CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Lift coefficient (http://www.cfd-online.com/Forums/openfoam-solving/60223-lift-coefficient.html)

msrinath80 May 8, 2006 11:45

Does anybody know how the lift
 
Does anybody know how the lift coefficient is calculated using the lift/drag utility in OpenFOAM 1.2. To my knowledge, the equation should be in the following lines. When using icoFoam, how does the utility know what the density (rho) is?

C_L = F_lift / (A_ref * 0.5 * rho * U_ref^2)

kumar2 May 8, 2006 15:29

Hi pUI the liftDrag utility
 
Hi pUI

the liftDrag utility is for solvers where pressure is pressure/density . you can check the dimensions of pressure in icoFoam to see what dimensions it is using and then apply a correction to the output of icoFoam

regards

kumar

anja May 9, 2006 04:17

Hi all, I also did a calcul
 
Hi all,

I also did a calculation with icoFoam and the results for p are of the dimensio [m2/s2]. Now I want to use FoamToTecplot.
Does that change the dimension of the pressure? Or do I have to do that myself? But therefor I have to know with which density icoFoam is calculating?!

Thanks
Anja

kumar2 May 9, 2006 05:03

Hi Anja foamToTecplot does
 
Hi Anja

foamToTecplot does not change the dimensions. so you will have to do the conversion yourself.

since icoFoam is solving p/rho , all fluid densities are same for icoFoam . i am not sure if viscosity is used by icoFoam . but if it is then you will have to change the viscosity to what you want

regards

kumar

anja May 9, 2006 05:18

Hi kumar, so I just need to
 
Hi kumar,

so I just need to know with which density icoFoam is calculating?? Where can I find that value??

Thanks
Anja

hjasak May 9, 2006 05:25

There is no density: it is con
 
There is no density: it is constant and the whole equation has been divided through by the density. This is why you get different units for nu and p, i.e. kinematic viscosity and kinematic pressure.

If you really have to have density, it is equal to 1.

Hrv

eugene May 9, 2006 05:27

icoFoam does not calculate a d
 
icoFoam does not calculate a density, it calculates p/rho, using a specified value of nu. You should choose rho based on the kinematic viscosity (mu) and rho you used to calculate dynamic viscosity nu.

msrinath80 May 9, 2006 05:28

But we never did input a rho t
 
But we never did input a rho to start with?

msrinath80 May 9, 2006 05:31

Does that also mean that the w
 
Does that also mean that the when the liftDrag utility extracts the forces on walls, it assumes a density of unity? So if I wish to use the definition as mentioned in the beginning of this thread, I should account for rho based on the nu I input say in the Aref term?

eugene May 9, 2006 05:45

My mistake its the other way r
 
My mistake its the other way round. nu is of course kinematic visc not dynamic.

You dont need to put in rho for icoFoam becuase you are solving p* = p/rho. Not p.

If you want to calculate lift and drag forces you have to pass rho into the calculation somehow. Otherwise you will end up calculating F/rho.

msrinath80 May 9, 2006 05:48

Actually F_Lift/rho is just wh
 
Actually F_Lift/rho is just what I need. However, since rho can be taken as unity as Hrv menttioned, I can modify A_ref to account for rho by using A_ref_eff = A_ref * rho. The 'rho' here would be based on the actual density I had in mind when I decided nu. Would this be ok?

anja May 9, 2006 05:54

So there is the equation: kin
 
So there is the equation:
kinematic viscosity mu = dynamic viscosity nu / rho

In the file "transportation Properties" you can write a value for:
nu [0 2 -1 0 0 0 0] certainValue
(shouldn't this be mu then??)

But, as OpenFoam uses rho=1kg/m the values (apart from the dimensions) for mu and nu are the same??

msrinath80 May 9, 2006 05:56

Anja, It should be the othe
 
Anja,

It should be the other way around:

kinematic viscosity nu = dynamic viscosity mu / rho

anja May 9, 2006 05:58

Yes, I just did not see the ot
 
Yes, I just did not see the other post, as long as I was writing mine.

But what about my last sentence before?

msrinath80 May 9, 2006 06:13

I guess 'mu' does not have muc
 
I guess 'mu' does not have much meaning in icoFoam. Case in point, since both sides of the transport equation are divided by rho, p* = p/rho as Eugene mentioned. So the pressure Openfoam calculates should be actually 'p/rho'. As a result, when we want to extract the pressure we should multiply the 'p' output with rho (this rho should be what you intended it to be, for instance, consider flow of water. rho = 1000 and mu = 0.001 => nu = 0.001/1000 = 0.000001 [all in SI units]). This is only for the grad(p) term. the 'mu grad(grad(v))' term in the original N-S equation is now 'nu grad(grad(v))' as it should be when it is divided by 'rho'.

The problem now is trying to follow 'rho'. If 'rho' needs to be passed for the calculation of lift coefficient, then one should multiply the pressure 'p' obtained from OpenFoam with 'rho' (which is 1000) to get the actual pressure.


However, to calculate C_L using:

C_L = F_lift / (A_ref * 0.5 * rho * U_ref^2)

one need not bother about calculating the actual pressure because the pressure itself is 'p/rho' and we can be certain that rho is 1000 here since we fixed nu to be 10^(-6). So the expression for C_L becomes:

C_L = F_lift / (A_ref * 0.5 * U_ref^2)

Hrv, Eugene: Does this sound OK?

hjasak May 9, 2006 06:17

Yup, it's good. Hrv
 
Yup, it's good.

Hrv


All times are GMT -4. The time now is 13:18.