CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   How to determine time step size and Max. iterations per time step. (http://www.cfd-online.com/Forums/fluent/98249-how-determine-time-step-size-max-iterations-per-time-step.html)

pratik c March 6, 2012 15:41

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

ghost82 March 7, 2012 04:47

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

pratik c March 7, 2012 05:38

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?

ghost82 March 7, 2012 05:52

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

pratik c March 7, 2012 06:28

Thank You Danielle.

duri March 9, 2012 16:20

Quote:

Originally Posted by ghost82 (Post 348068)
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.

sudhir.iisc March 11, 2012 05:59

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 (Post 348068)
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


cfd seeker March 12, 2012 11:42

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 March 13, 2012 14:02

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 (Post 348632)
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 March 13, 2012 14:25

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 (Post 348970)
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. ???


duri March 13, 2012 15:52

Quote:

Originally Posted by cfd seeker (Post 348970)
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.

mahi007 March 18, 2012 23:34

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

yashganatra June 19, 2013 07:10

Is it steady state or transient?

Tanjina June 19, 2013 11:09

time step
 
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.

yashganatra June 20, 2013 02:31

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

Tanjina June 20, 2013 10:03

2 Attachment(s)
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.

yashganatra June 20, 2013 12:15

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 ;

Tanjina June 20, 2013 17:16

2 Attachment(s)
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.

yashganatra June 21, 2013 01:34

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.
http://www.cfd-online.com/Forums/flu...-momentum.html

Tanjina June 21, 2013 14:15

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.


All times are GMT -4. The time now is 12:19.