CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   drag coefficient in ansys fluent 12.0 (

krishna June 16, 2010 12:56

drag coefficient in ansys fluent 12.0

Can any one help me to find the drag coefficient in Ansys fluent 12.0.

My project is to do analysis the pressures, velocities and Drag coefficient of a car model, at certain speed in both Cham Phoenics and Ansys Fluent softwares

I have designed a car model in Pro-E, and the anslysis is carried out in Cham Phoenics to find the pressures, velocities and Drag coefficient. Then I have imported the model in Ansys Fluent and the analysis is carried out to find the same parameters. But the results are different, Can any one know why? and where can I find the Drag coefficient in ansys fluent?

while doing it in Ansys I have used ICEM mesh file.

please help me out in this regard.

mbell10 June 17, 2010 06:25

how different are your results?

kdrbrk June 17, 2010 08:07

First, set the reference values in Fluent. speed and density is enough for force coefficient calculation.

then, under report, go to forces and select drag.
define the drag force direction.
select the car body on the right side.

print or write to a file.

krishna June 17, 2010 10:06

all the pressures in Pa

thank you

kdrbrk June 17, 2010 10:16

Are the operating conditions same?
by default, fluent operating conditions are set to 101300 Pa.
The pressures that you see is gauge pressure, the difference between pressure at that point and atmospheric pressure.

Max and min pres. an be different depending on the mesh, solver type, etc.
I suggest you to look for forces on the car.

But your results seem very different.
Do you use same method in both softwares?

krishna June 17, 2010 17:20

in fluent same operating pressure used.

in phoenics meshing is given more on the car body than the vaccant places

in ansys meshing is done in ICEM

i took only half body and created domain like walls and symmetry wall. then the meshing is done in ICEM and I have imported that file into ansys fluent.

in ansys i can see only drag convergence it came like 4.568e^5

but i need to find out the drag coefficient which should be in between 0.2 to 0.3

krishna June 17, 2010 17:33

meshing files attached
2 Attachment(s)
i have attached my meshing file in both phoenics and ansys, please have a look at it

kdrbrk June 18, 2010 01:37

first of all, you need a larger domain to have correct results, at least -as far as I know- 10 car length after the car. Thats what they say when you simply analze an airfoil.

In Fluent, you see the drag coeff., not drag convergence.

Just edit reference values.
They are used to derive the coefficient from force on that body.
If you write 1 for velocity and density of air, than you get directly total force on that body.
If you write correct velocity and density values, than you get CdA of that body.
If you exacty know the frontal area of the car, than write it as a reference value, like others, and you get Cd of the car.

krishna June 18, 2010 04:25


i will change the domain size and try it

previously i tried meshing for the bigger domain as u said but i got an error like ran out of memory, thats why i reduced the domain size.

any how i will try now once again

the domain size in both softwares should be same right?

thank you

kdrbrk June 18, 2010 05:28

if you want to compare the results between two solvers, it is best to use same mesh. but it is not always possible.

running out of memory is a common problem if you are using personal computer for analysis, just like me.

as a solution, you can reduce the mesh quality near the car surface, like not meshing the boundary layer and letting solver model it via wall functions.

by the way, for a more realistic boundary conditions, you can use these settings:

car = wall
symmetry plane = symmetry
rear surface = outflow
every other surface = velocity inlet(set velocity b.c. as "magnitude and direction")

that way you eliminate boundary layer due to ground.

hope this helps.

Note: I will be out till monday

good luck !

krishna June 18, 2010 07:23

I have tried it now, but i got the same error as you have mentioned,

i have used the same boundary conditions to get those results as I mentioned earlier

ok then meet you on Monday

thanks a lot, for your interest

enjoy your weekend

kdrbrk June 21, 2010 03:21

is your mesh almost same in two cases?
also be sure that parameters are same.
I do not know anything about Cham Phoenics, never used before.
maybe you can check its reference values.

note: solution methods also effect the result. be sure that you use same methods in both softwares.

krishna June 21, 2010 05:36

my mesh is different in both the cases
i think i got good results in cham phoenics , because i got drag coefficient as 0.36 (in general the drag coefficient should range from 0.2-0.3 for race cars)

but i am struggling in ansys, i got the forces on the car which is very high 66,54,179N approx, by using this value i have caluculated the drag coefficient. But the drag is very high.

In ansys we will graphs for residual, lift convergence and drag convergence

by using that drag convergence, is it possible to find the drag coefficient ?

thank you

kdrbrk June 21, 2010 06:39

did you scale the mesh after importing it to fluent?
now I realized that it may be the problem.
by default, fluent assumes the dimensions in in meters.
but cad softwares generally use milimeters.
so a 1 meter object is assumed as 1km in fluent.
that may be the reason for high values.

in fluent, you do not see the drag convergence, you see the drag coefficient !
coefficient is found by dividing the drag force by the reference values which are defined by you.
so if you define velocity, frontal area correctly, you will directly see the drag coeff.

jbritton June 21, 2010 07:49

Your mesh graduates from fine to course far too close to the body for me.

I would remesh drastically increasing the domain around the car and look at improving the mesh around the car too.

krishna June 21, 2010 16:16

i will check it once

thank you

jhthoh February 20, 2011 03:06

Hi, hope u all still active here. I m a beginner in this ANSYS Fluent and CFD. but i need to submit result in mid of march 2011. hope u all can help. My case is almost same as Krishna.

I doing my model in solidwork 2010,and i mesh it in ANSYS CFX mesh. then i import it to analyze in ANSYS 12.0 fluent. But i can't get any result. and i duno how to setup correctly for it.

as i read from above replies, how about the boundary condition for the ground?set it as a stationary wall?there are few reference values and i don't know how to setup them.

Hope you all can help.Thanks alot..

chirag September 29, 2011 15:29

check your Y+ value for the model which you have used and see whether its within range for that model.
the domain aft body(length L) must be around 4-4.5 L

If your com is running out of memory for generating mesh for longer domain then split the domain into 3 parts pre-body,body and aft body then combine them by using append case file in fluent. it really works. i have done it for making mesh for LES.

NOTE: care must be taken regarding interfaces they must have same position

rajendrrks May 2, 2013 13:29

plot cd v/s re
hello guys , me and my friends are doing non-newtonian fluid flow through orifice ...and at d result we have to analyse changes in cd with respect to reynold d moment wat problems we are facing is we dont know how to plot co-efficient of discharge against reynold's number...can anybody tell us how to plot cd v/s Re waiting for ur reply ..thanku ..:)

All times are GMT -4. The time now is 17:24.