[sigfridovalentino]

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

[Geon-Hong]

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,

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!

[sigfridovalentino]

Originally Posted by Geon-Hong

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,

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

[Alczem]

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 ).

[JRemington]

This is an old post, but I had the same problem. The airfoil in the incompressible/airFoil2D example is NOT NACA0012. It is not symmetrical, and it is too thick.


Furthermore the mesh fails the checkMesh test, and has the y+ problem indicated above.


The example is unsuitable for validation of OpenFoam.

[Svetlana]

Originally Posted by JRemington

This is an old post, but I had the same problem. The airfoil in the incompressible/airFoil2D example is NOT NACA0012. It is not symmetrical, and it is too thick.


Furthermore the mesh fails the checkMesh test, and has the y+ problem indicated above.


The example is unsuitable for validation of OpenFoam.

Could you please advise; what version of openfoam you are using.

[JRemington]

I'm using OpenFOAM versions 2412 and 13 on two different machines.


However, just by looking at the mesh, it is obvious that the airfoil is not NACA0012. Until you know what the mesh actually represents, there is no point in using the example for validation, as there are no experimental data for comparison.


See my other post for a satisfactory validation with NACA0012, using the NASA meshes.
Unable to validate OpenFoam installation with airFoil2D tutorial

[Yann]

JRemington is right, the airfoil2D tutorial default setup in not a NACA0012.

For those who might be interested, there is a NACA0012 blockMesh in the aerofoilNACA0012 tutorial:
https://develop.openfoam.com/Develop...rofoilNACA0012

[JRemington]

Thanks for pointing to that tutorial. However, it seems to be missing a file.
Attempts to run blockMesh in OpenFOAM version 2412 for the case result in this error message

Creating block mesh from "system/blockMeshDict"


--> FOAM FATAL ERROR: (openfoam-2412 patch=250528)
Cannot find surface "NACA0012.obj" starting from "/home/jim/tutorial/aerofoilNACA0012/constant/geometry/aerofoil"


From static Foam::fileName Foam::fileFormats::surfaceFormatsCore::checkFile(c onst Foam::IOobject&, const Foam::dictionary&, bool)
in file surfaceFormats/surfaceFormatsCore.C at line 297.

FOAM exiting

Presumably that surface contains all the interesting NACA0012 airfoil details.

[Yann]

Did you check/run the Allrun script?
The geometry has to be copied from the resources directory before running blockMesh. It should be there.

mkdir -p constant/geometry

cp -f \
    "$FOAM_TUTORIALS"/resources/geometry/NACA0012.obj.gz \
    constant/geometry

restore0Dir

runApplication blockMesh

[JRemington]

Ahh, thanks! I missed that step, and will study the results of the complete run.