[dmadhyastha]

Greetings Forum Members,

I am currently working on validation of CFD analysis of NASA SC(2)-0714 Supercritical Aerofoil with experimental results available from NASA reports. I found the agreement in lift coefficient is excellent but for drag and moment coefficient is poor at higher angles of attack. I have selected grid based on grid independence study. Even while doing grid independence the drag values were off by 25%.
The experimental data was available for Mach number = 0.75, Reynolds Number = 10 million, AOA range -2° to +1.5°.
Following are the solver settings I have used in FLUENT:

• Pressure based Navier Stokes Solver with double precision
• Density : Ideal Gas
• Viscosity : Sutherland Law with mu = 3.125 e-5 and T = 288.15K
• Turbulence Models used: SA, k-w SST, k-w SST with intermittency transition
• Boundary Conditions:
• Domain: Pressure Farfield
• Pressure = 101325 Pa
• Mach number = 0.75
• x-component: 1 (AOA = 0°)
• y-component: 0
• Temperature: 288.15 K
• Turbulent Viscosity Ratio: Left unaltered as 10, also tried 1; Intensity varied from 1 to 20%
• Discretisation: Second order for all equations, tried first order of turbulence equations
• Initialisation: FMG Initialization.
• Grid Quality:
• Overall Quality: above 0.9
• Min Ortho Quality: above 0.84
• Max Ortho Skew: below 0.16
• Mesh type: Structured
• Mesh Size: 168,000 quads
• Max Aspect Ratio: more than 10e4, Near the Aerofoil not exceeding 1000 (requirement for double precision solver)
• Wall y+: < 1, ~0.3-0.4

The drag coefficients for AOA = -2° to -0.5° are off by 0.03. For AOA = 0° to 1.5° The drag coefficients obtained are double fold the experimental value i.e. Cd from experiments = 0.018 (AOA = 1.5°) but from CFD Cd = 0.035.

I have tried density based solver with SA and k-w SST turbulence model, but I got similar results. I'm confident about the grid regarding the quality. Can somebody kindly advice me on how to obtain the drag coefficient which is near to experimental value?

P.S. I have closed the trailing edge as sharp trailing edge to satisfy Kutta condition. The trailing edge is not a vertical line but a point at centre of last y-coordinates.

[oozcan]

maybe this one is helpful for your problem : http://imechanica.org/files/fluent_1...02-airfoil.pdf

[dmadhyastha]

I have tried the method suggested in the workshop pdf, but that too does not work.

[Kushal Puri]

Originally Posted by dmadhyastha

Greetings Forum Members,

I am currently working on validation of CFD analysis of NASA SC(2)-0714 Supercritical Aerofoil with experimental results available from NASA reports. I found the agreement in lift coefficient is excellent but for drag and moment coefficient is poor at higher angles of attack. I have selected grid based on grid independence study. Even while doing grid independence the drag values were off by 25%.
The experimental data was available for Mach number = 0.75, Reynolds Number = 10 million, AOA range -2° to +1.5°.
Following are the solver settings I have used in FLUENT:

• Pressure based Navier Stokes Solver with double precision
• Density : Ideal Gas
• Viscosity : Sutherland Law with mu = 3.125 e-5 and T = 288.15K
• Turbulence Models used: SA, k-w SST, k-w SST with intermittency transition
• Boundary Conditions:
• Domain: Pressure Farfield
• Pressure = 101325 Pa
• Mach number = 0.75
• x-component: 1 (AOA = 0°)
• y-component: 0
• Temperature: 288.15 K
• Turbulent Viscosity Ratio: Left unaltered as 10, also tried 1; Intensity varied from 1 to 20%
• Discretisation: Second order for all equations, tried first order of turbulence equations
• Initialisation: FMG Initialization.
• Grid Quality:
• Overall Quality: above 0.9
• Min Ortho Quality: above 0.84
• Max Ortho Skew: below 0.16
• Mesh type: Structured
• Mesh Size: 168,000 quads
• Max Aspect Ratio: more than 10e4, Near the Aerofoil not exceeding 1000 (requirement for double precision solver)
• Wall y+: < 1, ~0.3-0.4

The drag coefficients for AOA = -2° to -0.5° are off by 0.03. For AOA = 0° to 1.5° The drag coefficients obtained are double fold the experimental value i.e. Cd from experiments = 0.018 (AOA = 1.5°) but from CFD Cd = 0.035.

I have tried density based solver with SA and k-w SST turbulence model, but I got similar results. I'm confident about the grid regarding the quality. Can somebody kindly advice me on how to obtain the drag coefficient which is near to experimental value?

P.S. I have closed the trailing edge as sharp trailing edge to satisfy Kutta condition. The trailing edge is not a vertical line but a point at centre of last y-coordinates.

Are you putting correct reference values, such as area temperature. Because that is important, cl and cd use that reference area to calculate the values

[dmadhyastha]

Originally Posted by Kushal Puri

Are you putting correct reference values, such as area temperature. Because that is important, cl and cd use that reference area to calculate the values

Yes. I have made sure the reference values are right. I have got lift coefficient matching with the experimental values. Only the drag and moment coefficients have disagreements at higher angles of attack.

[Kushal Puri]

Originally Posted by dmadhyastha

Yes. I have made sure the reference values are right. I have got lift coefficient matching with the experimental values. Only the drag and moment coefficients have disagreements at higher angles of attack.

if possible just send your case file and drag experimental value.

[dmadhyastha]

Originally Posted by Kushal Puri

if possible just send your case file and drag experimental value.

I'm afraid that's not possible as the case and data belongs to my employer.

[Kushal Puri]

Originally Posted by dmadhyastha

I'm afraid that's not possible as the case and data belongs to my employer.

I have some questions why you are not using density based solver as your mach number is 0.75 and flow is compressible.

Pressure atmospheric which you are defining, you calculated this pressure using mach number. I am correct ??

That pressure has to be total pressure and has to be calculated using compressible flow relation.

Clear these doubts so that we have some good discussion on why result is not matching

[dmadhyastha]

Originally Posted by Kushal Puri

I have some questions why you are not using density based solver as your mach number is 0.75 and flow is compressible.

Pressure atmospheric which you are defining, you calculated this pressure using mach number. I am correct ??

That pressure has to be total pressure and has to be calculated using compressible flow relation.

Clear these doubts so that we have some good discussion on why result is not matching

I have used both density based solver and pressure based coupled solver, both gave similar results.

Regarding pressure, I've obtained the pressure, temperature, Reynolds number and Mach number from the experiments. The experiments are done in cryogenic tunnel as the both Reynold number and Mach number are high.

If I match Reynolds number and Mach number for analysis and experiments, shouldn't the results be same?

[Kushal Puri]

Originally Posted by dmadhyastha

I have used both density based solver and pressure based coupled solver, both gave similar results.

Regarding pressure, I've obtained the pressure, temperature, Reynolds number and Mach number from the experiments. The experiments are done in cryogenic tunnel as the both Reynold number and Mach number are high.

If I match Reynolds number and Mach number for analysis and experiments, shouldn't the results be same?

My only concern is static pressure you are defining, you are defining as a atmospheric value, but it has to be less.

[dmadhyastha]

Originally Posted by Kushal Puri

My only concern is static pressure you are defining, you are defining as a atmospheric value, but it has to be less.

I found the boundary conditions for transonic tunnel analysis of the aerofoil and used the same for analysis.
The results are the same. There is no change.

I have matched Mach number and Reynolds number which I believe should work. The lift coefficient agrees well with the experiment, but the moment and drag coefficient does not agree at higher angles of attack.
I have given the right values in reference values too.

I don't understand where I am going wrong.

Sorry for replying late.

[dmadhyastha]

Greetings members!

I am replying after a long time. Since then my knowledge in the field of transonic aerodynamics, ICEM CFD and Fluent have improved drastically!

I was able to solve the issue following these procedures:

1. The closure of the aerofoil trailing edge to satisfy Kutta condition should not be done. In doing so, the geometry will not be represented correctly. So I created another grid with the blunt trailing edge.

2. The Mach number for which I was performing validation was the drag divergence Mach number of the aerofoil. Thus the flow around the aerofoil is going to approach transient conditions. It is not wise to simulate transient flow in steady state solver. Hence, the convergence-related issues. I chose experimental data for a lower Mach number to perform validation.

3. The wind tunnel data I had used were un-corrected data. I found correction factors and exact test section Mach numbers subsequently and corrected the data.

4. The boundary conditions as mentioned earlier by a forum member cannot be MSL conditions as it is a transonic tunnel. The boundary conditions were also changed to the values available in the reports.

5. It was observed that the domain size was small and was affecting the solution. The domain size was increased from10c to 50c to avoid this issue.

6. The grid was improved to capture the shock clearly (increased density near expected location of shock) while maintaining the quality and y+ values.

7. Density-based solver was used instead of Pressure based solver as the flow involves compressibility effects like shock.

8. I matched the lift coefficient values by varying the angles of attack. Once the lift coefficient matched, I compared the drag coefficient values.

By doing all the above-mentioned changes, I was able to get a very good agreement in drag coefficient value between experiments and CFD. I did take me some time to figure things out. Now that I have found how to go about the issues, I wanted to update and close the thread.

Thanks to all the forum members who have helped me solve the issue.