CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   problem : "reversed flow in 77 faces on outflow 12." (http://www.cfd-online.com/Forums/fluent/65705-problem-reversed-flow-77-faces-outflow-12-a.html)

aliamini June 23, 2009 16:32

problem : "reversed flow in 77 faces on outflow 12."
 
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- June 24, 2009 01:43

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 June 24, 2009 08:06

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- June 25, 2009 00:55

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 June 25, 2009 05:09

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- June 25, 2009 07:53

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 June 25, 2009 12:22

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.
:confused::confused:

-mAx- June 25, 2009 12:49

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 June 25, 2009 16:55

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.:confused::confused:

-mAx- June 26, 2009 00:36

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 June 26, 2009 03:29

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- June 26, 2009 04:01

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 June 26, 2009 15:02

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- June 26, 2009 16:41

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 June 27, 2009 02:57

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 February 6, 2014 15:06

Quote:

Originally Posted by -mAx- (Post 220654)
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


All times are GMT -4. The time now is 04:50.