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

Solution does not converge. Need help for project work at uni.

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 10, 2013, 00:59
Default Solution does not converge. Need help for project work at uni.
  #1
New Member
 
Samiullah Mahmood
Join Date: Dec 2012
Posts: 8
Rep Power: 4
samiullah is on a distinguished road
Hello there I am working on my final year project and I am trying to simulate slurry flow through a 0.1m pipe that is 5m in length.

Geometry
Centre of the inlet is at (0,0,0) and extends by 5m in the x axis. Diameter of the inlet is 0.1m.

Meshing
Meshing sizes are 0.002m min size, 0.005m max and max face size.
Inflation is set to be on from the pipe walls.
Inlet and outlet both labelled, Inlet being the end at (0,0,0)
Produces about 3.5 million elements

Setup
gravity is selected at -9.81m/s in the y direction.
Model is set as multiphase flow on, mixture option selected with 2 phases and additionally the 'Implicit Body Force' option is ticked.
k-e turbulence (2 equation) is selected
Materials - phase 1 is standard water (h2o) selected from fluent database, phase 2 is air with density 1600kg/m^3, viscosity 0.1kg/m^3 and diameter of 1mm (representing the solid being transported).
boundary conditions - for the inlet - phase 1 is 1m/s. phase 2 is set to 1.1m/s, multiphase volume fraction is set to 0.005 (5%). Hydraulic backflow diameter is set to 0.1m on the outlet.
Solution method is:
Gradient - Green-gauss Node Based
Momentum '2nd order upwind'
Turbulent kinetic energy '2nd order upwind'

On solution initialisation i have selected compute from inlet and the y and z velocities are changed to 0.1m/s before initialization.

I dont know if any of this helps but I have done over 3000 iterations and the solution has not yet converged, the settings above are what I have changed, everthing else is standard setting, so convergence is still and 1e^-3. All the settings have been suggested by my tutor at university.

Also i get messages on the iterations saying 'viscosity limited to viscosity ration of 1.000000e+05 in ### cells' where ### is a number that changes, usually ranging from 1-12.

What am i doing wrong to not get any results? This is for my university final year project so any help is deeply appreciated.
samiullah is offline   Reply With Quote

Old   March 10, 2013, 15:51
Default dear
  #2
Member
 
farzadpourfattah
Join Date: Mar 2013
Posts: 41
Rep Power: 4
farzadpourfattah is on a distinguished road
if you use density base solver start your run with small CFL such as 0.5 or less than or you can run first 1000 iterations first order and then use second order.
try kw sst turbulence model!
farzadpourfattah is offline   Reply With Quote

Old   March 11, 2013, 08:59
Default
  #3
New Member
 
Samiullah Mahmood
Join Date: Dec 2012
Posts: 8
Rep Power: 4
samiullah is on a distinguished road
Thank you for the response. Does the rest of my set up sound like it should give me a decent set of results if set up properly? Also If I was to run the simulation with water only, would I be able to run the settings you suggested? I am hoping to be able to include this in my results also.
samiullah is offline   Reply With Quote

Old   March 11, 2013, 15:10
Default
  #4
Senior Member
 
A CFD free user's Avatar
 
A-A Azarafza
Join Date: Jan 2013
Posts: 187
Rep Power: 4
A CFD free user is on a distinguished road
Hello
You're talking about slurry but I personally don't see slurry from the mixture of water and air! Am I wrong or it's exactly what you mean? Besides,why are you using mixture model for this case? If you intent to model a mixture of water and air, so I recommend you that use VOF or Eulerian models for your purpose. I used the mixture model once for my own case where I simulated sedimentation of solid inside a stirred tank and it worked out very good without any convergency problem. Hope it help.
A CFD free user is offline   Reply With Quote

Old   March 11, 2013, 15:54
Default
  #5
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11
oj.bulmer will become famous soon enough
Firstly, the choice of mixture model seems wrong since the density ratio is way more that 1. Eulerian multiphase model with Grace interphase drag correlation seems the best choice for this.

Also, you may want to take it slow and get convergence with first order before switching to second order.

Realizable model is the best in terms of convergence often. You may want to try that, if the solution time doesn't increase too much.

The high viscosity ratio is indication that either the flow is very turbulent, or that the turbulence boundary conditions have not been defined correctly. You can increase the limit of turbulent/laminar viscosity ratio but that will just remove the warning. You still have to see why the ratio is so large.

Lastly, you mention 5% air volume fraction, but that is equal to 0.05, not 0.005 as you mention. Check for this input in your setup.

OJ

Last edited by oj.bulmer; March 11, 2013 at 16:00. Reason: Volume fraction of air
oj.bulmer is offline   Reply With Quote

Old   March 11, 2013, 16:20
Default
  #6
New Member
 
Samiullah Mahmood
Join Date: Dec 2012
Posts: 8
Rep Power: 4
samiullah is on a distinguished road
I was using air with given density, diameter and viscosity to represent sand. If there is a better method then I appreciate any light you can shed on this. I am merely going by a tutorial handed to me by my project supervisor as a method he deemed satisfactory to simulate a slurry pipe.

I will be going from 5-25% air (sand) volume fraction in increments of 5% to see the effect, and also increasing the flow velocity from 1 - 4 m/s in 1 m/s increments.

Sorry for the typing error, I do use 0.05 as my volume fraction. So i should use eulerian multiphase model with grace inter-phase drag correlation? Can you please explain why so I can justify this choice in my report?

Thank you
samiullah 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
Help! Could anyone help me on Simulation of 2D airfoil? didiean FLUENT 38 March 8, 2013 22:04
GMRES-solver does not converge correctly staentz_b Main CFD Forum 2 February 14, 2013 07:55
ATTENTION! Reliability problems in CFX 5.7 Joseph CFX 14 April 20, 2010 15:45
Accuracy and convergence pawan1989 FLUENT 5 April 15, 2010 17:17
Wall functions Abhijit Tilak Main CFD Forum 6 February 5, 1999 02:16


All times are GMT -4. The time now is 03:21.