3D Naca wing divergence
 

Hi you all guys,

I'm working on a 3D naca wing of 1.018 m chord length with 0º 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 36º 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!

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.

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!

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.

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.

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

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

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

what are the domain extents now?

Angle of attack is 0º.

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...

Flow is incompressible? Any effect after increasing domain size?

something wrong there
 

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

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

Have you managed to avoid the divergence? How?

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

Which node distribution have you made?

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!

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.

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

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

Fluent cas & dat

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:

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.

I was thinking of more smooth mesh. :) Here it is...

How are those curved edges made? Splines curves?

Blocking > Edit edge (s) > Link edge

Source edge : The edge whose shape you need to copy to other edge.

Target edge : Whose shape is to be changed

Factor : 1 -3 . I've used factor of 3

It works for me too! You're the man!

I've applied this same setup with k-epsilon Realizable model to the 3D flat plate case with 70º angle of attack I've been dealing with. It's working too! I think the key is the courant number modification.
How does it afect to increase it from default 200 to 20,000?

What is the different between slip zero shear stress wall and symmetry BC?

I'm using default k and epsilon at the inlet but I'm gonna need to modifiy them. Would this make me change the mesh or reducing even more under-relax factors?

For how long should I maintain the reduced under-relax factors? It's making my simulations pretty slow...

It is cournt number for pressure-based coupled solver which couples continuity and momentum equation only. So the definition is not same as the cournt number we study in CFD course.


Fluent guide says, you can increase it to 200,000 and it worked for me for transition modelling of low pressure turbine. In fact this model was used first time for the the low pressure turbine case (i can give you that paper which made use of Fluent's pressure based coupled solver) due to fact that there is strong coupling of continuty and momentum equation. And when Simple type algorithms are used (which couples pressure - velocity fields loosely) they introduce errors for this class of problems and make the convergence difficult.


Both are same except that you need plane surface aligned with any plane for symmetry condition while slip condition can be applied to any surface. In fact I use slip condition due to my past practice. Some friends here always use symmetry condition. But in my point of view results should be same.

Why you want to change them? Do you want to match some test conditions for which you have specific values of turbulence parameters. Any how , you dont need to change any thing.

For pressure based coupled solver, we don't have option for URF!

Yes, I need to match some test turbulence conditions.

In the solution controls panel there's the option to modify explicit relaxation factors for momentum and pressure and under-relaxation factors for density, body forces, k, epsilon and turbulent viscosity. I've reduced to half all that values. Once the solution is converging, can I change them to default without risking the convergence?
Can I change to 2nd order schemes for k and epsilon to get a more accurate solution?

Ah those parameters. You can play with them. Generally speaking, I use default values.


I don't think turbulence needs second order accuracy. If you are not modelling transition type of flows, results wont change much. In transition dominated flows, I have observed no separation at all when used first order turbulence discretization.

Just think, you have already averaged out the quantities and now you want to add the averaged change in mean flow due to turbulence. How accurate would be averaged quantities with 2nd order accuracy ;) . Probably you will get same averaged values :rolleyes:

Even if it's converging, CD and CL are far from their correct values. I guess I have to let the simulation run longer. The problem is it's too slow!
I'm simulating the transient case for the 70º inclined flat plate with adaptive timestepping from 1e-3 to 1e-6 but it's always take a timesetp between 1e-5 and 1e-6 s. I've put 50 iterations per timestep.
I need at least 1s of simulation and it taking 1 day to do 4e-4s...