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

Drag and Lift coefficient (NACA 0012)

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 6, 2009, 05:36
Default Drag and Lift coefficient (NACA 0012)
  #1
New Member
 
Join Date: Jul 2009
Location: Nantes, France
Posts: 2
Rep Power: 0
remi_fr is on a distinguished road
Hello,
I'm making an analysis of a NACA 0012 airfoil in 2D in a flow of water. I compare my results (drag and lift coefficients) with experiments.
My problem is that my results are different by approximately 40% of the true values.
The mesh is good, I'm using the K-epsilon turbulence model, the Reynolds number is 2.88 10^6

Do you have any idea from where my error can result?
thank you
remi_fr is offline   Reply With Quote

Old   July 6, 2009, 08:36
Default
  #2
Senior Member
 
Join Date: Mar 2009
Posts: 203
Rep Power: 9
Maddin is on a distinguished road
Change you solver settings to get a lower different between exp and sim.
How big is you problem?! Maybe you should start to make a DES because the modell influence is very low.
Cell size and material values you also should change (and look if correct values!).
Maddin is offline   Reply With Quote

Old   July 6, 2009, 16:37
Default
  #3
f-w
Senior Member
 
Join Date: Apr 2009
Posts: 129
Rep Power: 8
f-w is on a distinguished road
What angle of attack are you simulating?
f-w is offline   Reply With Quote

Old   July 6, 2009, 23:16
Default
  #4
Senior Member
 
Aroon
Join Date: Apr 2009
Location: Racine WI
Posts: 148
Rep Power: 8
vishyaroon is on a distinguished road
How does your near wall resolution look like? As Maddin mentioned you can use DES if there is massive separation involved. However if there is little or moderate separation RANS should be good enough, but make sure you check the near wall grid spacing.
vishyaroon is offline   Reply With Quote

Old   July 7, 2009, 04:50
Default
  #5
SKK
Member
 
Join Date: Mar 2009
Posts: 55
Rep Power: 8
SKK is on a distinguished road
Also in your case i would think relative length of laminar/transition/turbulent flow over the airfoil would be of importance similar to in low pressure turbine blades. Generally Wilcox type k-w (particulalrly Menter's SST) equations are much better in predicting skin friction in adverse pressure gradient situations.
SKK is offline   Reply With Quote

Old   July 8, 2009, 09:58
Default
  #6
New Member
 
Join Date: Jul 2009
Location: Nantes, France
Posts: 2
Rep Power: 0
remi_fr is on a distinguished road
I'm using a mesh with 68210 cells, 117349 faces, 49515 verts. It is first untructured then structured near the wall.
I ran simulations with an angle of attack of 0, 2, 4, 6 and 8.
I tried to use a spalart allmaras turbulence model but the results are worth than with K-epsilon turbulence model.
"Two Layer All y+ Wall treatment" is automatically selectionned. Is it the good one?
Thx
remi_fr is offline   Reply With Quote

Old   July 8, 2009, 11:01
Default
  #7
Senior Member
 
Aroon
Join Date: Apr 2009
Location: Racine WI
Posts: 148
Rep Power: 8
vishyaroon is on a distinguished road
The S-A RANS model (not DES model) should be good enough for the case you are simulating.

I'm not sure of the near wall mesh requirements of the S-A model with the wall treatment, but it will help if you make sure your y+ is consistent with what the model prescribes.
vishyaroon is offline   Reply With Quote

Old   August 27, 2009, 09:30
Default
  #8
Member
 
nguyen van trieu
Join Date: Jul 2009
Posts: 69
Rep Power: 8
nvtrieu is on a distinguished road
Hi Remi_fr,

I'm a new in Star-CCM+. My problem seems like yours. Here are my model:
c=4m; external domain 140x140m
2D; Stationary; H2O; Segregated flow; Constand density; Steady; Turbulent; RANS; K-w; SST; Y wall treatment.
Mesher: surface remesher; Polyhedral mesher; Prism Layer Mesher.
Base size: 10m; Volumetric control: custom size: 1%
Boundaries: airfoil; inlet; outlet and 2 walls.
Initial conditions: velocity: vx=1; vy=0
Attack angle: alpha =0, 2, ...16 (stall)
Reports:
Lift coef: reference density=997kg/m3; ref. vel.=1m/s; ref. area=4m2; direction [0,1,0]
Drag coef: reference density=997kg/m3; ref. vel.=1m/s; ref. area=1m2; direction [1,0,0]

I used above settings and tried to use another ones but I didn't got the right results. Ex: Cl is not equal zero at zero attack angle; some times Cl is so small and negative sign.

I would like to receive any help for my problem!
Thanks alot!

Trieu.

Last edited by nvtrieu; August 27, 2009 at 10:04.
nvtrieu is offline   Reply With Quote

Old   August 28, 2009, 08:32
Default
  #9
Member
 
Kuan Tek Seang
Join Date: Mar 2009
Posts: 31
Rep Power: 8
seang is on a distinguished road
came across this problem. your mesh isn't fine enough. try increasing your mesh resolution, make sure you capture the geometry adequately. if you don't have a good description of the camber-line, you won't get good results.
seang is offline   Reply With Quote

Old   September 3, 2009, 00:17
Default
  #10
Member
 
nguyen van trieu
Join Date: Jul 2009
Posts: 69
Rep Power: 8
nvtrieu is on a distinguished road
Hi Seang,
Thanks for you reply! "the mesh is not fine enough" - I think so. Now I try to you another software to create a better grid like Gridgen. Because in "Star-CCM+" I don't now how to improve my grid. Do you have any idea about my physics model? Is it oke?
nvtrieu is offline   Reply With Quote

Old   September 3, 2009, 02:16
Default
  #11
Member
 
Kuan Tek Seang
Join Date: Mar 2009
Posts: 31
Rep Power: 8
seang is on a distinguished road
Quote:
Originally Posted by nvtrieu View Post
Hi Seang,
Thanks for you reply! "the mesh is not fine enough" - I think so. Now I try to you another software to create a better grid like Gridgen. Because in "Star-CCM+" I don't now how to improve my grid. Do you have any idea about my physics model? Is it oke?
There is some characteristics you can check, even with a laminar or inviscid solver. Try running at a few angle of attacks and construct the lift-curve slope.

1) The curve/line should pass through 0, that is, no lift at 0 angle of attack.
2) The gradient of the lift-curve slope (linear portion) should be 2 pi.

The stall point is harder to pin-point, this is where turbulence modelling comes into play in predicting the separation point etc.

It is not that difficult to control mesh density in star-ccm+. There are parameters to change in the Reference Values section of your Mesh Continua. Easiest thing to do is to leave most of these reference values alone and work on the base size alone (decrease base size for a generally more dense mesh). You can also go to the individual parts under the Regions tree to define mesh size parameters pertaining to a particular part (e.g. airfoil surface). For wall bounded flows, you might want to watch your prism layer properties too.
seang is offline   Reply With Quote

Old   September 3, 2009, 02:44
Default
  #12
Member
 
nguyen van trieu
Join Date: Jul 2009
Posts: 69
Rep Power: 8
nvtrieu is on a distinguished road
Hi Seang,

I've already run the simulation at the difference angle of attack (0-2-4-6... deg). At zero angle the lift coefficient is slight negative value. So I think the foil is not symmetry. Usually, I left the reference values in mesh cotinua. I just changed the base size of mesh. In my case, I set the value is 10m. Is it too large? After that I use a volume control with the meshe size equal 1% which relates to base size 10m. Finally, I got the nmber of cells is around 40000. It is impossible to increase more cells, because I use CPU Core 2 Duo E8400 3.0 Ghz & 3Gb RAM.
I don't know why the mesh at LE and TE seem not fine. Do you have any experient on this problem to improve it better?
Thanks you again!
nvtrieu is offline   Reply With Quote

Old   September 3, 2009, 03:56
Default
  #13
Member
 
Kuan Tek Seang
Join Date: Mar 2009
Posts: 31
Rep Power: 8
seang is on a distinguished road
What slope do you get? close to 2 pi?

base size, depends on the size of your largest domain. i wouldn't use this to control the mesh size near the airfoil surface. for this, i would go down to the region->part's mesh values. continuum's default surface curvature setting of 36 points in a circle should normally be enough, but you should reduce the surface size's absolute minimum and target size to a sensible level.
seang is offline   Reply With Quote

Old   April 6, 2010, 11:07
Default
  #14
Member
 
kdrbrk's Avatar
 
Burak
Join Date: May 2009
Posts: 90
Rep Power: 8
kdrbrk is on a distinguished road
I am new to Star ccm+ and still trying to learn things.
I know how to define boundary conditions in 3D, but I couldn't find how to do it in 2D. can someone please help?

I will also investigate airfoils in ground effect.
kdrbrk is offline   Reply With Quote

Old   July 6, 2010, 11:26
Default
  #15
Senior Member
 
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
abdul099 is on a distinguished road
kdrbrk,

maybe a little bit too late, but there's no other answer, so I will try to help...

In Star-ccm+, you can only generate a 2D-mesh if you convert a 3D-mesh to a 2D-mesh. So adjust the 3D mesh settings before converting to 2D. It is done in the same way as in 3D. You go to regions, expand the 2D-region, go to boundaries, expand the boundary...
Physics settings on boundaries could be set in 2D, also in the same way as in 3D.

If you try to simulate airfoils in ground effect, you should take care of the mesh between ground and airfoil, due to high pressure gradients in this area.

Best regards
abdul099 is offline   Reply With Quote

Old   October 6, 2010, 20:37
Default
  #16
Member
 
John
Join Date: Aug 2009
Posts: 93
Rep Power: 8
nomad is on a distinguished road
You also need to make sure that the 2D plane you're interested in lies in the z=0 plane.
nomad is offline   Reply With Quote

Old   October 19, 2010, 14:51
Default
  #17
New Member
 
Join Date: Oct 2010
Posts: 1
Rep Power: 0
Sakkie is on a distinguished road
I think you both have mesh problem and maybe physics problems as well. You should make a refined mesh on the trailing edge of the airfoil as the dissipation has a very big influence on drag. This refined mesh does not have to be very big but needs to be about the same length as your chord and obviously the width of the airfoil. Use a volumetric control to do this and make the refined mesh about 5mm. Depending on the size of your volume I think your cell count is far too low and you are going get it up to 2 000 000 if the chord is about 1m. And further you must use prism mesh of at least 20 layers in 15mm. Your surface size on the airfoil should be about 0.5mm - 5mm and a base size of 1m, your points on the curvature should be around 100. I cannot help you with the physics models as I do not have allot of knowledge regarding water as flower.
Basically:
  • Prism Mesh
  • Airfoil Surface Size
  • Refined mesh in the wake
Sakkie is offline   Reply With Quote

Old   March 2, 2015, 17:23
Default
  #18
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 299
Rep Power: 4
MBdonCFD is on a distinguished road
I realize this is probably about 6 years too late, but I would like to point out that there is considerable disagreement between published data sets for the NACA0012 in both lift and drag. That in itself would make the 0012 a difficult validation case, let alone the issues that arrise with airfoil analysis in general.
MBdonCFD is offline   Reply With Quote

Reply

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
lift & drag coefficient on airfoil n. natik FLUENT 8 March 31, 2015 19:02
Lift and drag coefficient with strange values for NACA airfoil antonio_ing OpenFOAM Running, Solving & CFD 16 September 13, 2012 12:21
Fluent Good Lift coefficient BAD drag coefficient Rif Main CFD Forum 4 March 9, 2010 11:52
Automotive test case vinz OpenFOAM Running, Solving & CFD 98 October 27, 2008 09:43
drag and lift coefficient No CD-adapco 5 July 13, 2004 10:21


All times are GMT -4. The time now is 07:37.