CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   Divergence of a 2d airfoil (http://www.cfd-online.com/Forums/star-ccm/111794-divergence-2d-airfoil.html)

fshak92 January 15, 2013 13:25

Divergence of a 2d airfoil
 
3 Attachment(s)
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.

abdul099 January 15, 2013 17:22

Do you have flat cells in the prism layers near the walls?

fshak92 January 15, 2013 20:20

Quote:

Originally Posted by abdul099 (Post 402052)
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.

siara817 January 16, 2013 03:19

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.

fshak92 January 16, 2013 07:30

Quote:

Originally Posted by siara817 (Post 402098)
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.

fshak92 January 16, 2013 13:27

5 Attachment(s)
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)

siara817 January 17, 2013 04:34

According to your residuals it seems that it is converging. I think it is too soon to decide according some hundreds of iterations.

fshak92 January 17, 2013 06:26

Quote:

Originally Posted by siara817 (Post 402378)
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?

siara817 January 18, 2013 08:16

Dear Omid,
It depends on the near wall treatment you have selected. Have you selected Two layer all y+...?

fshak92 January 18, 2013 12:30

Quote:

Originally Posted by siara817 (Post 402639)
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).

abdul099 January 18, 2013 16:51

Quote:

Originally Posted by omid88 (Post 402061)
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...*


All times are GMT -4. The time now is 23:21.