Modelling turbulent flow

[martijn]

I have a 2D model of a pipe with an obstruction in it. I am simulating air flow in this structure and would like to see turbulent flow. The pipe width is 5cm, and the average flow speed varies from 0.2 to 10m/s. The Lowest Reynolds number is 684, the highest 34000.
My expectations:
Re < 2500: laminar flow before and after the obstruction
2500 < Re < 4000: laminar flow before, turbulent after the obstruction
Re > 4000: turbulent flow before and after the obstruction.
However: the flow profile just seems to scale with the incident flow speed.
I know the simulation volume is too small to achieve a fully developed flow profile, but my observations are the same for a longer tube. Moreover, in the obstruction the flow speed should certainly be turbulent.
The simulation is steady state, so I a assume that the averaged values of a turbulent flow will be calculated, but then I would still expect that the boundary layer would get thinner for higher Re numbers.

I attached a number of velocity profiles (absolute value). The relevant parts of the SIF file are below

Summarising: Why don't I see any sign of turbulence?

Martijn


SIF file:
Body 1
Target Bodies(1) = 1
Name = "Body 1"
Equation = 1
Material = 1
End

Solver 1
Equation = Navier-Stokes
Procedure = "FlowSolve" "FlowSolver"
Variable = Flow Solution[Velocity:2 Pressure:1]
Exec Solver = Always
Stabilize = True
Bubbles = False
Lumped Mass Matrix = False
Optimize Bandwidth = True
Steady State Convergence Tolerance = 1.0e-5
Nonlinear System Convergence Tolerance = 1.0e-8
Nonlinear System Max Iterations = 25
Nonlinear System Newton After Iterations = 25
Nonlinear System Newton After Tolerance = 1.0e-5
Nonlinear System Relaxation Factor = 1
Linear System Solver = Iterative
Linear System Iterative Method = BiCGStab
Linear System Max Iterations = 500
Linear System Convergence Tolerance = 1.0e-8
Linear System Preconditioning = ILU0
Linear System ILUT Tolerance = 1.0e-3
Linear System Abort Not Converged = False
Linear System Residual Output = 1
Linear System Precondition Recompute = 1
End

Equation 1
Name = "Equation 1"
NS Convect = False
Active Solvers(1) = 1
End

Material 1
Name = "Air (room temperature)"
Viscosity = 1.983e-5
Heat Conductivity = 0.0257
Heat Capacity = 1005.0
Density = 1.205
Compressibility Model = Incompressible
Viscosity = 1.983e-5
Sound speed = 343.0
Heat expansion Coefficient = 3.43e-3
End

Boundary Condition 1
Target Boundaries(1) = 17
Name = "noslip"
Noslip wall BC = True
End

Boundary Condition 2
Target Boundaries(1) = 1
Name = "noslip"
Noslip wall BC = True
End

Boundary Condition 3
Target Boundaries(1) = 21
Name = "noslip"
Noslip wall BC = True
End

Boundary Condition 4
Target Boundaries(1) = 5
Name = "noslip"
Noslip wall BC = True
End

Boundary Condition 5
Target Boundaries(1) = 25
Name = "speed in"
Velocity 1 = 5
End

Boundary Condition 6
Target Boundaries(1) = 26
Name = "noslip"
Noslip wall BC = True
End

Boundary Condition 7
Target Boundaries(1) = 9
Name = "noslip"
Noslip wall BC = True
End

Boundary Condition 8
Target Boundaries(1) = 30
Name = "pressure out"
External Pressure = 0
End

Boundary Condition 9
Target Boundaries(1) = 13
Name = "noslip"
Noslip wall BC = True
End

[tzwinger]

Martijn,
I am astonished that you get convergence at all, especially with the higher Re-numbers.

perhaps you could take 2 measures:
1) switch in a turbulence model (k-epsilon, for instance)
2) try to resolve (I do not know how fine your mesh is now) finer around the cylinders

And finally, some effects (like von Karman vortices) I guess are rather of transient nature - so perhaps a transient run would also be something you might consider worth trying.

Best wishes,

Thomas

[raback]

Hi Martijn,

There is no automatic turbulence model that would come into the play. As Thomas suggests one way to see some effects of turbulence would be to solve all the time-scales (if the mesh is dense enough) and take a time-average of it. See, for example the tutorial on Vortex shedding. Averaged data could be obtained with the FilterTimeSeries solver (see Models Manual). Even the normal stabilization can be understood as some sort of LES model, but if you're really into this, you could try the a novel vms (Variational Multiscale) method for stabilization and use 2nd order elements. LES needs a denser meshes compared to RANS models but I presume that with these rather low Re numbers you could probably still use the LES style of approach. The method of preference will also depend on the nature of your study.

-Peter