# How to use ANSYS CFX to get the drag coefficient?

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

 September 24, 2005, 09:46 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!

 September 24, 2005, 14:09 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)

 October 7, 2005, 07:13 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?

 June 20, 2010, 06:05 #4 New Member   Join Date: May 2010 Posts: 17 Rep Power: 15 hi to find drag coefficient, in the above formulae what is A, is A = length * width * 0.8

 June 20, 2010, 06:22 #5 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,689 Rep Power: 143 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.

 January 23, 2012, 11:04 error help #6 New Member   Tom Walker Join Date: Jan 2012 Posts: 10 Rep Power: 14 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

 January 23, 2012, 16:37 #7 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,689 Rep Power: 143 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.

 January 23, 2012, 19:50 #8 New Member   Tom Walker Join Date: Jan 2012 Posts: 10 Rep Power: 14 thank you very much, I can't believe I was over thinking it like that!

October 1, 2015, 01:45
#9
Member

N B Khan
Join Date: Jan 2014
Posts: 39
Rep Power: 12
Quote:
 Originally Posted by ghorrocks 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...

October 1, 2015, 02:44
#10
Senior Member

Join Date: Feb 2011
Posts: 496
Rep Power: 18
Quote:
 Originally Posted by bestniaz 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.

October 1, 2015, 03:58
#11
Member

N B Khan
Join Date: Jan 2014
Posts: 39
Rep Power: 12
Quote:
 Originally Posted by Antanas What's the problem? You know formulas for Cd and Cl, so make corresponding CEL expressions for monitors.

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
 CFD.jpg (86.4 KB, 238 views) cfd2.png (16.2 KB, 215 views)

October 1, 2015, 05:12
#12
Senior Member

Join Date: Feb 2011
Posts: 496
Rep Power: 18
Quote:
 Originally Posted by bestniaz 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)```

October 1, 2015, 05:30
#13
Member

N B Khan
Join Date: Jan 2014
Posts: 39
Rep Power: 12
Quote:
 Originally Posted by Antanas 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"...