CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   How to find lift coefficient by fluent? (http://www.cfd-online.com/Forums/fluent/65095-how-find-lift-coefficient-fluent.html)

winterboy June 3, 2009 12:39

How to find lift coefficient by fluent?
 
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

-mAx- June 4, 2009 02:23

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

3g_nitro November 20, 2010 10:21

Quote:

Originally Posted by -mAx- (Post 218207)
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 ??

kdrbrk November 25, 2010 09:12

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.

RGRUIZ January 29, 2011 15:47

Quote:

Originally Posted by -mAx- (Post 218207)
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??

-mAx- January 31, 2011 02:22

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

John222 February 2, 2011 15:21

1 Attachment(s)
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

RGRUIZ February 2, 2011 18:41

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???

-mAx- February 3, 2011 02:10

Quote:

Originally Posted by John222 (Post 293328)
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.

-mAx- February 3, 2011 02:24

Quote:

Originally Posted by RGRUIZ (Post 293357)
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

John222 February 3, 2011 09:32

1 Attachment(s)
Quote:

Originally Posted by -mAx- (Post 293402)
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 :(

-mAx- February 3, 2011 09:44

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?

John222 February 3, 2011 09:47

Quote:

Originally Posted by -mAx- (Post 293462)
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?

-mAx- February 3, 2011 09:54

*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.

John222 February 3, 2011 17:24

Quote:

Originally Posted by -mAx- (Post 293464)
*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 February 3, 2011 17:48

1 Attachment(s)
Quote:

Originally Posted by -mAx- (Post 293464)
*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.

RGRUIZ February 3, 2011 23:36

-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

-mAx- February 4, 2011 02:22

Quote:

Originally Posted by John222 (Post 293531)
- 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

John222 February 4, 2011 07:42

Quote:

Originally Posted by RGRUIZ (Post 293561)
-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 February 4, 2011 07:43

Quote:

Originally Posted by -mAx- (Post 293565)
-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...


All times are GMT -4. The time now is 20:27.