Hi Can any body suggest me about the setting of reynolds number.I am able to simulate the flow upto Re 1600 quite nicely.But at Re 1700 solver gives an error "Reynolds number outside the range selected for turbulence model........" and the solution did not converge below 10^-4. Does anyone know that this error will affect my solution or not?

Manu

Hi Manu,

This is simply a warning, not an error. At higher Reynolds numbers the flow is typically turbulent and the warning is simply to alert you to the fact that a laminar solution may not be appropriate.

Note that the solver does not know what the relevant length and velocity scales are for your application. The Reynolds number reported by the solver is simply an estimate based on the global lenght (by taking the cube root of the volume) and velocity (by taking the RMS average velocity) scale. Your turbulence model selection may still be appropriate.

That said, your convergence problems may be arising from instability in the flow. Turbulence models typically increase the effective viscosity (by adding a turbulent viscosity component due to turbulent transport of momentum) and will stabilize the solution. You will often find that a laminar solution becomes unstable as the Reynolds Number increases.

Have a look at where the convergence problems are occurring by including the residuals in your backup or res file and review your model to determine whether laminar flow is a reasonable approximation.

Regards, Robin

Hi Robin, Thanks for your explaination.By the wayyou mean to say: 1)Above Re 1500 the laminar solution is not stable and i shud use some turbulence model to get it stablized.Is it a good idea to use turbulence model for laminar flow?

2)How can i check the convergence problem of my solution ?Where the problem actually coming in?Can you please write little more on this.

Thanks and Regards

Kirti

Hi Kirti,

That's not quite what I meant. If the Reynolds number is large, there may not be a "steady" laminar solution due to flow instability. This instability is what develops into turbulent flow later on, but it may not be turbulent in your range. YOU need to decide whether the flow is turbulent and use an appropriate model. The solver is just warning you to consider this.

Regards, Robin

Sorry, forgot your second question.

As I said in my previous post, turn on the output of residuals. You can do this in the Output Control section in Pre. With this enabled, you will be able to view the residuals in Post as a variable field. Search the forum for more posts on this topic.

Regards, Robin