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

turbulent viscocity limited to viscocity ratio

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 26, 2011, 04:53
Default turbulent viscocity limited to viscocity ratio
  #1
New Member
 
Alsemio
Join Date: Jan 2011
Posts: 7
Rep Power: 7
alsemio is on a distinguished road
Hi everyone
I was trying to run a car model with 1million cell aproximately using k epsilon turbulence model and I have the following problem :

Turbulent viscocity limited to viscocity ratio of 1.0000 in 400 cell
and the number of cell goes increasing

after many iteration appear to me the following message
Error:divergence detected in AMG:temperature
Error)

Can please anybody help me to solve this problem?
thank you all

see you in advance

Alsemio
alsemio is offline   Reply With Quote

Old   January 31, 2011, 17:04
Default
  #2
Member
 
David Stanbridge
Join Date: Apr 2010
Location: Norwich, UK
Posts: 58
Rep Power: 7
swiftaircraft is on a distinguished road
Have you tried running it with the energy equation off? I assume you are assuming a real gas. When this converges a little you should then be able to activate energy again. However for low speed flows it would not add that much to the accuracy of the simulation.
swiftaircraft is offline   Reply With Quote

Old   February 1, 2011, 15:48
Default Thanks David (Swiftaircraft)
  #3
New Member
 
Alsemio
Join Date: Jan 2011
Posts: 7
Rep Power: 7
alsemio is on a distinguished road
Hi David
First of all thank you for anwer me and help me with this problem
let me tell you that Im trying to solve a simple car simulation at 50 m/s speed using k-e solver
As well I turn off the energy equation because I using incompresible flow
so I cannot understand why do I have this problem

Fluent always show me turbulent viscocity ratio in xx cells and the number of cell rise

Thank you so much and I hope that someone else can help me to solve this I dont know what to do because I changed set up and still same problem

See you in advance

Alsemio
alsemio is offline   Reply With Quote

Old   February 1, 2011, 15:52
Default
  #4
Member
 
David Stanbridge
Join Date: Apr 2010
Location: Norwich, UK
Posts: 58
Rep Power: 7
swiftaircraft is on a distinguished road
How have you initialised the problem? Do you use fmg initialisation? What are your underrelaxation factors? Are you using a velocity inlet with an outflow outlet? I assume for defining the inlet turbulence you have used a low turbulent intensity. What is the maximum skewness in the model? Please provide as many details as possible.
swiftaircraft is offline   Reply With Quote

Old   February 1, 2011, 16:26
Default Hi David Alsemio
  #5
New Member
 
Alsemio
Join Date: Jan 2011
Posts: 7
Rep Power: 7
alsemio is on a distinguished road
Hi David thank you for help me Im new using CFD fluent so to answer you question Im using Gambit to mesh so I used 1.200.000 tetrahedral elements with skew below 0.8 only I have 98 elements between 0.8 and 0.9 and in Fluent I use k- e viscous model Standard I left the turbulent kinetic energy and turbulent dissipation ratio as default 1 (I dont understand to compute this values) I iniatilize with velocity in inlet
I hope to hear from you
Thanks a lot David
Alsemio
alsemio is offline   Reply With Quote

Old   February 1, 2011, 17:08
Default
  #6
Member
 
David Stanbridge
Join Date: Apr 2010
Location: Norwich, UK
Posts: 58
Rep Power: 7
swiftaircraft is on a distinguished road
Set the inlet turbulence using Intensity and Viscosity Ratio. Set Intensity to 0.05% and a viscosity ratio of 1. Initialise the flow with the values obtained when you select the name of your inlet in the "Compute from" drop down box. Then in the Fluent window type "sol ini fmg y". Do not use the quotation marks though. Also use the realizable k-epsilon model to start. Initially set the discretisation to first order. See if that helps. Also change default under relaxation factors so that Momentum is 0.3 and Pressure is 0.7.
swiftaircraft is offline   Reply With Quote

Old   February 1, 2011, 17:25
Default Thank so much David Alsemio
  #7
New Member
 
Alsemio
Join Date: Jan 2011
Posts: 7
Rep Power: 7
alsemio is on a distinguished road
Thank you so much David
I will try your advice I have my finger crossed
let me tell you the result if you want

See you in advance

Kind Regards

Alsemio
alsemio is offline   Reply With Quote

Old   February 1, 2011, 17:32
Default
  #8
Member
 
David Stanbridge
Join Date: Apr 2010
Location: Norwich, UK
Posts: 58
Rep Power: 7
swiftaircraft is on a distinguished road
Please let me know if it works.
swiftaircraft is offline   Reply With Quote

Old   February 2, 2011, 22:19
Default
  #9
Senior Member
 
Real Name :)
Join Date: Jan 2010
Location: United States
Posts: 180
Rep Power: 8
ComputerGuy is on a distinguished road
I would also ensure that your cells in the boundary layers are appropriate. The message typically "goes away" after the solution gets close to steady state. However, if your boundary conditions are not well defined, or your mesh is poor, they will continue to pop up. Finally, you can always set the solver limits on viscosity ratio to be slightly higher. It's cheap and isn't always effective, but you can give it a shot.

ComputerGuy


Quote:
Originally Posted by swiftaircraft View Post
Please let me know if it works.
ComputerGuy is offline   Reply With Quote

Old   February 4, 2011, 17:03
Default Thanks a lot Computerguy and Swiftaircraft
  #10
New Member
 
Alsemio
Join Date: Jan 2011
Posts: 7
Rep Power: 7
alsemio is on a distinguished road
Thanks a lot Computerguy and Swiftaircraft
I think both you are right
but I dont quite undertand how much and where to put viscocity ratio limits
kind regards
alsemio
alsemio is offline   Reply With Quote

Old   February 4, 2011, 17:17
Default hello David swiftaircraft
  #11
New Member
 
Alsemio
Join Date: Jan 2011
Posts: 7
Rep Power: 7
alsemio is on a distinguished road
Hi David
Sorry for bother just to know for cuiosity what does fluent do writting "sol ini fmg"

Thank you again
alsemio
alsemio is offline   Reply With Quote

Old   February 4, 2011, 19:49
Default
  #12
Senior Member
 
Real Name :)
Join Date: Jan 2010
Location: United States
Posts: 180
Rep Power: 8
ComputerGuy is on a distinguished road
Alsemio,

Check the following for how to enter limits:http://my.fit.edu/itresources/manual...g/node1381.htm


Quote:
Originally Posted by alsemio View Post
Hi David
Sorry for bother just to know for cuiosity what does fluent do writting "sol ini fmg"

Thank you again
alsemio
ComputerGuy 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
"turbulent viscosity limited to viscosity ratio" olivier FLUENT 11 October 10, 2015 05:49
hel (turbulent viscosity ratio limited) for supersonic combustion problem omar.2002bh FLUENT 2 September 5, 2012 11:04
Turbulent viscosity limited to viscosity ratio of 1.0000000e+5 eespi002 FLUENT 3 June 30, 2009 13:24
turbulent viscosity limited to viscocity ratio of gayatri FLUENT 2 February 27, 2007 13:22
Problem of Turbulent Viscosity Ratio Limited David Yang FLUENT 3 June 3, 2002 06:13


All times are GMT -4. The time now is 21:07.