CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

How to obtain total lift of 3D wing (Fluent)

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 13, 2015, 19:25
Default How to obtain total lift of 3D wing (Fluent)
  #1
New Member
 
United Kindom
Join Date: Jun 2015
Posts: 1
Rep Power: 0
Raco is on a distinguished road
Hello,

I have series of questions regarding lift and lift coefficient. If a 3D wing simulation if set up (for a specific velocity and density), I can then use the monitor lift coefficient CL to calculate the total lift using the equation L=0.5*rho*V^2*A*CL? if so...could I use the same CL for a different velocity and density or just for the values used in the simulation?

Also, is there a direct way to obtain total lift directly from fluent?

I know that these might be pretty basic questions but I'm just having trouble understanding this.

Many thanks for your help
Raco is offline   Reply With Quote

Old   June 18, 2015, 10:37
Default
  #2
Senior Member
 
scipy's Avatar
 
Alex Pasic
Join Date: Aug 2011
Location: Croatia
Posts: 199
Rep Power: 12
scipy is on a distinguished road
Send a message via Skype™ to scipy
C_L in Fluent is calculated base on the Reference values you've entered in Fluent (Setup -> Reference Values).

For a vehicle, C_D and C_L are calculated based on the frontal area of the vehicle - because people agreed that it would be so.

I think the reference dimension for a wing is wing area (surface area when you look at your wing from above/below). So, enter that under Area in m^2 in Reference values and the C_D & C_L that you get will be correct for your wing (there's no need to calculate by hand).

In order to get the exact forces you should make a Force Report (Results -> Reports -> Forces -> pick a direction vector and a wall/surface you want to calculate the force for (say surfaces of your wing, both lower and upper, end plates etc.. everything that's a part of the wing) -> click Print...

There you will see how viscous forces and pressure forces are divided and the overall force (consisting of viscous and pressure forces) and you can calculate the C_D and C_L by hand just to check. It will be also written in the force report on the right under Coefficients.

Direction vector is pretty obvious.. longitudinal one for drag force (all others 0) and vertical one for lift/downforce (all others 0).
scipy is offline   Reply With Quote

Old   June 18, 2015, 11:22
Default
  #3
Member
 
Radwanma
Join Date: Oct 2014
Posts: 30
Rep Power: 8
Radwanma is on a distinguished road
Hi all,

I have made the following full geometry for a rotor and a surface in ICEM but when read it in mesh just the rotor appears !!! How can I solve this problem , please?
Thanks,
Attached Images
File Type: jpg Untitled2.jpg (30.8 KB, 34 views)
File Type: jpg Untitled1.jpg (42.1 KB, 36 views)
Radwanma is offline   Reply With Quote

Old   November 4, 2016, 01:43
Default
  #4
New Member
 
jiyou
Join Date: Sep 2016
Posts: 5
Rep Power: 6
Freestream is on a distinguished road
Quote:
Originally Posted by scipy View Post
C_L in Fluent is calculated base on the Reference values you've entered in Fluent (Setup -> Reference Values).

For a vehicle, C_D and C_L are calculated based on the frontal area of the vehicle - because people agreed that it would be so.

I think the reference dimension for a wing is wing area (surface area when you look at your wing from above/below). So, enter that under Area in m^2 in Reference values and the C_D & C_L that you get will be correct for your wing (there's no need to calculate by hand).

In order to get the exact forces you should make a Force Report (Results -> Reports -> Forces -> pick a direction vector and a wall/surface you want to calculate the force for (say surfaces of your wing, both lower and upper, end plates etc.. everything that's a part of the wing) -> click Print...

There you will see how viscous forces and pressure forces are divided and the overall force (consisting of viscous and pressure forces) and you can calculate the C_D and C_L by hand just to check. It will be also written in the force report on the right under Coefficients.

Direction vector is pretty obvious.. longitudinal one for drag force (all others 0) and vertical one for lift/downforce (all others 0).

Every good note by Scipy. it is apparent that drag and lift are evaluated at parallel and perpendicular to free stream velocity.

Can i also ask if the lift force presented by FLUENT is presented in the aerodynamic center (often the quater chord point) or it actually doesn't matter??
Freestream is offline   Reply With Quote

Old   November 4, 2016, 08:17
Default
  #5
Senior Member
 
scipy's Avatar
 
Alex Pasic
Join Date: Aug 2011
Location: Croatia
Posts: 199
Rep Power: 12
scipy is on a distinguished road
Send a message via Skype™ to scipy
Quote:
Originally Posted by Freestream View Post
Every good note by Scipy. it is apparent that drag and lift are evaluated at parallel and perpendicular to free stream velocity.

Can i also ask if the lift force presented by FLUENT is presented in the aerodynamic center (often the quater chord point) or it actually doesn't matter??
You can report a force in any vector direction that you want (doesn't have to be parallel/perpendicular to free stream direction of flow). You just specify the sin/cos components of a unit vector.

Force is just an integrated value of pressure & viscous forces over all the surfaces of the body. Pressure forces do act at the center of pressure location (you can even report that in FLUENT), but viscous forces do not (so a moment reported around a CoP location will be 0 for pressure forces but it'll have some small value due to viscous forces).

Finding the location where forces are acting can be done either via CoP or some simple statics/mechanics using known forces and a moment around any point of your choosing.
__________________
If you're in need of some free quality CFD video tutorials - check out SiriusCFD @ YouTube
scipy is offline   Reply With Quote

Old   November 27, 2019, 14:59
Default
  #6
Member
 
Join Date: Aug 2018
Posts: 63
Rep Power: 4
esha is on a distinguished road
Quote:
Originally Posted by scipy View Post
C_L in Fluent is calculated base on the Reference values you've entered in Fluent (Setup -> Reference Values).

For a vehicle, C_D and C_L are calculated based on the frontal area of the vehicle - because people agreed that it would be so.

I think the reference dimension for a wing is wing area (surface area when you look at your wing from above/below). So, enter that under Area in m^2 in Reference values and the C_D & C_L that you get will be correct for your wing (there's no need to calculate by hand).

In order to get the exact forces you should make a Force Report (Results -> Reports -> Forces -> pick a direction vector and a wall/surface you want to calculate the force for (say surfaces of your wing, both lower and upper, end plates etc.. everything that's a part of the wing) -> click Print...

There you will see how viscous forces and pressure forces are divided and the overall force (consisting of viscous and pressure forces) and you can calculate the C_D and C_L by hand just to check. It will be also written in the force report on the right under Coefficients.

Direction vector is pretty obvious.. longitudinal one for drag force (all others 0) and vertical one for lift/downforce (all others 0).
Hi, I also have this basic question as I am doing 3D simulation first time, also using Fluent . I have used area value in reference value and using force vector for Cd x=1, y=0 z=0 and for Cl x=0, y=1 and z=0. But in a video why is used values for z alongwith other? can you please explain?
thank you!
esha is offline   Reply With Quote

Old   November 27, 2019, 16:35
Default
  #7
Senior Member
 
scipy's Avatar
 
Alex Pasic
Join Date: Aug 2011
Location: Croatia
Posts: 199
Rep Power: 12
scipy is on a distinguished road
Send a message via Skype™ to scipy
Quote:
Originally Posted by esha View Post
Hi, I also have this basic question as I am doing 3D simulation first time, also using Fluent . I have used area value in reference value and using force vector for Cd x=1, y=0 z=0 and for Cl x=0, y=1 and z=0. But in a video why is used values for z alongwith other? can you please explain?
thank you!
I don't quite understand what you meant to say, but vector directions depend on your model orientation inside the coordinate system and/or flow direction in the same system. Sometimes you don't need the Z value at all (if the Z axis comes out of the symmetry plane for example). If this wasn't your question, maybe try to formulate it slightly better.
__________________
If you're in need of some free quality CFD video tutorials - check out SiriusCFD @ YouTube
scipy is offline   Reply With Quote

Reply

Tags
3d wing, lift, lift coefficient, wing

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Willing to Pay/Freelancer Required/Mesh Generation for Wing Lift & Drag woodmark75 CFD Freelancers 15 April 5, 2015 08:02
Lift Values Way Off For Wing in Solidworks swkfmf FloEFD, FloWorks & FloTHERM 0 September 25, 2014 23:03
problem in using parallel process in fluent 14 aydinkabir88 FLUENT 1 July 10, 2013 03:00
initial condition effect on wing lift linyx FLUENT 24 June 9, 2013 09:35
Error in run Batch file saba1366 CFX 4 February 10, 2013 02:15


All times are GMT -4. The time now is 18:23.