CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Drag Coefficients (http://www.cfd-online.com/Forums/fluent/65883-drag-coefficients.html)

mahadevan.swamy June 29, 2009 12:53

Drag Coefficients
 
Hi,

I have a 3D body in a tunnel and when i peformed some iterations, I am so surprised to see that I am getting a very high drag coefficient like 130 - 140, which is totally impossible.

My reynold's number is 2210000 since air would be coming into the tunnel at a velocity of 27.76 m/s. I am using the K-E model and for the solution, I have chosen to go with SIMPLE algorithm and all parameters are set to Second Order Upwind except the Pressure which is set to standard. The inlet boundary conditions is set to a velocity of 27.76 m/s with 2.6% Turbulence Intensity and 0.525 m as my turbulence length scale since my model is 7500mm long.

Is there any explanations why I would be getting a very high number for drag?

schwarczi June 30, 2009 12:15

Drag Coefficients
 
Hello,

How many iterations have you made when got those high drag coeff. values? Are you sure that your calculation has already been converged?

Well, if you were just at the beginning
of the process, it isn't extraordinary if you can see too high or too low values. By the way, it would be worth to doublecheck in Fluent the reference values used for calculating the drag coefficients. Select Report -> Reference values and set your ref. velocity and projected surface area in appropriate way.

Hope this helps.
Sch.

mahadevan.swamy June 30, 2009 12:25

Yes that's where i made my mistake. I didn't set the area and length. That explains why I am getting high values for drag coefficients. Another question is in terms of setting the length, is it the length of the tunnel or the length of the body?

Now my values for drag is low. I am running about 10000 iterations and waiting for convergence. Thanks for your help.

schwarczi July 1, 2009 06:39

'Length' sets the reference length, which is used in the computation of the moment coefficient, so you don't need to specify it for calculating the drag and lift coefficients.

Sch.

mahadevan.swamy July 2, 2009 14:51

I have another question. When setting the reference values, at the top we say compute from "inlet". When we specify the area, should we specify the area of the inlet (tunnel) or the surface area of the body?

schwarczi July 2, 2009 16:20

'Compute from inlet' is nothing more just a helpful option to set the values in an easy way, but the 'area' means the projected area of the BODY not the domain (it can be calculated somewhere in Fluent).

Dimo July 6, 2009 09:11

Quote:

Originally Posted by schwarczi (Post 221284)
'Compute from inlet' is nothing more just a helpful option to set the values in an easy way, but the 'area' means the projected area of the BODY not the domain (it can be calculated somewhere in Fluent).

Yes just go to Report > Projected Areas and then select the direction and the surfaces you're interested in, and the projected area should be calculated.


All times are GMT -4. The time now is 15:18.