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

Time step dependence of convergence behavior of steady state simulations in CFX

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

Like Tree5Likes
  • 5 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   April 21, 2011, 05:43
Default Time step dependence of convergence behavior of steady state simulations in CFX
  #1
Senior Member
 
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 6
Chander is on a distinguished road
I am simulating steady state turbulent conjugate heat transfer problem in CFX. I am facing some convergence problems (residuals stabilize before reaching convergence criteria). I have gone through the FAQ regarding this available under CFD wiki ( http://www.cfd-online.com/Wiki/Ansys...gence_criteria) and tried to play with the time-step being used by the CFX solver.

Now I observe the following
1) With Automatic Timestep calculation, I am able to get convergence for my simulations if I reduce the Timescale factor to 0.1. So whatever automatic time-step is calculated by solver, I multiply it with 0.1.

2) I tried to get an idea of the physical time-step by plotting streamlines and observing the time variable on the streamlines (as outlined in the CFD wiki link above). However, the flow is very complex consisting of 3-dimensional vortices and the physical time estimate from streamlines is very large. And choosing a time-step based on a fraction (1/3 to 1/5) of this physical time leads to a large time-step and solver failure

3) Choosing the local timescale factor of 4 leads to very slow convergence.

I have asked similar question before on this forum. However, I have come back as I am not sure what I am doing is right.

My question is:
a) Is it fine to get convergence by such large reduction (1/10) in the automatically calculated time step? I have repeatedly checked my mesh and set-up and I have not been able to find any problem with that. I have also checked that I am not resolving any transient behavior in my simulation because the period of oscillation of residual changes with change in time-step.

b) The transient formulation being used in CFX for steady state simulation is fully implicit (correct me if I am wrong). Then why does the convergence behavior depend on choice of time-step? Isn't a fully implicit discretization unconditionally stable?

c) moreover, why should attainment of steady state depend on choice of time-step? Theoretically one can use as large a time-step as desired.
Chander is offline   Reply With Quote

Old   April 25, 2011, 07:25
Default
  #2
Senior Member
 
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 6
Chander is on a distinguished road
Anyone please...
Chander is offline   Reply With Quote

Old   April 25, 2011, 07:52
Default
  #3
New Member
 
Florent Duchaine
Join Date: Jan 2011
Location: Toulouse, France
Posts: 25
Rep Power: 6
Florent is on a distinguished road
what is your configuration?
Florent is offline   Reply With Quote

Old   April 28, 2011, 18:39
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
a) You can use any time step you like to get convergence. A larger timestep will usually get there quicker, that is why it is recommended.

b) Yes, CFX is fully implicit (although there are some physics models which are not, such as surface tension and particle tracking, but that is another matter). The importance of time step size is that is what CFX uses to stabilise the equations. A SIMPLE based solver uses under relaxation factors. CFX uses time step size.

c) Just as for under relaxation (URF) on SIMPLE based solvers, you want to use the largest URF which converges reliably. Then you often reduce it a bit for safety. Likewise in CFX you use the largest timestep which converges. As you approach convergence the equations often become more stable, meaning that you can increase the timestep size.

This means it is very common to start a CFX steady state run with a small timestep and run that for a few iterations to set the flow up, but then start increasing the time step size as the flow settles down. As you approach convergence you can often be running time steps 100 or 1000 times larger than you started with. Use the "Edit run in progress" feature of the sovler manager and you can do this without stopping and restarting the run.
Far, ftab, 86682164 and 2 others like this.
ghorrocks is offline   Reply With Quote

Old   May 3, 2011, 12:53
Default
  #5
Senior Member
 
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 6
Chander is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
This means it is very common to start a CFX steady state run with a small timestep and run that for a few iterations to set the flow up, but then start increasing the time step size as the flow settles down. As you approach convergence you can often be running time steps 100 or 1000 times larger than you started with. Use the "Edit run in progress" feature of the sovler manager and you can do this without stopping and restarting the run.
Thanks Glen again for the detailed reply. It clarified a lot.
I have one query here. In my simulations, I find that convergence stalls and when I reduce the timestep, it goes towards convergence. But when I reach near convergence I have to keep the time step small until the convergence is reached.
This is because in one of the simulations I tried the following:
1. I first got a solution with reduced time-step.
2. Then used this as initial condition with a larger time-step. The residuals actually went up and stabilized at the higher level (inside the red circle)! Does this point to some error in problem setup?
Attached Images
File Type: jpg momentum_residuals_komega.jpg (36.6 KB, 404 views)
Chander is offline   Reply With Quote

Old   December 23, 2013, 06:31
Default convergence problem
  #6
New Member
 
Bitte56
Join Date: Mar 2013
Location: India
Posts: 15
Rep Power: 4
ARohit is on a distinguished road
[QUOTE=ghorrocks;305513]a) You can use any time step you like to get convergence. A larger timestep will usually get there quicker, that is why it is recommended.

b) Yes, CFX is fully implicit (although there are some physics models which are not, such as surface tension and particle tracking, but that is another matter). The importance of time step size is that is what CFX uses to stabilise the equations. A SIMPLE based solver uses under relaxation factors. CFX uses time step size.

c) Just as for under relaxation (URF) on SIMPLE based solvers, you want to use the largest URF which converges reliably. Then you often reduce it a bit for safety. Likewise in CFX you use the largest timestep which converges. As you approach convergence the equations often become more stable, meaning that you can increase the timestep size.

This means it is very common to start a CFX steady state run with a small timestep and run that for a few iterations to set the flow up, but then start increasing the time step size as the flow settles down. As you approach convergence you can often be running time steps 100 or 1000 times larger than you started with. Use the "Edit run in progress" feature of the sovler manager and you can do this without stopping and restarting the run.[/ Sir, I am also having the convergence problem. I have attached image here. When i reduced time step, residuals actually went up. why? ]
Attached Images
File Type: jpg prob2.jpg (104.0 KB, 152 views)
ARohit is offline   Reply With Quote

Reply

Tags
cfx, convergence stall, steady state, time step

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
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
How to write k and epsilon before the abnormal end xiuying OpenFOAM Running, Solving & CFD 8 August 27, 2013 15:33
Time step of steady particle tracking payam_IUST FLUENT 1 October 12, 2009 08:19
false time step implementation for steady state Kushagra CFX 1 June 22, 2008 19:06
Small time step and CFX solver crashing Vanessa CFX 2 June 21, 2006 09:18


All times are GMT -4. The time now is 03:34.