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

How to determine time step size and Max. iterations per time step.

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

Like Tree16Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   March 6, 2012, 15:41
Default How to determine time step size and Max. iterations per time step.
  #1
New Member
 
Pratik
Join Date: Jan 2012
Posts: 11
Rep Power: 5
pratik c is on a distinguished road
I am trying to simulate airflow through a room and am performing a transient calculation. Could someone please tell me how to determine time step size and max iterations per time step?
rgd and hashim84 like this.
pratik c is offline   Reply With Quote

Old   March 7, 2012, 04:47
Default
  #2
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 918
Rep Power: 15
ghost82 will become famous soon enough
Hi,
A rule of thumb is to set time step< deltax/u
where deltax is the smallest cell size and u is the velocity.

Usually I set max iteration per time step equal to 50 or 100, depending on residual values (if I want convergence at 10^-3 ^-4 I set near 50, if I want 10^-7 closest to 100).

Daniele
saha2122, rgd and hashim84 like this.
ghost82 is offline   Reply With Quote

Old   March 7, 2012, 05:38
Default
  #3
New Member
 
Pratik
Join Date: Jan 2012
Posts: 11
Rep Power: 5
pratik c is on a distinguished road
Sorry I am quite new to this. Could you please tell me how to determine the smallest cell size?. And also what number of time steps would I need?
rgd likes this.
pratik c is offline   Reply With Quote

Old   March 7, 2012, 05:52
Default
  #4
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 918
Rep Power: 15
ghost82 will become famous soon enough
Pratick,
the smallest cell size can be determined from your grid.
If you have done your grid with your pre processor, gambit for example, you know what is the cell size, and where your domain is more refined.
If you have for example one of the smallest quad cell measuring 0.001x0.005, then your smallest cell size will be 0.001.
If you have tri cell then take the smallest side of the cell.

The total number of time steps depends on your simulation: it can be 1 s or 20 s (i.e. total number of time step=1s/timestep or 20s/time step), it depends on your system and on what you are looking for.
If this is your case, you can estimate and take into account a transient period and a period in which your system reaches a pseudo-steady state.

Daniele
saha2122, silverra1n and rgd like this.
ghost82 is offline   Reply With Quote

Old   March 7, 2012, 06:28
Default
  #5
New Member
 
Pratik
Join Date: Jan 2012
Posts: 11
Rep Power: 5
pratik c is on a distinguished road
Thank You Danielle.
pratik c is offline   Reply With Quote

Old   March 9, 2012, 16:20
Default
  #6
Senior Member
 
duri
Join Date: May 2010
Posts: 130
Rep Power: 7
duri is on a distinguished road
Quote:
Originally Posted by ghost82 View Post
A rule of thumb is to set time step< deltax/u
where deltax is the smallest cell size and u is the velocity.
This is correct for explicit schemes but solver take cares of it. In case of implicit solver we can go for higher time steps (>100 times). This results in faster solution.
Start with some characteristic length to characteristic velocity ratio. Reduce or increase the time step by an order based on the no. of iterations it takes to converge.
duri is offline   Reply With Quote

Old   March 11, 2012, 05:59
Default
  #7
New Member
 
sanjay
Join Date: Nov 2010
Location: Bangalore
Posts: 1
Rep Power: 0
sudhir.iisc is on a distinguished road
Hi Daniele,

It would be better to adjust the time step such that maximum iteration/time step not more then 20. If Solution is not converging within this pseudo time step (iteration) then prefer to decrease physical time step.


Quote:
Originally Posted by ghost82 View Post
Hi,
A rule of thumb is to set time step< deltax/u
where deltax is the smallest cell size and u is the velocity.

Usually I set max iteration per time step equal to 50 or 100, depending on residual values (if I want convergence at 10^-3 ^-4 I set near 50, if I want 10^-7 closest to 100).

Daniele
sudhir.iisc is offline   Reply With Quote

Old   March 12, 2012, 11:42
Default
  #8
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
I want to ask what is the role of Courant No. in determining the time step size??
As we know Courant No. = velocity*delta(t)/delta(x), by this equation time step size is directly proportional to Courant No, so can we use bigger time step size by increasing the Courant No. ???
cfd seeker is offline   Reply With Quote

Old   March 13, 2012, 14:02
Default
  #9
Member
 
banty
Join Date: Mar 2012
Posts: 52
Rep Power: 5
banty is on a distinguished road
But in case of wave tracking, even with the implicit solver time step should be taken such that wave should be not move more then one cell in single time step.

Quote:
Originally Posted by duri View Post
This is correct for explicit schemes but solver take cares of it. In case of implicit solver we can go for higher time steps (>100 times). This results in faster solution.
Start with some characteristic length to characteristic velocity ratio. Reduce or increase the time step by an order based on the no. of iterations it takes to converge.
banty is offline   Reply With Quote

Old   March 13, 2012, 14:25
Default
  #10
Member
 
banty
Join Date: Mar 2012
Posts: 52
Rep Power: 5
banty is on a distinguished road
Role of Courant no depends upon the solvers setng.

In case of pressure based and density based (both explicit and implicit) solver with backward euler (1st and 2nd order), time step(physical time step) is entered by the user based on physics involved and CFL no & no of sub iteration decides the speed of convergence.

But in case of explicit-explicit density based solver, time step (physical time step) is decided by the CFL no (User Input) and based on Courant No. = velocity*delta(t)/delta(x).





Quote:
Originally Posted by cfd seeker View Post
I want to ask what is the role of Courant No. in determining the time step size??
As we know Courant No. = velocity*delta(t)/delta(x), by this equation time step size is directly proportional to Courant No, so can we use bigger time step size by increasing the Courant No. ???
banty is offline   Reply With Quote

Old   March 13, 2012, 15:52
Default
  #11
Senior Member
 
duri
Join Date: May 2010
Posts: 130
Rep Power: 7
duri is on a distinguished road
Quote:
Originally Posted by cfd seeker View Post
I want to ask what is the role of Courant No. in determining the time step size??
As we know Courant No. = velocity*delta(t)/delta(x), by this equation time step size is directly proportional to Courant No, so can we use bigger time step size by increasing the Courant No. ???
Yes you can use but it can only control the time step size of inner iterations. It will help in faster convergence of inner iteration but remember there is a restriction on this value due to numerical stability (even for implicit). In unsteady problem physical time steps are more important that numerical time steps to capture a phenomenon.
duri is offline   Reply With Quote

Old   March 18, 2012, 23:34
Default
  #12
Member
 
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 4
mahi007 is an unknown quantity at this point
Hello

I am doing analysis of flow past circular cylinder. Can anyone suggest me what are the solver settings?

And how to calculate time step?

Regards
Mahindra
mahi007 is offline   Reply With Quote

Old   June 19, 2013, 07:10
Default
  #13
Member
 
Yash Ganatra
Join Date: Mar 2013
Posts: 67
Rep Power: 4
yashganatra is on a distinguished road
Is it steady state or transient?
yashganatra is offline   Reply With Quote

Old   June 19, 2013, 11:09
Default time step
  #14
Senior Member
 
Tanjina Afrin
Join Date: May 2013
Location: South Carolina
Posts: 161
Rep Power: 4
Tanjina is on a distinguished road
Hi,

I have also similar question, but couldn't find any definite answer. i am trying to model a flow through a circular pipe from a rectangular reservoir. I used workbench for meshing. It's triangular mesh. element size is 6e-3m. How can I determine time step. I modeled 3D. I couldn't find any option called iteration/time step, but in may tutorial I saw it.
Tanjina is offline   Reply With Quote

Old   June 20, 2013, 02:31
Default
  #15
Member
 
Yash Ganatra
Join Date: Mar 2013
Posts: 67
Rep Power: 4
yashganatra is on a distinguished road
Post some more details. Attach photos of the mesh.
1. Is it steady state or transient?
2. Laminar or turbulent?
You can find the option in FLUENT in the Run Calculation settings in the Problem Setup tab on the left
yashganatra is offline   Reply With Quote

Old   June 20, 2013, 10:03
Default
  #16
Senior Member
 
Tanjina Afrin
Join Date: May 2013
Location: South Carolina
Posts: 161
Rep Power: 4
Tanjina is on a distinguished road
Hi,

This is 3-D transient time, turbulent two phase flow problem . I have attached two photo with this reply. please have a look on calculation setting photo.

More details : I want to let the water flow from the reservoir to circular pipe and let air fill up the empty place of reservoir which will be created after water going to reservoir.
Attached Images
File Type: jpg calculation setting.jpg (92.4 KB, 142 views)
File Type: jpg Mesh _full.jpg (96.1 KB, 113 views)
Tanjina is offline   Reply With Quote

Old   June 20, 2013, 12:15
Default
  #17
Member
 
Yash Ganatra
Join Date: Mar 2013
Posts: 67
Rep Power: 4
yashganatra is on a distinguished road
I see that divergence is being detected? For which quantity (momentum,energy etc) it is getting detected? Are you using VOF Model?Can't this be done in 2D also?Give snaps of Solution Methods and control ; from what I make out by referring to various threads, if the solution is not converging better to reduce time step.
See literature - a similar problem, what was the time stepping used ;
yashganatra is offline   Reply With Quote

Old   June 20, 2013, 17:16
Default
  #18
Senior Member
 
Tanjina Afrin
Join Date: May 2013
Location: South Carolina
Posts: 161
Rep Power: 4
Tanjina is on a distinguished road
I see that divergence is being detected? For which quantity (momentum,energy etc) it is getting detected? Are you using VOF Model?Can't this be done in 2D also?Give snaps of Solution Methods and control ; from what I make out by referring to various threads, if the solution is not converging better to reduce time step.
See literature - a similar problem, what was the time stepping used ;

At First, it showed AMG divergence: x-momentum. then I reduce momentum in relaxation factor from 1 to 0.7, 0.1. then model completed its run. But residual is not decreasing. its increasing with saw tooth shape.

yea I have used VOF model. Actually pipe is circular and tank is rectangular, so I didn't understand how can I model it in 2D.

Please find the screenshot of solution method and control.
Attached Images
File Type: jpg solution control.jpg (96.9 KB, 76 views)
File Type: jpg solution method.jpg (98.3 KB, 75 views)
Tanjina is offline   Reply With Quote

Old   June 21, 2013, 01:34
Default
  #19
Member
 
Yash Ganatra
Join Date: Mar 2013
Posts: 67
Rep Power: 4
yashganatra is on a distinguished road
Hi,
What I meant was that you can model the cross section. Why have you used Non Iterative Time Advancement? I have never worked with it so I have no idea about this. Check if your boundary conditions are correct.
Are those the default solution methods?
I did a quick search and found this thread. Hopefully it will help you.
Error: Divergence detected in AMG solver: x-momentum
yashganatra is offline   Reply With Quote

Old   June 21, 2013, 14:15
Default
  #20
Senior Member
 
Tanjina Afrin
Join Date: May 2013
Location: South Carolina
Posts: 161
Rep Power: 4
Tanjina is on a distinguished road
I just followed the step described in Tutorial 20, ink jet problem. My problem was little bit similar to that. That's why I used non -iterative time advancement.

I reduced under relaxation factor, after doing that model run its full time step I specified, but result was not expected.

I think I make some mistake in inlet BC. Can you suggest me anything about BC?

I can describe what I want to model and what I used in BC if you are interested.
Tanjina 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
Time step size and max iterations per time step pUl| FLUENT 31 August 21, 2015 04:46
Superlinear speedup in OpenFOAM 13 msrinath80 OpenFOAM Running, Solving & CFD 18 March 3, 2015 06:36
Time step size, number of time steps and max iterations per time step guido_88 FLUENT 4 August 30, 2012 14:49
icoLagrangianFoam OF1.6 myNewParticleSolver heavy_user OpenFOAM 16 February 11, 2012 06:15
Transient simulation not converging skabilan OpenFOAM Running, Solving & CFD 12 September 17, 2007 17:48


All times are GMT -4. The time now is 02:08.