August 16, 2018 at 2:10 amHHK1992Subscriber
I am trying predict the cd, cl and cm of 2D airfoil (NACA0012) with sharp trailing edge and to compare with this technical report. While cl gives excellent agreement (less than 1%), cd and cm shows large deviation (my best was 25%). I am sharing a few snaps and set up info.
Set up info:
1. Structured meshing in ICEM CFD, y+ almost close to 1 with 200k~250k cells.
2. Steady, coupled solver, pseudo transient
3. SA or k-omega SST turbulence model
4. Air (Ideal gas, Sutherland's law of viscosity)
5. Static pressure is adjusted to meet Re = 5.97E6 and Ma = 0.15
6. Far field boundary at 100 times chord distance away.
7. Reference area = 1* chord
8. Components were resolved to set AoA and force report definitions
9. Tried FMG initialization
Kindly give me some suggestions.
August 16, 2018 at 6:26 amDrAmineAnsys Employee
Not only y+~1 is important but also the number of grid point sin the boundary layer (10-15). Because of AoA you need to adjust the force vectors for the evaluation of Cd, Cl and Cm. As you said lift is fine I think that you might made a mistake with the vectors. Check if you have set the reference values as coming from farfield boundary zone.
August 16, 2018 at 8:23 amHHK1992Subscriber
Thank you so much for replying.
1. I have kept more than 400 points on the airfoil surface but no luck!
2. The force vectors were resolved. If 'x' is the AoA, drag component is i*cos(x)+j*sin(x) and lift component is i*-sin(x)+j*cos(x). I kept the location of moment center (25% of airfoil chord) in moment report. Please correct if I am wrong.
3. The reference values were kept based on far-field boundary except reference area which was given as 1*chord. To be sure, I calculated the Re once more from reference values and was equal to the value desired (Re = 5.97E6).
Kindly walk me through this. I have been trying since 2 weeks.
August 16, 2018 at 11:46 amDrAmineAnsys Employee
How big is your AoA?
August 17, 2018 at 12:54 amHHK1992Subscriber
It is equal to 12.25 deg.
August 17, 2018 at 6:03 amDrAmineAnsys Employee
How did you calculate the farfield static pressure and static temperature? Can you please show the values?
August 17, 2018 at 6:48 amHHK1992Subscriber
I have fixed the static temperature at 310 K (based on this website) and calculated the static pressure such that Re = 5.97E6 and M = 0.15. I have used the following relations as attached in the image. On calculating I get static pressure as 25629.5 Pa.
I think since Re and M are maintained as same as that of experiment (in the technical report), cd, cl and cm should be same.
Thank you so much for your time.
August 17, 2018 at 7:47 amDrAmineAnsys Employee
I would calculate the static pressure and static temperature based on isentropic relationships to get static values from stagnation values. The reference temperature might be the stagnation one. P0 is the ambient total / stagnation pressure. The case is very sensitive to Boundary conditions.
We have done the NACA0012 for AoA of 1.55 ° and Ma=0.7 and the results were fine.
August 17, 2018 at 8:57 amHHK1992Subscriber
Thank you very much! I will check those values again.
I have a few more questions. Kindly make your reply.
1. Which turbulence model would you recommend for this case?
2. What should be the range of y+ for the above turbulence model? (Attempts to create low y+ lead high aspect ratio cells in ICEM and divergence in Fluent)
3. What should be the value of AoA above which transient analysis is inevitable?
August 17, 2018 at 9:20 amDrAmineAnsys Employee
1/SST is the most convenient cheap one for turbulent flows for standard applications
2/yplus~1 with 10-15 cells in the boundary layer
3/whenever it starts stalling transient run might be btter
4/In the workshop (belongs to ANSYS FLuent Training a mesh with 76314 cells was fine).
- You must be logged in to reply to this topic.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Suppress Fluent to open with GUI while performing in journal file
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2023 Copyright ANSYS, Inc. All rights reserved.