CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

How to use ANSYS CFX to get the drag coefficient?

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By Antanas

Reply
 
LinkBack Thread Tools Display Modes
Old   September 24, 2005, 09:46
Default How to use ANSYS CFX to get the drag coefficient?
  #1
victorzcc
Guest
 
Posts: n/a
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!
  Reply With Quote

Old   September 24, 2005, 14:09
Default Re: How to use ANSYS CFX to get the drag coefficie
  #2
Rui
Guest
 
Posts: n/a
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)

  Reply With Quote

Old   October 7, 2005, 07:13
Default Re: How to use ANSYS CFX to get the drag coefficie
  #3
victor
Guest
 
Posts: n/a
Many thanks for you reply! Can you sent the tutorial of drag coefficient?
  Reply With Quote

Old   June 20, 2010, 06:05
Default
  #4
New Member
 
Join Date: May 2010
Posts: 17
Rep Power: 8
krishna is on a distinguished road
hi

to find drag coefficient, in the above formulae what is A,
is
A = length * width * 0.8
krishna is offline   Reply With Quote

Old   June 20, 2010, 06:22
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,405
Rep Power: 97
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   January 23, 2012, 12:04
Default error help
  #6
New Member
 
Tom Walker
Join Date: Jan 2012
Posts: 10
Rep Power: 6
tomwalker is on a distinguished road
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
tomwalker is offline   Reply With Quote

Old   January 23, 2012, 17:37
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,405
Rep Power: 97
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   January 23, 2012, 20:50
Default
  #8
New Member
 
Tom Walker
Join Date: Jan 2012
Posts: 10
Rep Power: 6
tomwalker is on a distinguished road
thank you very much, I can't believe I was over thinking it like that!
tomwalker is offline   Reply With Quote

Old   October 1, 2015, 01:45
Default
  #9
Member
 
N B Khan
Join Date: Jan 2014
Posts: 36
Rep Power: 4
bestniaz is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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
bestniaz is offline   Reply With Quote

Old   October 1, 2015, 02:44
Default
  #10
Senior Member
 
Join Date: Feb 2011
Posts: 283
Rep Power: 9
Antanas is on a distinguished road
Quote:
Originally Posted by bestniaz View Post
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.
Antanas is offline   Reply With Quote

Old   October 1, 2015, 03:58
Default
  #11
Member
 
N B Khan
Join Date: Jan 2014
Posts: 36
Rep Power: 4
bestniaz is on a distinguished road
Quote:
Originally Posted by Antanas View Post
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.
Attached Images
File Type: jpg CFD.jpg (86.4 KB, 57 views)
File Type: png cfd2.png (16.2 KB, 48 views)
bestniaz is offline   Reply With Quote

Old   October 1, 2015, 05:12
Default
  #12
Senior Member
 
Join Date: Feb 2011
Posts: 283
Rep Power: 9
Antanas is on a distinguished road
Quote:
Originally Posted by bestniaz View Post
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 likes this.
Antanas is offline   Reply With Quote

Old   October 1, 2015, 05:30
Default
  #13
Member
 
N B Khan
Join Date: Jan 2014
Posts: 36
Rep Power: 4
bestniaz is on a distinguished road
Quote:
Originally Posted by Antanas View Post
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"...
bestniaz is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
drag coefficient in ansys fluent 12.0 krishna FLUENT 18 May 2, 2013 13:29
Incorrect Drag and Drag Coefficient for flow over a cylinder ozzythewise Main CFD Forum 8 June 13, 2012 06:24
FSI using CFX and ANSYS Bi Chang CFX 2 May 10, 2005 04:47
ANSYS to acquire CFX Fred FLUENT 0 February 18, 2003 22:04
ANSYS to acquire CFX Fred CD-adapco 0 February 18, 2003 22:03


All times are GMT -4. The time now is 19:39.