Hello Everyone, I have a big problem with StarCD and I hope you can help me.

I'm using StarCD 3.22, and I have to simulate a transonic airfoil in a wind tunnel. The objective is to calculate lift and drag coefficients of the airfoil and compare them to wind tunnel experimental results (experimental results are: Cl=0.803; Cd=0.0168). My problem is that the mass doesn't converge, the mass residual stays high (about 3.e-1).

The airfoil is a RAE-2822, and the test conditions are:

Mach number at inlet: 0.73 Angle of Attack: 3.19 degrees Reynolds Number: 6.5e+6

From these data, and fixing a static temperature of 300K, I can obtain the following values (using the definition of Reynolds number, the equation of state for ideal gases and the isoentropic correlations between static values, stagnation values and Mach Number):

Stagnation Temperature: 331.974K Velocity Magnitude: 252.770738m/s Density: 0.469604kg/m^3 Static Pressure: 40449.81Pa Stagnation Pressure: 57657.57Pa K(inlet)=3/2*I^2*V^2=1.5*0.02^2*252.770738^2= 38.33583 Epsilon(inlet)=Cmu^(3/4)*K(inlet)^(3/2)/1= 39.0022

The walls of the wind tunnel are at a distance of +-20 chords in y direction, 10 chords in â€"x direction, 30 chords in +x direction.

I did the mesh with a macro written by me and the mesh around the airfoil is in this picture (click to enlarge):





There is about a total 100000 cells in the grid. As you noticed, I inclined the wind tunnel 3.19 degrees, so I calculated appropriate director cosines for boundaries definition. I applied Symmetry Boundaries (it's a 2d simulation), a Stagnation Boundaries (for the cells at the beginning of the wind tunnel, as an inlet boundary) and Pressure Boundary (for the cells at the end of the wind tunnel, as an outlet boundary), shown in this picture:



The settings of the boundaries are in these pictures:





I used manual initialization, initializing U=250; V=15; p=100000; T=300; K=K(inlet); Epsilon=Epsilon(inlet).

I use a pseudo-transient algorithm (SIMPISO) with 1.e-5 time step, and default relaxation factors. Differencing schemes are Upwind for all, but for density I use CD with 0.01 blending factor (that is, 1 percent of CD and the rest Upwind). Obviously I set density as Ideal-f(T,p). The residuals are shown in this figure, you can see that it simply doesn't converge!



Any suggestions? Is the grid ok or I have to redesign it? All suggestions are welcome, I tried almost everything but nothing worked for me.

Thanks

You should use STAR-CCM+. STAR-CCM+ has a coupled solver which is better for solving high Mach number problems where there is a strong coupling of the density and velocity fields.

Thak you for your answer.

Unfortunately I can only use this software and this release, because it's for an university exam, so we can't choose the software to use. We have to deal with this.

Is there any trick or something that could help? I tried initializing different speeds and pressures manually, but there is always a residual that is asintotic to an high value (about 10^-1). The required residual is at least 10^-3. I also tried starting with SIMPISO and after 20 iterations switching to SIMPLE (steady-state) or increasing the time step length to speed up convergence, nothing worked.. I read about lowering the relaxation factor of pressures down to 0.001 but didn't worked.. This simulation is driving me crazy!

Run it transient.

What about the results if you ignore the convergence.

What is your Cl like, this seems to be what you are interested in and you haven't mentioned how accurate that is and how stable it is? The mass convergence could be missleading, always keep an eye on what the simulation is trying to achieve, residuals are a good indicator of convergence but not the be all and end all.

What does the flowfield look like? Any possible signs of vortex sheding? What is the y+ on the wall, why are you only using first order differencing?

Sorry for all the questions but in reality residuals tell us very little about what is going wrong, just that something is (maybe)

Thanks for all your answers.

@ William Blake: if I ignore convergence the wind tunnel is something like "stratified" in the x direction, all vertical sections have very different mach numbers (actually, looking at the mach number plot in Star is something like watching a vertical peace flagship...), and on the airfoil I have something that is similar to an oblique shock wave in the shape, starting from the nose of the airfoil. This happens when I run it in pseudo-transient (SIMPISO), do you mean I should try to run with PISO?

@Ben: my Cl is very low, actually it's the first thing I check when I stop the simulation. It ranges from 0.3 to a 0.6, so it's lower than the 0.8 it should be. I used first order differencing (upwind) because it basically takes the value of the upwind cell and fills the flowfield with inlet conditions very fast (our techer suggested to start with upwind and then, when negative densities problem is no more a threat, restart with an higher order scheme).My y+ is between 37.85 and 213.0, so I used an high reynolds turb model (k-w/SST/High Reynolds), you can see the y+ here:



Actually, the best result I obtained in terms of residuals and "watch inspection" is surprisingly with SIMPLE (steady state), with very low relaxations (U-mom,V-mom = 0.15; pressure = 0.005; k-w 0 0.5; temp = 0.4), with density blending factor at 1.e-3, reference pressure set at 0 on a cell at the end of the wind tunnel, and using MARS as differencing scheme, with these settings I obtained residuals all lower than 10-4 with the exception of the mass that stabilized at 3.e-4... residuals are all ok but the cl is only 0.45 and the mach number is below 1 on the top surface and this isn't ok as a shock wave should be there. Here are my best results (extrusion on the z direction is 1 chord):





I'm seriously thinking it's a problem of this mesh

I would recommend to use other boundary condition so that the flow field is similar to what you expect with pressue and stagnation boundaries. After convergence make a field restart with your boundary conditions. This approach helps for many many problems!

I recomend try:

1) relaxations u,v,w =0.7 ; p = 0.005 and other default

if it is not help try other turbelence model (k-e HiRe)

And if it is not help try refine mesh and use k-e Hybrid, or LowRe turbulence model (y+=0.1...5)

Try it

Yes, you should run it transient with PISO.

Why do you use stagnation BC? I think combination Inlet+Pressure is good for this simulation. The second: you can see the 1-st Q-NET WorkShop (http://www.qnet-cfd.net). They test some turbulent models for transonic flow around aurfoil and wing and they said, SST and nonlinear k-e models are the best in this case. But you can use lowRe SST. HighRe SST gives bad result for shock wave.

Sorry for my English