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

Mesh size and solver residuals...

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 15, 2008, 12:44
Default Mesh size and solver residuals...
  #1
Scott
Guest
 
Posts: n/a
I have a simple pipe flow problem, where the flow makes a 90 deg change in direction at the intersection of two pipes. There is no radius/bend at the intersection, so there is some flow separation and recirculation at the corner. The fluid is water, Re > 20,000.

The pipes I'm modeling have an ID of about .25". The mesh element size throughout most of the pipe is on the order of .050". In the area of pipe intersection, I have refined the mesh element size to be on the order of .025". I have 15 layers of inflation, with approximately 10 of those layers within the estimated hydrodynamic boundary layer thickness.

When I attempt to solve this simulation in steady-state, with an SST turbulence model (5% inlet turbulence) and all initial conditions set to auto, the momentum and turbulence residuals approach 1e-4 after about 40 iterations, but then start to fluctuate and slowly rise, never reaching convergence. When I attempt to solve this simulation using the k-e turbulence model, I reach a 1e-4 residuals convergence on fluid momentum components after 120+ iterations, but just barely. For the k-e model, if I plot the abs of the momentum residuals, the cells that still have high (>1e-4) residuals are those where the flow is experiencing separation and/or recirculation. See the following photo (u momentum residuals plotted with gray volumes):

http://74.220.219.65/~scottpol/image...wResiduals.jpg

I have tried further mesh refinement in these areas (decreasing the element size from ~.025" down to ~.01"), but it actually made convergence worse. Does anybody have any suggestions on modifications to my mesh or model setup that might help me reach a definite and accurate solution without oversimplifying the flow? I appreciate the help. Thanks!
  Reply With Quote

Old   December 15, 2008, 14:52
Default Re: Mesh size and solver residuals...
  #2
CycLone
Guest
 
Posts: n/a
Hi Scott,

The high residuals indicate the flow is changing significantly in these cells. In your case the change is due to velocity fluctuations at the interface; similar to turbulent vortex shedding, though the steady state solver will not be resolving these directly.

Refining the mesh will make it worse because your are increasing the velocity gradient (by getting closer to the shear layer) and also allowing the mesh to transport smaller turbulent" features.

Try increasing your timestep. Since CFX uses a false timestep, increasing the timestep will allow the solution to propegate further at each iteration. This may wash out the fluctuations and help converge the solution.

-CycLone

  Reply With Quote

Old   December 15, 2008, 15:36
Default Re: Mesh size and solver residuals...
  #3
Scott
Guest
 
Posts: n/a
Thanks for the reply. I've played around with the timescale a little, but perhaps not sufficiently?...

The advection time for my model is about .2 sec. I've tried setting the physical timescale to .2 sec, 2 sec, and 20 sec, but the convergence using k-e turbulence doesn't seem to improve much (if anything, the convergence appears "bouncy" at the higher timescales), and I wasn't able to achieve convergence using sst turbulence at any of those timescales.

Any thoughts on setting the Gradient Relaxation or Blend Factor Relaxation? I'm not familiar with these, but I see some references to them in the "Problems with Convergence" section of the help manual.

Thanks again, Scott

  Reply With Quote

Old   December 15, 2008, 15:47
Default Also...
  #4
Scott
Guest
 
Posts: n/a
I forgot to mention, I have been using double precision to solve this model.
  Reply With Quote

Old   December 15, 2008, 16:43
Default Solved...
  #5
Scott
Guest
 
Posts: n/a
Here's how... I ran the model to a 1e-4 rms convergence with a k-e turbulence model and the fluid timescale set to 10x my advection time (case 1). Then, I ran the model again to a 2e-5 rms convergence with a timescale of 1x my advection time, using case 1 results as the initial conditions (case 2). Now I'm running it a third time with a timescale of 0.1x my advection time, to rms residuals of 1e-5, and it seems to be on the path towards convergence. Sweet.
  Reply With Quote

Old   December 15, 2008, 18:10
Default Re: Solved...
  #6
Glenn Horrocks
Guest
 
Posts: n/a
Good to hear you are on the path to convergence. You might find this a useful reference in future:

http://www.cfd-online.com/Wiki/Ansys...gence_criteria
  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
Convergence Centurion2011 FLUENT 24 May 9, 2015 08:02
Superlinear speedup in OpenFOAM 13 msrinath80 OpenFOAM Running, Solving & CFD 18 March 3, 2015 06:36
Naca 0012 (compressible and inviscid) flow convergence problem bipulsaha FLUENT 1 July 6, 2011 07:51
On Setring Step Size in unsteady Solver of FLUENT lzgwhy FLUENT 0 August 19, 2009 22:44
Gambit problems Althea FLUENT 21 February 6, 2001 08:05


All times are GMT -4. The time now is 11:15.