Dear Will,

Thanks for your message. We have applied the ACM solver to any internal flows, so it is interesting see your progress.

"What is the meaning of ma = 0.2? Do you mean the max velocity/ac-zeta? I think for ideal incompressible flow, ma = 0."

I meant the Mach number of the real life application that your are trying to simulate. The pressure residual (div u), which is more stiff to converge than velocity residuals, is kind of an indicator how far the pseudo waves which distribute the pressure have travelled. For truly incompressible flows (elliptic p, residual = 0), the information from an arbitrary point would have to propagate everywhere in the domain within every physical time-step. However, since the physical problems are never incompressible, but low-Mach, it may not be necessary to drive the pressure residual all the way to zero as long as the information has propagated over important length scales. I understand if you want to reproduce an incompressible test case you want to be as incompressible as possible, but for low-Mach industrial applications this is not necessarily the case.

The residuals in your cases are still quite high and they would benefit from multip and BDF2. Just to give you some tips, I tend to keep constant number of iterations, set the dt/dtau ratio between 5 and 10, and aim for u,v,w < 1e-4 pressure typically < 1e-3 . For example, for a Taylor-Green vortex Re=1,600, the level of convergence after 3 multigrid cycles

[solver-dual-time-integrator-multip]
pseudo-dt-fact = 1.7
cycle = [(4, 1), (3, 1), (2, 1), (1, 1), (0, 2), (1, 1), (2, 1), (3, 1), (4, 3)]

is

1254,10.002000000000095,3,0.00244778059095,0.000476855091426,0.000476823492017,0.00043626471224.

Using the same cycle and again 3 cycles per time step, the convergence of turbulent Jet at Re=10,000 is

240000,1799.9950000010913,3,0.00204563896311,0.000209207025143,0.000196374204824,0.000183716409294.

I used dt/dtau = ~7 in both cases.

Please also note that it can take considerable amount of time to dissipate initial transient waves. I'm expecting this phenomenon to be highlighted with internal flows because the waves are trapped inside the domain. I would suggest developing the flow with P=1 and restart with higher P after the flow has transitioned to turbulent.

Cheers,

Niki






On 12/02/18 05:01, Will wrote:
Dear Nikki,

What is the meaning of ma = 0.2? Do you mean the max velocity/ac-zeta? I think for ideal incompressible flow, ma = 0.

My pesudo convergence history is attached below. My case is 3d turbulent flow with Re_tau = 180.

I mapped the result from a 2nd order mesh (Originally 0.23 million cells already turbulent) case to the 1st order one (1.3 million cells) and started the simulation at 0.0s ended 1s.

case 1 is 0.23 million cells 2nd order mesh (1.8 million in pyfrm)
case 2 is 1.29 million cells 1st order mesh (1.29 million in pyfrm)

dt = 0.0005 and pseudo dt = 0.00001 with l2 norm tolerance.

Case 1 was run in backward-euler and euler psedo time stepping with 2nd order accerlater. The simulation ended at t = 40.95s. Tolerance is quite low (attached)

In case 2, due to the GPU memory size limit, I couldnt use bdf2 or higher solver or the multip accerlerator. Instead, backward-euler and rk4 are applied.

For case 1, tol finally reached nearly 2e-3. Near wall region matches with paper results, while centerline velocity is a bit of higher.

For case 2, I havent done any post processing yet. However, although the tol is extremely high, the visualized result seems to be reasonable. So, I am confusing the plausible tol threshold.

Best regards,
Will







--
You received this message because you are subscribed to the Google Groups "PyFR Mailing List" group. To unsubscribe from this group and stop receiving emails from it, send an email to pyfrmailinglist+unsubscr...@googlegroups.com <mailto:pyfrmailinglist+unsubscr...@googlegroups.com>. To post to this group, send email to pyfrmailinglist@googlegroups.com <mailto:pyfrmailinglist@googlegroups.com>.
Visit this group at https://groups.google.com/group/pyfrmailinglist.
For more options, visit https://groups.google.com/d/optout.

--
You received this message because you are subscribed to the Google Groups "PyFR 
Mailing List" group.
To unsubscribe from this group and stop receiving emails from it, send an email 
to pyfrmailinglist+unsubscr...@googlegroups.com.
To post to this group, send an email to pyfrmailinglist@googlegroups.com.
Visit this group at https://groups.google.com/group/pyfrmailinglist.
For more options, visit https://groups.google.com/d/optout.

Reply via email to