Hi Zach,
I tried running your case for couple of outputs and did not experience
the odd behaviour in your .vtu file (attachment). However, in your mesh
the dimensions are scaled differently. For instance, the cylinder
diameter is D=~285, while the values in the .ini file are specified for
D=1 used in my mesh.
Cheers,
Niki
On 15/03/17 20:27, Zach Davis wrote:
Hi Niki,
Thanks for the explanation. I’ll look into this method a bit further
based on the paper reference you provided. Something seems to be
amiss with solution files. I’ve attached the *.pyfrm *.vtu and *.ini
files I have generated for this case; though, the mesh is one of my
own creation. If someone could explain what’s happening with the
*.vtu file based on the *.pyfrm mesh input, then that would be
appreciated.
Best Regards,
Pointwise, Inc.
Zach Davis
Pointwise®, Inc.
Sr. Engineer, Sales & Marketing
213 South Jennings Avenue
Fort Worth, TX 76104-1107
*E*: [email protected] <mailto:[email protected]>
*P*: (817) 377-2807 x1202
*F*: (817) 377-2799
enc
On Mar 15, 2017, at 8:42 AM, Niki Loppi <[email protected]
<mailto:[email protected]>> wrote:
Hi Zach,
AC stands for the method of artificial compressibility. Instead of
relying on a Poisson based projection, the system is driven towards a
divergence free state by introducing artificial pressure waves
through the continuity equation. The formulation preserves the
hyperbolic nature of the system, but destroys the time accuracy,
which is then recovered with dual time stepping. For the ac
formulation you can refer to
http://www.sciencedirect.com/science/article/pii/S0021999116001686
The artificial compressibility factor ac-zeta is the coefficient of
the fluxes in the continuity equation. This results in characteristics
V + c, V, V - c,
where c = sqrt(V^2 + ac-zeta) is the pseudo speed of sound. Thus, in
the current implementation ac-zeta is the free parameter that is used
to downscale the speed of the pseudo-waves to globally reduce the
pseudo system stiffness. The parameter is something that one can
experiment with, typical values varying from 1.25 - 10 times the
freestream velocity. Currently, I am looking into making ac-zeta and
pseudo-dt spatially and temporally varying.
The source terms specify a sponge region near the domain edges
(|y|>5, x<-5, x>25) to damp the initial pressure wave that is
generated when the simulation is started from scratch. Please note
that the sponge turns off at t=5 because of the (1 - tanh(1.5*(t -
5.0)))*0.5 coefficient. You can see how the sponge works if you write
the solution files before t=5.
The plugin [soln-plugin-pseudostats] is used to output the residual
of the pseudo time problem to monitor the divergence. The
[soln-plugin-residual] on the other hand computes the "residual" of
two consecutive real time steps. The [soln-plugin-fluidforce] plugin
can be used with the ac systems.
Coarsening the mesh and increasing the order is something that would
be beneficial, especially when using a polynomial multigrid for
accelerating the pseudo time problem. P-multigrid should be added in
the next release.
Thanks,
Niki
On 14/03/17 23:37, Zach Davis wrote:
Tuesday, 14 March 2017
Peter & Freddie,
I believe the mesh export issue from Pointwise using the PyFR
exporter has been resolved in PyFR 1.6. I still seem to have issues
running using the OpenCL backend which persistently complains about
an invalid workgroup size. It use to work at one point, but
something has changed in the intervening releases which is causing
problems for me at least. I’ve tried adjusting the values per
Freddie’s guidance to no avail. He also suggested a tool that might
be helpful in determining the appropriate workgroup size needed for
my card. Unfortunately that tool seems to be NVIDIA card specific
requiring installation of NVIDIA software that won’t run on my
machine. I’m using an AMD card instead, and the tool won’t compile
due to missing dependencies. It’s not a pressing matter, but just
something that I thought you both might want to be aware of.
Nikki,
I’ve looked over your incompressible 2d-cylinder case, and I was
wondering if you could elaborate a bit, or point me to some
reference, about how you came up with the source terms you’re using
in the input file. It also appears that the
[soln-plugin-pseudostats] is used in place of the
[soln-plugin-residual] namelist for incompressible cases—is that
right? Does the [soln-plugin-fluidforce] namelist still work for
the ac-navier-stokes solver? Another question if you don’t
mind—what is this artificial compressibility factor, ac-zeta and why
is value of 6.0 used? Oh, and what does the ac prefix stand for?
Thanks!
I think it would be interesting to see how coarse of a higher-order
mesh could be made for this case while increasing the polynomial
solution basis such that you essentially recover the linear mesh
spacing in each element, and see if you could capture one or more
vortices within a single element with any noticeable diffusion over
time.
Best Regards,
Pointwise, Inc.
Zach Davis
Pointwise®, Inc.
Sr. Engineer, Sales & Marketing
213 South Jennings Avenue
Fort Worth, TX 76104-1107
*E*: [email protected] <mailto:[email protected]>
*P*: (817) 377-2807 x1202
*F*: (817) 377-2799
--
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 [email protected]
<mailto:[email protected]>.
To post to this group, send email to
[email protected]
<mailto:[email protected]>.
Visit this group at https://groups.google.com/group/pyfrmailinglist.
For more options, visit https://groups.google.com/d/optout.
--
Niki Andreas Loppi MSc
Postgraduate Researcher
Department of Aeronautics
Imperial College London
South Kensington
London
SW7 2AZ
UK
--
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 [email protected]
<mailto:[email protected]>.
To post to this group, send email to [email protected]
<mailto:[email protected]>.
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 [email protected].
To post to this group, send an email to [email protected].
Visit this group at https://groups.google.com/group/pyfrmailinglist.
For more options, visit https://groups.google.com/d/optout.
