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

Time step size & convergence absolute criteria

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 2, 2013, 12:30
Default Time step size & convergence absolute criteria
  #1
New Member
 
yui tsang
Join Date: Mar 2013
Posts: 1
Rep Power: 0
yuitsang is on a distinguished road
Hi,

I am a student currently working on a simulation of a confined room with a steady inlet using fluent. My model is struggling to get converged (10^-4) with a steady approach and therefore I am trying to use a transient approach instead. My question is how I should determine the time step size and convergence absolute criteria.
I have read from previous relevant post in which time step size was said to be equal to delta x/velocity, where delta x is size of the smallest cell. however, I wonder how I could determine the velocity for that?
On top of my question about the convergence absolute criteria, I also noticed that residuals is not the only indicator for convergence. It was suggested in another post we could check if the solution is converged by implementing some control/monitor points. I wonder what this means explicitly.

Background of case:
-Room with demensions of 4.6x3.36x3m with Displacement Ventilation system.
-Inlet and outlet are defined as mass-flow inlet and pressure-outlet.
-the only heat source in the room is human - defined as heat flux of 160W/m2 on the head

Thank you very much for your time on my post!


Matthew

Last edited by yuitsang; March 2, 2013 at 14:02.
yuitsang is offline   Reply With Quote

Old   March 4, 2013, 04:42
Default
  #2
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,099
Rep Power: 16
RodriguezFatz will become famous soon enough
Good questions!
1. Your "non-converged" solution, how do the results look like? Completely wrong or not? If not, you could use the velocity you get there to estimate your velocity for the transient case. The "dx / dv" comes from the Courant criterion, or Courant-Friedrich-Lewy = CFL criterion (http://en.wikipedia.org/wiki/Courant...Lewy_condition). This is the maximum time step you can use, when you use a explicit time integration. It means, that a fluid particle does not move more than one cell during a single time step and is needed for stability in explicit time integration. As I understand it, it is not relevant for implicit time-integration, which you should use anyway most of the times. Main advantage of explicit time integration is, that it is easier to implement. Since you bought Fluent, this is fortunately not relevant to you...
Now, what I suggest is to take one characteristical lenght scale "L" of your system (such as the room size) and have - let's say - 20 time steps for the fluid to travel through the domain, so that dt = L / (20*v).
You can increase that number (20) later, if you don't get the results you are looking for or have numerical problems.

2. Small residuals can however mean, that your solution is still not final, thus it changes from iteration to iteration (but slowly). Sometimes you can monitor some characteristical value inside you domain, such as the (area integrated) heatflux through the outlet, or some force on a body and plot it each iteration. At best, this is your value of interest and some (area or volume) integral value. In Fluent you can go to "Monitors -> Surface Monitors" or "Volume Monitors" and create one.
If this value stops changing when iterating, your solution also converges. This is a good additional (to the residuals) tool.

3. Can you post a picture of you setup and of your mesh? You should be able to get convergency, also for the steady state...
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   March 6, 2013, 11:02
Default
  #3
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11
oj.bulmer will become famous soon enough
You may need to do the timestep study to understand what timestep is just enough to bring down your residuals to the convergence criteria you are happy with (say 1e-5 etc). Or, easier way is to use adaptive timestepping to let FLUENT determine its ideal timestep.
This way we ensure that every timestep is converging.

Regarding the convergence criteria, for transient analysis there are different scenarios. If the case can finally come to steady, you should see the monitors straight. If the case is periodic, you will keep seeing the periodic oscillations. In this case you will need to monitor the periodicity in the monitors, and then stop when have simulated enough long. If it is chaotic, the monitor oscillations can be indeterministic and you may need to monitor certain volumetric parameters to make sure the simulation has run long enough.

For your case, you may also consider plotting volumetric mass imbalance and total volumetric heat generated in the system as well. There may be a point where total heat in the room will stay constant with increase in time, this may be yoru convergence.

OJ
oj.bulmer is offline   Reply With Quote

Old   March 21, 2013, 01:32
Default transient convergence enquiry
  #4
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
Dear all,

with reference to the attachment, what are the oscillations mean please?
i'm performing a fluid-thermal coupling 3D transient analysis for a total time of 2400s. as seen on the attachment, less than 100s, i'm getting oscillations in the T-Energy RMS residual plot on all components.

on the fluid side, the turbulence RMS residuals and others have reached 1e-4 criteria, but not for heat transfer, and this calculation is still on-going.

Please help!
Thanks.
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   March 21, 2013, 05:53
Default
  #5
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11
oj.bulmer will become famous soon enough
This is a FLUENT forum and from your image, it seems that you are using CFX. If may be appropriate to post this question on CFX forum.
http://www.cfd-online.com/Forums/cfx/

Have you read all the documentation on CFD FAQ here:
http://www.cfd-online.com/Wiki/Ansys_FAQ

The residuals don't seem right. In transient simulation, you should make sure that your imbalances are reduced to within 1% for every timestep. I can't see the plot of imbalances in your image.

OJ
oj.bulmer is offline   Reply With Quote

Old   April 15, 2013, 04:27
Default
  #6
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
Dear OJ,
thanks for the advice.

what if the imbalances are not within 1% between every timestep? what does that indicate i should check please?
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   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
Superlinear speedup in OpenFOAM 13 msrinath80 OpenFOAM Running, Solving & CFD 18 March 3, 2015 06:36
How to write k and epsilon before the abnormal end xiuying OpenFOAM Running, Solving & CFD 8 August 27, 2013 15:33
OF 1.6 | Ubuntu 9.10 (64bit) | GLIBCXX_3.4.11 not found piprus OpenFOAM Installation 22 February 25, 2010 14:43
Navier-Stokes time step size Martin Main CFD Forum 2 June 6, 2008 03:38
Phase locked average in run time panara OpenFOAM 2 February 20, 2008 15:37


All times are GMT -4. The time now is 21:02.