Hi all,

i'm running a 3-D simple pipe bifurcation with Fluent 6 and having a problem with the solution converging.

i've used this geometry in laminar flow and turbulent intersection but this turbulent bifurcation won't play ball.

i'm using standard k-epsilon and every so often i get a message saying, "turbulent viscosity ratio limited to 1e5 in 1 faces" and then the residuals for k and epsilon rise. this happens repeatedly and they never fall below 1e-1.

any ideas anyone???

Thanks

Richard.

Go thorugh this forum (Search) for posts related to this error. There are quite a few tips and pointers.

Usually this problem happens when the grid is too coarse in some part of the domain, or if your discretization scheme is not accurate enough.

Try increasing the grid density where the turbulent viscosity ratio is high and to use a higher order discretization scheme.

Best regards,

ap

usually what you said is correct, but sometimes it just work this way, i recently did one calculation on a very fine mesh (around 3.3 million cells) and wall yplus is as low as 0.6 in sensetive areas, when i do steady calculaton fluent does not give any warning, well with the same mesh for unsteady flow the solver always keep on giving warning about viscosity (i can't afford to make the mesh more fine now, its already too fine)

this was with version 6.2, and with version 6.1.22, for the same calculations, even for mesh as coarse as 1 million cells solver do not give any warning, steady or unsteady case (i mean for both the solvers i am keeping the geomtery and boundary conditions same, only mesh change ...and irony is the mesh i am using is supposed to be better as mostly it is prismatic or hexa mesh, instead of all tets for earlier)

If you're using wall functions, a value of 0.6 for y+ is too small.

The suggested values are 30 < y+ < 60 for wall functions, while if you use the enhanced wall treatment y+ should be around 1 (which seems your case).

Best regards,

ap

Hi ap,

You can certainly throw some light on my problem. I am simulating gas-solid flow in a riser using Eulerian-kinetic theory-granular model. I solve fluid flow eqns + vol fraction + gran temp eqn. Use second order scheme for all except for vol fraction where i use first order(would QUICK be benificial here?).

Initially i solved gas phase only turnig off vol fraction and gran temp. Everything is fine.

Now, when started solid flow calculation, the 'Viscosity ratio limit' warning came. Initially it came for gas phase turbulent viscosity limit. Slowly it disappeared. Then again the warning started coming but observed that it was for solid phase viscosity limit. Ofcourse, i use per phase std k-eps model.

I checked the area of problem. It is near the solid inlet region which is from two sides(2D geometry), same as Arastoopour considerred.

I have run around 700 time steps for solids with 0.0005 s timesteps. Warning still seems to be coming. I'm not sure if I should continue the simulation or should stop and check for the problem.

I think that, Fluent allows us to set this limit to avoid the instability of the calculation. But I fear if it would lead to the wrong solution. it takes long time getting results.

Thanks for you time and help.

-US

The QUICK scheme is only beneficial if you're using a hex grid aligned with your flow. In other cases it's just second order accurate.

However, you can use second order upwind. FLUENT 6.2 hides it (I don't know why) for volume fraction in the Eulerian model. You can still use it however enabling it through the text command line.

Type solve->set->expert and answer yes when FLUENT asks you if you want to use all existing discretization schemes. You'll find second order upwind in the drop down list also for the volume fraction.

The turbulent viscosity ratio limitation is a great problem with FLUENT Eulerian gas-solid flows simulations. It's related to the underestimation of the solid phase viscosity by the kinetic theory and I wasn't able to completely solve it.

The problem is more evident if you use the algebraic equation for the granular temperature (the only one available in FLUENT 6.0 and 6.1), while it becomes less evident if you switch to the PDE (only FLUENT 6.2).

I simulated the Arastoopour (actually the riser is of Knowlton et al. (1995)) riser too for my thesis of degree. I was able to reproduce the Arastoopour simulation and I obtained similar results using the k-eps model. However the problem with the viscosity limitation always appears.

I tried to increase the limitation, but this didn't solve the problem.

P.S. I advise you that the solution of adopting two lateral inlets for the riser, instead of simulating it in 3D brings to bad results, as Arastoopour stated too. The shape of the solid volume fraction radial profiles is definitely wrong. In 3D, with much more computational time, you'd obtain good results.

Best regards,

ap