[wc34071209]

Hi,

When I enable 'pseudo transient', the Courant number disappears in the Control tab.

What is the essential difference between pseudo-transient and steady-state for coupled pressure based solve in Fluent?

Thank you!

Originally Posted by LuckyTran

That's actually an under-relaxation factor for the coupled solver and hence why it is listed with the under relaxation factors in the Fluent GUI. It has no direct connection to time-stepping and the CFL number (i.e. you can use the coupled solver for steady-state problems). But the change in the solution from one iteration to the next is analogous to some change in time so that urf's can also be interpreted as local shortening/lengthening of this time-stepping and it turns out that this characteristic time-step so happens to be the cell Courant number so finally it makes sense at the end to call this something related to a courant number. Unfortunately the Fluent devs decided to simply call it courant number to make it confusing rather than something like CFL multiplier.

oj's post earlier in this thread gave a really detailed explanation of the meaning of CFL (which is actually a urf).

See also 21.4.4.2 in the Fluent Theory Guide.

A CFL of 200 is equivalent to an implicit under-realxation factor of 0.995 (not much under-relaxation). An infinite CFL is urf = 1 and CFL of 1 is urf = 0.5. The default value has changed over time from 50 to 100, I guess it is 200 now. Higher is better so you probably do not want to mess with this option until your solution diverges.

[AhmadHij]

Originally Posted by LuckyTran

That's actually an under-relaxation factor for the coupled solver and hence why it is listed with the under relaxation factors in the Fluent GUI. It has no direct connection to time-stepping and the CFL number (i.e. you can use the coupled solver for steady-state problems). But the change in the solution from one iteration to the next is analogous to some change in time so that urf's can also be interpreted as local shortening/lengthening of this time-stepping and it turns out that this characteristic time-step so happens to be the cell Courant number so finally it makes sense at the end to call this something related to a courant number. Unfortunately the Fluent devs decided to simply call it courant number to make it confusing rather than something like CFL multiplier.

oj's post earlier in this thread gave a really detailed explanation of the meaning of CFL (which is actually a urf).

See also 21.4.4.2 in the Fluent Theory Guide.

A CFL of 200 is equivalent to an implicit under-realxation factor of 0.995 (not much under-relaxation). An infinite CFL is urf = 1 and CFL of 1 is urf = 0.5. The default value has changed over time from 50 to 100, I guess it is 200 now. Higher is better so you probably do not want to mess with this option until your solution diverges.

So I am working on a 2D transient simulation of a vertical axis wind turbine. I tried first to run the simulation at tip speed ratio (TSR 2.58). Things were fine, but when I moved to TSR 1, I am getting a very low results in comparison with experimental results in terms of comparing the power coefficient Cp. I am using the coupled pressure-velocity solver (it is pressure based type) so I noticed that in the solution control panel, there is a flow courant number that is 200 by default. I changed it to 1, and run the simulation. I got close results to experimental.

Can I use a flow courant number equals to 1 since it is giving better results than the default number 200 ?

[oj.bulmer]

Exactly, so what does this Courant number means? There's not too much info in Fluent theory guide.

A bit of theory:

The algebraic approaximation of integral balance for any control volume is given as:



Patankar (1980,1981) proposed the underrelaxation factor as



This is same as equation 20-60 in ANSYS Help documentation of FLUENT.

The implementation of CFL in this context is:

or,

Consequently the governing equation for the control volume becomes:



One may wonder why bother using CFL instead of , when the governing equation is same. But a little observation will bring clarity such that the equation advances in time , where . In case of steady state, this formulation can be used in with pseudo transient solver. Thus CFL represents a more intuitive definition of implicit underrelaxation.

Essentially, use of CFL helps advance the solution by multiples of timesteps defined by cell Courant number (the original one, not solver). Essentially, for smaller timestep, the coefficient will be large and solution will be slow, universally. The multiple of CFL helps in keeping timesteps different in different regions of the domain, with different values of , instead of employing a singular timescale over whole domain. Thus timestep becomes location specific and is different throughout the domain. This helps in convergence, because in case of single universal timestep, its value may be too small somewhere (in case of higher velocities) so the solution in this region will progress slow in time or too large elsewhere (in regions of small velocities) so the solution in this region may just diverge inducing instability.

One of the most important aspect of using this formulation instead of under relaxation factor is that with CFL you have a wider range of advancement factors. Under relaxation factors of 0.9,0.95 and 0.99 imply CFL values of 9, 19, 99 respectively. Thus use of CFL gives a wider (or refined) range of pace-change than URF. Higher values of CFL will advance the solution with larger timesteps, increasing pace of solution. But it is wise to do it gradually than suddenly.

OJ

[macfly]

Originally Posted by oj.bulmer

A bit of theory:

The algebraic approaximation of integral balance for any control volume is given as:



Patankar (1980,1981) proposed the underrelaxation factor as



This is same as equation 20-60 in ANSYS Help documentation of FLUENT.

The implementation of CFL in this context is:

or,

Consequently the governing equation for the control volume becomes:



...

Thanks for the theory! But there is still something I don't understand: when we adjust the Flow Courant Number (under Solution Controls), why can we still adjust the URFs? The way I see the equations, the solver uses either the CFL formulation or the formulation. Why can we adjust both?

[Jonathan]

Dear OJ,

Thanks very much for this post. It is very helpful

Could i just ask a few additional questions if possible? According to some documentation i found on the web produced by ANSYS, the Courant No. in the context of the PBCS in Fluent affects the diagonal dominance of the coefficient matrix, and therefore the solution stability - and this is clear in the context of linear solver convergence theory etc. Effectively, this does the same thing as the implicit URF's in the segregated solvers ...

However, in one of your posts below, you mention the explicit under-relaxation (relaxation of variables) affects the inner loops of the PBCS? Could i ask you to clarify this further? Do you mean the linear solver loops? i.e. PBiCG solver loops etc? Or where exactly in the algorithm are the explicit URF's applied?

I know in OpenFOAM, for instance, in their SIMPLE implmentation, they use explicit under-relaxation for the pressure equation, but implicit (equation) URF's for MOM, TKE and Eps etc.

I wonder if you would mind explaining this a little further?

Also, in your current (this) post, you use the following nomenclature:

, where .

I was wondering whether you could just explain your nonemclature? obviously is time ... is cell-volume, i.e. mesh size? Also i am assuming is some sort of global time step??

One of the most important aspect of using this formulation instead of under relaxation factor is that with CFL you have a wider range of advancement factors. Under relaxation factors of 0.9,0.95 and 0.99 imply CFL values of 9, 19, 99 respectively. Thus use of CFL gives a wider (or refined) range of pace-change than URF..

I never thought of it this way - that is very helpful! thanks!

Finally - could you comment on how the explicit URF's affect the simulation behaviour? As per above, i know Courant No. in this context affects the convergence stability - how then do the explicit URFs participate? Are they related somehow to the need to deal with the governing equation non-linearities?

Again, thanks very much for the post,
best regards
Jonathan

[Far]

Originally Posted by Bollonga

For a 1.7 Gb mesh, 8 cores parallel, 12 Gb RAM it's taking 45 min for each step.

Also, I will have to do a transient laminar case and steady/transient k-omega SST, which solver setup should I use? SIMPLEC? PISO?

Thanks in advance!

You need to add more resources to run 8 million mesh.

For transient case PISO and coupled are good option as they can accommodate larger time steps... And I would prefer coupled. Still not checked the results, accuracy and speed of these two schemes...