Hi there,

If a flow is turbulent in nature, should its simulation converge with laminar model?

Kindly guide.

Many Thanks,

Best Regards, KM

Numerically speaking, there ought to be no problem. However, you won't resolve the "proper" physics.

D.

Hi KM and Deke,

Actually, numerically there are a lot of issues for both convergence and accuracy. If the flow should be turbulent, you'll be trading off one for the other by running laminar. Here's why...

Turbulence results when the diffusive transport of momentum is much smaller than the advective transport of momentum and is no longer sufficient to damp out fluctuations (The ratio of advective to diffusive transport is the Reynolds Number).

If the Reynolds number is high, the solver will not converge as the solution will be locally unstable. A turbulence model resolves this issue by adding a turbulent Eddy Viscosity (which is representative of the mixing due to turbulent effects) to the Dynamic Viscosity (which is a fluid property arising from molecular interaction), resulting in a higher Effective Viscosity, which varies according to the flowfield. The higher effective viscosity lowers the effective Reynolds number and therefore stabilizes the flow. In some cases numerical instability can still arise if the local eddy viscosity is insufficient to lower the effective Reynolds number.

That said, you may still be able to converge a higher Reynolds number laminar steady state solution without turbulence. If you mesh is coarse (and further if you use 1st order upwind advection), there will be sufficient numerical diffusion (due to errors, not physics) to stabilize the flow. The problem with this is that the numerical diffusion has nothing to do with the physics, so the effective viscosity is grid dependant, not solution dependant. The same occurs for turbulent flows, of course, but the numerical diffusion is likely to be small compared to the eddy viscosity (as opposed to large vs. the dynamic viscosity).

So, in summary, the effective viscosity is:

Effective Viscosity = Dynamic Visc. + Eddy Visc. + [numerical diffusion]

Where the numerical diffusion isn't actually calculated by the solver, but rather results from numerical errors due to discretization.

The local flow will be stable if the Effective Viscosity is high enough to damp out fluctuations. The accuracy of the Dynamic Viscosity is dependant on your fluid properties, the accuracy of the Eddy Viscosity depends on the turbulence model, and the Numerical Diffusion should be minimized by refining your grid and using a higher order advection scheme.

Hope this helps!

-CycLone

[Derick]

Hi

Can someone please explain what happens when you use a laminar physics model when the Reynolds number is high? I'm trying to find out what happens when I use a laminar physics model to simulate the flow through a U-bend with a Reynolds number of 10,000. The U-bend diameter is 20 mm.

[karachun]

You get Laminar parabolic velocity distribution across channel instead of turbulent core velocity distribution.


https://en.wikipedia.org/wiki/Law_of_the_wall
In general you achieve wrong resistance of U-bend because both friction and shape losses are Reynolds dependent.

[ghorrocks]

Sorry, Karachun, that is not correct. Give it a try and you will see what happens - you will not get a laminar parabolic profile. It is not stable and will not converge (not unless your mesh is vastly under-resolved, and then you will just get an inaccurate simulation).

What you will get is a transient, fluctuating flow field. If you refine the mesh enough that the simulation becomes DNS or LES-like you will get the turbulent flow profile after temporal averaging (which is unlikely, you need super-fine meshes for these). What is more likely is you get an under-mesh-resolved LES like simulation with a velocity profile approaching the turbulent profile but not accurately. The finer the mesh the more accurate it will be. Note that you cannot do this as a steady state simulation, you will need a transient simulation.

[karachun]

Thanks for comment, I will try to model this problem later.

[Antanas]

Originally Posted by Derick

Hi

Can someone please explain what happens when you use a laminar physics model when the Reynolds number is high? I'm trying to find out what happens when I use a laminar physics model to simulate the flow through a U-bend with a Reynolds number of 10,000. The U-bend diameter is 20 mm.

If I'm not mistaken, when you use the Laminar model in CFX it solves Navier-Stokes equations, not RANS. So if your flow is actually turbulent, only those turbulent scales will be accounted for that are larger than the mesh size, because no subgrid modeling is involved. So unless your mesh is fine enough you may get a worse result than with RANS + Turbulence model.