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 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 komega 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 underrelaxation 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 1e8s the same is happening. I've also tried the underrelax factors reduction with same results. I've also tried the laminar case and kepsilon 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 ydirection? 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 nonzero angleofattack. 
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.

Quote:
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.

Quote:
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 underrelaxation factors and if it doesn't work I'll try a more viscous fluid. 
Quote:

1 Attachment(s)
Reduced underrelax factor haven't worked for the steady kom 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? 
Quote:
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.

Quote:
Maybe it takes longer to reach divergence with the larger domain. Quote:

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 
Quote:
Quote:
Would you mind passing me that mesh files to see how each node distribution is? Thanks a lot Far! 
1 Attachment(s)
Please make the domain at least 1015 upstream and 2030 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. 
.......................................


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:
Gradient: Least Squares cell based or GreenGauss cell/node based? How relevant is this? Pressure: 2nd order is more suitable than PRESTO! scheme? Momentum: 2nd order rather than Quick or Powerlaw? Thanks. 
All times are GMT 4. The time now is 07:57. 