CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   How to use ANSYS CFX to get the drag coefficient? (http://www.cfd-online.com/Forums/cfx/21640-how-use-ansys-cfx-get-drag-coefficient.html)

victorzcc September 24, 2005 09:46

How to use ANSYS CFX to get the drag coefficient?
 
I used CFX to simulation a bluff body. CFX offers viscous force and pressure force,but it doesn't the coefficient. How can I get the coefficient of the bluff body? Please the master-hands help me! Thanks a lot!

Rui September 24, 2005 14:09

Re: How to use ANSYS CFX to get the drag coefficie
 
Hi,

In CFX-Post you can obtain force_x()@Surface, force_y()@Surface and force_z()@Surface.

If the velocity is aligned with the x-axis, you could obtain the drag coefficient as Cd = force_x()@Surface / (0.5*Rho*U^2*A)


victor October 7, 2005 07:13

Re: How to use ANSYS CFX to get the drag coefficie
 
Many thanks for you reply! Can you sent the tutorial of drag coefficient?

krishna June 20, 2010 06:05

hi

to find drag coefficient, in the above formulae what is A,
is
A = length * width * 0.8

ghorrocks June 20, 2010 06:22

A is a representative area. For bluff bodies that is usually the frontal area by for airfoils they frequently use the planform area. Check you use the right area definition.

But this is very basic stuff which is dicussed in most introductory fluid mechanics books. Go to your library and look it up.

tomwalker January 23, 2012 12:04

error help
 
I know this is quite an old post but I don't know where else to turn..

when I try and do force calculations in CFX i get an error message that says

"Only geometries with surface data
are allowed for calculating force"

what does this mean and how do I generate surface data?

Thanks

Tom Walker

ghorrocks January 23, 2012 17:37

It means exactly what it says - you can only calculate force on surfaces. You are trying to calculate force on a point, line or volume body and that is not meaningful.

tomwalker January 23, 2012 20:50

thank you very much, I can't believe I was over thinking it like that!

bestniaz October 1, 2015 01:45

Quote:

Originally Posted by ghorrocks (Post 263738)
A is a representative area. For bluff bodies that is usually the frontal area by for airfoils they frequently use the planform area. Check you use the right area definition.

But this is very basic stuff which is dicussed in most introductory fluid mechanics books. Go to your library and look it up.

First of all thank you Sir for your quick help...
Sir, Kindly tell me how to monitor the value of Cd or Cl...
In case of Fluent, we can monitor it and later on, we can also plot the graph of Cd vs time or Cl vs time.... but
I am unable to monitor the Drag force or lift force on cylinder while using CFX...
Please help

Antanas October 1, 2015 02:44

Quote:

Originally Posted by bestniaz (Post 566039)
First of all thank you Sir for your quick help...
Sir, Kindly tell me how to monitor the value of Cd or Cl...
In case of Fluent, we can monitor it and later on, we can also plot the graph of Cd vs time or Cl vs time.... but
I am unable to monitor the Drag force or lift force on cylinder while using CFX...
Please help

What's the problem? You know formulas for Cd and Cl, so make corresponding CEL expressions for monitors.

bestniaz October 1, 2015 03:58

2 Attachment(s)
Quote:

Originally Posted by Antanas (Post 566042)
What's the problem? You know formulas for Cd and Cl, so make corresponding CEL expressions for monitors.

Thanks for your response and sorry as my question is silly but I am new in this area...so please help

I tried to make the expression as show in image... In CEL, I couldnt find the exact way to write formula..
In my case Vel=0.034m/s
density=1.185kg/m^3
Projected Area=0.02m^2
Drag forces are in x direction

ACtually Even in writing formula in EXPRESSION, it is not possible to separate Force in x and y component for Drag and lift coefficient respectively.

Antanas October 1, 2015 05:12

Quote:

Originally Posted by bestniaz (Post 566048)
Thanks for your response and sorry as my question is silly but I am new in this area...so please help

I tried to make the expression as show in image... In CEL, I couldnt find the exact way to write formula..
In my case Vel=0.034m/s
density=1.185kg/m^3
Projected Area=0.02m^2
Drag forces are in x direction

ACtually Even in writing formula in EXPRESSION, it is not possible to separate Force in x and y component for Drag and lift coefficient respectively.

1. To access force X-component use force_x
2. You should write values along with their dimensions in square brackets.
3. You may use variables names to access their values.

Your CEL for Cd may look like that:

Code:

2*force_x()@Cylinder / (Projected Area*massFlowAve(Density)@inlet
*(massFlowAve(Velocity)@inlet)^2)


bestniaz October 1, 2015 05:30

Quote:

Originally Posted by Antanas (Post 566057)
1. To access force X-component use force_x
2. You should write values along with their dimensions in square brackets.
3. You may use variables names to access their values.

Your CEL for Cd may look like that:

Code:

2*force_x()@Cylinder / (Projected Area*massFlowAve(Density)@inlet
*(massFlowAve(Velocity)@inlet)^2)


Thank you Sir,,,
I did it... Thank you again...
Actually, In post CFD, there is "force_x" term available while write the formula in EXPRESSION...but in CFX pre, there is only term "force ()@region..."...so I was bit confused how to insert "force_x" component... but now i simply write manually "_x" in available term " force ()@region"...


All times are GMT -4. The time now is 06:56.