
[Sponsors] 
August 27, 2014, 05:37 
NACA 0012 2D validation

#1 
New Member
Join Date: Aug 2014
Posts: 15
Rep Power: 4 
I have no good experience to aerodynamic analysis. I did some assignments in University days but I want to laern more and doing the validation as per given from here http://turbmodels.larc.nasa.gov/naca0012_val.html.
However I first run at angle of 10 deg but I get very small Cl. I think I am doing some mistake in setup or calculation. Few questions... I read in books that in 2D, the lift coefficient Cl is per unit span length, so the equation for coefficient of lift is: cl_2D=Lift per span length/(0.5 * rho * V^2 * C) In 3D it is CL_3D=Lift/(0.5 * rho * V^2 * A) C is chord length, and rho and V are the freestream conditions and A is planform area.. Now, if I do 2D simulation in fluent and 3D simulation in CFX (small thickness one element thick with symmetry), is this Cl calculation would tally with the NASA validation data? I wonder because though CFX only one element thick 3D airfoil will create similar lift as compared to 2D FLUENt because of symmetry at both end, but in 2D equation we have lift per span length. How do I calculate cl_2D coefficient in 2D if I know lift force? Will it same as CL_3D if I do a finite length airfoil?? Sorry for my poor English, its not my first language 

August 27, 2014, 06:26 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
When you do a 1 element thick simulation in CFX then you have to remember the force it calculates on the wing is over the area you modelled  so includes the element thickness. You have to divide by the element thickness to get the lift per unit length.


August 27, 2014, 06:34 

#3 
New Member
Join Date: Aug 2014
Posts: 15
Rep Power: 4 
Hi ghorrocks,
Thank for quick suggestion. I was thinking about whether I consider CFX simulation as 2D or 3D. But isnt 3D one element thick with symmetry at both ends giving same lift force as 2D in fluent? Can you also comment how I would calculate the cl in FLuent which is pure 2D? What should be the lift force per length there? Thanks 

August 27, 2014, 06:38 

#4 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
If you do a correct 2D simulation in Fluent (as a true 2D model) and CFX (as a 1 element thick 3D model) and you divide the CFX result by the element thickness you should get the same answers.
Try the fluent forum for details on Fluent. 

September 2, 2014, 04:07 

#5 
New Member
Join Date: Aug 2014
Posts: 15
Rep Power: 4 
Hi Ghorocks,
I spend time to model airfoil domain 100 mm thick and please have look my calculation below: Mesh: 500,000 mesh with hex structural elements, and it is onyl one element thick in the span dirrection. Problem setup: Left curve boundaries set as per the components u and v dependign on angle 10 deg, and top, bottom and right straight boundaries are opening with entrainment option. Turbulent model is SST, and discretzation scemes high resolution for mass/momentum and second order for turbulent quantities. Y+ values less than 7 on airfoil surface Results of velocity and pressure: Results of lift: I start with 10 deg angle of attack just to make sure I setup everything right. But when I substitue this value of lift to the above calculation sheet, I get cl value very low. It is useless to do all angles if I can not do 10 degree correctly. What am I missing?? Can you please help me? Thanks Last edited by cfdseeker; September 2, 2014 at 06:06. 

September 2, 2014, 19:08 

#6 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
Use the force_y() CEL expression to get the force, not the function you used.
So what CL do you get, what CL are you comparing to and where did you get that CL from? Also, have you read the FAQ on accuracy? http://www.cfdonline.com/Wiki/Ansys..._inaccurate.3F You should be able to get CL on a foil like this accurate to a few percent. 

September 4, 2014, 04:36 

#7 
New Member
Join Date: Aug 2014
Posts: 15
Rep Power: 4 
Hi Ghorrocks:
My geometry, boundary conditions is from here: http://turbmodels.larc.nasa.gov/naca0012_val.html I compare data with following NASA paper of LAdson (page 6, 0.15 Mach, 2 million Re): http://ntrs.nasa.gov/archive/nasa/ca...9880019495.pdf I Also correct my formula with your suggestion and add the sine/cosine components from both force_x and force_y in stream direction (I was considering only one component earlier) And I get much better results now: For accuracy I ensure the mesh is fine for the first run (I then will run more fine meshes for mesh independence). Also, I monitor drag, lift, imbalance for convergence. Please have look the plots How do I improve drag prediction?: 1) I get good result for lift but drag is overpredicted. Do you think that is because of high Y+? Will results improive if I fine the mesh near wall to Y+ value close to 1 so it resolve boundary layer? THe boundry layer expected to be fulyl turbulent so it will be very thin and maybe capturing that gradients for velocity/vorticity will give better results for viscous drag?? 2) Currently I am running as constant density because MAch no. is very low and compressibility effects is negligible. If I change to ideal gas, will it be more correct? 3) Is opening BC with entrainment option right? 4) Will I get better result if I incline the mesh domain to angle of attack so it is parallel to stream? Thanks for your help 

September 4, 2014, 07:35 

#8 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
It is normal to have CL much more accurate than CD. Correct drag requires much more careful work. This FAQ describes what you should consider as you try to get it more accurate: http://www.cfdonline.com/Wiki/Ansys..._inaccurate.3F
You are looking for small errors, so you need to try things which will only have a small effect. I suggest compressibility is possibly a factor you need to consider, but only after you have fully converged an incompressible flow model on mesh, residual and boundary proximity. 

September 4, 2014, 09:40 

#9 
New Member
Join Date: Aug 2014
Posts: 15
Rep Power: 4 
I have some experience of CFD modeling in CFX and I make sure the residual is less than 10^4, imbalance less than 0.5% and monitors flat (~12% change for last 2030% of total iterations) so that quantities not changing much.
I will do error analysis for domain length and other inputs like compressibility etc. Nasa advise 500 chord length but I take 30 chord lengths. Now I know my setup work so I will make larger domain and test so that boundaries dont effect the results too much. The result is very much depend on the mesh size I suppose because changing mesh size to double gives different result. So getting very fine mesh is important to capture gradients. I will use NASA guideline for mesh independence (http://www.grc.nasa.gov/WWW/wind/val.../spatconv.html). I also saw instable behaviour close to 16 deg where stall is expect, meaning the separation needs to be captured correct. There is some work to do here I will update the post with any new things I find soon. Thank you 

September 8, 2014, 17:22 

#10 
New Member
Join Date: Aug 2014
Posts: 15
Rep Power: 4 
Hi ghorocks,
I finish my simulations and I get much results now, have look: I got fed up with ANSYS meshing but. It really sucks. I have to specify 4000 as bias factor to reduce my first cell height to 0.8 mm . But if I specify more than 4000 factor, meshing gave error. So i switched the meshing package I love, ICEM CFD. IT give me very good control on mesh and quality I try to resolve all boundary layer, and achieve Y+ value close to 2. Have a look my boundary resolution I also find that the turbulent models predicts turbulent bounrdary layer on all airfoil surface which is not the case, in reality the airfoil near leading edge has laminar boundary layer and the rest of it is turbulent. But since RANS turbulent models predicts turbulent boundary layer everywhere, the viscosity is overestimate (viscosity ratio high everywhere on surface). So wall shear stress and viscous forces on wall are high, so drag is high. I try to model with SST gamma theta, but intermittancy equation take very long time to reduce imbalance, and it was unstable too. So I decide to use the normal 2 equation kw SST model to verify tripped data of Ladson, where the laminar boundary layer toward the leading ege of airfoil is disturbed to form turbulent one. Even so, my drag results are not accurate at high angle, it is consistent with NASA CFD solvers too, they overpredict the drag at high angle. I may look at RSM, but again it is the RANS model so will have similar limitation. I now move to verify the 3D ONERA M6 wing http://www.grc.nasa.gov/WWW/wind/val.../m6wing01.html Hope I achieve good result for that too. Thank you for your time nad suggestions, it helps me lot. I will post more information when I have more result for 3D wing 

September 8, 2014, 18:10 

#11 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
These look like a pretty good set of results, nice work. Your CL is very good and CD is pretty good  but CD, especially at higher angles of attack is difficult. I agree with your comments on the turbulence transition. If you wanted to get the CD results better then the turbulence transition model is the way to go (not RSM). But if you know the turbulence trip point then do no use the gamma theta model but use specified intermittency to define the trip point.


September 9, 2014, 06:05 

#12 
New Member
Join Date: Aug 2014
Posts: 15
Rep Power: 4 
HI Glen
THanks I will keep mind the point about specifing the intermittancy. It seem interesting but I have to read more in reference about trip point. Also, I want to ask on the same subject, I read about "meshless" CFD codes online: Xflow: kinetic solver and uses generalise Finite Difference for points in domain adn solve Lattice Boltzmann equations not NS equations NOGRID: Base on Finite POintsent Method I read some theory in this nice report : http://aerocomlab.stanford.edu/Pape...final_katz.pdf And "meshless" is not correct anyway because we creating points in space for anyway, just dont have to bother about mehs quality. I dont have much expereicne on this, but mostly I read that this Langrangian meshless methods good only for external flow, and not very good for solving internal flows where shear stresses are high. Normal meshing solvers that solve Eulerian NS equations works better for internal flow. Have you any experience on this? THanks 

September 9, 2014, 06:17 

#13 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
A little experience in LatticeBoltzmann methods. They are adaptations of gas Kinetic theory so when the fluid is close to a low pressure gas they work well. They also seem to work pretty well for general CFD as well. At the moment they do not have the same extensive physics as the Navier Stokes solvers do but they are evolving rapidly. A big strength is that the flows are inherently transient, so most turbulent simulations are in effect LES simulations.
I do not know anything about NOGRID. 

September 9, 2014, 07:12 

#14 
New Member
Join Date: Aug 2014
Posts: 15
Rep Power: 4 
Did you find the LAttice Boltzmann approach fast as compared to normal Eulerian solvers based on NS equation, in term of runtime, and also equal accurate? Also, do you recomend this methods for itnernal flow like pipe flow?
Thanks for all the comments 

September 9, 2014, 07:16 

#15 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
The strength of LB methods is definitely in external flows at high Re. I do not know whether it is appropriate for pipe flow or Eularian models  you will have to work that out for your specific case.


December 30, 2014, 16:42 
Boundary Validation

#16 
Senior Member
Hasan K.J.
Join Date: Dec 2011
Location: Bristol, United Kingdom
Posts: 196
Rep Power: 6 
Hey,
By any chance did you validate boundary layer growth on the walls for NACA 0012 ? Regards, Hasan K.J
__________________
"Real knowledge is to know the extent of one's ignorance."  Confucius 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
NACA 0012 validation Drag problems  leo_NM  FLUENT  7  August 8, 2014 14:18 
Naca 0012 validation, Cd value is too high.  Peter88  OpenFOAM  4  January 21, 2014 17:10 
2D NACA 0012 Airfoil Validation  nvtrieu  FLUENT  0  May 30, 2013 10:22 
Validation of NACA 0012 pressure and velocity contour  Tom Lucius  FLUENT  1  December 27, 2011 22:49 
Validation of NACA 0012 pressure and velocity contour  Tom Lucius  Main CFD Forum  0  December 26, 2011 10:20 