Turbulent viscosity limited issue
 

Hello,
I am new to Ansys Fluent and tried to set up a simple simulation, where water flows through a round 300mm long pipe with s radius of 50mm.
For starting I selected a Pressure-based Steady State simulation without gravity.

I always get the warning: Turbulent Viscosity limited to viscosity ratio of 1e5 in 630900 cells, which shouldnt be possible with my model.

For models I did activate Energy Equations and the Viscosity model: K-Omega SST. Everything else is turned off.

As Fluid I choose liquid water.

My Inlet is a pressure Inlet and my outlet is a pressure outlet (Had the same issue with a (velocity inlet/outflow). As the pressure in the inlet and outlet i tried different setting. I even have the issue, when I have absolutly no movement (same pressure in the inlet as in the outlet). For now I take 1bar as Inlet and 0.95bar as outlet)

Dynamic Mesh is turned off.

The reference values are from the inlet. with 1bar Pressure and and 0m/s as default.

My solution Methods are :
Scheme: Coupled
Gradient: Least square Cell Based
Pressure: Second Order
Momentum: Second Order Upwind
Tke: 3rd Order MUSL
Sdr: 2nd Order Upwind
Energy: 2nd Order Upwind

Solution Controls are the default ones.

When I initialize my solution now with the hybrid Initialization I get the warning: Turbulent Viscosity limited to viscosity ratio of 1e5 in 630900 cells.

When I run the simulation it doesnt get much better. I sometimes get the warning: Reversed flow on outlet.

I guess my initial values are horrible or my viscosity model is wrong. I get better results with k-epsilon. But I guess it is only, because k-epsilon isnt good at calculating near wall turbulence.

Any suggestions?

Best regards,

FFD

Did you check the BC's for the turbulence parameters?

You should provide good guesses for the turbulent intensity at the inlet.

Also try the standard initalization after you double checked BC's, just to see if it's any different. What is the mesh check giving you?

Check your boundary conditions for the turbulence, the k and omega or the k and the epsilon. The default user input is a turbulence intensity and a length scale and people rarely put in meaningful values for these.

The initial condition is also important. Do a standard initialization instead of a hybrid one.

Thank you for the answers. I will try it today and tell about the outcome. I just wanted to add some infos:
- I checked the Wall y+ condition and I can see that my y+ is partly over 1000
- Also I realised that the simulations runs perfectly fine when I choose air as fluid material insstead of water..

Ok. So I checked everything now:
The Turbulence parameters are:
In the BC (inlet and outlet)
Tke: 1m^2/s^2
Sdr: 1 1/s
both are constant.

Under Solution Controls I didnt changed anything. But the Under Relaxation Factors are:
Density: 1
Body Forces: 1
Tke: 0.8
Sdr: 0.8
Turbulent Viscosity: 1
Energy: 1

The standart initialization had the same issue:
As Gauge Pascal I choose the Inlet value of 1bar.
X and Y velocity are 0 m/s (which is correct in my model)
Z Velocity is around 2m/s
Tke and Sdr are 1
and the Temperature is 300K.

The Mesh Check gives me the following warning:
WARNING: The mesh contains high aspect ratio quadrilateral,
hexahedral, or polyhedral cells.
The default algorithm used to compute the wall
distance required by the turbulence models might
produce wrong results in these cells.
Please inspect the wall distance by displaying the
contours of the 'Cell Wall Distance' at the
boundaries. If you observe any irregularities we
recommend the use of an alternative algorithm to
correct the wall distance.
Please select /solve/initialize/repair-wall-distance
using the text user interface to switch to the
alternative algorithm.
Maybe an additional information:
I use Hypermesh for creating the Mesh with a CFD TetraMesh. Hypermesh than generates me a .cas file for FLUENT.
It seems that my Mesh isnt optimal. But it is well refined. What should I do while meshing?

Did you leave the default parameters for Turbulence BC?

You need to make sure that these values are plausible. You can also switch the specification method to "Intensity and hydraulic diameter" make a good assumption about intensity and set the diameter at the inlet. I usually do this, because i'm to lazy to caculate the actual values for k and omega.

For your mesh: Yeah, usually not good when FLUENT is complaining about the mesh. Problem seems that your turbulent viscosity ratio is limited in all cells (true?) so there seems to be a problem involving also good cells, not just the bad ones..

A tke of 1 is pretty high, this number is usuallly ~0.5
A Sdr of 1 is also super low. This number is usually O(1000)

The simulation runs fine for water and not air because for one fluid the values are meaningful and the other, not.

Hello,
I solved the issue. It actually was the Tke and sdr.I just calculated it. The Tke was about 0.003 and the sdr about 160. So there were huge differences. Now it runs stable. Thank you very much for the help.

Did you import mesh from hypermesh to fluent?
I am facing similar problems.

Shrirang

hi, I know the post is old, but I got a similar problem. How did you calculate it exactly ?