CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

simpleFOAM NACA0012 (α=8) cL, cD not matching published data

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   April 4, 2012, 03:33
Default
  #21
Senior Member
 
Ralph Moolenaar
Join Date: Aug 2010
Location: 's-Hertogenbosch, the Netherlands
Posts: 120
Rep Power: 6
Ralph M is on a distinguished road
Maybe you guys tried to switch from SA turbulence modelling to something like K-Omega or K-epsilon? If all turbulence models give the same answer your source of problem has to be somewhere else
__________________
CFD for marine applications? Go to http://www.marinecfd.com/ and join the OF Ship Hydromechanics Group: http://www.cfd-online.com/Forums/gro...mechanics.html
Ralph M is offline   Reply With Quote

Old   April 4, 2012, 05:44
Default
  #22
Member
 
Joe
Join Date: Dec 2011
Location: Groton, CT
Posts: 67
Rep Power: 5
jferrari is on a distinguished road
Quote:
SimpleFOAM is turbulent solver, but we can use it for laminar flow calculation with little modification. One needs to edit RASProperties file and switch off turbulence (control/RASProperties).
Thanks for pointing this out.
jferrari is offline   Reply With Quote

Old   April 4, 2012, 09:13
Default
  #23
Senior Member
 
Mihai Pruna
Join Date: Apr 2010
Location: Boston
Posts: 190
Blog Entries: 1
Rep Power: 7
mihaipruna is on a distinguished road
Quote:
Originally Posted by jferrari View Post
Mihai, you mentioned that you were looking to stay in the laminar flow regime, but you're posting in this thread about simpleFoam. This is a turbulent solver. The laminar solver is icoFoam. Which solver are you using? What Reynolds number are you using? If you're using simpleFoam, what turbulence model are you using?
Joe, I need to use simpleFoam but I would like to compare my results with,preferably, published laminar airfoil data for validation.
Alternatively, I can use xfoil to get more realistic turbulent data.

Regardless, my numbers with OF are not even in the ballpark, and was hoping I made some silly mistake easily spotted by the sharp eyes here. Looks like the Cl is off by a factor of 10 for the 5 degree AOA study!
__________________
Mihai Pruna's Bio
mihaipruna is offline   Reply With Quote

Old   April 4, 2012, 09:39
Default
  #24
Member
 
Joe
Join Date: Dec 2011
Location: Groton, CT
Posts: 67
Rep Power: 5
jferrari is on a distinguished road
Quote:
Maybe you guys tried to switch from SA turbulence modelling to something like K-Omega or K-epsilon? If all turbulence models give the same answer your source of problem has to be somewhere else
I hadn't thought of this. I'll try a different turbulence model and compare results. I have a SA run going on now.... I assume it should be to 20,000 iterations by the time I get out of work, it was at about 13,000 when I checked it before work this morning. After that finishes I'll try k-epsilon and compare with SA.
jferrari is offline   Reply With Quote

Old   April 4, 2012, 09:46
Default
  #25
Member
 
Joe
Join Date: Dec 2011
Location: Groton, CT
Posts: 67
Rep Power: 5
jferrari is on a distinguished road
Quote:
Regardless, my numbers with OF are not even in the ballpark, and was hoping I made some silly mistake easily spotted by the sharp eyes here. Looks like the Cl is off by a factor of 10 for the 5 degree AOA study!
If you're off by a factor of 10, based on the only information you've provided, I think your span is the issue.
jferrari is offline   Reply With Quote

Old   April 4, 2012, 13:10
Default
  #26
Senior Member
 
Mihai Pruna
Join Date: Apr 2010
Location: Boston
Posts: 190
Blog Entries: 1
Rep Power: 7
mihaipruna is on a distinguished road
that would be nice, but if you look at the two files, the L and A ref are the same.
__________________
Mihai Pruna's Bio
mihaipruna is offline   Reply With Quote

Old   April 4, 2012, 15:10
Default
  #27
Senior Member
 
sail's Avatar
 
Vieri Abolaffio
Join Date: Jul 2010
Location: Always on the move.
Posts: 308
Rep Power: 8
sail is on a distinguished road
---edit: i got confused by the many type of foils this thread is about---
__________________
http://www.leadingedge.it/
Naval architecture and CFD consultancy
sail is offline   Reply With Quote

Old   April 4, 2012, 18:51
Default
  #28
Member
 
Joe
Join Date: Dec 2011
Location: Groton, CT
Posts: 67
Rep Power: 5
jferrari is on a distinguished road
So I sort of had some success. I'm not calculating a lift coefficient of 0.9226 and a drag coefficient of 0.0089670 - agreeing very well with Abbot and Von Doenhoff. However, my nuTilda field looks kind of strange - check it out:



There are two patches meeting where all that turbulence has gathered. On the right patch nuTilda has a zeroGradient boundary condition and nut has a calculated boundary condition with value set to $internalField. On the upper patch nuTilda has a fixed value of zero and nut has a nutUSpaldingWallFunction boundary condition.

Does anybody know what's going on with nuTilda and nut here?
jferrari is offline   Reply With Quote

Old   April 5, 2012, 10:43
Default
  #29
Member
 
Join Date: Oct 2010
Location: Germany
Posts: 39
Rep Power: 6
Ivanet is on a distinguished road
Hi JFerrari,
are you doing the mesh with blockMesh? You could use splines instead of straight edges when defining your blocks . This would allow you to have a better control on the orthogonality of your cells (specially in the boundary layer).
By the way, why do you use an O-Grid for this profile? Usually C-Grids are better for sharp trailing edges.
Greetings
Ivan
Ivanet is offline   Reply With Quote

Old   April 5, 2012, 11:38
Default
  #30
Member
 
Joe
Join Date: Dec 2011
Location: Groton, CT
Posts: 67
Rep Power: 5
jferrari is on a distinguished road
Hi Ivan,

I am meshing with blockMesh - though I hadn't thought using splines to make the block boundaries - I'll try that. The reason I'm using an O-grid is because ultimately I want to dynamically pitch the airfoil to study dynamic stall. I figure that my first step is to get accurate results for the steady case - then rotate the O-grid for the unsteady case.

Or at least that's my plan... Is this the best way to go about pitching the airfoil?
jferrari is offline   Reply With Quote

Old   April 5, 2012, 12:14
Default
  #31
Member
 
Join Date: Oct 2010
Location: Germany
Posts: 39
Rep Power: 6
Ivanet is on a distinguished road
Hi Joe,
Interesting, actually I am trying to do exactly the same like you: dynamic stall studies on a pitching blade. My plan is also getting first decent results on a static case and then go for the rotating case.
The alternative to the O-Grid would be a C-Grid embedded in an O-Grid.
Greetings
Ivan
Ivanet is offline   Reply With Quote

Old   April 8, 2012, 12:30
Default
  #32
Member
 
Joe
Join Date: Dec 2011
Location: Groton, CT
Posts: 67
Rep Power: 5
jferrari is on a distinguished road
Quote:
Hi Joe,
Interesting, actually I am trying to do exactly the same like you: dynamic stall studies on a pitching blade. My plan is also getting first decent results on a static case and then go for the rotating case.
The alternative to the O-Grid would be a C-Grid embedded in an O-Grid.
Greetings
Ivan
Interesting to find someone else working on exactly this, Ivan.

It's been a busy Easter weekend - I haven't gotten anything done since I last posted.

Currently I'm revisiting my mesh, trying to make it better.
jferrari is offline   Reply With Quote

Old   April 17, 2012, 04:39
Default Force coefficient
  #33
Member
 
ehsan
Join Date: Mar 2009
Posts: 92
Rep Power: 8
ehsan is on a distinguished road
Hello

Once we try to calculate lift and drag coefficient with force command inside the controlDict of simplefoam, I encountered the error that force.c could not find rho. I like to know how I could get forces for incompressible flow solutions (done with simplefoam).

Thanks
ehsan is offline   Reply With Quote

Old   April 17, 2012, 05:09
Default
  #34
Member
 
Join Date: Oct 2010
Location: Germany
Posts: 39
Rep Power: 6
Ivanet is on a distinguished road
Quote:
Originally Posted by ehsan View Post
Hello

Once we try to calculate lift and drag coefficient with force command inside the controlDict of simplefoam, I encountered the error that force.c could not find rho. I like to know how I could get forces for incompressible flow solutions (done with simplefoam).

Thanks
Try it again including this in your controlDict
rhoName rhoInf;
rhoInf 1.225; //density of your fluid

Good luck
Ivan
Ivanet is offline   Reply With Quote

Old   April 17, 2012, 08:53
Default
  #35
Member
 
ehsan
Join Date: Mar 2009
Posts: 92
Rep Power: 8
ehsan is on a distinguished road
Thanks a lot
ehsan is offline   Reply With Quote

Old   April 17, 2012, 09:26
Default
  #36
Member
 
Joe
Join Date: Dec 2011
Location: Groton, CT
Posts: 67
Rep Power: 5
jferrari is on a distinguished road
A friend of mine has provided me with a beautiful structured mesh of a NACA 0012 airfoil in an O-grid I'll post a link to it when I'm home and have access to my files). He built it in gridgen and converted it to openfoam format, which created all boundaries as a single patch. I'm currently working to get this mesh more usable - using autoPatch and/or createPatch.


I just wanted to keep this thread updated for anyone following.
jferrari is offline   Reply With Quote

Old   April 17, 2012, 17:53
Default lift & drag coefficients
  #37
New Member
 
Farshad Rezaei
Join Date: Apr 2012
Posts: 10
Rep Power: 5
Farshad585 is on a distinguished road
Hi
I'm a new user in OpenFOAM. I've run NACA0012 by using simpleFoam. I used a common file to compute lift and drag coefficients. but my lift and drag coefficients are too low. I think it is related to Aref & lref in computing the coefficients. could anyone tell me what should i do for Aref & lref?
thanks alot
Farshad585 is offline   Reply With Quote

Old   April 17, 2012, 19:53
Default
  #38
Member
 
Joe
Join Date: Dec 2011
Location: Groton, CT
Posts: 67
Rep Power: 5
jferrari is on a distinguished road
Farshad, not sure what you mean by common file. You should be using the forces library that's already in OpenFOAM. If you think that the problem is with lref or Aref, you can compare those values to those that you have in your geometry.
Farshad585 likes this.
jferrari is offline   Reply With Quote

Old   April 18, 2012, 00:52
Default
  #39
New Member
 
Qiang
Join Date: Mar 2012
Posts: 12
Rep Power: 5
wangqiangele is on a distinguished road
Dear vkrastev,

My model is a 3D twisted and tapered blade. How could I get the Cl, Cd at specific section?


Best regards,
Qiang Wang
wangqiangele is offline   Reply With Quote

Old   April 18, 2012, 06:58
Default
  #40
Member
 
Join Date: Oct 2010
Location: Germany
Posts: 39
Rep Power: 6
Ivanet is on a distinguished road
Quote:
Originally Posted by wangqiangele View Post
Dear vkrastev,

My model is a 3D twisted and tapered blade. How could I get the Cl, Cd at specific section?


Best regards,
Qiang Wang
You should do a patch for the specific section you are interested in and then use the forces lib.
Greets
Ivan
Ivanet 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
fluentMeshToFoam multidomain mesh conversion problem Attesz OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 12 May 2, 2013 10:52
matching variable data with grid point data anfho OpenFOAM Programming & Development 0 May 6, 2011 15:28
Naca0012 k-e mpirun gives fpe whereas simpleFoam not Pierpaolo OpenFOAM 1 May 8, 2010 03:08
NACA0012 Data as a function of Re for a VAWT model psd Main CFD Forum 1 July 31, 2009 22:04
How to update polyPatchbs localPoints liu OpenFOAM Running, Solving & CFD 6 December 30, 2005 18:27


All times are GMT -4. The time now is 14:51.