Calculating Coefficient of Drag in ANSYS Fluent
Hi,
I am doing research in automotive aerodynamics and I am using Fluent for CFD. I need to know how to calculate the parameters such as Drag coefficient Lift, and pressure coefficient and also how to plot these along the vehicle length. I have tried to extract these from the solution but I am not sure if its correct way to it...so please see the steps that I did and tell me if this is the way to go.. After solving the flow, I did; 1. Reports> projected area>select the front end, direction vector in flow direction>copy the calculated value in reference area. 2. Reports>forces>select all vehicle wall zones>define direction in flow direction>print. Please suggest any good tutorials that address automotive aerodynamics in fluent. Thanks. 
in reference values set the free stream velocity and the projected surface area.
under "monitors" you can see the drag and lift options where you can print, plot and write the values. select the vehicle surfaces from there by clicking on them. 
That graph shows the Cd convergence...I guess I should take the value corresponding to the last iteration when the solution has converged..right?

If the run is steady and the if the cd plot settles down even after running in second order, then the value corresponding to the last iteration is your cd value.

Thanks Naren...Cheers!

Btw..can I plot the values of Cd at particular points...say along the length of the vehicle?

I dont know exactly, but you can try this.
Display  Plots XYplot On Y axis select the pressure coefficient vaue and X axis function as curve length. Select the surface from the list by clicking on them. Hope this helps 
The value you should plot is Cp along the vehicle centerline. Best way to do this is probably to split the vehicle into an "upper" and "lower" surface and then plot two individual Cp lines along those surfaces at a certain lateral coordinate (probably 0 as you care about Cp along the middle/centerline of the car).
Cd is just a value that Fluent calculates based on force.. So you can always double check it by going to Reports > Forces > Then pick an axis in which you have the direction of flow (Z for example) and then put in 1 (or 1 if the flow is opposite in direction to the axis in question) and report the force. It will list a pressure drag force, a viscous drag force and a total (sum of the two). Then if the frontal area of your car is for example 1.84 m^2 you can easily calculate the Cd by using the formula that Fluent uses too: Cd = 2*Fd / rho*(v^2)*A where you know the free stream velocity v, the frontal area A, the density of air rho and the reported drag force F that you got from Fluent.. If you used a symmetry condition in Fluent, you've got only ~1/2 of the drag force calculated, so you would use only 1/2 of the frontal area A to get the Cd (same goes for a Reference value in Fluent.. if using symmetry enter 1/2 of A). 
Quote:
then I guess mirror surfaces is only used to graphical purpose...right?? btw fluent also gives coefficients when I use the Reports>forces... Thanks. 
Yes. Symmetry doesn't necessarily mean "mirror about this plane", symmetry is a no shear force wall basically (same as if you had a wall boundary condition with specified zero shear force).
When you are doing a force report, then yes  you pick all the surfaces of your car (half car basically, if you used symmetry) and then when you report a force in the X, Y or Z direction (wherever your airflow is coming from), the reported force is only ~1/2 of the drag force that the car would experience if you calculated the full model without the symmetry. Fluent calculates your Cd with this force in the Drag monitor, and the reference value for area that you put in Reference values. The way to get the correct Cd right away, is to set the frontal area in the Reference values to 1/2 of the total frontal area of the car.. so what you get is 1/2 drag force being mixed in with the 1/2 of the frontal area so you get a Cd which is again similar to the one you would get without symmetry. 
thanks...that clears everything....
Thanks a lot! 
Mass flow rate with respect to symmetry plane
Hi all,
I am modelling a 3D pipe. Since pipe is symmetry with respect to z axis, I made the half pipe. After simulating, I calculated the mass flow rate for outlet from the velocity is 16 and from fluent, I got 6.45 for outlet mass flow rate. Does fluent calculated all the parameter for half of the geometry ? After reading this thread, I think I should also multiply the mass flow rate found from fluent by 2 to get the actual mass flow rate through the outlet. Please clarify my query. Regards, Tanjina 
Yes you have to multiply

Hi,
I am trying to model a circular object in 3d in fluent.. it is in contact with the stationary ground plane which is acting as a floor. The value of CD I am getting is approximately double of what I am expecting and I am sure all my reference values are correct, eg the area is the cross section area of the frontal face etc. The object and the ground floor are walls with the surrounding walls of the domain set to symmetry condition. Does anyone have any idea why my values or CD are approximately double? I have a feeling after reading the earlier messages in this thread that it could be due to the area and the symmetry plane but I don't know if that is something i should be changing and if so why? Regards 
Let me know the BCs please

The object is a wall, the floor and the contact patch with the ground is also a wall. Velocity inlet for the inlet and pressure outlet for outlet with the sides and top of the domain are symmetry. Hope that helps

All times are GMT 4. The time now is 21:34. 