[Rick]

Hi Everyone,

I am trying to simulate water flow around a valve. To model valve closure I need to use a gap model to avoid splitting the fluid computational domain when the valve is fully closed. The problem is that around the location where the gap model is used the turbulence viscosity ratio increases a lot and I get the warning message below that persists during the valve closure time. My question is that can I trust the results during the time intervals in which I am getting this warning message? The turbulence model is K-Omega SST (transition is modeled using the gamma-transport equation.

Warning message:
"turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 335234 cells"

Many thank in advance

[shereez234]

Possibly this has either to do with either
a)your flow boundary conditions - inaccurate levels of turbulence for k and omega in the free stream.

b) with your mesh having large anisotropic high aspect ratio cells with low cell skewness or orthogonality.

More specifically abnormal gradients are being created due to low cell quality.
Could you double check your mesh quality and free stream turbulence?

[Rick]

Dear shereez234,

Thanks for your help and for letting me know about the mechanism that causes such problems!

I performed mesh quality evaluation in Fluent. Here are the results:

----------------------------------------------------------------------------
Mesh Quality:

Minimum Orthogonal Quality = 1.61579e-01 cell 18808 on zone 2 (ID: 766474 on partition: 11) at location ( 8.30393e-03, 3.22117e-02, -1.36920e-02)

Maximum Aspect Ratio = 2.18969e+01 cell 41211 on zone 2 (ID: 220672 on partition: 6) at location (-5.59163e-03, 2.09249e-02, 3.77195e-03)
----------------------------------------------------------------------------

I don't think the mesh quality is an issue here because if I perform the same simulation without the gap model, this warning message goes away after a few time steps.

a)your flow boundary conditions - inaccurate levels of turbulence for k and omega in the free stream.

I calculated the turbulence intensity and length scale based one the instructions given on the web page below. I also tested the effects of different values for these parameters and can confirm that they have no effects.

https://www.afs.enea.it/project/nept...ug/node238.htm

[shereez234]

Yes, your mesh quality and freestream looks good, I was just double checking,
I am sorry I don't understand what the Gap Model is. Do you have any pictures? Are you using any kind of deforming mesh? You might also want to low under-relax your turbulence viscosity parameter !

[Rick]

Hi shereez234,

Your help is greatly appreciated. I understood important points from your posts.

Lowering the URF for turbulence viscosity may solve the problem. I need time to test it.

Thank you again!

[LoGaL]

If the simulation is not converged, there's no reason to worry about backflow or limited turbulent viscosity. The problem is that it is not converged, and this is causing all the other things. I do not think lowering the URF will fix the issue.

[Rick]

Dear Lorenzo,

Thanks for the reply. I think the simulation converges. The residuals for all equations (including the turbulence model equations) except that of the continuity get lower than 1e-05 easily. However, the continuity equation's residuals remain high (between 0.001 and 100). I searched the forum for this and found that the continuity equation residual is calculated using a different approach and depends on the residual at the fifth iteration, which depends on the initial values. So, if my initial values are close to the converged values, then the residuals remain high. Please correct me if I am wrong.

To ensure that the simulation is converged, I plot the volume-averaged values of velocity and pressure in the computational domain and check if their values get plateaued by increasing the number of iterations in each time step.

As I said, the high turbulent viscosity ratio warning message persists when the gap model is activated. It goes away if I disable the gap model.

[LoGaL]

Nono believe me, unless you are initializing the flow field from a previous simulation ( and I bet you are using hybrid initialization or the solution without the gap instead ), the continuity residual should drop a lot. If it got stuck at 0.001 your simulation is not converged.

To check convergence, i wouldn't plot volume average quantities, but local ones at a point. Volume average tend to smooth oscillations, especially if the flow is stable in a zone but not stable in another. Also, some look at the flow field ( e.g. velocity contours) is normally enough.. If you see weird vortices or flares, usually the steady RANS is not converged, and it maybe it will never do it.

[Rick]

Thanks for letting me know about the local values monitoring and the velocity contours. Very good idea!

I plotted the instantaneous velocity contours on a couple of mid-planes and can confirm that despite having a residual of 60! the velocity contours do not experience any variations after the 15th iteration out of 25 allowed iterations in each time step.

[LoGaL]

Oh it’s unsteady solver already? For which reason by the way?

[shereez234]

I agree with Lorenzo that lowering the URF value is not the best solution. However, sometimes, when you lower your URF in the initial 100 iterations or so, the solution can go towards convergence rather than divergence. You can increase URF from this point again (after the initial transient).

I believe at this point we will need more details about the simulation to help more. Can you please describe your simulation details? Turbulence model, unsteady time step size, whether you are using an explicit time stepping, implicit time stepping.

If you can show a) some screenshots of your mesh (which I asked before if it is a dynamic moving mesh?) and b) screenshot of simulation residuals.

ps: the continuity equation residual also depends on the approach you are using, SIMPLE, SIMPLEC, PISO, Coupled etc .... Loosely speaking I believe the continuity equation here refers to the pressure correction/pressure Laplace equation dependent on the momentum equation matrix A in the SIMPLE/C/R and PISO algorithm. Correct me if I am wrong.

[Rick]

Hi Lorenzo,

Yes. It is. Since the inlet and outlet pressure profiles are time-dependent and we want to simulate a transient problem, not a steady one.

[Rick]

Hi shereez234,

Thank you for your help. I am not allowed to show the entire mesh, but I will present zoomed-in pictures of different locations in the computational domain.