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

Problem with convergence

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 23, 2015, 06:18
Default Problem with convergence
  #1
New Member
 
Iman Sengupta
Join Date: May 2015
Location: India
Posts: 14
Rep Power: 10
Iman Sengupta is on a distinguished road
I am working on CFD simulation of hydrocyclone for steady state condition. For a particular set of dimensions I have used mesh density in the range of 300000. I have used VOF for multiphase model, RSM for turbulence model. I have used QUICK for momentum, PRESTO for pressure field convergence and scheme is SIMPLE. Under relaxation factors are kept as default. I have some problem with convergence. When the residual term of continuity equation approaches the range of 10^-6 the solution is converged but at first residual term of continuity is decreasing and then it increases. After slight decrease again it saturates at the range of 10^-3 of 10^-4. I found out that the some skewed meshes in geometry was causing this problem. By slight modification in geometry I removed all skewed meshes. But still the problem is there. When I am applying first order upwind scheme for momentum, instead of QUICK there is no problem. When I am using QUICK or second order upwind scheme I have trouble with convergence. Can anybody help me please.
Iman Sengupta is offline   Reply With Quote

Old   June 23, 2015, 06:55
Default
  #2
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 162
Rep Power: 13
jamalf64 is on a distinguished road
This can help you :
http://www.cfd-online.com/Forums/flu...2-cyclone.html
jamalf64 is offline   Reply With Quote

Old   June 23, 2015, 07:05
Default
  #3
New Member
 
Iman Sengupta
Join Date: May 2015
Location: India
Posts: 14
Rep Power: 10
Iman Sengupta is on a distinguished road
Thank you for the link but that didi not help me to solve my problem.
Iman Sengupta is offline   Reply With Quote

Old   June 23, 2015, 07:09
Default
  #4
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 162
Rep Power: 13
jamalf64 is on a distinguished road
Please describe your problem in detail
jamalf64 is offline   Reply With Quote

Old   June 23, 2015, 07:19
Default
  #5
New Member
 
Iman Sengupta
Join Date: May 2015
Location: India
Posts: 14
Rep Power: 10
Iman Sengupta is on a distinguished road
I am working with CFD simulation of a hydrocyclone under steady state condition. I have adopted VOF for multiphase flow model and RSM as turbulence model. For my geometry the mesh density is in the range of 300000. I have used QUICK scheme for momentum field calculation and PRESTO for pressure field calculation. I used SIMPLE for solving the problem. When I am using first order upwind scheme for momentum field computation I get converged results but for better accuracy I am using QUICK scheme and I am getting some problem with convergence.
Iman Sengupta is offline   Reply With Quote

Old   June 23, 2015, 07:21
Default
  #6
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 162
Rep Power: 13
jamalf64 is on a distinguished road
Please describe why VOF?
jamalf64 is offline   Reply With Quote

Old   June 23, 2015, 07:30
Default
  #7
New Member
 
Iman Sengupta
Join Date: May 2015
Location: India
Posts: 14
Rep Power: 10
Iman Sengupta is on a distinguished road
I want to check the pressure field and velocity field inside hydrocyclone. I am injecting pure water as feed. Due to rotational motion inside hydrocyclone and high turbulent field, a low pressure zone is formed along the axis of the hydrocyclone. As both the outlets are open to atmosphere air will be sucked into hydrocyclone and an air core will be formed. This air core has great influence on pressure and velocity field of hydrocyclone. To track the shape of air core VOF is used.
Iman Sengupta is offline   Reply With Quote

Old   June 23, 2015, 07:36
Default
  #8
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 162
Rep Power: 13
jamalf64 is on a distinguished road
Ok. You can't use steady state and you must run your problem unsteady. Please read about vof model from fluent user guide.
jamalf64 is offline   Reply With Quote

Old   June 23, 2015, 07:40
Default
  #9
New Member
 
Iman Sengupta
Join Date: May 2015
Location: India
Posts: 14
Rep Power: 10
Iman Sengupta is on a distinguished road
If I use explicit VOF model, I must use unsteady state model. But for implicit model I can run steady state model. I adopted implicit VOF.
Iman Sengupta is offline   Reply With Quote

Old   June 23, 2015, 07:47
Default
  #10
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 162
Rep Power: 13
jamalf64 is on a distinguished road
Fluent user guide :
. A steady-state VOF calculation is sensible only when your solution is independent of the initial conditions and there are distinct inflow boundaries for the individual phases. For example, since the shape of the free surface inside a rotating cup depends on the initial level of the fluid, such a problem must be solved using the time-dependent formulation
jamalf64 is offline   Reply With Quote

Old   June 23, 2015, 07:57
Default
  #11
New Member
 
Iman Sengupta
Join Date: May 2015
Location: India
Posts: 14
Rep Power: 10
Iman Sengupta is on a distinguished road
Thank you for the suggestion. I will try with transient problem.
Iman Sengupta is offline   Reply With Quote

Old   June 23, 2015, 07:59
Default
  #12
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 162
Rep Power: 13
jamalf64 is on a distinguished road
Be success,
Jamal
jamalf64 is offline   Reply With Quote

Old   June 23, 2015, 08:44
Default
  #13
New Member
 
Join Date: Jun 2015
Posts: 7
Rep Power: 10
Llume is on a distinguished road
Sorry I posted on the wrong discussion and I'm trying to delete this
Llume is offline   Reply With Quote

Reply

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
Convergence problem in Fluent for quenching process kaeran FLUENT 4 December 1, 2014 03:14
Rotate frame reference convergence problem! wjy-c CFX 2 September 26, 2014 07:03
Centrifugal pump OpenFOAM, convergence problem, ANSA model RDD OpenFOAM Running, Solving & CFD 0 July 5, 2014 10:12
Convergence Problem in Axisymmetric Periodic Flow atheresia FLUENT 3 February 10, 2014 04:00
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 02:17


All times are GMT -4. The time now is 21:33.