[Gunni]

Hi guys!

I am working on a validation case for my thesis in OpenFOAM, simulating a flow around a circular cylinder, using kOmegaSST. I wanted to fully resolve the viscose sublayer with this turbulence model. But the drag coefficient I get was always too high.

These are the parameters of my case:

Cyclinder diameter: 10 mm
Flow velocity: 20 m/s
kinematic viscosity: 2e-5
Re=10000
y+_max=2.7
y+_average=1.34
y_min=1.31e-5m
Max. aspect ratio= 4.7


My boundary conditions are (I tested also other BCs with no success):

k:
internal=0.06
inlet=freestream (0.06)
outlet=freestream(0.06)
wall=fixedValue(1e-12)

nut:
internal=0.24
inlet=calculated
outlet= calculated
wall= fixedValue(0)

omega:
internal=63
inlet=freestream(63)
outlet=freestream(63)
wall=omegaWallFunction(63)

p:
internal = 0
inlet= freestreamPressure
outlet=freestreamPressure
circile=zeroGradient

U:
internal=20
inlet=freestream(20)
outlet= freestream(20)
circle=fixedValue(0)


The drag coefficient is calculated with the function "forces" in the controlDict file. Accourding to the text books of Schlichtling, I should get a drag coefficient of 1.2, but the results are around 1,64. I tried a lot of different boundary conditions, and also played with the schemes, but all the results have little difference.

I tried the same settings under the kkl-Omega, getting the same results as the kOmegaSST.

While simulating this case for high-Re (y+=32) and with wall functions, I get a quite satsifying drag coefficient around 1.1.

I have uploaded my complete case, so hopefully someone can help me with this.

[fredo490]

Are you sure of the turbulence properties ? Do you have any specification of the wind tunnel used ?

Your omega looks a bit low to me. You can try to use the toolbox of this website to get a proper value: http://www.cfd-online.com/Tools/turbulence.php

Edit, what is your domain size ? And is you mesh fine enough behind the cylinder to reveal the vortex ?

You can also try to run the simulation as an unsteady case.

[Gunni]

Thanks a lot for your reply!!

The boundary conditions was a left over from a previous setup, but my experience was, that it doesn't have a huge influence on the drag coefficient. But to be on the safe side I started another case with the following BCs:

k:
internal=0.015
inlet=freestream (0.015)
outlet=freestream(0.015)
wall=fixedValue(1e-12)

nut:
internal=1.55e-3
inlet=calculated
outlet= calculated
wall= fixedValue(0)

omega:
internal=13
inlet=freestream(13)
outlet=freestream(13)
wall=omegaWallFunction(0)

p:
internal = 0
inlet= freestreamPressure
outlet=freestreamPressure
circile=zeroGradient

U:
internal=20
inlet=freestream(20)
outlet= freestream(20)
circle=fixedValue(0)

I am not sure how fine the mesh should be behind the cylinder, so I uploaded a picture of it, maybe you can give me your opinion?

I forgot to mention the case runs unsteady under pimpleFoam.

Edit: The domain is 2D 0.5mx0.5m, with 83000 cells.

[Gunni]

The result of the drag coefficient using the new Boundary conditions are still too high. I get a value around 1.634.

Please help!

[Gunni]

Does nobody have an idea? Can someone please check if the function I use to calculate the drag coefficient is correct?

forces
{
type forceCoeffs;
functionObjectLibs ( "libforces.so" );
outputControl timeStep;
outputInterval 1;
patches
(
circle
);

// pName p;
//UName U;
log true;
rhoName rhoInf;
rhoInf 1;
CofR ( 0.25 0.12 0 ); //center of rotation
liftDir ( 0 1 0 );
dragDir ( 1 0 0 );
pitchAxis ( 0 0 1 );
magUInf 20;
lRef 0.01; //Reference length
Aref 1e-5; // Reference area
}

[Rafael_Coelho]

Hi Gunni,

I am very glad I found your post. I am working in a very similar problem. I reinstalled OF last month and decided to run some very basic cases to calibrate some useful meshs/cases. I am simulating a 30mm cylinder in a wind tunnel 300mmX300mmX3000mm blowing air at 10m/s. I know it is a big domain and I could be using a 2D domain but my real problem needs a 3D simulation.
One of the reasons I am using this case is because I have some experimental results from this experiment. We measured the flow using hot wire anemometry and PIV. I also using Schlichtling as a reference and I am also expecting a Cd of 1.2.
I am using simpleFoam and not pimpleFoam.

I will upload my case.

Regards,
Rafael

[tomas89]

Hello guys!

I'm working with a similar case but with a NACA, Would be very helpful for me to know how do you fix a min and max y+ coefficient and how to plot the residuals, y+, drag...

I know I'm not helping but your topic was the best to answer my question.

Thanks in advance,
Tomas

[Rafael_Coelho]

Hi Tomas,

There is no way to "set" a minimum or maximum y+ value, they are consequence of flow and size of the cells near the wall. The link below shows good way to estimate the cell of cell you need to get a desirable y+ value.
http://www.computationalfluiddynamic...t-cell-height/

To plot the variables you can follow the steps on this topic:
http://www.cfd-online.com/Forums/ope...residuals.html

Why you dont change your problem to a cylinder? My next step is a NACA0012, but I want to validate my case first.

Hope that help

[tomas89]

Hello!
Thanks for your reply Rafael_Coelho. I'm doing a validation with a NACA because afterwards I have to do a specific foil. About the problem that Gunni has, when I get wrong results is meanly because of the lRef and Aref... About Aref, is it a fronta-area or topview-area? (for the cylinder won't make much more sense the question.. hahaha)

[Rafael_Coelho]

Hi Tomas,

The cylinder simulation can be tricky due to the flow vortices, so if you can simulate the flow around a cylinder you are closer to solve the flow around a NACA profile. I will probably run the NACA tomorrow. Aref is what ever you want. In the cylinder case we are using frontal area, but could be using "wet" area. If you are comparing Cd and Cl you must know how your reference data was calculated, that is why we are using Schlichting.

It will be nice if you post some of your results and BCs anyway.

Regards,
Rafael

[Rafael_Coelho]

Some more discussion: http://www.cfd-online.com/Forums/ope...tml#post445016

[Rafael_Coelho]

I just ran it using pimpleFoam. Got Cd=1.175.

http://youtu.be/2LsQC_LJ8uo

[Gunni]

Hello Rafael,

thank you very much for your reply! I am still getting a cd=1.44. I will look into your case and hopefully see my mistakes in the simulation.

Edit: I have looked into your case, it seems that you are using a high-Re approach. While running my case at high-Re(y+=32) I also get satifying results but the problems surfaces at resolving the viscous sublayer. Have you tried to fully resolve the viscous sublayer?

[Pat84]

Hi,

I don't know the OF version you are using, but if it is an older version, than you might have a look at this post:

http://www.cfd-online.com/Forums/ope...nce-model.html

Best regards,
Patrick

[Rafael_Coelho]

Hi Gunni,

I´ve added 10 layers to capture the bondary layer. Didn´t have time to postprocess enough and didn´t check the y+.

Regards,
Rafael

[bia]

i have the same problem as mentionned. i'm not familiar with ansys but i'm trying to be so please help me .i'm trying to have a drag coefficient about 1.33.but i always find Cd =0.988.
my study is a laminar flow around a circular cylinder the diametre of the cylinder =15 mm the box is 750x400mm2.
Re=150.
may be a have a problem with the reference values.i set reference area= PI*D
length =PI*D/2 and depth =1.
FOR THE RESIDUAL I SET 1 e-08
max iterations per time step =40
these are tha best values i've made to be so closer but i still far away .

[davibarreira]

Hey bia, I got values close to yours... Im simulating at Reynolds 1e5 and 1e4. Did you manage to get the proper results? Also, my lift seems to be too high, does anyone have the same problem?

[Rasmusiwersen]

For whoever it might concern in the future, a solution to this problem can be the domain size. I've just performed simulations alike the ones presented in this post, where the domain extenden for only 10 diameters downstream. This lead to increased drag coefficients! Should be, as you say approx 1.22 but i got 1.4.

Increasing the domain to 50 diameters, the coefficients dropped instantly. Haven't got the final coefficient yet (performaing a convergence study), but it looks much more promising!

Happy foaming (Y)

/Rasmus