Hi Fluent User´s I write to you to know if someone can help me because I have been running fluent and after the set up fluent shows me the folowing Turbulent viscosity Limited to viscosity Ratio 1.000 000e+005 in (Nº) cell Could you please Anybody answer me what does mean?

Thank you so much Adrian

The default solver limit on viscosity ratio is 10,000. What that message means is that Fluent calculated a viscosity ratio in X number of cells that exceeded the set limit and capped it to the given limit value. The limit on viscosity ratio can be changed in your solver settings; I usually use a number on the order of 1e6.

absolutely right!john S.

Hi! I think that in general is better (but depends on the case) not to modify the default value of VTR. You can try to change the model of turbulence, which model of turbulence are you using? and what range of velocity field have you got? Are there big differences on velocities depending on the zone or do you have big recirculation zones? xavi

Xavarin, I too get this warning sign. My flow has few low and high pressure zones, and velocity varies from 1 m/s to 200 m/s in the flow domain. Any help in setting up any turbulence model or any help in getting this simulated correctly?

Im working with cars AT 60 m/s of velocity and K-Epsilon model with std configuration and 2000000 of cells and first order upwind so when I try change to second orden to better accuracy fluent shows me turbulent viscosity limited to viscosity ratio if anybody caa give me an advice I will thank greetings Adrian

Hi John and Adrian, I had similar problems with multiphase flow in a tank, with a big range of Reynolds Numbers (and velocities) and tried K-E RNG and performed very well, the VTR was stabilized...this is because k-E RNG performs very well when you have very different Reynolds numbers in the domain..try this!! I guess should work although sometimes this VTR message error could be due to other causes.... best luck!! Xavarin

start with good intial guess for k, and eps.

If you starting with default values of fluent you are likely to get this warning if mesh size is large.

small value for k, (that is low turbulence) and high for eps or omega.

I usually start with k = 0.0001, eps or omega = 5 or 50 whatever you like as long as higher much higher than k.

Hi all! I have been working on multiphase modeling. I have the same problem when I use the per-phase k-epsilon multiphase model. I tried to increase the limit of turbulent viscosity ratio to 1e6, 1e7 and 1e8, but this problem still occured. So could you please help me to solve this problem?

Hi mates I would like to know in which part of fluent set up must I to put this K - Epsilon values? and why yours values that advice me are they so diferent ? beside what turbulence model is better for cars? I mean k - Eps or S.Allmaras ? Thank you all and I hope to help in another issue to you all

greetings

Adrian

Hi,

I may suggest to do what the other people suggested. That is by changing the turbulence model or use of the same model after increasing the number of cell points. You also can try techniques like increasing the velocity at different steps staring from a low velocity.

Best wishes

[Deside]

Originally Posted by Adrian
;153766

Hi mates I would like to know in which part of fluent set up must I to put this K - Epsilon values? and why yours values that advice me are they so diferent ? beside what turbulence model is better for cars? I mean k - Eps or S.Allmaras ? Thank you all and I hope to help in another issue to you all

greetings

Adrian

The K - Epsilon values are set up under Solution > solution initialization