
[Sponsors] 
February 11, 2011, 19:19 
Forces and Torques in 2D

#1 
New Member
Brady
Join Date: Jan 2011
Location: Calgary, Alberta, Canada
Posts: 12
Rep Power: 7 
I am trying to determine the lift, drag and torques on an inclined plate in a flow. When I run a 3D simulation I can simply go to the Forces and Torques Report and they are all there in every direction for my plate. However, when I do a 2D analysis (Control volume is one element wide with symmetry on both sides) the Forces and Torques Report disappears.
Is there a way to get CFX to show forces and torques on a body when I run the simulation in this way? Is it the symmetry planes that don't allow this report to be calculated? I want to compare what CFX calculates to some literature values. Currently, I am using a polyline to get a plot of the pressure across the surface of the plate and then integrating via the trapezoid rule to calculate the Force per unit Depth. If I were to convert this into lift and drag all values would cancel and give me the formulas I am testing. Thanks for your help. Brady 

February 12, 2011, 06:21 

#2 
Senior Member
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 10 
CFX is funny when it comes to 2D calculations. I'm studying 2D airfoils, but since CFX cannot perform 2D simulations, it automatically extrudes my 2D airfoil mesh to 3D and gives it a seemingly arbitrary span of 0.4 m.
Keeping that in mind, I now have to adjust the coefficient of lift and drag values by considering that the "span" is 0.4 m. 

February 12, 2011, 06:28 

#3 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,709
Rep Power: 98 
I was not aware the forces and torques disappear in a 2D (1 element thick) model. Sounds strange. Are you sure you have set it up correctly?
Try calculating the forces in CFDPost. Hopefully that can get them. Your current calculation is not using the proper integration points of the simulation and is not including viscous forces so is an approximation. Hopefully you are aware of that. 

February 12, 2011, 06:30 

#4 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,709
Rep Power: 98 
Josh  the recommended thickness for 2D models is the element edge length of the smallest element. This makes for more robust numerics. You can set the extrusion length in the import options I think.


February 12, 2011, 11:39 

#5 
New Member
Brady
Join Date: Jan 2011
Location: Calgary, Alberta, Canada
Posts: 12
Rep Power: 7 
Thanks for the replies everyone.
Glen, yes I was aware of the viscous forces but they slipped my mind (no pun intended) when I wrote this thread. How to I calculate the forces using CFD Post? Sorry, it is probably an elementary question but I am still quite new to the software. Thanks again, Brady 

February 12, 2011, 16:43 

#6 
Senior Member
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 10 
Glenn 
Thanks for the input. I had no idea. I was encountering problems when importing ICEM 3D meshes made for CFX, so I just exported them from ICEM as 2D Fluent meshes and Pre would automatically extrude them (though 0.4 m is obviously much larger than the minimum element edge length). Will changing the depth of the "2D" mesh actually save simulation time or make the simulation more robust? Brady  There is a function calculator in Post where you can select Force X, Force Y, etc. (or, for perunit lift/drag, you can use forceNorm). 

February 13, 2011, 06:56 

#7 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,709
Rep Power: 98 
Josh: It *might* improve numerical stability. If it is not a problem then it will make no difference, but if it is then using the correct extrusion depth will make your simulation converge faster (or converge at all).


February 15, 2011, 17:36 
@ Glen and Brady

#8 
Senior Member
Ugly Kid Joe
Join Date: Aug 2010
Posts: 193
Rep Power: 8 
Is there a way to include/exclude viscous force ??????
When we use force_x or y, doesn't it automatically consider Pressure force and viscous force ????????? I am trying to simulate a 1 way FSI of a flow over a cylinder. For the vertical motion of the cylinder I am using Force_y in my CEL expression. My displacements are way too low. Probably this might be one of the reasons ???? Thanks guys 

February 15, 2011, 17:48 

#9 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,709
Rep Power: 98 
force_x/y/z is the total force, pressure and viscous effects are included.
If you just want the pressure force then integrate the pressue over the surface. 

February 16, 2011, 17:55 

#10  
New Member
Brady
Join Date: Jan 2011
Location: Calgary, Alberta, Canada
Posts: 12
Rep Power: 7 
Quote:
Could you explain what you mean by I am using the incorrect integration points? Thanks, Brady 

February 16, 2011, 20:40 

#11 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,709
Rep Power: 98 
Read the documentation about the numerical method. Control volume variables are stored at the nodes, but the calculations are done at the integration points as per the finite element method. Thus the most accurate calculations are done using the integration points.


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
How to calculate pressure forces using custom field functions?  tsagaro  FLUENT  6  April 13, 2011 04:03 
FORCES ON AEROFOILS IN CFX4.4  G CARNIE  CFX  2  May 16, 2002 13:46 