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

Lift/Drag prediction Foil FX 78-PK-188-20

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 24, 2015, 04:59
Default Lift/Drag prediction Foil FX 78-PK-188-20
  #1
New Member
 
Join Date: Dec 2014
Posts: 9
Rep Power: 3
matmax-168 is on a distinguished road
Hello,
currently I'am calculating the drag polar and the lift envelope for the aerofoil above. Even with intensive investigations I become not satisfying results.

I have done several calculations with different meshes to get the mesh independent solution. The calculation area is a 3d swept mesh with one element in dept.

First I tryed steady simulations with a unstructured mesh and changed the AOA in several design points for getting the fully polars in one run.
I obtain very better results when using the Gamma Theta Transition model. But then I have to do transient runs for the reason of laminar separation bubbles. For better results I also tryed a better mapped mesh where I change the angle of the incoming air.

When looking at the lift envelope there is a short lift drop between Zero degree AOA and the total separation. (laminar turbulent transition moves to leading edge) In the simulation this appears later and therefore to big lift is calculated for the AOA above this point.
-Avarage Yplus is about .5 (may plus <1) as in the limit for good boundary layer resolution neccesary.
-observed no deviation in results when using more than 300 knodes at the foil contour (in stream direction)
-The distance to the boundaries is about 20m.
-Tu is low <1%

Now I have absolutely no idea what else to change in the simulation, to get better results. Thanks for every helpful advice!
Attached Images
File Type: jpg rund.jpg (96.3 KB, 29 views)
File Type: jpg foil 2d_R20m.jpg (95.8 KB, 27 views)
File Type: jpg übergang kann weicher gemacht wenn nl_steuerung durch kante in mitte.jpg (97.6 KB, 30 views)
File Type: jpg lift envelope2.JPG (34.4 KB, 30 views)
File Type: jpg drag polar2.JPG (29.9 KB, 24 views)

Last edited by matmax-168; August 24, 2015 at 05:15. Reason: supplement
matmax-168 is offline   Reply With Quote

Old   August 24, 2015, 06:31
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,838
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Your results are close - so you know you have the basics set up correctly. But to get the result accurate to those last few percent requires careful work.

* You have done a mesh sensitivity check (excellent) but the quality of your mesh is not great. There are several high aspect ratio elements I can see. Have a look how other researchers mesh airfoils, especially the C grid method.
* You need to check some of your other assumptions with sensitivity analysis: boundary proximity, convergence tolerance, time step size (for the transient runs).
* Also check how sensitive your simulation is to inlet turbulence levels and surface roughness on the airfoil.
* Are you using a second order advection scheme?
ghorrocks is offline   Reply With Quote

Old   August 24, 2015, 07:12
Default
  #3
New Member
 
Join Date: Dec 2014
Posts: 9
Rep Power: 3
matmax-168 is on a distinguished road
Hello Glenn,
fast answer, that is fantastic!
I will try to improve the mesh when all other suggestions will not help. So I have to reach lower AR right?

* Are you using a second order advection scheme?

" SOLVER CONTROL:
Turbulence Numerics = High Resolution
ADVECTION SCHEME:
Option = High Resolution
END
CONVERGENCE CONTROL:
Maximum Number of Coefficient Loops = 5
Minimum Number of Coefficient Loops = 1
Timescale Control = Coefficient Loops
END
CONVERGENCE CRITERIA:
Residual Target = 1e-06
Residual Type = MAX
END
TRANSIENT SCHEME:
Option = Second Order Backward Euler
TIMESTEP INITIALISATION:
Option = Automatic"

Thank you very much!
matmax-168 is offline   Reply With Quote

Old   August 24, 2015, 07:55
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,838
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Yes, you want the aspect ratio to approach 1. The C grid is good here because if you expand the radial mesh spacing in proportion to the radius then you get approximately aspect ratio 1 elements all the way out.

* The hires advection scheme will revert to upwinding (ie first order) in some areas. Check the velocity.beta variable in the post processor to see where it has gone first order. In your case I would suggest using a purely second order system like hybrid with the blend factor=1.0.
* Make the max number of coefficient loops larger, 10 is a good number.
* Your convergence tolerance is very tight. Are you sure you need it that tight?
ghorrocks is offline   Reply With Quote

Old   September 1, 2015, 05:49
Default
  #5
New Member
 
Join Date: Dec 2014
Posts: 9
Rep Power: 3
matmax-168 is on a distinguished road
Hello Glenn,

I have tryed a better mesh qualtity but the results will not improve.

A only second order advection scheme neither.

Wall roughness will not have much influence because the surface of aerofoils is very smooth, so that it can be managed as hydraulical smooth.

Wall proximity has a large influence for my drag values but they will not reduce the lift. - thats the point, it looks like cfx is overshooting lift for the reason of delayed separation or specific the laminar transition.
There is the typical buckle in the lift envelope, where the transition onset is equal to the leading edge. Then only turbulent boundary layer covers the suction side till separation, which declares the fast increase of drag.
For that reason I thougt my results are strongtly dependent on inlet turbulence but even when changing the intesity I have no remarkable changes.

Additional I have observed that the staedy state runs give nearly the same results, even when theire convergence did not fall below max Resi 1e-2! (transient: max Resi stable 1e-4, total time 4s, TS = 0.001s...0.01 s)

Now I have absolutely no idea what I can change.
In the some papers from ansys I have seen they have gained very reliable drag polars and lift envelopes.

Thank you very very much!
Attached Images
File Type: png 150x SP feiner.png (122.8 KB, 19 views)
matmax-168 is offline   Reply With Quote

Old   September 1, 2015, 08:02
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,838
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Have you looked at upstream turbulence levels? Also I have had some success in the past by applying wall roughness in excess of what the physical model actually had. Worth a try at least.

Your mesh does look higher quality but you still have some high aspect ratio elements near the trailing edge. But this is probably not contributing much to the problem.

Do the papers you have describe what they did in detail?
ghorrocks is offline   Reply With Quote

Old   September 1, 2015, 10:51
Default
  #7
New Member
 
Join Date: Dec 2014
Posts: 9
Rep Power: 3
matmax-168 is on a distinguished road
Well in one paper they also recognized this lift overshoot, they fixed it with an "in-house existent" correction implementation for the SST model. I have read the location of transition may be strongly dependent of Inlet viscosity ratio. For now I did not varied this value because in post, it seems that the free stream is very laminar, which I classified appropriate.

Using 1st order turbulence numerics instead of HiRes gives more unrealistic results althoug better convergence can be observed.

I will now try several roughness values and also use some other fixed inlet viscosity ratios. Is there a different to enter the roughness by wall-boundary or by transition model options?
matmax-168 is offline   Reply With Quote

Old   September 1, 2015, 18:39
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,838
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Quote:
Is there a different to enter the roughness by wall-boundary or by transition model options?
I do not understand this question.
ghorrocks is offline   Reply With Quote

Old   September 7, 2015, 04:33
Default
  #9
New Member
 
Join Date: Dec 2014
Posts: 9
Rep Power: 3
matmax-168 is on a distinguished road
Sry I was not reading correcticly. At boundary condition "rough-wall" you have to enter the equivalent sandgrain roughness and when setting a roughness at the wall you have to enable the roughness correlation for Gamma Theta Transition by entering the geometric roughness - as said in the ansys manual.

Unfortunately this did not reduce my lift prediction. Maybe I have chosen the wrong values.

In some literature I found possible roughness values for wing surfaces about ks=0.002mm. As far as I understood the different notes and indices this must be the equivalent sand grain roughness right? But how can I determine the geometric roughness then? ... I have read the chapter in Schlichting (boundary layer theory) about this, anyhow I can not figure it out.

I have also changed the Inlet turbulence and eddy viscosity ratio so that a min. turbulence > 0.1% around the profile is ensured. (belonging to ansys manual) Nevertheless lift prediction gives an overshoot. Higher free stream turbulences will give correctly lift reduction but for the cost of strong drag increase.
matmax-168 is offline   Reply With Quote

Old   February 21, 2016, 01:35
Default
  #10
New Member
 
Alejandro Garcia Aguilar
Join Date: Feb 2016
Posts: 3
Rep Power: 2
Alex Garcia is on a distinguished road
Hello matmax, I am trying to do a similar approach as yours for a whole glider I am using inflation techniques and proximity curvature method, my mesh looks fine I'm getting values of y plus lowers than one but I am interested to learn how you set up your mesh? Also can you teach me how you set up your solver and your approach to get polars in one single run?
Alex Garcia is offline   Reply With Quote

Reply

Tags
accuracy, drag coefficient, lift coefficient, tranisitional flow

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


Similar Threads
Thread Thread Starter Forum Replies Last Post
Problem with 2-d oscillating foil cib10166 FLUENT 1 April 7, 2014 14:03
Foil Bearing Simulation Bajji OpenFOAM 4 May 1, 2013 23:47
Prdctn of lift/drag co-efficnt of 2D foil influent Dutta FLUENT 0 August 28, 2008 18:07
foil using static frre stream flow Phil FLUENT 0 November 11, 2002 09:57
drag prediction in FLUENT Hua FLUENT 0 November 4, 2002 00:16


All times are GMT -4. The time now is 19:41.