I will work out with this. Thanks..
In transient flow in the convergence history graph (the coefficient of lift (CL) vs Flow time) the calibrations on CL is very high i.e scale of 100 is used, so CL line looks like straight (but there is some oscillation which i cannot see precisely), how can I change or set the CL scale?

I have a question related to this for my special case.

For my case, the transient behavior is not significant. The solution of my simulation is not time dependent according to the transient simulation results. But I have to run the transient simulation just because the steady state solution doesn't not converge. In this case, I'm wondering will large time step bring me faster to the steady solution than the small time step (here we assume they converge to the same residual level every time step with the same iteration number)? If I choose the large time step as 0.0001, and the smaller one as 0.00001. Will the large time step transient simulation bring me to the steady solution almost 10 times faster then the small one?

I think so.
With larger time step, the solution evolves faster from the initial conditions towards the final solution.
But since you encountered difficulties with a steady-state solver, dont expect this to hold true for arbitrary time step sizes. The transient solver might have the same difficulties converging the solution when the time step size is too high.

But will it be 10 times faster? I also encounter the problem of choosing large time step or small one now. Large time step need more iterations to converge at every time step. But it doesn't seem to evolve much faster from the initial conditions towards the final solution. It seems to me that, for this kind of 'stead' case, large time step can never be better than small one. Maybe it's better to have time step very small?

If the flow is really time-dependent, you will get to the same point with 10 times less time steps if you choose a time step 10 times larger, provided both time step sizes are able to resolve the relevant transient effects.
Of course with an implicit method you will need more iterations per time step to achieve the same level of convergence.

But since you are using a transient solver as a computational workaround for a flow that might have no transient effects at all or at least we dont know the time scale of the flow, I would not expect the exact same behavior.

Lets have a look at a simple example, the couette flow between two parallel plates initially at rest.
The flow actually is time-dependent, but if the Reynolds number is sufficiently low, it will reach a steady state, a linear velocity profile between the two plates.
So we could simulate the long-term-solution of this flow both with a steady solver or with a transient solver.

But how long will it take for the transient solver? The viscous time scale at which the flow develops is

If we choose the time step size of the transient solver to be 1/10th of the viscous time scale, we need an order of 10-100 time steps to reach the steady state.
If we choose a time step size of 1/1000th of the viscous time scale, we need an order of 1000-10000 time steps to reach the same solution, which will obviously take longer.

To conclude: It is not always better to have a small time step size.

time step size in vof method
 

I am working on 2 phase flow using vof method and i want to know how to calculate the time step and the number of time steps and how to determine the maximum number of iterations per time step?

Global Courant Number in Fluent 15.0
 

Hi everyone.

I am currently investigating multiphase flow in a pipe with regards to how it develops. I am currently using a grid size of 2 and the highest input velocity is 0.3m/s. In order to have my Courant number less than 1, I am using a fixed time step of 0.0006s.

However, I am getting a Global Courant number of 5.03. Would this affect the accuracy of my simulation? And if so how do I reduce the Global Courant number and is there even a need to do so?

Thank you.

See this link
http://cape-forum.com/index.php/topi...2.html#msg1392
William provides guidelines for CFL numbers using VOF approach in FLUENT. They are also summarized here.

CFL number greater than some value (generally, 1, 2.5 for multi-stage FLUENT solver) would result in numerical instability when using explicit formulation. It is allowed for implicit solver, however, rising CFL leads to increased numerical error due to the fact that every mesh-based solution becomes less precious when increasing step size (both time step and mesh step, the latter just means coarsening the mesh). However, if you have no transient effects you can use higher CFL.
You can run several calculations refining the time-step, the results should converge to some values (it's like mesh convergence, just refining time-step instead of mesh element size).

Time step!
 

I have two situations in unsteady state simulation of two phase flow in fluidized bed (gas-solid):
1- time step is 0.0001
2- time step is 0.001
in each case solution converge in each time step. in the case 1, after 10000 time step, solution is achieved for t=1 s. in the case 2, after 1000 time step, solution is achieved for t=1.
my question is:
two solution should be same for t=1?

Only if the solution is independent of the time step size already for the larger time step.

thanks for your answer
how can in found that the solution is independent of time step?

By doing almost exactly what you described ;)

Run the same simulation with at least three different time step sizes. Compare the solutions, e.g. by plotting a variable of interest over the time step size.
The factor between the the different time step sizes does not have to be as large as 10. A factor of 2 should be sufficient.
"Pro" tip: if you want to know if the simulation is independent of the time step size for a time step size of lets say 0.01s. You don't need to run two additional simulations with even smaller time step sizes which can be a computationally expensive task.
You might as well run two additional simulations with larger time step sizes, e.g. 0.02s and 0.04s.

with this much less time step you sure will get convergence easily and get better results but if you have to solve for like 80 seconds. It will take a lot of time. What you you do to solve in this situation?? And my second question is refining mesh and using low time step, does it help to get better results than using less fine mesh and time step of 1E-05

Hello Lucky Tran,

"As you decrease the time-step size, the residuals typically decrease faster. The initial guess to the next iteration uses the final solution from the previous time-step. Since the difference in physical time between time-steps is smaller, the difference in solution between the previous time-step and current time step is smaller and this causes the residuals to decrease faster when the time-step is shortened."

My case: I am simulating an airfoil at Re 1million using K omega sst intermittency. Please correct me if im wrong but...

From the highlighted statement,

My understanding is that if i want the lift and drag to converge faster (roughly), i should just maintain using a bigger time step because the change in solution is bigger. Later reduce the time step to increase accuracy (smaller changes in the solution).

I also saw your suggestion in another thread saying that 20 inner iteration is a good choice for each time step and it is better to run 20 iter x 2 timestep rather than 40 iter x 1 timestep.

I am somehow confused with this second statement, if the lift and drag can converge faster (rough values) using a bigger time step, should`nt we increase the total number of bigger timestep and once it settles down (somewhat constant) then use a smaller timestep.

Hope you can please clarify. Thank you!

p/s Just noticed theres a second page. Flotus1 I believe already answered this question