CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   FLUENT: Reference values, Boundary Conditions, Drag Co-efficient and Downforce (http://www.cfd-online.com/Forums/fluent/126395-fluent-reference-values-boundary-conditions-drag-co-efficient-downforce.html)

Harshal November 16, 2013 04:35

FLUENT: Reference values, Boundary Conditions, Drag Co-efficient and Downforce
 
Hello all,
I have recently undertaken a project in vehicle aerodynamics and I need some guidance. In my project work, I have to do two simulations.
Simulation 1: Keep the car stationary and the give the wind velocity and

Simulation 2: Give the car it's velocity and keep the wind stationary. Then, I have to compare the results.

I have questions regarding reference values, boundary conditions and drag co-efficient.

1) Reference values:
In the 'Area' option, I have given the projected surface area of the car in the X direction, since I want to know the drag. What should I give for the 'Length' option ? The car length ?
Also, for the 'Velocity' option what should I input. I think I should give 0 for Simulation 1 and the car velocity for simulation 2, but I am not sure.

2) Boundary Conditions:
In boundary conditions, there is an option for 'Hydraulic Diameter'. The car, that I am analysing sits in a rectangular 3D wind tunnel. Therefore, I have given the 'Hydraulic Diameter' for Inlet and Outlet as that of a rectangular vent, namely (2*a*b) /(a+b) where 'a' is the width and 'b' is the height. Is this correct.

3) Drag Co-efficient:
I am not sure whether Fluent directly gives the drag co-efficient or not. For every iteration it shows the cd value, but I think it's the cd convergence values and not the absolute cd value. Am I correct ?
Or should I just calculate the cd value from the drag force ?

4) Downforce:
I know that I can get the downforce from the Reports>Forces option. The question is, that in my 'Reference Values', in the 'Area' option, I plan to give the projected car surface area in x direction. Will this lead to a wrong downforce value ? (Since downforce calculation need projected area in the Z direction and not X direction)

Thank You for your help,
Regards,
Harshal

smhosseini November 18, 2013 03:51

Hi Harshal,
In simulation 1, you should consider velocity inlet and an outlet condition, and stationary wall for car. In simulation 2, you should consider a moving wall and you don't need any inlet or outlet condition. I don't know anything about calculation of drag in fluent.
Be successful.

Harshal November 19, 2013 05:20

Quote:

Originally Posted by smhosseini (Post 462344)
Hi Harshal,
In simulation 1, you should consider velocity inlet and an outlet condition, and stationary wall for car. In simulation 2, you should consider a moving wall and you don't need any inlet or outlet condition. I don't know anything about calculation of drag in fluent.
Be successful.

Hello smhosseini,
thank you for your replies. They have very helpful !

Regards,

Harshal

Kokemoor November 19, 2013 12:01

Reference values are only used to calculate non-dimensional coefficients, such as the coefficient of drag. Their settings will not affect physical values such as force. Regarding 3), check out the Fluent User's Guide, chapter 28.15.3 on force and moment monitors.

stuart23 November 21, 2013 08:56

Simulation 2 will not work.

Except for the rare case that your car is actually a flat plate...

smhosseini November 21, 2013 10:27

Quote:

Originally Posted by stuart23 (Post 462917)
Simulation 2 will not work.

Except for the rare case that your car is actually a flat plate...

Hi dear Stuart,
Could you tell me why the simulation 2 won't work?
I think he can consider the external wall of the car as moving wall. Isn't it?

flotus1 November 21, 2013 14:21

Without moving/deforming meshes, a moving wall can only have a tangential velocity component.
The only shape where this makes sense is indeed a flat plate or a rotating cylinder/sphere.

Harshal November 24, 2013 11:20

Quote:

Originally Posted by flotus1 (Post 462969)
Without moving/deforming meshes, a moving wall can only have a tangential velocity component.
The only shape where this makes sense is indeed a flat plate or a rotating cylinder/sphere.

Hello, flotus1,
thank you for your reply. Could you please explain what you mean by moving/deforming mesh ? I'm going through the Fluent user handbook. Do you mean moving frames of reference or moving mesh ? Also, in moving mesh there are two types : sliding and dynamic. Can you please explain which option to use ?

Thanks,

Harshal

flotus1 November 24, 2013 12:49

None of them.
For an external aerodynamics simulation of a vehicle, the only sensible approach is number 1.
Dont forget to model the floor as a moving wall.

Harshal November 24, 2013 13:06

Quote:

Originally Posted by flotus1 (Post 463288)
None of them.
For an external aerodynamics simulation of a vehicle, the only sensible approach is number 1.
Dont forget to model the floor as a moving wall.

Hi, thanks for the reply.
Just out of curiosity, if I give inlet velocity in BOTH the simulations and in the 1st take road as moving wall and in second give velocity to the car, would there be any difference in the results ?

Thanks,

Harshal

Harshal November 27, 2013 06:37

Quote:

Originally Posted by flotus1 (Post 463288)
None of them.
For an external aerodynamics simulation of a vehicle, the only sensible approach is number 1.
Dont forget to model the floor as a moving wall.

Hello flotus1,
I want to ask you about the moving wall condition. I have created a velocity inlet and given the wind velocity. Now I have defined the road as a moving wall and have given the car velocity to it (which is same as the velocity-inlet velocity ). The question is should I select the road (moving wall) as 'relative to adjacent zone' or as 'absolute' velocity ?

Thanks,

Harshal

flotus1 November 27, 2013 07:26

Since you have no moving zones, both options should yield the same result.

Harshal November 27, 2013 07:31

Quote:

Originally Posted by flotus1 (Post 463720)
Since you have no moving zones, both options should yield the same result.

Ok ! Thanks a lot !

Harshal

Harshal April 10, 2014 09:06

Doing multiple simulations for different speeds
 
Hello all,
I need your help. I have to find out the Cd and Cl values for a car using k-epsilon and k-omega models for multiple speeds (about 15 different speeds). Can some one please tell me how to do that ?

Thanks a lot,

Harshal

Harshal April 18, 2014 15:18

Which area does Fluent take to calculate lift force on a car
 
Hello all,
I wanted to know which area does fluent consider to calculate lift force for a car. From what I found out, the area considered for calculating lift force varies from object to object.

So, can someone please tell me how to find out the area, which Fluent uses for calculating lift force on a vehicle.

Thanks,

Harshal

flotus1 April 19, 2014 06:20

The area Fluent uses for calculating coefficients can be found (and changed) in the reference values section.

Harshal April 20, 2014 04:08

Quote:

Originally Posted by flotus1 (Post 487017)
The area Fluent uses for calculating coefficients can be found (and changed) in the reference values section.

Hello flotus,
as far as I know, for the Cd value, the area projected in X direction (frontal area) is considered while for Cl, the area projected in Z direction (car viewed from top) is considered. As these two values are different, I wanted to know which area value to put in the Reference Values. I want to have both, the Cd and the Cl.

Harshal

flotus1 April 22, 2014 05:59

You could set the area to some specific value (1mē would be quite handy) and multiply the lift and drag coefficients fluent produces by any factor you want.

engrmansoor2534 May 2, 2014 05:51

problem with flow domain
 
I m new to fluent.I am doing analysis in fluent.but my domain seems upside down(inverted):mad:
How can i fix it::;
kindly help me..

Harshal August 1, 2014 06:23

Hello all,
I recently completed my project work. This was my first experience with CFD and I thank you all for your help and guidance. Without your support, it would not have been possible for me to complete this project.

Thank You all !

Harshal


All times are GMT -4. The time now is 19:13.