
[Sponsors] 
How to use ANSYS CFX to get the drag coefficient? 

LinkBack  Thread Tools  Search this Thread  Display Modes 
September 24, 2005, 09:46 
How to use ANSYS CFX to get the drag coefficient?

#1 
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 masterhands help me! Thanks a lot!


September 24, 2005, 14:09 
Re: How to use ANSYS CFX to get the drag coefficie

#2 
Guest
Posts: n/a

Hi,
In CFXPost you can obtain force_x()@Surface, force_y()@Surface and force_z()@Surface. If the velocity is aligned with the xaxis, 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 
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: 16 
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: 17,826
Rep Power: 144 
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: 17,826
Rep Power: 144 
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:
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 

October 1, 2015, 02:44 

#10  
Senior Member
Join Date: Feb 2011
Posts: 496
Rep Power: 18 
Quote:


October 1, 2015, 03:58 

#11  
Member
N B Khan
Join Date: Jan 2014
Posts: 39
Rep Power: 12 
Quote:
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. 

October 1, 2015, 05:12 

#12  
Senior Member
Join Date: Feb 2011
Posts: 496
Rep Power: 18 
Quote:
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:
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"... 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
drag coefficient in ansys fluent 12.0  krishna  FLUENT  19  April 12, 2018 00:49 
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 21:04 
ANSYS to acquire CFX  Fred  Siemens  0  February 18, 2003 21:03 