[aliamini]

Hi
It's my first post in this Forum.
I try to solve a problem in fluent. The problem is a steady state water flow in a chamber with one inlet and one outlet. The radius of this chamber is ten times bigger than inlet and outlet parts. of course inlet of this chamber has some intricacies that causes difficulties.
after different kinds of methods and initial conditions and checking the geometry this warning is still showing.
warning :

"reversed flow in 77 faces on outflow 12.
turbulent viscosity limited to viscosity ratio of 1.000000e+005 in 138423 cells."

This is very interesting that in all conditions and iterations, finally I reach to a constant numbers in the error text. that are 77 faces on outflow and 138423 cells limited viscosity ratio. and after about 50 iterations these numbers remain constant even after 1000 iterations.
Thank you for your help.

[-mAx-]

switch outflow with pressure-outlet
*reversed flow indicates that you have an vertex at your outlet
*turbulent viscosity warning is basicaly a problem of turbulence setting and/or mesh issue (skewness)

[aliamini]

But naturally the vortex should not happen.
I examined your suggestion about pressure outlet but warnings is still showing with larger numbers of faces involve.
after 1000 iterations with these warnings I checked the contour plot of pressure and velocity. I don't know why a big part of my domain in the middle of chamber don't have any contour value and remained dark.( inlet and outlet of domain have contour values.)
I don't know what it means and what should I do to convergence.
thanks a lot for your answers.

[-mAx-]

Warnings can occure at the begining of the computation, as the solution isn't converged.
The number of cells involved in the warning may decrease and the warning should disappear.
Post a picture of the contour, you described...

[aliamini]

http://xs540.xs.to/xs540/09264/velocity_contour734.jpg
http://xs540.xs.to/xs540/09264/pressure_contour246.jpg

These are velocity and pressure contours.
inlet is in the bottom and outlet is in the top.
As you see the big fraction of both contours are empty.
and afetr some iterations it seems that the condition of converging doesn't change and all the residuals and faces that have reverse flow remain constant.

[-mAx-]

create planes in your domain (sweep / surface)
and check if you still have this phenomenon.
Check also the mass conservation between inlet and outlet (report/fluxes/mass-flow-rate)

[aliamini]

I checked sweep planes but the problem has remained.
a big part of domain doesn't have value in contour plot.
mass flow rate is OK.
further I found that I had forgotten to scale my domain to millimeter.
after this correction the problem of limited viscosity ratio solved and my solution converged. but the problem of reversed flow remained unsolved and when I checked the sweep planes and contour plots, a big big part of my domain remains dark and without any value
what does it mean?
even after conversion I have many faces with reverse flow and a big part of my domain doesn't have any value.

[-mAx-]

Is your model well meshed inside?
If you create a plane in the middle of your domain, can you see cells where you get no data?
If you create path lines from inlet, do you have lines where you get no data?

[aliamini]

http://xs.to/xs.php?h=xs940&d=09264&...elocity450.jpg
http://xs.to/xs.php?h=xs940&d=09264&...ressure744.jpg
http://xs.to/xs.php?h=xs940&d=09264&f=path_line914.jpg

These are the pictures that you suggest.
unfortunately I think I have many cells that have no data.
I think this solution thinks that it doesn't need to fill the chamber.
but I think in experiment surely in steady state condition, chamber must be full of water.

[-mAx-]

pathlines seem to be ok.
The warning about reversed flow is link with your short outlet. You may extend it.
Check you mesh (in Gambit?) if the region in the middle is connected with the other region

[aliamini]

How can I check the connection of my mesh in gambit?
In the Gambit,first I meshed some faces and then meshed my volume.
In Fluent I checked it and understood that I have grids in all part of volume. but about connection I don't know how can I check it.

[-mAx-]

if you only have one volume, then you don't have any connection's problem
Else in gambit, click on the icon with the magnifying glass. The interface between connected volumes should be pink

[aliamini]

I have only one volume so what's the problem about cells that don't have any data?
Maybe in the solution their velocity should be zero. on the other hand actually they are motionless and don't influence the solution.
What do you think?

[-mAx-]

re-plot the contour of velocity, disable the autoscale option.
Set the min to 0 and the max to 1m/s
Enable the "filled" option.
et re-post the pictures.
It should show the low velocity distribution in the middle of your domain.
You may adjust the max velocity in the scale, to capture the distribution.
If you see an discontinuity, then you have a problem.
If not, then it should be ok (but I don't know anything from what you want to compute)

[aliamini]

http://xs.to/xs.php?h=xs840&d=09266&..._scaled257.jpg

Hi
your thought was true. This model doesn't have any problem. only the scale of contour causes this misunderstanding. My goal is velocity profile in outlet and I wanted to be sure that my model is physically realistic.
Thanks a lot for your answers.

[itsme_kit]

Originally Posted by -mAx-

re-plot the contour of velocity, disable the autoscale option.
Set the min to 0 and the max to 1m/s
Enable the "filled" option.
et re-post the pictures.
It should show the low velocity distribution in the middle of your domain.
You may adjust the max velocity in the scale, to capture the distribution.
If you see an discontinuity, then you have a problem.
If not, then it should be ok (but I don't know anything from what you want to compute)

hi

I experienced the problem as to 'turbulent viscosity limited to viscosity ratio' and temperature limit

I'm modelling air flow around a 3D building in addition with solar load model

I have a solid base to be treated as soil

The bottom of soil is set to a constant temperature as a heat sink

However, I couldn't understand why the temperature of side wall of soil has reached the temperature limit

It doesn't make sense

Can you help me a little bit?

Thanks