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

Divergence of a 2d airfoil

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 15, 2013, 13:25
Default Divergence of a 2d airfoil
  #1
Senior Member
 
Join Date: Dec 2011
Posts: 121
Rep Power: 5
fshak92 is on a distinguished road
I'm trying to do a rod-airfoil simulation by meshing in ccm+ and solving in OpenFOAM.For testing the validity of mesh in ccm+, i should have a converged solution in ccm but it does not converge.
You can see the general view of the geometry , as well as the magnified pictures of the mesh.
I've tested the wall distance around airfoil and cylinder in a wide range(10^-4 to 10^-7 ) and most of the turbulent solvers.But the residual(for turbulent parameters) goes up and i get very high velocity around airfoil and cylinder(something about 10^6) .
The inlet velocity is 100.
'velocity inlet' for the left middle boundary, 'pressure outlet' (right boundary) and 'wall' for other boundaries.

I would appreciate any idea,particularly on the mesh quality.
Attached Images
File Type: jpg Airfoil2d.jpg (96.1 KB, 15 views)
File Type: jpg Airfoil-MagnifiedCylinder.jpg (99.1 KB, 12 views)
File Type: jpg Airfoil-MagnifiedFoil.jpg (86.1 KB, 17 views)

Last edited by fshak92; January 15, 2013 at 14:00.
fshak92 is offline   Reply With Quote

Old   January 15, 2013, 17:22
Default
  #2
Senior Member
 
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
abdul099 is on a distinguished road
Do you have flat cells in the prism layers near the walls?
__________________
We do three types of jobs here:
GOOD, FAST AND CHEAP
You may choose any two!
abdul099 is offline   Reply With Quote

Old   January 15, 2013, 20:20
Default
  #3
Senior Member
 
Join Date: Dec 2011
Posts: 121
Rep Power: 5
fshak92 is on a distinguished road
Quote:
Originally Posted by abdul099 View Post
Do you have flat cells in the prism layers near the walls?
Around airfoil or walls?
If you mean the first layer distance to airfoil, I've changed it from 10^-4 to 10^-7 , and as you know, it makes a quadrangle cells with very low width in contrast to its length.
but on the walls, the first layer distance is in the range of 10^-2 and only 5 layers have been used.Therefore it is not so flat.
But the strange velocity(about 10^6) is happened around airfoil and cylinder and not the walls.

Thanks in advance.
fshak92 is offline   Reply With Quote

Old   January 16, 2013, 03:19
Default
  #4
Senior Member
 
siara817's Avatar
 
siamak rahimi ardkapan
Join Date: Jul 2010
Location: Copenhagen, Denmark
Posts: 218
Rep Power: 9
siara817 is on a distinguished road
Hi Omid

Do you have energy solver or you considered it to be isothermal?
If yes, try once to run with first order scheme and then if converged change to second order.
__________________
Good luck
Siamak
siara817 is offline   Reply With Quote

Old   January 16, 2013, 07:30
Default
  #5
Senior Member
 
Join Date: Dec 2011
Posts: 121
Rep Power: 5
fshak92 is on a distinguished road
Quote:
Originally Posted by siara817 View Post
Hi Omid

Do you have energy solver or you considered it to be isothermal?
If yes, try once to run with first order scheme and then if converged change to second order.
Hi
Thank you all for your consideration.
No i did not use any energy solver.
It seems the problem is related to mesh.

Last edited by fshak92; January 16, 2013 at 13:27.
fshak92 is offline   Reply With Quote

Old   January 16, 2013, 13:27
Default
  #6
Senior Member
 
Join Date: Dec 2011
Posts: 121
Rep Power: 5
fshak92 is on a distinguished road
And these are the pictures for the new trimmer mesh.
I forgot to set an initial velocity.After set it to 50m/s, the residual became a little better.But after each iteration the turbulent viscosity of more cells are limited.(in the first picture,the red cells are the limited ones)
Attached Images
File Type: jpg airfoil2d_TurbulentViscosity.jpg (98.7 KB, 15 views)
File Type: jpg airfoil2d_Trimmer_velocity.jpg (99.9 KB, 10 views)
File Type: jpg airfoil2d_Trimmer_velocity2.jpg (89.0 KB, 9 views)
File Type: jpg airfoil2d_Trimmer_velocity3.jpg (76.6 KB, 9 views)
File Type: jpg airfoil2d_Trimmer_residual.jpg (97.2 KB, 13 views)
fshak92 is offline   Reply With Quote

Old   January 17, 2013, 04:34
Default
  #7
Senior Member
 
siara817's Avatar
 
siamak rahimi ardkapan
Join Date: Jul 2010
Location: Copenhagen, Denmark
Posts: 218
Rep Power: 9
siara817 is on a distinguished road
According to your residuals it seems that it is converging. I think it is too soon to decide according some hundreds of iterations.
__________________
Good luck
Siamak
siara817 is offline   Reply With Quote

Old   January 17, 2013, 06:26
Default
  #8
Senior Member
 
Join Date: Dec 2011
Posts: 121
Rep Power: 5
fshak92 is on a distinguished road
Quote:
Originally Posted by siara817 View Post
According to your residuals it seems that it is converging. I think it is too soon to decide according some hundreds of iterations.
Thank you for your reply.
But the number of cells in which turbulent viscosity are limited,are increasing by iteration significantly...
The boundaries for 'top' ,'below' 'top-left' and 'below-left' are considered as 'wall',are they correct?!Because the problem is defined in a way that we have walls there.
But the velocity on those walls are nearly zero, Do you know how the turbulence models work there?

Last edited by fshak92; January 17, 2013 at 12:38.
fshak92 is offline   Reply With Quote

Old   January 18, 2013, 08:16
Default
  #9
Senior Member
 
siara817's Avatar
 
siamak rahimi ardkapan
Join Date: Jul 2010
Location: Copenhagen, Denmark
Posts: 218
Rep Power: 9
siara817 is on a distinguished road
Dear Omid,
It depends on the near wall treatment you have selected. Have you selected Two layer all y+...?
__________________
Good luck
Siamak
siara817 is offline   Reply With Quote

Old   January 18, 2013, 12:30
Default
  #10
Senior Member
 
Join Date: Dec 2011
Posts: 121
Rep Power: 5
fshak92 is on a distinguished road
Quote:
Originally Posted by siara817 View Post
Dear Omid,
It depends on the near wall treatment you have selected. Have you selected Two layer all y+...?
Thank you Mr. Rahimi
I used all y+ wall treatment. and it seems it distinguishes between the walls according their y+.
I refined the mesh in the region i had problem with turbulent viscosity and now this problem has been solved,,but still the residual for K is high(more than 1).
fshak92 is offline   Reply With Quote

Old   January 18, 2013, 16:51
Default
  #11
Senior Member
 
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
abdul099 is on a distinguished road
Quote:
Originally Posted by omid88 View Post
Around airfoil or walls?
If you mean the first layer distance to airfoil, I've changed it from 10^-4 to 10^-7 , and as you know, it makes a quadrangle cells with very low width in contrast to its length.
but on the walls, the first layer distance is in the range of 10^-2 and only 5 layers have been used.Therefore it is not so flat.
But the strange velocity(about 10^6) is happened around airfoil and cylinder and not the walls.

Thanks in advance.
I mentioned flat cells at "walls", and I'm pretty sure, your airfoil is a wall boundary. All other would not make any sense.
Now you say, the high velocity is located close to the airfoil boundary, where you HAVE flat cells (low width in contrast to its length). And you have even reduced the first layer thickness to an extremely low value (10^-7 is not suitable for an airfoil, 10^-4 or 10^-5 is a much more suitable range for this "low" inlet velocity).
So I suspect that's the main reason for your issues. And if so, please adjust your mesh resolution to create reasonable aspect ratios or increase your first prism layer thickness.

But even if I'm wrong, please check your y+ values at airfoil and cylinder since it should be in a reasonable range.

*Sometimes I wish this f... CCM+ solver wouldn't be that f... stable. In early versions it would just have been blowing up, but now it continues with nearly every setting - no matter if it makes sense or not...*
__________________
We do three types of jobs here:
GOOD, FAST AND CHEAP
You may choose any two!
abdul099 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
Low Speed Airfoil Mancusi FLUENT 7 April 3, 2014 06:11
Quarter Burner mesh with periosic condition SamCanuck FLUENT 2 August 31, 2011 11:34
Modeling Backflow for a 3D Airfoil (Wing of Finite Span) Josh CFX 9 August 18, 2009 11:31
Airfoil boundary condition Frank Main CFD Forum 1 April 21, 2008 18:36
Divergence problem when airfoil exceed pitch angle zonexo Main CFD Forum 2 April 4, 2007 04:22


All times are GMT -4. The time now is 10:07.