[Far]

This is the post where Re=40 results are posted and mesh file link is also provided. http://www.cfd-online.com/Forums/mai...r-re-40-a.html

Boundary conditions wre:

Dia = 1 m (necessary for Reynolds number)

Density = 40 Kg/m3

Viscosity = 1

Velocity = 1 m/sec

You can check your self how fast is coupled solver.

Yes you are right memory requirements are high, approximately twice of SIMPLE

[oj.bulmer]

I am not suspecting the idea. Personally, am a big fan of CFX's multigrid coupled solver. In one of the cases involving porous interface, for same mesh/physics, CFX converged within 80 iterations while FLUENT had to go till 1000!

I just like to observe things in totality

Cheers
OJ

[Far]

Are you talking about Fluent 14 + versions. One thing should be noted that in CFX CFL is not provided as option to user and it is decided by solver.

[oj.bulmer]

Yes, 14.5. Also, given sudden change of properties across the porous interface, I typically use local timescale option instead of auto/physical timescale, which smartly changes the timescales globally (ie, equivalent to variable CFL).

But of course you can always provide aggressive local timescale factor for faster convergence. Some opine that it is necessary to run last few iterations using Physical/auto timescale, while some think running local timescales "enough" is sufficient, ie when we witness flatter monitors and reduced imbalances.

OJ

[macfly]

Originally Posted by oj.bulmer

Oh well, I think there is a bit confusion over the concept of under-relaxation. There are two types:

1) (Explicit) Under-relaxation of variables: For pressure-based coupled algorithm, this would under-relax the individual variables in inner iterations. Notice that the under-relaxation type for momentum and pressure is EXPLICIT!

2) (Implicit) Under-relaxation of equations: For pressure-based coupled algorithm, CFL applied tries to under-relax the equations through full IMPLICIT coupling. The choice of CFL will influence the local timescale and eventually the solution of the equations, as specified in earlier (long) post. Essentially when CFL is used, the separate under-relaxation of flow equations is not needed. But for turbulence equations, URFs still needs to be specified.

Typical values of Explicit URFs (in pressure-based coupled case) for pressure/momentum being 0.75, it can be further increased to accelerate inner iterations. But for higher order schemes for momentum etc, often it needs to be reduced to say 0.5 etc, with very bad meshes requiring further reduction at times. Any divergence in AMG solver should indicate the high CFL value, which needs to be reduced.

OJ

Ok, got it. Sorry to waste your time. Thanks.

[daandb]

Originally Posted by oj.bulmer

Oh well, I think there is a bit confusion over the concept of under-relaxation. There are two types:

1) (Explicit) Under-relaxation of variables: For pressure-based coupled algorithm, this would under-relax the individual variables in inner iterations. Notice that the under-relaxation type for momentum and pressure is EXPLICIT!

2) (Implicit) Under-relaxation of equations: For pressure-based coupled algorithm, CFL applied tries to under-relax the equations through full IMPLICIT coupling. The choice of CFL will influence the local timescale and eventually the solution of the equations, as specified in earlier (long) post. Essentially when CFL is used, the separate under-relaxation of flow equations is not needed. But for turbulence equations, URFs still needs to be specified.

Typical values of Explicit URFs (in pressure-based coupled case) for pressure/momentum being 0.75, it can be further increased to accelerate inner iterations. But for higher order schemes for momentum etc, often it needs to be reduced to say 0.5 etc, with very bad meshes requiring further reduction at times. Any divergence in AMG solver should indicate the high CFL value, which needs to be reduced.

OJ

Thanks for the great explanation so far! What i still dont really understand is why these two different under-relaxation (implicit/explicit) are not present with the segrated solver (in any casethey cant be changed). I guess this is due to the fact the coupled and segrated solver work differently. Can you explain me what the difference is between them and how this corralates to the difference in the under-relaxations settings?

[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

[hellsblade.91]

Hi all just a question to all of you as ai also have a pressure velocity coupling shouldnt explicit courant no be equal to 1 and not the standard 200 value given by fluent in explicit sims courant no is upto 1 is what i found on some blogs but i didnt find something in the fluent manual

[LuckyTran]

Originally Posted by adasgupta91

Hi all just a question to all of you as ai also have a pressure velocity coupling shouldnt explicit courant no be equal to 1 and not the standard 200 value given by fluent in explicit sims courant no is upto 1 is what i found on some blogs but i didnt find something in the fluent manual

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.

[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 ?