What Mach number are you simulating? By any chance, is it the experimental case of McCroskey's results?

Dear Hanye Azimi

The flow is highly unsteady and requires adequate mesh refinement, time stepping and turbulence modelling.

Our recent publication might be of your interest:

Article Numerical Modelling of Stall and Post Stall Events of a Sing...

@ Tapan K. Sengupta

Mach number doesn't matter in this case, The flow is imcompressible.

I wish to validate with this paper :

"dynamic stall simulation of a pitching airfoil under unsteady free stream velocity" , 'Journal of fluids & structures , 2013

The reduced frequency equals to 0.1 so the flow is unsteady not a highly unsteady one.

So you think that it's related to the mesh,yeah?

Thanks for recommending ur paper. I'll read it.

Dear hanye

I highly recommend that check the wall y+. It should be less that 1 for upper and lower surfaces of the airfoil. In addition, upstream domain for the airfoil should be large enough to improve the accuracy of results. I suggest that choose 20 airfoil chord or higher for upstream domain.

Haney: The McCroskey's data is also for incompressible flow. However, our own compressible code clearly identifies a supersonic pocket. You may like to look at the following reference:

Investigation of compressibility effects on dynamic stall of pitching airfoil - Jyoti Sangwan, Tapan K. Sengupta and Prasoon Suchandra, Phys. of Fluids, vol. 29, pp 076104 (2017)

Hope this helps. The point is, FLUENT is simply not good enough!

@ Tapan K. Sengupta

All right. I'll look at ur job.

Thank you for ur reply

@ Hossein Fatahian

The domain is large enough but y+ is not as much good.

Thanks

@Hanye as pointed out by Professor Tapan, there is something important with these type of flow configurations. As we expect we have local acceleration which is expected in airfoils. Thus, if your Mach number is around 0.3 your solver might find issues with those compressible pockets. These problems are difficult to spot and they add spurious information into your computations.

Interesting question

@ Julio Mendez Thanks for ur information

My mach number is less than 0.3 ( M=0.005)

Was that such a great secret to not reveal it in the first place? Does that mean we should be getting very accurate results from FLUENT?

Dear madam

Can you please tell me which model you are using in fluent?

Also I like to know what is your Y+ value near the airfoil.

ok, then the other option left are: inconsistency in the boundary conditions or turbulence model is not appropriate

some information:

Re=1.35*10^5

k=0.1 chord length=1 so f=0.06 & omega=0.37

model: K-Omega SST (low Reynolds)

I tried many mesh

The mesh which has y+ = 9 has worse result than others that their y+ is more than 50

As this flow is highly unsteady, one requires a very high accuracy method that keeps the velocity field solenoidal, and there should not be numerical diffusion affecting physical diffusion. Also, one must minimize dispersion error (for a time-averaged field? isn't that self-contradictory? Please do not ask me!). Lastly, if one is still interested in time-averaged results (of dynamic stall!! - what is that???) then one must invest a lot of time tuning bells and whistles to develop a better turbulence models. The last activity is literally a curve fitting exercise with known results and can be very time consuming and back-breaking! It is also very unlikely that the same turbulence model will not work for another reduced frequency. At this point in time, we wish you the very best and hope you succeed.

Professor Sengupta ! Appreciate for ur ideas & for ur time.

Regarding UDF, some parameters have not been defined as real, e.g. f omega[ ], ... Some parameters are declared but haven't been used. I think you should read the values defined by UDF after compiling, hooking and simulating to ensure that UDF is working well.

Please check the reference parameters and also try to run unsteady simulation with converged steady-state results to initialising the flow.

Please also do check the effect of reduced frequencies and try to run other test case as well. I have also performed similar study and you can refer my paper.

Conference Paper CFD Simulation of Blade Flows With High Amplitude Pitching

Thanks Ramesh. I really should run other test case.

I have had converged steady results as initialized values.

Hi Hanye,

Are you trying to validate with the paper of Lee and Gerontakos (JFM 2004)? It's not a simple job because of the transition which might have a significant effect on the numerical simulation.

I noted that you are using DEFINE_GRID_MOTION macro. Why not to use CG_MOTION macro instead? The sole pitching is a solid-body rotation so it is much easier to simulate the flow using the latter macro. I hope you will find this comment useful.

Regards,

Ehsan

Thanks Ehsan Asgari for the comment. Certainly it's useful. You're right! transition region is complicated. Probably it's not proper for me at the moment. It's best to simulate an easier pitching motion. Have you got any suggestion?

I guess you should first see the numerical methods in recent papers for the same airfoil and pitching condition. For instance, the paper introduced by Kuldeep dagar could be a good guide for you. I think they have investigated different turbulence models in their paper. See how close you can get to the numerical results presented in the paper. If your results are close enough, then you should not be worried about the experimental data.

Second, if you cannot afford the computational cost of the more sophisticated turbulence models which take transition into account, you may switch to a higher Reynolds number at which transition would have a negligible effect. For that purpose please see our papers:

Article The Role of Frequency and Phase Difference Between the Flow ...

Article Active Flow Control of Dynamic Stall By Means of Continuous ...

Also, think about the required UDF Macro I suggested for the pitching motion.

Regards,

Ehsan

I tried to validate with this paper:

" Dynamic stall simulation of a pitching airfoil under unsteady free stream velocity" by Gharali & Johnson,2013

In this paper the method was new & a bit strange. The airfoil & the whole computational domain was oscillating together.As I mentioned in my question, I haven't succeed in this way so I returned to another method, known dynamic mesh! Layering & remeshing ! Now the lift Coefficient history is validated.

I'm grateful to everyone who helped me & answered to my question. I'm still look forward to any idea about that method (moving whole the domain)

Hanye Azimi

Take this file.

I used this file for validation by this paper.

You can improve mesh quality.

https://www.dropbox.com/s/31k9o06khu6m4rr/Files.rar?dl=0

Best regards

Thanks Alireza !

I took a look at ur file. It's dynamic mesh ,too. I thought that rotating whole the domain together means not using dynamic mesh method. I used UDF for fluid(only fluid ). Maybe you're right and gharavoli has used dynamic mesh for airfoil,inner domain,outer domain , ....

anyway I didn't achieved the expected result by oscillating whole the domain. See the auto save animation.

Hayne Azimi

It seems your whole C mesh grid is moving instead of your airfoil. I think this is not your desired results. Professor Amar Hameed is correct about the UDF dentition. For your convenience, I am attaching a sinusoidal motion of an airfoil with animation.

Regards,

Akib

Dear all,

I have the same case for run in Ansys Fluent 18.2. I can grab lift and drag coefficients in static form but in dynamic form (pitching airfoil) i do not know how to calculate lift and drag coefficients at different AoA.

I will be so grateful to any hints about this problem.

Kind Regards,

Milad

@ Milad Mousavi

You need to compile an User Defined Function to Fluent in order to simulate a pitching motion.

The lift Coeff is calculated the same as the static state. Fluent gives you the lift & drag Coeff per each time step. you could obtain angles per each time step by your own helping pitch equation. So you have lift & drag Coeff per each mean angle.

Good Luck

Hanye Azimi

Thank you so much for your answer.

But for my udf function i do not know whether to use macro DEFINE_ZONE_MOTION or CG_MOTION ?

Is there any changes in mesh interface ?

Then in dynamic mesh which one i must select between remeshing, layering and smoothing ?

Thank you in advance

Regards.

@Milad Mousavi

Your welcome!

If you wish to move only the airfoil, It's best to compile a DEFINE_CG_MOTION.

Smoothing and Remeshing would be proper, probably.

Hanye Azimi

Thank you for your answer.

for calculating Cl vs AoA, after grab Cl vs Time, we must use this function a(t)=A*sin (wt) or

a(t)=-A*w*cos (wt) ?

Why we use a(t)=-A*w*cos (wt) as function?

@ Milad Mousavi

a1(t) = Amplitude*sin(omega*time) (a1: motion function)

a2(t) = omeg*Amplitude*cos(omega*time) (a2: velocity :derivation of motion function)

You should write the derivation of the motion function in UDF. Your motion function may be sinusoidal or a cosine one.Up to your case.

Dear Hanye Azimi

I tried to validate airfoil with dynamic mesh but my lift coefficients did not match with experiment. After that i try to simulate without dynamic mesh and try to oscillate whole domain but i see the Cl vs Time is always on straight line on zero. I use dynamic mesh and my udf is same as you. My turbulence model is k-w sst and my reynolds number is 135000. I use piso solver.

I will be so grateful if you could advise me on this error.

Thank you in advance.

@ Milad Mousavi

Are you trying to validate with the same paper? "dynamic stall simulation of a pitching airfoil...." by Gharali and Johnson?

1- Is your mesh OK?

2- Have you notice to boundary conditions?(right boundary Pressure outlet and others velocity inlet)

3- About moving whole the domain method, you should define motion in "cell zone" . You applied UDF for what part of your mesh?

I need more details to find out the mistake.

Sure!

Hanye Azimi

My validation case is Tim lee 2004 but for verification i use gharali and johnson 2013.

my mesh is ok. skewness is good and i had 120 k cells around airfoil with boundary layer (y+

@ Milad Mousavi

Try both!

1- Apply UDF to the airfoil and use dynamic mesh method ( Remeshing and Smoothing)

2- Apply UDF to the fluid (without any smoothing,remeshing ....)

It works!

while using dynamic mesh method, in dynamic mesh zones which category should i assign to airfoil? rigid body or user define?

also if rigid body, then what should be my center of gravity? should i leave it as (0,0)? (as i am oscillating airfoil about quarter of chord).

@ Tariq Khan

Rigid body

centre of gravity depends on your project. Mine was 0.25*Chord the same as the reference papper

Hanye Azimi ,

Hello. My student is try to validate oscillating airfoil motion dynamic stall simulation of a pitching airfoil...." by Gharali and Johnson . Do you have a user defined file that can work for that? We have a CG_Motion UDF but it changes the angular velocity and we don't know how to translate that to angle of attack changes. Thank you for your help.

Kamran Fouladi

Kamran Fouladi

Hi

I used this:

* define motion variables */ a = 15*(pi/180); /* Amplitude */ f=0.06; /* frequency */ w = 2 * pi *f; /* Angular Frequency */

/* define airfoil motion */ omega[2] = -a*w*cos(w*time); /* z-component of angular velocity */

What's wrong with angular velocity?

It's been defined the angular velocity and pitch amplitude,both in the above Udf. So, the angle of attach is defined either.

Don't hesitate to ask more. I hope I could help.

Best

Hi,

Thank you. This helps. A couple of questions:

(1) Is f (frequency) in Hz?

(2) How do you calculate angle of attack from angular velocity. I am thinking

delta AOA=angular velocity*delta time

I am not sure if that works in Fluent.

Also, I would appreciate if you can share your validation paper.

Thank you so much.

Kamran Fouladi

Hello Dr. Fouladi

I have shared my validation. It's available in projects parts. Also you could read my conference paper, it's in Persian.

1-frequency is in 1/s here.

2- Pitching motion is defined as

Alfa(t)= Amp0+ Amplitude*omega*function of motion

function is sinusoidal or cosine here.

So Alpha(t)=Amp0+ Amplitude*omega*sin(omega*time)

omega is angular velocity

As you see angle of attack is calculated by angular velocity.

Anytime!

Hello Hanye,

This is certainly very helpful. I think I got ours to work. Thanks for your help.

Also, I could not find your conference paper. I was just curious of your results.

By the way, this is the UDF I got from ANSYS for oscillating airfoil. As you can see they used f in Hz.

/**********************************************/

/* flapMDM.c */

/* UDF for specifying a time-varying omega */

/* */

/* Simulates +/- angFlip deg flapping with a */

/* cycle of FN Hz. */

/* */

/**********************************************/

#include "udf.h"

#define FN 34.4

#define angFlip 1.01

#define omegpi 2.0*M_PI*FN

#define omegMx angFlip*M_PI*omegpi/180.0

DEFINE_CG_MOTION(dm, dt, cg_vel, cg_omega, time, dtime)

{

real omega, tm;

tm = time - 0.5*dtime;

omega = omegMx*cos(omegpi*tm); /* rotational speed about axis*/

cg_vel[0] = 0.0;

cg_vel[1] = 0.0;

cg_vel[2] = 0.0;

cg_omega[0] = 0.0;

cg_omega[1] = 0.0;

cg_omega[2] = omega;

}

Khaili Mamnoon.