CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Force Function Calculator Ansys CFD Post (http://www.cfd-online.com/Forums/cfx/127104-force-function-calculator-ansys-cfd-post.html)

sharadram1989 December 3, 2013 16:15

Force Function Calculator Ansys CFD Post
 
Hi guys,

My question is very basic.

I read through the Ansys 14.5 manuals but it doesn't seem to answer my question so posting on here!

I have a lorry model sat in a wind tunnel setup (Drawn on XY plane and extruded through Z axis).

Now when I need to find the Drag Force on this lorry, I click on Function Calculator in CFD post and select the Z component for direction and it displays a force.

My question is How does Ansys calculate this force? Does it use the generic Drag Equation = 0.5*rho*Usquared*Area?

And if so what Area is it using? Is it all of the surface area of the lorry or just the cross sectional frontal area?

Thanks in Advance!

ghorrocks December 3, 2013 18:03

No, it is not using drag=0.5*rho*A*U^2 :)

It is integrating the pressure and wall shear over the surface of the body.

sharadram1989 December 3, 2013 18:21

Ah I'm guessing that equation originally comes from Navier stokes equations then. Will need to read into that stuff.

Forgot to mention that I have applied an inflation layer on the lorry. I calculated the boundary layer thickness and applied it as the inflation layer.

But I'm guessing that with or without these layers that is how Ansys will always solve it?

Thanks for the help!! :D

ghorrocks December 3, 2013 18:31

Regardless of how you have meshed it it integrates over the surface. The meshing will "just" determine the accuracy of the simulation, not the approach.

sharadram1989 December 3, 2013 18:35

Thanks ever so much. Has made it clearer now!

kiyoshi9 January 30, 2014 04:10

I want find drag force and force of water axial turbine
 
1 Attachment(s)
I want know value drag force and force at water turbine blade
The water axial turbine have eigth blade.
I use Calculate Function in CFD Post (Ansys 13)
result force in Program is much greater than the experimental result.

Thank a lot,
Natthawut

ghorrocks January 30, 2014 04:51

FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

Spinassien August 14, 2014 03:44

Hello World,
if i calculate the force in any direction, is the answer the sum of pressure force and wall shear or only one of the components?

Spinassien August 14, 2014 03:50

i thin k i found the Answer by myself:
The force on a boundary is calculated using momentum flow data from the results file, if it is available. The result can be positive or negative, indicating the direction of the force. For non-boundary locators, an approximate force is always calculated.
CFD-Post calculates the approximate force as follows:
  • If the locator is a wall boundary, the force is equal to the pressure force.
  • For all other locators, the force is equal to the pressure force plus the mass flow force (due to the advection of momentum).
  • In all cases, if wall shear data exists in the results file, the viscous force is added to the calculated force.

crusen mind April 19, 2016 11:00

so if i am getting negative value for drag instead of getting positive value. it means that my wing has stalled.

ghorrocks April 19, 2016 18:33

A stalled wing should produce lots of drag.

Negative drag means your simulation is inaccurate. There is a small possibly you are doing a strange case when the really drag is negative, such as accelerating airfoils, rapid pitch changes or something like that. But then the negative drag is just a temporary thing.

crusen mind April 20, 2016 01:37

well i am getting positive value for my lower angle of attack and at higher angle of attack say 9 deg i am getting negative drag value.

ghorrocks April 20, 2016 03:34

So my previous post went on to say "Negative drag means your simulation is inaccurate". So you need to do the normal checks and sensitivity analyses to get an accurate result.

Please post an image of what you are modelling, your output file and how you are working out the drag.

crusen mind April 20, 2016 04:35

http://www.cfd-online.com/Forums/mem...t-pressure.jpghttp://www.cfd-online.com/Forums/mem...ty-vectors.jpghttp://www.cfd-online.com/Forums/mem...780t-dmian.jpghttp://www.cfd-online.com/Forums/mem...re779t-cat.jpghttp://www.cfd-online.com/Forums/mem...-ansa-mesh.jpg

crusen mind April 20, 2016 05:51

i set my convergence criteria ie 10e-5.

ghorrocks April 20, 2016 06:00

Your images are too small to be useful. Please attach the full resolution images. Also:
* Describe what the images are showing
* Attach your output file.

crusen mind April 20, 2016 07:32

3 Attachment(s)
  1. ansa mesh file shows how the volume is created around the model.
  2. cat shows 3 view of the model.
  3. velocity vectors shows flow around the model.
I am trying to show what my model looks like, and how it is meshed

crusen mind April 22, 2016 14:21

now I realized that my meshing is wrong that i have to change it. Any ideas how to do it and to do stability analysis, verification and validation. I dont people to guide me that's why i am asking lot of doubt. so please dont think that i am troubling u guys. thanks a ton for help so far and i hope u provide it continously.

ghorrocks April 23, 2016 07:16

Assuming your foil is moving at a reasonable Re number (1e5 or higher), then your mesh is too coarse and you have no inflation layers. You will need inflation layer for good boundary layer resolution and I am sure a mesh size sensitivity study will show your mesh is too coarse.

As for stability analysis, verification and validation - these are complex topics and I cannot describe them in a forum post. Do some background reading on the topic from CFD textbooks (or even wikipedia is a good place to start) and then ask any questions you might have on the forum.


All times are GMT -4. The time now is 22:04.