Forces and Torques in 2D
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 
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. 
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. 
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.

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 
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). 
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).

@ Glen and Brady
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 
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. 
Quote:
Could you explain what you mean by I am using the incorrect integration points? Thanks, Brady 
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.

All times are GMT 4. The time now is 05:41. 