CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   3D Naca wing divergence (http://www.cfd-online.com/Forums/fluent/114332-3d-naca-wing-divergence.html)

Bollonga March 9, 2013 06:11

3D Naca wing divergence
 
5 Attachment(s)
Hi you all guys,

I'm working on a 3D naca wing of 1.018 m chord length with 0 angle of attack. You can see the domain extents in picture 1.
I've done an hexa mesh with a min quality of 0.6, min angle of 36 and max volume change of 4.7 so mesh is pretty good. (see files prj, tin and blk)

In Fluent I'm using k-omega SST model with inlet conditions: 34 m/s, TI=0.5% and turbulent legth scale of 0.07 (7% of chord length as suggested in Fluent User Guide). Initialization is always from inlet. k and omega schemes are 1st order.

For the steady case, reverse flow appears from the very first iteration and keep growing until turbulent viscosity ratio is limited to 1e5 in too many cells. I've tried reducing under-relaxation factor by half and by an order of magnitude. Divergence takes longer to appear but it happens all the same.

For the transient case, using adaptive timestepping starting at 1e-8s the same is happening. I've also tried the under-relax factors reduction with same results.

I've also tried the laminar case and k-epsilon standard with enhanced wall function steady/transient but all of them diverges.

Can it be a domain extent problem?
Or a mesh density problem? In the wake? In the y-direction?
Or an initialisation problem?
Or set up problem?

I've been told to try to start with a higher viscosity fluid and to reduce it until reaching the actual fluid properties (air). Is that necessary? I supposed it was a rather simple case.

Any suggestion is welcome. Please, ask me any info you may need.

Thanks a lot!

blackmask March 9, 2013 06:47

Were I doing this kind of simulation, I would at least double the extends in each direction.

The most probably reason for the divergence problem is incorrect boundary condition. What are the b.c. for the upper and lower surface? By any chance did you specify the velocity normal to those surfaces?

If you are not simulating the wind tunnel blockage effect and simply want to study the aerodynamic characteristics of this airfoil, then I suggest replacing the upper, inlet and lower curves by a simple curve, say a parabola. It facilitates specifying the b.c. with non-zero angle-of-attack.

Bollonga March 9, 2013 07:09

BC at bottom, top and side faces are symmetry. Inlet face has normal to boundary velocity. Outlet face is pressure outlet.

I've chosen this domain shape for symplicity, the airfoil is just part of a more complex geometry so I just want to check the convergence of this simple case.

I will try to double the extension in all directions. Should I keep the same node distribution or increase it? Now it's 30 nodes upwind with hyperbolic distribution from 0.25 in the farfield to 0.05 next to the airfoil. Backwind is 100 nodes hyperbolic from 0.01 next to the airfoil to 0.25 in the farfield. Spanwise there are 75 nodes uniformly distributed.
I would like to reduce the computational cost to the minimum possible.

I'll share my results for the wider domain. Thanks!

Far March 9, 2013 07:21

Your model is symmetric? Use slip wall for all wall boundaries except symmetry.

Bollonga March 9, 2013 07:25

Quote:

Originally Posted by Far (Post 412709)
Your model is symmetric? Use slip wall for all wall boundaries except symmetry.

The only wall BC is that of the airfoil so I should keep it as non-slip, right?
If I were to simulate the ground, I should use the slip wall condition?
Yes, the model is symmetric.

Far March 9, 2013 07:37

Bottom, top, side (not connected to wing) be defined as slip wall and side 2 (connected to wing) be defined as symmetry.

Bollonga March 9, 2013 09:43

Quote:

Originally Posted by Far (Post 412715)
Bottom, top, side (not connected to wing) be defined as slip wall and side 2 (connected to wing) be defined as symmetry.

Slip wall is a stationary wall with 0 specifed shear stress, right?
The wing comes form side to side of the domain, so both sides have symmetry BC.
I've made the domain bigger but TVR limitation appears again and doesn't decrease. I'll give it a try with reduced under-relaxation factors and if it doesn't work I'll try a more viscous fluid.

Far March 9, 2013 09:49

Quote:

Originally Posted by Bollonga (Post 412728)
Slip wall is a stationary wall with 0 specifed shear stress, right?
The wing comes form side to side of the domain, so both sides have symmetry BC.
I've made the domain bigger but TVR limitation appears again and doesn't decrease. I'll give it a try with reduced under-relaxation factors and if it doesn't work I'll try a more viscous fluid.

Yes slip wall is wall with zero shear stress. It's almost similar to symmetry with few exceptions.

Bollonga March 9, 2013 09:55

1 Attachment(s)
Reduced under-relax factor haven't worked for the steady k-om SST case (see residuals). I'll try with the more viscous fluid.

Far March 9, 2013 10:14

why such severe divergence ? ! Did you specify angle of attack?

what are the domain extents now?

Bollonga March 9, 2013 11:09

Quote:

Originally Posted by Far (Post 412735)
why such severe divergence ? ! Did you specify angle of attack?

what are the domain extents now?

Angle of attack is 0.

Domain is: 10c upwind,10c up, 10c down et 36c downwind. Spanwise the domain is 5c.

I don't know why such a sever divergence from the beginning...

Far March 9, 2013 12:13

Flow is incompressible? Any effect after increasing domain size?

Far March 9, 2013 12:25

something wrong there
 
I dont see any problem in convergence with short domain even. However, I have made some minor adjustments to blocking.

Bollonga March 9, 2013 12:29

Quote:

Originally Posted by Far (Post 412753)
Flow is incompressible? Any effect after increasing domain size?

Yes, flow is incompressible.
Maybe it takes longer to reach divergence with the larger domain.

Quote:

Originally Posted by Far (Post 412753)
I dont see any problem in convergence with short domain even. However, I have made some minor adjustments to blocking.

Have you managed to avoid the divergence? How?

Far March 9, 2013 12:35

check your ICEM files and you will find that you have not associated vertex to point at sharp trailing edge.

Also I've made the spacing equal in both directions (normal and tang) at trailing edge. So cells at the trailing edge on both sides (on wing and in wake) are of square shape.

Moreover I've reduced mesh size to 0.6 million by reducing mesh sizing in spanwise direction which is waste of resources as you are modelling it as an infinite wing and symmetry conditions are applied.

Residuals are reduced by 4th order within 100 iterations and with second order flow scheme. Turbulence model is SST and steady state mode.

Normal wall spacing is not changed, therefore Y+ is maintained

Bollonga March 9, 2013 12:58

Quote:

Originally Posted by Far (Post 412759)
Also I've made the spacing equal in both directions (normal and tang) at trailing edge. So cells at the trailing edge on both sides (on wing and in wake) are of square shape.

Which node distribution have you made?

Quote:

Originally Posted by Far (Post 412759)
Moreover I've reduced mesh size to 0.6 million by reducing mesh sizing in spanwise direction which is waste of resources as you are modelling it as an infinite wing and symmetry conditions are applied.

Which distribution have you let for the z-direction?

Would you mind passing me that mesh files to see how each node distribution is?

Thanks a lot Far!

Far March 9, 2013 13:05

1 Attachment(s)
Please make the domain at least 10-15 upstream and 20-30 downstream.

Files are attached.

I have used pressure based coupled solver. Other options used are : High order term relaxation. 2nd order flow scheme. Cournt number 20,000.


up and down boundaries are slip walls. Did not specify the turbulence level, used default settings.

Far March 9, 2013 13:17

.......................................

Far March 9, 2013 13:19

Fluent cas and dat attached. upload will take some time.

Fluent cas & dat

Bollonga March 9, 2013 13:36

1 Attachment(s)
I was asking you some more questions, but having cas and dat files is great! However dropbox shows error 404 and doesn't seem to be uploading...:mad:

Quote:

Originally Posted by Far (Post 412765)
Other options used are : High order term relaxation. 2nd order flow scheme. Cournt number 20,000.

Under-relax factors an order of magnitud reduced is appropiate? Do I need to reduce all of them?

Gradient: Least Squares cell based or Green-Gauss cell/node based? How relevant is this?

Pressure: 2nd order is more suitable than PRESTO! scheme?

Momentum: 2nd order rather than Quick or Power-law?

Thanks.


All times are GMT -4. The time now is 19:09.