CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   Forces and Torques in 2D (

recon9 February 11, 2011 19:19

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.


Josh February 12, 2011 06:21

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.

ghorrocks February 12, 2011 06:28

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.

ghorrocks February 12, 2011 06:30

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.

recon9 February 12, 2011 11:39

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,


Josh February 12, 2011 16:43

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).

ghorrocks February 13, 2011 06:56

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).

vmlxb6 February 15, 2011 17:36

@ 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

ghorrocks February 15, 2011 17:48

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.

recon9 February 16, 2011 17:55


Originally Posted by ghorrocks (Post 294937)
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.


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



ghorrocks February 16, 2011 20:40

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 10:12.