CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT > Fluent Multiphase

steady state simulation diverge

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 13, 2015, 19:40
Default steady state simulation diverge
  #1
Senior Member
 
Join Date: Oct 2014
Posts: 124
Rep Power: 8
Ema40 is on a distinguished road
Hi all.

I am simulating an open channel flow with geometry discontinuities (with rapid changes in the cross sections...), in a steady state.

Why does it diverge? In a steady state there is not the temporal discretization, thus the divergence of the solution does not depend on the mesh size, right?
Can the divergence be caused by the boundary conditions?

Thank you
Ema40 is offline   Reply With Quote

Old   October 20, 2015, 08:27
Default
  #2
Member
 
Jim
Join Date: May 2015
Posts: 47
Rep Power: 8
CFDYourself is on a distinguished road
a few points, I am also having trouble with divergence of a steady state model currently.

- it does depend on the mesh. If the mesh quality is poor, your simulation will struggle to converge.
- the mesh density near the wall ("inflation layer") needs to be the right size for your turbulence model. y+ of first cell = ca. 30 to 300 for wall functions, y+ = 1 if the boundary layer is being resolved.
- you may have issues solving particular flow features in your model, such as detachment or high-shear regions.
- easy things you can try to aid/investigate convergence issues:
-reduce the URFs, then return them to defaults once solving.
-make material properties constants, not dependent on T or P.
-model isothermal & no chemistry case first.
-make transport eqns 1st order or solve with a simpler model to begin with.
-contour plot -> residuals -> mass imbalance.
CFDYourself is offline   Reply With Quote

Old   October 20, 2015, 15:54
Default
  #3
Senior Member
 
Join Date: Oct 2014
Posts: 124
Rep Power: 8
Ema40 is on a distinguished road
Thank you very much.
I resolved using the QUICK scheme instead of Second Order.

How do you mean with the last sentence (mass unbalance)?

Thank you
Bye
Ema40 is offline   Reply With Quote

Old   October 21, 2015, 08:22
Default
  #4
Member
 
Jim
Join Date: May 2015
Posts: 47
Rep Power: 8
CFDYourself is on a distinguished road
on the last point:

it lets you colour the mesh in fluent in terms of "mass imbalance", which can help identify cells that are potentially causing problems with convergence.
CFDYourself is offline   Reply With Quote

Old   October 21, 2015, 10:13
Default
  #5
Senior Member
 
Join Date: Oct 2014
Posts: 124
Rep Power: 8
Ema40 is on a distinguished road
Thank you very much!
Do you know also how to plot water depths in open channel flow? Because in the Contour plot option there is not water depth.

Thank you
Regards
Ema40 is offline   Reply With Quote

Old   July 21, 2018, 14:09
Default
  #6
New Member
 
Gujrat
Join Date: Jul 2018
Posts: 2
Rep Power: 0
iitpandey@3 is on a distinguished road
Creat a plane (vertical), iso-clip it with water phase having min - 0.499 and max -0.501. it will track the water depth for VOF 0.5. now, go to xy plot in post processing portal. and get the water depth..if it does not work ..do let me know

()
iitpandey@3 is offline   Reply With Quote

Reply

Tags
boundary conditions, divergence, open channel flow, steady state vof

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
mass flow in is not equal to mass flow out saii CFX 12 March 19, 2018 05:21
Solver for transonic flow? Martin Hegedus OpenFOAM Running, Solving & CFD 22 December 16, 2015 04:59
Setting the height of the stream in the free channel kevinmccartin CFX 10 July 9, 2015 21:36
Steady state simulation with transient partilcle tracking mali28 FLUENT 2 February 7, 2013 14:25
steady state simulation manoj FLUENT 1 March 20, 2004 07:15


All times are GMT -4. The time now is 20:18.