Forces and Torques in 2D

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

 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: 9 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: 11 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: 14,318 Rep Power: 110 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 CFD-Post. 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: 14,318 Rep Power: 110 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: 9 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: 11 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 per-unit lift/drag, you can use forceNorm).

 February 13, 2011, 06:56 #7 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,318 Rep Power: 110 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: 9 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: 14,318 Rep Power: 110 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

Join Date: Jan 2011
Posts: 12
Rep Power: 9
Quote:
 Originally Posted by ghorrocks 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.
Glenn,

Could you explain what you mean by I am using the incorrect integration points?

Thanks,

 February 16, 2011, 20:40 #11 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,318 Rep Power: 110 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 Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post tsagaro FLUENT 7 June 23, 2017 15:45 G CARNIE CFX 2 May 16, 2002 13:46

All times are GMT -4. The time now is 11:59.