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

SOLUTION DOES NOT CONVERGE

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 11, 2008, 03:25
Default SOLUTION DOES NOT CONVERGE
  #1
Jibran Haider
Guest
 
Posts: n/a
can anyone tell me what should i do if my solution doesnot converge or it diverges.
  Reply With Quote

Old   July 11, 2008, 03:28
Default Re: SOLUTION DOES NOT CONVERGE
  #2
joao
Guest
 
Posts: n/a
Hi Jibran,

It is difficult to say what to do without any information about your particular simulation.
  Reply With Quote

Old   July 11, 2008, 03:37
Default Re: SOLUTION DOES NOT CONVERGE
  #3
Jibran Haider
Guest
 
Posts: n/a
I am trying to run a simulation of steady, laminar flow of air around a circular cylinder in cross flow placed in a duct. For this purpose I have created a 2 dimensional mesh in GAMBIT 2.2.30 and solved it in FLUENT 6.3.26. when i iterate for lower velocities such as less than 0.1 m/s the solution converges but it doesnot converge for higher velocities.
  Reply With Quote

Old   July 11, 2008, 04:45
Default Re: SOLUTION DOES NOT CONVERGE
  #4
joao
Guest
 
Posts: n/a
What is the behaviour of the residuals? Is there a divergence or is it that they simply won,t come down to the level you've prescribed?
  Reply With Quote

Old   July 11, 2008, 12:06
Default Re: SOLUTION DOES NOT CONVERGE
  #5
umesh javiya
Guest
 
Posts: n/a
I dont know...but....may be ur flow becomes turbulence at higher velocity.... so switch on turbulence model.....
  Reply With Quote

Old   July 12, 2008, 00:47
Default Re: SOLUTION DOES NOT CONVERGE
  #6
Jibran Haider
Guest
 
Posts: n/a
occasionally they diverge but most of the time they donot come down to the required criteria of 10^-3.
  Reply With Quote

Old   July 12, 2008, 00:52
Default Re: SOLUTION DOES NOT CONVERGE
  #7
Jibran Haider
Guest
 
Posts: n/a
Umesh the Reynold's Number i am checking for is around 200 so i dont think i need to turn on the turbulence model as the critical reynold's number for crossflow over a cylinder is 5*10^5.
  Reply With Quote

Old   July 13, 2008, 03:03
Default Re: SOLUTION DOES NOT CONVERGE
  #8
Osman Turan
Guest
 
Posts: n/a
I think the critical reynold's number for crossflow over a cylinder is not 5*10^5. This value is critical for surface such as flat plat in external flow. For flow around an obstacle, the critical Re > = 20000.

  Reply With Quote

Old   July 13, 2008, 04:58
Default Re: SOLUTION DOES NOT CONVERGE
  #9
umesh javiya
Guest
 
Posts: n/a
hi jibran....

Yes Osman is right...re=1e5 is criteria for flate plate....and for flow around obstacles have transition reynolds number is very low....I really dont know but you could check in literatures....it may happen even below 200
  Reply With Quote

Old   July 13, 2008, 12:12
Default Re: SOLUTION DOES NOT CONVERGE
  #10
Micael
Guest
 
Posts: n/a
I agree, transition may be well below Re=200 for external flow.
  Reply With Quote

Old   July 14, 2008, 02:50
Default Re: SOLUTION DOES NOT CONVERGE
  #11
Hossam
Guest
 
Posts: n/a
i believe for flow over cylinder at Re=200 the flow is still laminar, transition to turbulence on the cylinder wall doesn't occur untill Re=1000, at Re =200 the well known Von Karman vortex street will occur, and the wake will propagate untill far downstream the cylinder (see aerodynamics for enginnering students chapter 7 for example)this flow is an unsteady laminar flow. you may enhance convergence by extending the flow domain downstream the cylinder,try the unsteady solver or if you want to keep the steady olver try the coupled solver instead of the segragated, use velocity inlet and outflow boundary conditions for the inlet and outlet respectively. also as this flow is dominated by vortices so you have to ensure that your mesh is fine enough for example i did a similar computation and a grid independent solution was reached with 250000 volume cells for 2d computations
  Reply With Quote

Old   July 14, 2008, 12:20
Default Re: SOLUTION DOES NOT CONVERGE
  #12
Isaac
Guest
 
Posts: n/a
Hossam is right. The flow inherently becomes unsteady due to vortex shedding. If your residuals do not diverge but show oscillating behavior, then even if they go below your set critereon, you cannot consider the solution to be converged. Try unsteady and if you are using outflow condition, make sure that the normal flux across that boundary is zero as is required by the BC. You might have to extend your flow domain beyond what you currently have.
  Reply With Quote

Old   July 16, 2008, 00:48
Default Re: SOLUTION DOES NOT CONVERGE
  #13
David
Guest
 
Posts: n/a
I just met a similar problem and I have solved it by switching my laminar model to the SKE turbulence model.
  Reply With Quote

Old   July 19, 2008, 03:52
Default Re: SOLUTION DOES NOT CONVERGE
  #14
Jibran Haider
Guest
 
Posts: n/a
Hey guys! Take a look at this paragraph taken from Heat Transfer by Cengel (2nd edition - chapter 7) "The characteristic length for a circular cylinder or sphere is taken to be the external diameter D. Thus, the Reynolds number is defined as Re = VD/υ where V is the uniform velocity of the fluid as it approaches the cylinder or sphere. The critical Reynolds number for flow across a circular cylinder or sphere is about Recr ≈ 2x10^5. That is, the boundary layer remains laminar for about Re ≤ 2x10^5 and becomes turbulent for Re ≥ 2x10^5."

  Reply With Quote

Old   July 28, 2008, 13:20
Default Re: SOLUTION DOES NOT CONVERGE
  #15
Masood Kamal
Guest
 
Posts: n/a
Hi Jibran

U scaled ur model according to the scale u amde the model in. FLUENT by default take meters as units for length.
  Reply With Quote

Old   July 30, 2008, 11:23
Default Re: SOLUTION DOES NOT CONVERGE
  #16
Dale
Guest
 
Posts: n/a
Flow is genrally turbulent for Re over 1e3 for a cylinder. What Cengal is discussing is the boundary layer, which will remain laminar until the Re number increaces over 2e5. Boundary layer and general flow regime are different concepts. If Re is less than 150 then you should expect laminar vortex street, over 300 and turbulent. In between is transistional. Over 2e5 becomes a turbulent boundary layer with a characaristic low drag coeficient.
  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
what should I do if the solution didn't converge? Beeny FLUENT 6 August 27, 2011 00:04
Solution Does Not Converge Rif Main CFD Forum 3 March 7, 2008 06:33
What to do if solution doesn't converge Sharon FLUENT 1 February 15, 2007 01:40
TRANSIENT SOLUTION CONVERGE MARK Main CFD Forum 3 November 2, 2006 11:08
what to do when solution doesn't converge? Jenny CFX 5 January 28, 2004 05:00


All times are GMT -4. The time now is 13:22.