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

How to find lift coefficient by fluent?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 3, 2009, 12:39
Post How to find lift coefficient by fluent?
  #1
New Member
 
Pooya Kabiri
Join Date: Jun 2009
Posts: 1
Rep Power: 0
winterboy is on a distinguished road
Hi everybody,

I used fluent to model flow around NACA 0015.
I got cl & Cd for the same flow and airfoil from Xfoil and want to compare Xfoil results with fluent results.
I want to find Cl and Cd by fluent and my problem is the numbers which I have to enter for X,Y,Z of force vector.
do you know what should I put in there and how many iterations should I have at least to get acceptable answer for Cl and Cd?
Thank you in advance
winterboy is offline   Reply With Quote

Old   June 4, 2009, 02:23
Default
  #2
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,836
Rep Power: 29
-mAx- will become famous soon enough
enter 1 0 0 for Force Projection on x-axis
enter 0 1 0 for Force Projection on y-axis
enter 0 0 1 for Force Projection on z-axis
Now choose the right force you want to observe, and enable the plot option in monitor/force
Fluent will plot the accorded Coeff while iterating.
Your solution will be full converged if the the plotted coefficient remains constant while iterating.
You also have to set the right reference values for getting the right Coefficient
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   November 20, 2010, 09:21
Default
  #3
New Member
 
umar
Join Date: Nov 2010
Posts: 2
Rep Power: 0
3g_nitro is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
enter 1 0 0 for Force Projection on x-axis
enter 0 1 0 for Force Projection on y-axis
enter 0 0 1 for Force Projection on z-axis
Now choose the right force you want to observe, and enable the plot option in monitor/force
Fluent will plot the accorded Coeff while iterating.
Your solution will be full converged if the the plotted coefficient remains constant while iterating.
You also have to set the right reference values for getting the right Coefficient
when you do that it shows the values for the coefficient of pressure, so how do you work out CLift ??
3g_nitro is offline   Reply With Quote

Old   November 25, 2010, 08:12
Default
  #4
Member
 
kdrbrk's Avatar
 
Burak
Join Date: May 2009
Posts: 90
Rep Power: 7
kdrbrk is on a distinguished road
before iterations, set "monitors-lift" and define the lift vector (ex: y=1)
and select your airfoil (must be a wall) for which the lift will be monitored.
also dont forget to set correct ref. values.

than begin iteration and it will show you "cl" in each step by default.
kdrbrk is offline   Reply With Quote

Old   January 29, 2011, 14:47
Default
  #5
New Member
 
Ruben Ruiz
Join Date: Sep 2010
Posts: 20
Rep Power: 6
RGRUIZ is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
enter 1 0 0 for Force Projection on x-axis
enter 0 1 0 for Force Projection on y-axis
enter 0 0 1 for Force Projection on z-axis
Now choose the right force you want to observe, and enable the plot option in monitor/force
Fluent will plot the accorded Coeff while iterating.
Your solution will be full converged if the the plotted coefficient remains constant while iterating.
You also have to set the right reference values for getting the right Coefficient
Hi max, one question..I am modelling a 2D airfoil, the right references values should be:

Area: What value should i use?? The edge length of the airfoil multiply by the depth???

Depth: is this the length of the wing??
RGRUIZ is offline   Reply With Quote

Old   January 31, 2011, 01:22
Default
  #6
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,836
Rep Power: 29
-mAx- will become famous soon enough
Check tutorial 3: Modelling external compressible Flow.
The references values you give are independant from your solution.
Compute your model, and then you can apply your refences values.
Even if you gave wrong Ref. Values, you can correct them without re-iterating.
They are just factors.
Important are pressure and viscous forces computed during iterations
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   February 2, 2011, 14:21
Default
  #7
Member
 
John
Join Date: Jan 2011
Posts: 58
Rep Power: 5
John222 is on a distinguished road
I have the same problem and your answer indeed helped me a lot. I have monitored the Cl and Cd and while iterating I found out that my coefficients are not constant in the plot what I am supposed to do in this situation. Please explain in details I am a beginner.

Check pictures attached.

R.I.P for your dear friend Herve.

Thanks
Attached Images
File Type: jpg drag.jpg (15.2 KB, 288 views)
John222 is offline   Reply With Quote

Old   February 2, 2011, 17:41
Default
  #8
New Member
 
Ruben Ruiz
Join Date: Sep 2010
Posts: 20
Rep Power: 6
RGRUIZ is on a distinguished road
Hi max...i figure it out that if i change the depth on reference values i get differents cl y cd results..why is that if the equation is: Cl=F/(0.5*density*velocity*velocity*Area)..

Another question what if the angle of attack is different than zero, which velocity value on farfield should be taken to calculate the lift coefficient???
RGRUIZ is offline   Reply With Quote

Old   February 3, 2011, 01:10
Default
  #9
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,836
Rep Power: 29
-mAx- will become famous soon enough
Quote:
Originally Posted by John222 View Post
I found out that my coefficients are not constant in the plot what I am supposed to do in this situation. Please explain in details I am a beginner.
Thanks
You are iterating. Your computation doesn't converged yet, and your coefficient (monitor) will oscillate till it reaches its converged value.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   February 3, 2011, 01:24
Default
  #10
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,836
Rep Power: 29
-mAx- will become famous soon enough
Quote:
Originally Posted by RGRUIZ View Post
Hi max...i figure it out that if i change the depth on reference values i get differents cl y cd results..why is that if the equation is: Cl=F/(0.5*density*velocity*velocity*Area)..

Another question what if the angle of attack is different than zero, which velocity value on farfield should be taken to calculate the lift coefficient???
*Check Online Help >>> "For 2D problems, an additional quantity, Depth, can also be defined. "

*I would say you can take the cosine of your angle as factor. But since the angles are small, it won't affect your coeff (needs to be confirmed/invalidate from aero experts).
Check tutorial 3 and compare velocity value given in Ref. with Mach Number
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   February 3, 2011, 08:32
Default
  #11
Member
 
John
Join Date: Jan 2011
Posts: 58
Rep Power: 5
John222 is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
You are iterating. Your computation doesn't converged yet, and your coefficient (monitor) will oscillate till it reaches its converged value.
OK I did 500 iterations and I found that my line is stable if you can see in the picture attached.

Is my solution converged, and how to compare 1st order with 2nd I am running now in 2nd order (pressure and momentum).

I see no difference really is the difference from the drag and lift forces or the plot of the iterations to drag.

How to do a GIS, I probably done it already?



R.I.P to your friend again
Attached Images
File Type: jpg Cd NEW.jpg (16.0 KB, 172 views)
John222 is offline   Reply With Quote

Old   February 3, 2011, 08:44
Default
  #12
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,836
Rep Power: 29
-mAx- will become famous soon enough
you need also to check your residuals (plot/residuals...)
If all the residuals fall down, let iterate and check if your monitoring still stay constant.
Regarding your comparison between first and second order: write your force monitoring on a file (one file for 1st order, and one for second).
Write also case and data before switching to second order.

What is GIS?
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   February 3, 2011, 08:47
Default
  #13
Member
 
John
Join Date: Jan 2011
Posts: 58
Rep Power: 5
John222 is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
you need also to check your residuals (plot/residuals...)
If all the residuals fall down, let iterate and check if your monitoring still stay constant.
Regarding your comparison between first and second order: write your force monitoring on a file (one file for 1st order, and one for second).
Write also case and data before switching to second order.

What is GIS?
- What do you mean by all residuals fall down, I know how to get the residuals plt but how to know if they are down?

- grid independence study?
John222 is offline   Reply With Quote

Old   February 3, 2011, 08:54
Default
  #14
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,836
Rep Power: 29
-mAx- will become famous soon enough
*Residuals charts decreasing (>> converging)
*Grid independant study: then you need to recompute your stuff on a refined grid.
You reached the solution if your solution isn't influenced by the grid refinement.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   February 3, 2011, 16:24
Default
  #15
Member
 
John
Join Date: Jan 2011
Posts: 58
Rep Power: 5
John222 is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
*Residuals charts decreasing (>> converging)
*Grid independent study: then you need to recompute your stuff on a refined grid.
You reached the solution if your solution isn't influenced by the grid refinement.
- does my graphics & animations plots of static pressure changes when changing from 1st order to 2nd order discretization, and what actually changes in 2nd order discretization.

- and I still didn't get the full idea of grid independent study, I have tried to refine my grid as best as I could. Do I have to do another very well done mesh and compare both answers or what?

- Please check your email.


Thanks dude.
John222 is offline   Reply With Quote

Old   February 3, 2011, 16:48
Default
  #16
Member
 
John
Join Date: Jan 2011
Posts: 58
Rep Power: 5
John222 is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
*Residuals charts decreasing (>> converging)
*Grid independant study: then you need to recompute your stuff on a refined grid.
You reached the solution if your solution isn't influenced by the grid refinement.

Here is my mesh. Is it possible to do a 2nd order with it and is it converged enough.
Attached Images
File Type: jpg mesh.jpg (91.6 KB, 177 views)
John222 is offline   Reply With Quote

Old   February 3, 2011, 22:36
Default
  #17
New Member
 
Ruben Ruiz
Join Date: Sep 2010
Posts: 20
Rep Power: 6
RGRUIZ is on a distinguished road
-John..

The grid independent study is like this:

You have to have different mesh faces: example 10.000-20.000-30.000 and fix a parameter you want to study like Cf, Cl, Cd if any this values change less than 5% from mesh 10.000 and 30.000 means that it won´t be any different if you do a mesh with 40.000 faces because you are going to get very similar results, so you considerer that the 30.000 faces is okay for what you are doing.

hope it help you
RGRUIZ is offline   Reply With Quote

Old   February 4, 2011, 01:22
Default
  #18
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,836
Rep Power: 29
-mAx- will become famous soon enough
Quote:
Originally Posted by John222 View Post
- does my graphics & animations plots of static pressure changes when changing from 1st order to 2nd order discretization, and what actually changes in 2nd order discretization.

- and I still didn't get the full idea of grid independent study, I have tried to refine my grid as best as I could. Do I have to do another very well done mesh and compare both answers or what?
-read case for with 1st order>> initialize>> compute and write your coeff in a file. When converged, write case & data.

read case & data from previous 1st order solution>> switch to 2nd order >> Initialize or don't(if you start from converged 1st order solution you will get faster convergence) >> compute and write your coeff in a different file.
Load your 2 graphs in excel, or whatever... and compare


- You don't need to generate a very fine grid: follow what RGRUIZ said
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   February 4, 2011, 06:42
Default
  #19
Member
 
John
Join Date: Jan 2011
Posts: 58
Rep Power: 5
John222 is on a distinguished road
Quote:
Originally Posted by RGRUIZ View Post
-John..

The grid independent study is like this:

You have to have different mesh faces: example 10.000-20.000-30.000 and fix a parameter you want to study like Cf, Cl, Cd if any this values change less than 5% from mesh 10.000 and 30.000 means that it won´t be any different if you do a mesh with 40.000 faces because you are going to get very similar results, so you considerer that the 30.000 faces is okay for what you are doing.

hope it help you
Sorry but when you say different mesh faces do you mean the Sizing (maximum face size) I am using (car.x_t) geomtry file from Ansys.
and in the max face size by default its 1.78m.
can someone tell me the full steps of how to change mesh faces 10.000-20.000-30.000.
John222 is offline   Reply With Quote

Old   February 4, 2011, 06:43
Default
  #20
Member
 
John
Join Date: Jan 2011
Posts: 58
Rep Power: 5
John222 is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
-read case for with 1st order>> initialize>> compute and write your coeff in a file. When converged, write case & data.

read case & data from previous 1st order solution>> switch to 2nd order >> Initialize or don't(if you start from converged 1st order solution you will get faster convergence) >> compute and write your coeff in a different file.
Load your 2 graphs in excel, or whatever... and compare


- You don't need to generate a very fine grid: follow what RGRUIZ said

Very helpful understood you, and testing now...
John222 is offline   Reply With Quote

Reply

Tags
fluent, lift coefficient

Thread Tools
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 On
Pingbacks are On
Refbacks are On


LinkBacks (?)
LinkBack to this Thread: http://www.cfd-online.com/Forums/fluent/65095-how-find-lift-coefficient-fluent.html
Posted By For Type Date
Drag coefficient simulation in ANSYS 12.0 Fluent - Forum - F1technical.net This thread Refback November 21, 2013 11:39

Similar Threads
Thread Thread Starter Forum Replies Last Post
Problem with lift force coefficient summer FLUENT 0 May 7, 2008 10:35
Lift force coefficient for 2-phase flow Summer FLUENT 0 April 29, 2008 17:58
negative lift coefficient? please help! fumie FLUENT 1 October 9, 2007 03:52
Zero Coefficient of Lift Problem MH FLUENT 0 February 25, 2007 11:48
lift coefficient in vof kiran FLUENT 0 August 8, 2005 05:30


All times are GMT -4. The time now is 08:28.