CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

turbulent viscosity limited to viscosity ratio

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   September 10, 2012, 15:11
Default turbulent viscosity limited to viscosity ratio
  #1
New Member
 
Alexandra
Join Date: Sep 2012
Posts: 9
Rep Power: 4
Alex_B is on a distinguished road
Hello, dear all!
May be you can help me!
My task look like this:

-2D case, Mixture model, k-e standart viscosity
-cilinder with little adding inside (see picture Снимок.jpg)
-there is mixture inside cilinder (air volume fraction 0.95 + water 0.05) (like spray)
-velocity inlet 5m\s and Initial gauge pressure is 10000000 Pa (turbulence: intensity and visc.ratio 5 and 5)
-pressure outlet 9992500 Pa (turbulence: intensity and visc.ratio 5 and 5)

And again and again I have messages like:
reversed flow in 255 faces on pressure-outlet 11.

turbulent viscosity limited to viscosity ratio of 1.000000e+08 in 43005 cells


and after this

Error: Divergence detected in AMG solver
Error Object: #f


I try to implement all advices from this forum, but I have this bad massages.
So I suggest, that my problem in aerosol model. May be I implement wrong viscosity model or something like this.

Please, may be you can help me?

Alex
Attached Images
File Type: jpg Снимок.JPG (21.7 KB, 30 views)
Alex_B is offline   Reply With Quote

Old   September 10, 2012, 17:45
Default
  #2
Member
 
Yon Han Chong
Join Date: Jun 2012
Posts: 77
Rep Power: 5
yonchong is on a distinguished road
It looks like the calculation is hitting the turbulence viscosity limit because the solution is diverging rather than converging.

There are a number of reasons why this could be happening but how are you initialization the solution? If you have the latest version try the hybrid initialization.

What does the velocity vector plot looks like? Is there any spike in the velocity plot?
yonchong is offline   Reply With Quote

Old   September 11, 2012, 01:42
Default
  #3
New Member
 
Alexandra
Join Date: Sep 2012
Posts: 9
Rep Power: 4
Alex_B is on a distinguished road
Quote:
Originally Posted by yonchong View Post
It looks like the calculation is hitting the turbulence viscosity limit because the solution is diverging rather than converging.

There are a number of reasons why this could be happening but how are you initialization the solution? If you have the latest version try the hybrid initialization.

What does the velocity vector plot looks like? Is there any spike in the velocity plot?

Thank you for reply!
I use hybrid initialisation.
I try to change mixture consistance (0.95 water + 0.05 air) and it's work and calculates well. I try to send printscreens of my initialisation.
Thank you !

Last edited by Alex_B; September 11, 2012 at 03:32.
Alex_B is offline   Reply With Quote

Old   September 11, 2012, 03:34
Default
  #4
New Member
 
Alexandra
Join Date: Sep 2012
Posts: 9
Rep Power: 4
Alex_B is on a distinguished road
see attachement please
Attached Images
File Type: jpg 1.jpg (29.6 KB, 34 views)
File Type: jpg 2.jpg (42.2 KB, 34 views)
File Type: jpg models.jpg (41.1 KB, 34 views)
File Type: png materials.PNG (40.0 KB, 28 views)
File Type: jpg phases.jpg (33.2 KB, 28 views)
Alex_B is offline   Reply With Quote

Old   September 11, 2012, 03:36
Default
  #5
New Member
 
Alexandra
Join Date: Sep 2012
Posts: 9
Rep Power: 4
Alex_B is on a distinguished road
continue of attachements
Attached Images
File Type: jpg inlet_mixture.jpg (35.9 KB, 23 views)
File Type: jpg inlet_air.jpg (43.8 KB, 23 views)
File Type: jpg inlet_water.jpg (40.1 KB, 23 views)
File Type: jpg inlet_water_2.jpg (36.4 KB, 22 views)
File Type: jpg cell_zone_conditions.jpg (33.6 KB, 20 views)
Alex_B is offline   Reply With Quote

Old   September 11, 2012, 03:38
Default
  #6
New Member
 
Alexandra
Join Date: Sep 2012
Posts: 9
Rep Power: 4
Alex_B is on a distinguished road
the last attachement)
Attached Images
File Type: png initialization.PNG (40.2 KB, 21 views)
File Type: jpg solution_order.jpg (40.9 KB, 22 views)
File Type: jpg solution_controls.jpg (35.5 KB, 19 views)
File Type: jpg solution_controls_advanced.jpg (47.1 KB, 21 views)
Alex_B is offline   Reply With Quote

Old   September 11, 2012, 03:39
Default
  #7
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 899
Rep Power: 15
ghost82 will become famous soon enough
Just a consideration, maybe it's not useful to you: have you set correctly primary and secondary phases?

For the first case: 0,95 air, 0,05 water air is the primary phase in the "phase panel";
For the second case: 0,95 water, 0,05 air, water is the primary phase.

Daniele
ghost82 is offline   Reply With Quote

Old   September 11, 2012, 04:07
Default
  #8
New Member
 
Alexandra
Join Date: Sep 2012
Posts: 9
Rep Power: 4
Alex_B is on a distinguished road
Quote:
Originally Posted by ghost82 View Post
Just a consideration, maybe it's not useful to you: have you set correctly primary and secondary phases?

For the first case: 0,95 air, 0,05 water air is the primary phase in the "phase panel";
For the second case: 0,95 water, 0,05 air, water is the primary phase.

Daniele

Yes, it is correct!
Thank you!
Alex_B is offline   Reply With Quote

Old   September 11, 2012, 04:45
Default I seems to understand my problem!!!!!
  #9
New Member
 
Alexandra
Join Date: Sep 2012
Posts: 9
Rep Power: 4
Alex_B is on a distinguished road
So, I think that my mistake was big diameter of secondary phase.
Buy I try to check this.
Alex_B is offline   Reply With Quote

Old   September 11, 2012, 04:55
Default
  #10
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,094
Rep Power: 16
RodriguezFatz will become famous soon enough
Hi Alex, some ideas:
1) Did you run a simulation with just air? Did it work?
2) Your grid is hard to see, but it looks kind of strange. Do all cells have the same size? Why wouldn't you have smaller cells at the walls?
3) Did you "patch" your zone to 5% water after initialization?
4) The other day, this message vanished after changing the inlet conditions. Did you try to set "Intensity and Hydraulic diameter" to somehow reasonable values?
5) What is the fraction of backflow of secondary phase at the oulet?


BTW: Your description / inital post is perfect. I wish everyone would introduce his/her problem like this!
RodriguezFatz is offline   Reply With Quote

Old   September 11, 2012, 13:00
Question
  #11
New Member
 
samiullah
Join Date: Aug 2012
Posts: 21
Rep Power: 4
samidabest is on a distinguished road
i'm new user on ansys ... and i have to work on ansys fluent so plz send me tutorials of ansys fluent 12 or 13 or 14 if any one have my email is samiullahh09me08.muet@gmail.com
samidabest is offline   Reply With Quote

Old   September 11, 2012, 13:51
Default
  #12
Member
 
Yon Han Chong
Join Date: Jun 2012
Posts: 77
Rep Power: 5
yonchong is on a distinguished road
Open up Fluent and tutorials can be found in Help menu.

If not, just do google search on Fluent Tutorial. You will find plenty.
yonchong is offline   Reply With Quote

Old   September 12, 2012, 09:14
Default
  #13
New Member
 
Alexandra
Join Date: Sep 2012
Posts: 9
Rep Power: 4
Alex_B is on a distinguished road
Quote:
Originally Posted by RodriguezFatz View Post
Hi Alex, some ideas:
1) Did you run a simulation with just air? Did it work?
2) Your grid is hard to see, but it looks kind of strange. Do all cells have the same size? Why wouldn't you have smaller cells at the walls?
3) Did you "patch" your zone to 5% water after initialization?
4) The other day, this message vanished after changing the inlet conditions. Did you try to set "Intensity and Hydraulic diameter" to somehow reasonable values?
5) What is the fraction of backflow of secondary phase at the oulet?


BTW: Your description / inital post is perfect. I wish everyone would introduce his/her problem like this!
Thank you for reply!
1) Yes, I tryed . It almost work (fluxes- ok, and velocity contours looks normal (I think)))))) (see attachement)
2) I have smaller size of cells close the wall.(mesn is ok)
3) Sorry, what mean ""patch" zone to 5%" ?
4)Where I can find "Intensity and Hydraulic diameter" parameters
5) fraction of backflow of secondary phase at the oulet- I havn't this parameter in outlet/ secondary phase/
I try to calculate the same task, but with symmetry conditions at the axis of me old geometry, and my calculation crushes(((

sorry, may be you send me your email, and I'll send you my case file? If it's ok for you (botyachkova.alexandra@gmail.com).

Thank you for reply!
Attached Images
File Type: png AIR.PNG (21.8 KB, 10 views)
Alex_B is offline   Reply With Quote

Old   September 12, 2012, 09:33
Default
  #14
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,094
Rep Power: 16
RodriguezFatz will become famous soon enough
3) When you initialize, Fluent sets the second phase density to zero inside your domain. You have to patch it "by hand" by clicking on the "Patch..." button just below the "Initialize" button. Here you can choose the domain and value you want to patch to a certain value! I guess the window will be self-explanatory. Setting the density fraction to, let's say, the inlet flow fraction will normally get the initial guess closer to the final solution.
4) You can find it in the inlet boundary condition panel under "Turbulence->Specification Method". You can choose between different ways of telling the solver boundary values for the turbulence - "Intensity and Hydraulic diameter" is one of them. You should also have a look at the turbulent viscosity by means of a contour plot. Where does the limitation problem occur?
5) Under "Boundary Conditions -> Your Outlet (2nd phase) -> Multiphase ->", can't you find a Backflow field? Try setting it to zero.
RodriguezFatz is offline   Reply With Quote

Old   September 12, 2012, 10:22
Default
  #15
New Member
 
Alexandra
Join Date: Sep 2012
Posts: 9
Rep Power: 4
Alex_B is on a distinguished road
Quote:
Originally Posted by RodriguezFatz View Post
3) When you initialize, Fluent sets the second phase density to zero inside your domain. You have to patch it "by hand" by clicking on the "Patch..." button just below the "Initialize" button. Here you can choose the domain and value you want to patch to a certain value! I guess the window will be self-explanatory. Setting the density fraction to, let's say, the inlet flow fraction will normally get the initial guess closer to the final solution.
4) You can find it in the inlet boundary condition panel under "Turbulence->Specification Method". You can choose between different ways of telling the solver boundary values for the turbulence - "Intensity and Hydraulic diameter" is one of them. You should also have a look at the turbulent viscosity by means of a contour plot. Where does the limitation problem occur?
5) Under "Boundary Conditions -> Your Outlet (2nd phase) -> Multiphase ->", can't you find a Backflow field? Try setting it to zero.



Thank you!
As I understand, you talk about Standart initialisation. But I use Hybrid.
Alex_B is offline   Reply With Quote

Old   September 12, 2012, 10:30
Default
  #16
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,094
Rep Power: 16
RodriguezFatz will become famous soon enough
I am not sure, but I think it is the same for hybrid. Just click on initialize and than contoure-plot your secondary phase fraction. I guess it will be zero inside your domain. To initialize it with 0.05, you have to use the "Patch" button.

Last edited by RodriguezFatz; September 12, 2012 at 13:18.
RodriguezFatz is offline   Reply With Quote

Old   September 12, 2012, 13:17
Default
  #17
New Member
 
samiullah
Join Date: Aug 2012
Posts: 21
Rep Power: 4
samidabest is on a distinguished road
i want to know to create the macros to use the macro model of heat exchanger in fluent
samidabest is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Problem with divergence TDK FLUENT 10 September 8, 2012 01:11
Turbulent viscosity ratio limited to 1.10^5 in boundary layer ingestion loicflouriot FLUENT 0 May 27, 2012 07:31
"turbulent viscosity limited to viscosity ratio" olivier FLUENT 9 May 14, 2008 09:48
Turbulent viscosity limited to viscosity... Cyril FLUENT 16 October 4, 2007 06:12
On limiting to turbulent viscosity ratio! varghese FLUENT 2 November 15, 2003 09:56


All times are GMT -4. The time now is 07:07.