[waseeqsiddiqui]

1) How does one set Courant number and time step size for transient density based implicit simulation?
2) How does one set Courant Number for pressure based steady coupled simulation?

[LuckyTran]

Please... be... specific. Also the Fluent manual has a ton of information to get started. There's also tutorials.

You are asking how to drive a car. Well it depends what you want the car to do! Do you want to turn left, turn right, accelerate, brake, or maybe just park the car and don't drive it?

By this example I mean you should describe what you are trying to simulate in Fluent (meaning what type of physics) but also what result you are trying to obtain! If you are solving only heat conduction in only a solid, hardly any of these settings matter!

[waseeqsiddiqui]

Okay the Fluent Manual gives a very general and brief explanation on Courant Number. My case is simple diverging pipe flow using pressure inlet and mass flow outlet.
I have learned from the manual that explicit CFL shall be very low while implicit can be set higher. Similarly, their formula including the term grid spacing and delta x.
More specifically,
1) What is the basic difference between time steps and CFL number?
2) How do I adjust my CFL number and time steps in transient situation?
3) What exactly is time step Independence?
4) If CFL is calculated for a mesh of y plus less than 1, is the grid spacing the length of the lowest mesh element?
5) How does P-V Coupled Courant differ compared to density based ones? Why is it set pretty high in steady case?
Thank you for your response. Apologies for bombarding too many questions.

[LuckyTran]

1) Time-step is the delta t in your simulation. There's two things that get easily confused by newbies, CFL and Courant number. The Courant number is a characteristic non-dimensional propagation rate for some reference time, velocity, and length scale (similar to Reynolds number, Mach number, etc). In the CFD context, you take the time-step size, the local cell size, and the local cell velocity. That means the Courant number is a field in x,y,z and time.

The CFL condition is a stability criterion for stable simulations and it is most often expressed as a Courant number needing to be less than 1.

2) How to adjust time-step? It is a user input right, in the GUI it's on the same page where press the calculate button.

3) Your solution should not depend on the time-step size that you take if it is time-step independent (similar to mesh independence). But it's wrong to say that it is independent, it's better to say sensitivity.

4)Here you mean Courant number and not CFL because CFL is a formal stability criteria that depends on the particular flow. The Courant number can be computed on any grid, regardless of whether it is y+ 1 or y+ 100000. The CFL criteria is that the Courant number should always be less than some critical value or the solution becomes unstable. To show that the Courant number is globally less than the CFL number, it is sufficient to simply check the maximum Courant number. If you use global time-stepping (where every cell in your mesh advances in time the same delta t) then the Courant number depends only on the local velocity and local cells size. The smaller the cell size, the larger the Courant number. Hence, if you were to guestimate a Courant number, it's a good idea to estimate it using your maximum expected velocity and your smallest cell size. This is just for an initial guess and for a predetermined time-step size because you don't actually know the local cell velocity yet. You'll know the actual Courant number after you run the simulation. If you don't like the Courant number that you achieve, you can adjust your time-step size and/or redo the mesh. Although the Courant number is an entire field in x,y,z and time, it's utility is normally just to check whether the CFL condition is satisfied and people often talk as if there is only one magical Courant number. They even forge that Courant number changes with time.

5) When you use the pressure-based solver with the COUPLED P-V solver, the Flow courant number there is very very very very very different than its meaning in any other place in Fluent. The Flow courant number there is easier to interpret as an under-relaxation factor. If you understand under-relaxation factors, then there is a cute formula to convert from this particular Flow courant number into an equivalent urf. You can also read this particular thread. For steady state simulations, the flow Courant number should be relatively low (50,100,200). This looks like a big number, and it is. For transient simulations, the flow Courant number should be set to infinity (I use 1e7). To understand why it is labeled Flow courant number, you have to fully understand the thread I linked. When you use implicit under-relaxation, even if you use a steady state solver, the calculation will still behave like a transient one. You want the Courant number high so that your solution converges faster (i.e. in fewer iterations). Implicit solvers can tolerate very large Courant numbers (Courant number can be >> 1 compared to explicit time-stepping). Well you can do the conversion to an equivalent urf to appreciate this. Some schemes (SIMPLE is a very good example) are quite unstable and need a lot of urf's to stabilize them. The reason for SIMPLE being unstable is exactly because it doesn't solve the coupled P-V problem but uses a predictor-corrector method. SO when you do use a COUPLED solver.... it's more stable and higher urf's or Flow Courant numbers can be used.