CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS (http://www.cfd-online.com/Forums/ansys/)
-   -   Problem with drag coefficient (http://www.cfd-online.com/Forums/ansys/105597-problem-drag-coefficient.html)

newminde August 3, 2012 07:18

Problem with drag coefficient
 
Hi everyone, I'm modeling Turbulent flow around cylinder, the main aim is to dicover Cd dependence on Reynolds numeber.
The cylinder is in the infinite field, material air, Diameter of cylinder 1m, Re=10000.
Model RNG,k-epsilon.
I'm changing only tubulent kinetic energy and tubulent Dissipation Rate.
And the resut is Cd=0.58, in case it should be approximatelly 1.1-1.2.
Maybe someone had done similar work, and have some advices.

Regards,
Mindaugas

flotus1 August 3, 2012 07:31

I encountered the same problem at Re=10^5. The best result I got was at about 70% of the experimental value.

Maybe you could try a k-omega based turbulence model or even RSM.
Don't worry though, I wouldn't expect a RANS model to yield perfect results in the detached flow over a blunt body.

newminde August 3, 2012 07:36

I thing the main problems are:
1) Bad mesh, at monday I'll try to change it.
2) Bad calculation of Turbulent kinetic energy, turbulent dissipation rate.
Also I have tried to change turbulent intensity and hydraulic diameter, but as I understand hydraulic diameter is essiantial only for pipes.
But project is 2D cylinder.

Laminar flow was quit good 1-3% inaccurate.

I thing for this exeriment k-epsilon model is good.

flotus1 August 3, 2012 07:48

I already did a mesh dependency study for this case.

Changing the turbulent kinetic energy and its dissipation rate at the inlet is not the right way to fix the results.
You can assume that the measurement was carried out with very low turbulent intensities upstream of the cylinder.
So increasing k at the inlet in your simulation might yield a higher C_d, but then the simulation no longer corresponds to the experiment.

newminde August 3, 2012 07:54

But you certainly must change parametres on the boundary conditions, because turbulence parametres dependent on Reynols number.

quate
Note by default, the FLUENT GUI enters k=1 m/s and ε =1m/s. These values
MUST be changed, they are unlikely to be correct for your simulation.

flotus1 August 3, 2012 08:09

But which value do you want to use? Unless you have a model of the wind tunnel that was used for the experiment, it seems impossible to me to "guess" correct values.

Aren't wind tunnels usually equipped to produce a homogneous flow field with very little turbulent disturbances?

flotus1 August 3, 2012 17:38

BTW: The turbulence parameters at the inlet do NOT depend on the Reynolds number of the flow around the cylinder.

Just imagine that in the experiment, instead of the cylinder with 1m diameter, a smaller with d=0.1m is used.
The Reynlods number decreases by a factor of 10, but the flow in the wind tunnel is still the same with the same turbulent quantities.

newminde August 6, 2012 01:45

All parametres can be defined:

http://hpce.iitm.ac.in/website/Manua...ug/node217.htm

I don't know what is a problem?
Maybe others have modeled turbulence flow and results were approximately equals to experimental ones?

newminde August 7, 2012 02:50

Results become more accurate. Re=10000 , Cd=0.9. I have changed turbulent model Spalart-Allmaras, turbulent intensity 0.5 and turbulent length scale 0.07, but still the result should be 1.15-1.2.
Maybe some advices, how to improve results.

flotus1 August 7, 2012 03:34

A wall-resolving LES should yield better results here.

Still there is the problem of the unknown Reynolds stresses and length scales at the inlet, which becomes even more crucial in a LES.
In my opinion, 0.9 is quite a good result as an approximation of the drag coefficient.


All times are GMT -4. The time now is 13:07.