[DaveyBaby]

Hi,
B<A <=> A>B :-)
You could try a steady-state sim to get results to initialise the unsteady one, then adjust the timestep such that for this initial velocity field the Courant number will be less than about 0.7.
Then run it for a bit and see what is happening with your Courant Number, adjusting the timestep accordingly. You may find that you have a refined grid where you don't need much spatial resolution and if your Courant numbers are highest here you can coarsen the mesh accordingly so that you can increase your timestep. Watch y+ values as well to make sure they are appropriate for your model.
Then you could play around with grid coarsening/refinement and timestep size to get the balance you are happy with, always maintaining Courant numbers lower than 1. It is ok if far from your domain of interest there are isolated (in time and space) instances of C>1, but this is not ideal.

[hwsv07]

Originally Posted by DaveyBaby

Hi,
B<A <=> A>B :-)

gosh. i wrote that wrongly. i have edited my post.

i mean to say it as:

A should takes less time than B because higher Courant => larger timestep => less iterations to reach simulation end time.

so did u meant it to be as such?

Originally Posted by DaveyBaby

Hi,
B<A <=> A>B :-)
You could try a steady-state sim to get results to initialise the unsteady one, then adjust the timestep such that for this initial velocity field the Courant number will be less than about 0.7.
Then run it for a bit and see what is happening with your Courant Number, adjusting the timestep accordingly. You may find that you have a refined grid where you don't need much spatial resolution and if your Courant numbers are highest here you can coarsen the mesh accordingly so that you can increase your timestep. Watch y+ values as well to make sure they are appropriate for your model.
Then you could play around with grid coarsening/refinement and timestep size to get the balance you are happy with, always maintaining Courant numbers lower than 1. It is ok if far from your domain of interest there are isolated (in time and space) instances of C>1, but this is not ideal.

i have run my unsteady simulation and monitoring the entire domain's courant number. i found that my C was slightly > 1 (~1.2) for a few hundred iters (inclusive of inner iters) before dropping below 1.

other than reducing the timestep (which will increase the simulation time), do you know if it is possible to increase the size of the time step for each iter as the iteration is marching forward?

[DaveyBaby]

In version 10 under Solvers>Implicit Unsteady>Time-Step you can use a field function to define the time-step size if you like instead of it just being a constant. Among the independent variables, you can select time and define a timestep=f(t). You can probably do this in some earlier versions as well.
The problem is, you need to know a priori what the solution will be to know what timestep is ok.

[DaveyBaby]

Looking over this forum, it seems that I have also made some assumptions in my answers that may or may not be relevant to your case. I would thoroughly recommend searching the whole set of forums for "Courant" and find an answer that is appropriate to you. It seems that this issue of Courant number is more complex than I thought, I am only dealing with a subset of cases. Although a good rule of thumb is to keep Courant numbers below 1, this is not a complete answer, it seems that a timestep dependency study may allow you to have them higher.

[hwsv07]

im running 9.06 and it doesnt have this feature - only has constant timestep input.

[DaveyBaby]

For now, I would recommend monitoring it periodically and checking that C<1.
From reading around the forums, I have found that the issue is more complex than I previously thought, to the point where it is hard to give a faultless response. I have started a thread in the Main CFD forum, hoping to draw together a lot of responses from experienced users, maybe it will be of interest to you.

[hwsv07]

Originally Posted by DaveyBaby

In version 10 under Solvers>Implicit Unsteady>Time-Step you can use a field function to define the time-step size if you like instead of it just being a constant. Among the independent variables, you can select time and define a timestep=f(t). You can probably do this in some earlier versions as well.
The problem is, you need to know a priori what the solution will be to know what timestep is ok.

ok i managed to get my hands on Version 10.02.012 from my support.

I opened my casefile which was created in version 9, but I do not see this field function option to set the size of my time-step.

are you sure this is an option within version 10? can u show a screen shot please.

[DaveyBaby]

It is not immediately obvious, I would say it is a badly designed route via the gui.
Solver>Implicit Unsteady
Right click "Implicit Unsteady", click "Edit"
Left click [...]
Left click [...] in the next pop-up

[hwsv07]

awesome i found it.

pardon my ignorance, but is it possible to do like an "if/else" definition?

to recap - im trying to increase the size of the timestep as my simulation progresses. so say, for the iter<=5000 , timestep=0.01 ; for iter>5000, timestep = 0.05.

[DaveyBaby]

Yes it is. Field functions are very versatile. If you search "Field Function Programming Reference" under help you will find all you need. Remember this bit of the help menu, I have probably used it more than anything else but it's not easy to remember the root to it through the menu so best to search it.

[hwsv07]

Originally Posted by DaveyBaby

Yes it is. Field functions are very versatile. If you search "Field Function Programming Reference" under help you will find all you need. Remember this bit of the help menu, I have probably used it more than anything else but it's not easy to remember the root to it through the menu so best to search it.

thanks. i figured it out.

on another question: is it possible to create a Report that gives a "1" or "0" when my stopping criterion has been achieved?

Upon achieving the stopping criterion, I want to be able to change a setting and then continue my simulation.

[DaveyBaby]

Probably, using "Expression Report", and using "Time" and "Iteration" in the definition. I have never done this though. Please let me know if you find a way!

[hwsv07]

i didn't find a way to do that. Right now, Im just doing it manually.

[hwsv07]

Im not sure it is the same issue as with other CFD softwares.

In CCM, for implicit unsteady cases, there is also a Courant number for the inner iterations - which from my understanding ; adjusts the psuedo timestep to obtain a result at the particular timestep.

I'm monitoring my Courant Number on the global timestep and it is below 1.

How do i set the Courant Number in Coupled Implicit>>Courant Number?

[Nabuchadresar]

I'm running a unsteady simulation. I am testing what best time-step and best mesh refinement, but I don't know which one should I do first. Any advice?

[hwsv07]

Originally Posted by Nabuchadresar

I'm running a unsteady simulation. I am testing what best time-step and best mesh refinement, but I don't know which one should I do first. Any advice?

I suggest doing a steady case, get the mesh resolution right first - make sure the results correspond to a known reference.

Then move to the unsteady case.

[Nabuchadresar]

Originally Posted by hwsv07

I suggest doing a steady case, get the mesh resolution right first - make sure the results correspond to a known reference.

Then move to the unsteady case.

Good idea.

Thank you.