CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > Siemens > STAR-CCM+

Diverging Turbulence

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

LinkBack Thread Tools Search this Thread Display Modes
Old   May 23, 2011, 12:59
Default Diverging Turbulence
New Member
Join Date: May 2009
Location: Seattle, USA
Posts: 18
Rep Power: 17
nickninevah is on a distinguished road
Hi All,

I have a transient multiphase simulation with mesh deformation. (See attached pictures) Problem is that the turbulence equations keep diverging. I am modelling a set of water locks that slowly fill with a set of barges inside. The mesh deformation models the movement of the barges with the rising water level. Mesh deformation is linked to move with the position of the average water level. (I defined it on a velocity basis to ensure I got the initial mesh velocity with my first iterations.) No matter what I do, the problem is the same thing every time. I get a good initialization, and then as I step through time, the turbulence residuals slowly get larger. Eventually, after 20 - 120 time steps, depending on what settings I use, the model blows up and crashes. Any ideas why this is happening, and what I can do to stop it?

I have tried k-e, k-w, and Spalart-Allmaras. Currently I am using Spalart-Allmaras to try and get it stable. I have an under-relaxation factor 0.60 for my turbulence solver. I have added a linear ramp to the solver, with an initial value of 0.20 ramping up to 0.60 over 12 iterations. No matter what I do, the simulation eventually diverges, and only with turbulence. All other residuals show strong convergence. Further, I only have problems with my lower region (the bottom region shown in my pictures.) This is where the water enters through an extensive set of pipes. The pipes are meant to stop the water velocity and create smooth flow into the lock.

Some simulation settings:
Rough reynolds number: 1.55x10^5
Average cell size: 5.0 ft
Average surface cell size: 1.0 ft
Timestep: 0.05 s
Iterations between timestep: 45 (120 on initialization)
Total solution time: 32.0 s

Attached Images
File Type: jpg Scene_1GeomFluid00087.jpg (95.5 KB, 124 views)
File Type: jpg Scene_3preVessels00090.jpg (72.6 KB, 93 views)
File Type: jpg Scene_4strMidPlane00108.jpg (83.5 KB, 79 views)
File Type: jpg residuals output.jpg (57.5 KB, 94 views)

Last edited by nickninevah; May 24, 2011 at 11:13.
nickninevah is offline   Reply With Quote

Old   May 27, 2011, 17:01
Join Date: May 2010
Posts: 40
Rep Power: 16
Ladnam is on a distinguished road
I usually fix my diverging turbulence by reducing the relaxation factor for the turbulent viscosity to 0.1 and increasing the max viscosity ratio a couple of orders of magnitude.
Ladnam is offline   Reply With Quote

Old   May 27, 2011, 18:06
Senior Member
sail's Avatar
Vieri Abolaffio
Join Date: Jul 2010
Location: Always on the move.
Posts: 308
Rep Power: 17
sail is on a distinguished road
couple of suggestions in random order of importance

make sure you mesh is good, avoid highly skewed elements and big differences in volume of contiguous cells

make sure your courant number is sensible

try to link the timestepping advancement not on the number of iterations, but on the residual. some timestep might require more iterations to get convergence.

if the movement of the barges is fast, compared to the mesh size, try reducing the timestep.
sail is offline   Reply With Quote

Old   May 28, 2011, 12:44
Default Problem Fixed
New Member
Join Date: May 2009
Location: Seattle, USA
Posts: 18
Rep Power: 17
nickninevah is on a distinguished road
Thanks for the advice all. In the end, I reduced my timestep by an order of magnitude and that fixed all my problems. I probably didn't need to cut it by a full factor of 10, but I'm working with limited computer resources. It takes me sooooo long to test any change that I'm happy to just leave it where I know it will definitely be stable.

Thanks again.
nickninevah is offline   Reply With Quote


diverge, divergence, instable, turbulence, unstable

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
Turbulence length scale and integral length scale rizhang CFX 2 April 22, 2016 07:22
Question on Turbulence Intensity Eric FLUENT 1 March 7, 2012 04:30
Discussion: Reason of Turbulence!! Wen Long Main CFD Forum 3 May 15, 2009 09:52
Code release: Flow Transition and Turbulence Chaoqun Liu Main CFD Forum 0 September 26, 2008 17:15

All times are GMT -4. The time now is 21:09.