CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Airfoil NACA0012 drag and lift coefficient validation

Register Blogs Community New Posts Updated Threads Search

Like Tree1Likes
  • 1 Post By Geon-Hong

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 13, 2024, 10:23
Default Airfoil NACA0012 drag and lift coefficient validation
  #1
New Member
 
Sigfrido Valentino
Join Date: Mar 2024
Posts: 2
Rep Power: 0
sigfridovalentino is on a distinguished road
Hello everyone,
I've recently started some CFD simulations in OpenFOAM 10, but I'm facing some problems with drag and lift coefficient calculation.
I'm basically using Openfoam's simpleFoam Airfoil 2D NACA0012 tutorial and have reproduced the conditions described here:https://www.openfoam.com/documentati...l-2d-resources. Inside the controlDict file I inserted the functions to calculate the drag and lift coefficient, but the values ​​obtained do not match the experimental data (https://turbmodels.larc.nasa.gov/NAC...on_expdata.dat), for example, using the configuration described in the first link, for an angle of attack of 0° I get cd=1.69e-02 instead of 0.809e-02.
There are similar discussions on the forum, but despite having tried what had been recommended to others (lowering the solver tolerances, increasing the number of iterations, checking the initial conditions several times, ...) it didn't work. What's strange is that this and other tutorials (like the rhoSimpleFoam airfoil one) don't give me results comparable to those of the experimental data.
You can find all the files in this repository of mine: https://github.com/sigfridovalentino/airfoil2dnaca0012
Thank you all
sigfridovalentino is offline   Reply With Quote

Old   March 15, 2024, 08:10
Default You should check the model again. It doesn't look like NACA0012 airfoil
  #2
Member
 
Geon-Hong Kim
Join Date: Feb 2010
Location: Ulsan, Republic of Korea
Posts: 36
Rep Power: 16
Geon-Hong is on a distinguished road
Hi,

I have a question. Is the airfoil really NACA0012? Where did you get the airfoil data?

First of all, your airfoil doesn't seem to be NACA0012. Even the airfoil looks like a cambered one. And the thickness ratio is over 18%, not 12%. Please check if the model is NACA0012 or not. Please refer to fig 1.

Second, the mesh has too high y+. y+ of your mesh shows,

Code:
patch walls y+ : min = 2368.4886, max = 19630.814, average = 14302.302
This means that the wall bounded flow is not resolved properly. (fig 2)


In addition, in my opinion, your mesh is too coarse to simulate an airfoil (fig 3). I recommend you to review the model and mesh first.

Good luck!
Attached Images
File Type: jpg fig 1.jpg (34.3 KB, 23 views)
File Type: png fig 2.png (6.0 KB, 14 views)
File Type: jpg fig 3.jpg (196.2 KB, 21 views)
AtoHM likes this.
Geon-Hong is offline   Reply With Quote

Old   March 15, 2024, 08:30
Default
  #3
New Member
 
Sigfrido Valentino
Join Date: Mar 2024
Posts: 2
Rep Power: 0
sigfridovalentino is on a distinguished road
Quote:
Originally Posted by Geon-Hong View Post
Hi,

I have a question. Is the airfoil really NACA0012? Where did you get the airfoil data?

First of all, your airfoil doesn't seem to be NACA0012. Even the airfoil looks like a cambered one. And the thickness ratio is over 18%, not 12%. Please check if the model is NACA0012 or not. Please refer to fig 1.

Second, the mesh has too high y+. y+ of your mesh shows,

Code:
patch walls y+ : min = 2368.4886, max = 19630.814, average = 14302.302
This means that the wall bounded flow is not resolved properly. (fig 2)


In addition, in my opinion, your mesh is too coarse to simulate an airfoil (fig 3). I recommend you to review the model and mesh first.

Good luck!

Hi Geon-Hong,
thank you for your kind reply.
The mesh I'm using is the one given on the very same page 'Turbulent flow over NACA0012 airfoil (2D)' of the User Guide of OpenFOAM (link to the page: https://www.openfoam.com/documentati...l-2d-resources, link to the repository with the mesh: https://develop.openfoam.com/Develop...Foam/airFoil2D).
I'm super confident with the fact that you are right about the issue, nevertheless I cannot validate the drag and lift coefficients by using the other tutorials given with OpenFOAM 10, for example the rhoSimpleFoam-airfoil NACA0012 one, even if I'm setting the same initial conditions of the experiment.
Thank you
Attached Images
File Type: jpg Screenshot from 2024-03-15 13-15-16.jpg (56.5 KB, 10 views)
sigfridovalentino is offline   Reply With Quote

Old   March 15, 2024, 10:34
Default
  #4
Senior Member
 
Join Date: Dec 2021
Posts: 251
Rep Power: 6
Alczem is on a distinguished road
The mesh is probably responsible here, but are you also sure you are using the correct reference area to compute your Cd? There is a factor of around 2 between the two Cd, and I have made this mistake when comparing drag coefficients between bodies but using irrelevant reference areas. I would rather compare the drag and lift forces to make sure it has nothing to do with postprocessing the data (but again, the y+ is NOT fine ).
Alczem is offline   Reply With Quote

Reply

Tags
airfoil 2d, data validation, drag coefficient, lift coefficient, openfoam tutorial


Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Calculation of lift and drag coefficients on airfoil CoolHersheys OpenFOAM Post-Processing 5 September 27, 2021 07:04
oepnfoam naca0012 I can not get the correct lift coefficient and drag coefficient cheng1 OpenFOAM 4 April 20, 2021 00:43
Airfoil Coefficient of Lift and Drag - Published Data vs CFD Results Mick2450 CFX 4 April 23, 2020 20:18
wrong SU2 calculation for lift and drag coefficient for NAC4421 mechy SU2 7 January 9, 2017 06:18
High drag for airfoil compared to XFOIL and wind tunnel data Ry10 SU2 15 October 30, 2016 18:27


All times are GMT -4. The time now is 05:24.