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

Continuity Divergence

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

Like Tree3Likes
  • 2 Post By CFDtoy
  • 1 Post By k_k

Reply
 
LinkBack Thread Tools Display Modes
Old   May 18, 2011, 11:43
Exclamation Continuity Divergence
  #1
New Member
 
araz
Join Date: May 2011
Location: Toronto, Canada
Posts: 19
Rep Power: 6
aras is on a distinguished road
Hi,

I have an internal flow inside a pipe. the pipe has many small details inside it in a way that 85% of the flow path inside the pipe is blocked with details.

the operating pressure inside the pipe is high (10 Mpa). I have used K-w turbulence model and the solution is steady state.

I am using pressure-based solver with PISO velocity-pressure coupling. spatial discretization is 1st order momentum and pressure is PRESTO.

I have set the URFs to 0.7 density, 0.3 pressure, and 1 drag force

I am getting continuity divergence right from the 4th or 5th iteration.

can anybody give me a hint what might has gone wrong?

thx alot
aras is offline   Reply With Quote

Old   May 18, 2011, 12:43
Default
  #2
New Member
 
Join Date: Sep 2009
Posts: 6
Rep Power: 7
CosmicRay is on a distinguished road
Have you tried refining the mesh?!!
CosmicRay is offline   Reply With Quote

Old   May 18, 2011, 12:53
Default
  #3
New Member
 
araz
Join Date: May 2011
Location: Toronto, Canada
Posts: 19
Rep Power: 6
aras is on a distinguished road
that's the thing. I have around 4 million mesh right now and I am near my machine capacity.

But how can I be sure that this is the mesh issue?
aras is offline   Reply With Quote

Old   May 18, 2011, 13:07
Default
  #4
New Member
 
Join Date: Sep 2009
Posts: 6
Rep Power: 7
CosmicRay is on a distinguished road
check the Y+ values around the walls in Fluent. check the skewness of the cells in the preprocessor. Try to use parallel solver if you are not using it to increase your machine capacity
CosmicRay is offline   Reply With Quote

Old   May 18, 2011, 23:26
Default convergence issue
  #5
Senior Member
 
CFDtoy
Join Date: Mar 2009
Location: United States
Posts: 145
Blog Entries: 2
Rep Power: 8
CFDtoy is on a distinguished road
Hi,
are you running compressible flow here? reduce p relax to 0.1, use SIMPLE scheme, upwind settings for all variables.

mesh issues are definitely worth a look but first check your settings. I will also pay attention to initialization of k,w etc..start with high turb energy and dissipation rates to stabilize flow..

Check turb model - start with k-e and then move to k-w. k-e is very dissipative and see if you attain convergence.

Does your pipe have several steps, potential recirculation zones or simply pipe?

Cheers,

CFDtoy
aras and Chong070940103 like this.
__________________
CFDtoy
CFDtoy is offline   Reply With Quote

Old   May 19, 2011, 10:55
Default
  #6
k_k
Member
 
Kailash
Join Date: May 2011
Location: London, UK
Posts: 45
Rep Power: 6
k_k is on a distinguished road
hi,

The obstacle in the flow domain can severely affect convergence. To attain a converged solution place the inlet/outlet boundaries atleast 5-10 times the height of the obstacle. Start the solution with a small under-relaxation factor.

Cheers
aras likes this.
k_k is offline   Reply With Quote

Old   May 19, 2011, 11:17
Default
  #7
New Member
 
araz
Join Date: May 2011
Location: Toronto, Canada
Posts: 19
Rep Power: 6
aras is on a distinguished road
Quote:
Originally Posted by CFDtoy View Post
Hi,
are you running compressible flow here? reduce p relax to 0.1, use SIMPLE scheme, upwind settings for all variables.

mesh issues are definitely worth a look but first check your settings. I will also pay attention to initialization of k,w etc..start with high turb energy and dissipation rates to stabilize flow..

Check turb model - start with k-e and then move to k-w. k-e is very dissipative and see if you attain convergence.

Does your pipe have several steps, potential recirculation zones or simply pipe?

Cheers,

CFDtoy


thx for the response.


by high turbulence energy and dissipation, how much you mean? when I am initializing the flow from inlet, it has some values calculated from the inlet, should I make them higher? if yes, roughly how many times?

I tried with k-e instead of k-w with smaller URFs and now I am getting an OK(not excellent) convergence. since my pipe has many walls in there with many obstacles, do you suggest k-e with wall function or k-w?
aras is offline   Reply With Quote

Old   May 19, 2011, 11:19
Default @ CFD-Toy
  #8
New Member
 
araz
Join Date: May 2011
Location: Toronto, Canada
Posts: 19
Rep Power: 6
aras is on a distinguished road
and do you suggest SIMLE or SIMPLEC?

by the way when I change the outlet from pressure outlet to outflow, I am having difficulty to get convergence for the same case, any suggestion on that?

Last edited by aras; May 19, 2011 at 12:57.
aras is offline   Reply With Quote

Old   May 19, 2011, 14:46
Default
  #9
New Member
 
MadhuVC
Join Date: Feb 2011
Posts: 27
Rep Power: 6
madhuvc is on a distinguished road
@aras,

if you have a pressure inlet I guess its advisable to use pressure outlet BC. Trying using SIMPLE scheme for coupling, STANDARD for pressure scheme, you can change schemes and methods accordingly later.
madhuvc is offline   Reply With Quote

Old   May 19, 2011, 14:59
Default mass flow inlet
  #10
New Member
 
araz
Join Date: May 2011
Location: Toronto, Canada
Posts: 19
Rep Power: 6
aras is on a distinguished road
I have a mass flow inlet. do you think which one should I use? outflow or pressure outlet?
aras is offline   Reply With Quote

Old   May 19, 2011, 15:07
Default
  #11
New Member
 
MadhuVC
Join Date: Feb 2011
Posts: 27
Rep Power: 6
madhuvc is on a distinguished road
outflow boundary condition ..hope this helps..
madhuvc is offline   Reply With Quote

Old   May 19, 2011, 15:14
Default outflow
  #12
New Member
 
araz
Join Date: May 2011
Location: Toronto, Canada
Posts: 19
Rep Power: 6
aras is on a distinguished road
but I am getting divergence with outflow while it converges with pressure outlet, any specific reason, you think of?
aras is offline   Reply With Quote

Old   October 26, 2011, 01:16
Default
  #13
New Member
 
satyendra
Join Date: Jun 2010
Posts: 15
Rep Power: 7
satyendra is on a distinguished road
hi cosmicRay,

i am trying to solve an incompressible ideal gas problem having two mass flow inlet conditions and two pressure outlet conditions ( i cannot use outflow BC since according to chapter 7, fluent user guide this is not allowed ). hence I have set target mass flow at outlet. But the continuity is not converging. any idea where i am going wrong.

rana
satyendra is offline   Reply With Quote

Old   October 26, 2011, 05:23
Default
  #14
k_k
Member
 
Kailash
Join Date: May 2011
Location: London, UK
Posts: 45
Rep Power: 6
k_k is on a distinguished road
hi,

In my experience, mass flow boundary conditions always show slower convergence. The divergence in you case, I suspect is because the pressure is not explicitely specified in atleast one boundary. I suggest you the following,

1. Try using velocity inlet boundary conditions rather than mass flow inlet. As you are simulating an incompressible flow, it doesnt make a difference as density is fixed.

2. Use pressure outlet at one of the outlet boundary and outflow in the other (if that is allowed in Fluent)

Try these and let us know what happens.

Cheers
k_k is offline   Reply With Quote

Reply

Tags
continuity error, divergence, internal flow

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
How to write k and epsilon before the abnormal end xiuying OpenFOAM Running, Solving & CFD 8 August 27, 2013 15:33
Convergence moving mesh lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 15:09
Transient simulation not converging skabilan OpenFOAM Running, Solving & CFD 12 September 17, 2007 17:48
IcoFoam parallel woes msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58
Could anybody help me see this error and give help liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 19:07


All times are GMT -4. The time now is 09:12.