl, cd, cm

Hi, Santos

Thanks for your reply,
The following list is the files I enclosed here.

1. Mesh-wide view
2. Mesh-close view
3. General Check Domain: Check and Report Quality message for the mesh in General.
4. Yplus-SST-4D AoA-Ma08-PFF: Yplus graph, Transition SST solver, Angle of Attack 4 Degree, Mach number 0.8, Boundary Condition-Pressure Far Field
5. Yplus-SST-4D AoA-Ma08-Vel Inlet-Pressure Outlet: Same as the above except the Boundary Condition-Velocity Inlet and Pressure Outlet

Pressure Far Field (PFF) model sets the edge of the domain as the PFF, and Velocity Inlet and Pressure Outlet one sets the front edge of the domain as Velocity Inlet and the rear one as Pressure Outlet.
And I tried several solvers (SA, k-epsilon, k-omega, SST, RSM), but the trend of their result showed similar.

Could you please check if the mesh consition is OK or not?
According to the ANSYS help, y+ should be about 1 or greater than 30. As you can see, both of the Yplus graphs exceed 30 and below 300 that you mentioned. But, there is an obvious difference between the two graphs. The pressure far field model seems to show something like shock or separation after 0.4m on position axis while the vel. inlet model has clear line.
Do you know what makes this difference?

In addition, please let me know how to adjust the Yplus to near 10. As you can see, the value has the order of 2. Do I have to make the mesh more fine or coarse?

Thank you,
For more information, I will attach more images on the next message.

Have a good day,

I attached the below list additionally.

1. Ystar-SST-4D AoA-Ma08-PFF (pressure far field)
2. Ystar-SST-4D AoA-Ma08-Vel Inlet-Pressure Outlet
3. Result-Cd-SST-4D AoA-Ma08-PFF: Drag coefficient for PFF model.
4. Result-Cd-SST-4D AoA-Ma08-Vel Inlet-Pressure Outlet: Drag coefficient for Vel Inlet and Pressure Outlet.
5. Mesh nose and tail.

Could you let me know what the difference is between the Yplus and Ystar?

With respect to the Drag coefficients, the result of Pressure Far Field model shows a periodic trend, while the other one shows the converged value(around 0.008) but it is away from the experimental result (0.05).
Like Yplus, the two models have completely different result, even though only different thing is the setting of the edge line of the domain each other.
Could you explain why?

Thank you.

Hi, cfdraj

Thank you for your reply.

I tried two different cases in terms of the boundary condition setting.

Case 1: Pressure Far Field set up. In the picture of the Boundary Condition attached, Edge A and B are set as Pressure Far Field and the airfoil surface as wall.

Case 2: Velocity inlet and Pressure Outlet set up. In the picture, Edge A is established as Velocity Inlet and Edge B as Pressure Outlet. The airfoil surface is same as Case 1.

But, the results of them are clearly different as I explained to Santos above.

Also, I enclosed the BC set up dialog windows and monitor set up window of Drag, Lift, Moment.

Please check and share your knowledge.

Thanks,
Have a good day.

Hi cocobi, now I see your problem. The thing is you seem to be unfamiliar with the problematics of compressible or transsonic flow.

About the mesh : Your values of Y+ are good but they are not regular enough. The mesh is very fine on the leading edge and gets coarser along the chord. I thing that it should be better (especially to get values of Cd and Cl) to have a mean and more constant value of y+ on your airfoil. But remeshing can be long and I don't know if you are willing to do that.

The core of the problem is the lack of expectation. When launching a calculation, you shall expect a result. In this case, you are at M0.8, so the air on the upper surface (and sometimes also on the lower surface) will accelerate up to Mach 1, giving you a shock.
Look at these nice wind tunnel pictures, that will help you understand the physics of the transsonic flow : http://www.supercoolprops.com/articl...irfoils_p2.php

So the result you get with the Pressure FF seems correct.
Remember, if you set up a case with non compressible air and velocity-inlet fluent will not know the speed of sound and therefore the shock will not appear and the results will be physically very wrong.

But also remember that the set up for boundary conditions is not a physical stuff, it is a consequence of your reflexion.
I'll give you the following tip to help you choose:

1. Know whether or not the air will be compressible. The air is indeed always compressible but we neglect the compressibility under M0.3. So:

If incompressible:
Set Fluent to Pressure Based
Set the boundary conditions to Velocity Inlet / Pressure Outlet

and you are good to go.


If compressible (Every steps are crucial !):
Set Fluent to Density Based
Go to Material - Air and set the density to Ideal Gas and Viscosity to Sutherland (that will activate the energy equation)
Set the boundary to Pressure FF

and you are good to go



Also, you put a screenshot of your Cd evolution over time. The convergence is fast in incompressible but longer in compressible. Clearly your compressible case is not converged, be patient and these waves will surely be flattened over time and you'll get your convergence.
Remember that when you are compressible you have multiple physical effects (temperature, density, mach, speed of sound, viscosity) and the equilibrium is indeed longer for Fluent to get.

And if anything I said is unclear to you, you shall go and spend time reading and understand the comprehensive explanations you'll get in Fluent Theory and User's Guide
https://www.sharcnet.ca/Software/Flu...l/ug/node3.htm
https://www.sharcnet.ca/Software/Flu...l/th/node3.htm


Hope that helps, retry with proper set up and we'll see :)

Why would you do that? As I understand it, y+=10 is one of the worst choices at all, since it is much too high to resolve the viscous layer but also too low to use a wall function. It is right there, where you don't want to have your first grid point.

Yes my mistake I agree with you. That is comprehensivly explained in Fluent help, although I never quite like the fact of voluntarely degrading the boundary layer density from 10 to 30 for example. But it seems that it might increase the results accuracy so...

With a regular computer it's hard to reach y+ around 1 so 30 is probably the best choice.

The turbulence (wall) model has two choices:
a) calculate the near wall behavior itself, which needs an y+ of about 1
b) use the log-law function, which is valid for y+ > 30
Both are violated for y+=10, so the accuracy generally gets better when you increase (or decrease) a y+ of 10.

Hi, Santos,

I am really appreciating for your help.
I am changing the mesh right now, and be careful to set the boundary conditions following your explanation.

I am really clear thanks to your kind explanation.

Just one more question of the sonic speed.
You explained the speed under Mach 0.3 can neglect its compressiblity.
Does that mean I have to consider compressible flow for over Mach 0.3, unconditionally, or because the flow can reach to mach 0.7 which is transonic during travelling the airfoil surface?

Generally speaking, the mach of transonic speed ranges from 0.7 to 1.2 as far as I know, so I thought the flow under 0.7 could neglect its compressibilty.

Of course, for the previous case, it is completely the lack of my knowledge.. ^^;;

Regarding the website, both explorer and chrome cannot connect to 'supercoolprops.com' website. I hope it would be just a IP traffic problem at this moment and then be fine later.

Thank you again.
Have a nice day!

Hi, RodriguezFatz,

Thank you for your explanation.
It is very helpful for me as well as Santos' one.

Just one question I have here.
Do you mean the log-law function stands for a wall function?
If yes, I will be completely clear, but if not.... I would be afraid to be confused..

In any case, you showed me a clear standard when I choose turbulence model. Thank you for that.

Have a good day!

Yes. Maybe there are other wall functions... but log-law is definitly the "default".

About the picture I send, you can look here
https://www.google.fr/search?q=trans...A8qi0QXkjYCgDA

Page 5 and 6 you have nice wind tunnel pictures showing you the phenomenom.


About your theorical question. Yes generally speaking a flow is transsonic between 0.7 and 1.2. In fact the definition of a transsonic flow is a flow where you have a clear supersonic and subsonic zone. So it indeed depends on the geometry. For example modern aircrafts have a very high transsonic limit (the goal is indeed to reduce the supersonic points to save drag and fuel). The basis of that is the area rule for the fuselage, discovered by the German manufacturer Junkers during the WWII. Using low thickness airfoil also helps because it reduces the speed increase on the upper surface ofthe airfoil.

Anyway, compressibility and transsonic flow are different. The air is always compressible (otherwise aircrafts wouldn't have speed indication under M0.3 and I would be in trouble with my ultralight !) and you get dynamic pressure even at a very low speed.
But in general the physics is simplified under M0.3 and the air is supposed as incompressible (Bernouilli law).

You can use a incompressible setup to slightly higher speed if you want, but if you get close to transsonic you must choose compressible (St-Venant law) otherwise you'll miss the important shock phenomenom.

About the turbulence model, my teachers gave me a simple answer : k-Epsilon for internal flow (turbine, tubes etc...) and Spalart-Allmaras for external flow (aircraft, airfoils...). I like when it's simple !!

Thank you, RodriquezFatz

Have a good day!

Thank you, Santos.
Your explanation was absolutely helpful.

Have a good day!

Guys, which reference values for area, lenght and depth do you use in the 2D airfoil analysis ?

hi, guys
I know it's been a long time since last post in this thread but i hope you would see it & could help me.
I am working on simulation of a rotor blade, as i know i should use pressure far field boundary since the blade tip Mach number in my case is around 0.8. now my questions are:

1- in the pressure far field boundary condition you should enter Mach number, is this related to blade tip Mach number and i should enter M=0.8 or this is far field Mach number and i should enter M=0 (since my case is in hover)?

2- I don't need flow field far from the blade so i just want to model near blade region but as it's said in fluent user guide when you use pressure far field BC your region radius must be 20 cord length! what can i do about this? if i want to reduce my solution domain(to save computation time) is there any other BC i can use instead of Pressure far field ?(note that flow is compressible in my case)

any help would be greatly appreciated

M= 0.8 for the FarField condition, of course


There is a reason for the Fluent guide to propose the 20 chords empiric rule. The foil will create a pressure variation that will spread several chords away from your airfoil so for your boundary condition you must have the infinite flow without any perturbation caused by the airfoil. You can simulate in a domain that is too small but this will create either divergence or possible false results.
To save computational time, you may use a coarse mesh close from the boundary and a refined mesh near your foil. If you separate and count you'll see that the number of nodes that you need to reach the 20 chord distance between the airfoil and the BC is nothing in comparison with the number of nodes that is needed to simulate only the first millimeter of the boundary layer...

Charles

Hi, Santos
Thanks for your reply,

i just don't understand why we should use M=0.8 for far field Mach number. far from the rotor, air is in stagnation so it's velocity and Mach number is zero. where is my mistake?

Your mistake is a confusion between real life and simulation. In real life the air is considered stagnant and the rotor moves through it. In simulation or in a wind tunnel the simulated object is fixed in space and the air moves around it. This changes nothing for the result and it makes everything much simpler !
It's all about referential.

Think of it this way, if you put a GoPro on an aircraft wing. From your point of view the wing will not move while the air will be flowing towards the wing. That is the case you want to simulate with CFD. (like this : http://youtu.be/0TNV2xRiTK4)

Simulating real life case is possible if you use a boundary condition with zero velocity and make your object move in the domain with variable mesh. This have zero interest obviously.