Divergence of a 2d airfoil

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

January 15, 2013, 13:25
Divergence of a 2d airfoil
#1
Senior Member

Join Date: Dec 2011
Posts: 121
Rep Power: 5
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
 Airfoil2d.jpg (96.1 KB, 15 views) Airfoil-MagnifiedCylinder.jpg (99.1 KB, 12 views) Airfoil-MagnifiedFoil.jpg (86.1 KB, 17 views)

Last edited by fshak92; January 15, 2013 at 14:00.

 January 15, 2013, 17:22 #2 Senior Member   Join Date: Oct 2009 Location: Germany Posts: 637 Rep Power: 12 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!

January 15, 2013, 20:20
#3
Senior Member

Join Date: Dec 2011
Posts: 121
Rep Power: 5
Quote:
 Originally Posted by abdul099 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.

 January 16, 2013, 03:19 #4 Senior Member     siamak rahimi ardkapan Join Date: Jul 2010 Location: Copenhagen, Denmark Posts: 218 Rep Power: 9 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

January 16, 2013, 07:30
#5
Senior Member

Join Date: Dec 2011
Posts: 121
Rep Power: 5
Quote:
 Originally Posted by siara817 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.

January 16, 2013, 13:27
#6
Senior Member

Join Date: Dec 2011
Posts: 121
Rep Power: 5
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
 airfoil2d_TurbulentViscosity.jpg (98.7 KB, 15 views) airfoil2d_Trimmer_velocity.jpg (99.9 KB, 10 views) airfoil2d_Trimmer_velocity2.jpg (89.0 KB, 9 views) airfoil2d_Trimmer_velocity3.jpg (76.6 KB, 9 views) airfoil2d_Trimmer_residual.jpg (97.2 KB, 13 views)

 January 17, 2013, 04:34 #7 Senior Member     siamak rahimi ardkapan Join Date: Jul 2010 Location: Copenhagen, Denmark Posts: 218 Rep Power: 9 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

January 17, 2013, 06:26
#8
Senior Member

Join Date: Dec 2011
Posts: 121
Rep Power: 5
Quote:
 Originally Posted by siara817 According to your residuals it seems that it is converging. I think it is too soon to decide according some hundreds of iterations.
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.

 January 18, 2013, 08:16 #9 Senior Member     siamak rahimi ardkapan Join Date: Jul 2010 Location: Copenhagen, Denmark Posts: 218 Rep Power: 9 Dear Omid, It depends on the near wall treatment you have selected. Have you selected Two layer all y+...? __________________ Good luck Siamak

January 18, 2013, 12:30
#10
Senior Member

Join Date: Dec 2011
Posts: 121
Rep Power: 5
Quote:
 Originally Posted by siara817 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).

January 18, 2013, 16:51
#11
Senior Member

Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
Quote:
 Originally Posted by omid88 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!

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Mancusi FLUENT 7 April 3, 2014 06:11 SamCanuck FLUENT 2 August 31, 2011 11:34 Josh CFX 9 August 18, 2009 11:31 Frank Main CFD Forum 1 April 21, 2008 18:36 zonexo Main CFD Forum 2 April 4, 2007 04:22

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