Hi Zach,
I have taken a quick look at your problem, and also at the finer
mesh that you have attached; the nominal size of elements close to
the aerofoil is now about right (for p=3), but I have a few
further suggestions:
1.) The fluid domain is very large relative to the
aerofoil. Whilst such large sizes are suggested for CFD
validation, they are also difficult and expensive to work with.
I would suggest using a smaller domain in this first instance:
around ten times the size of the aerofoil. Once the simulation
is running, it is a simple task to expand the domain and check
for any untoward interactions with the fluid boundaries.
2.) It is generally best to avoid large jumps in element sizes.
In practice: the smoother the transition, the better.
3.) I would also recommend switching to non-dimensional form. In
particular, there is a very low free-stream density being set in
this case (of order 1e-4), which could well be the primary
problem. Also--on a human level--it would make checking for
consistent units much faster (at least for me). I've not had
time to check this, but it is always worth checking again.
Best,
Antony
--
Antony Farrington MEng ACGI
AMIMechE
Postgraduate Researcher
Department of Aeronautics
Imperial College London
On 11/06/14 22:08, Zach Davis wrote:
All,
I've attached a finer mesh that includes 8960 quad elements
which I'm using, and I have reduced my time step to 1.0e-6
(which is pretty small given my experience even for explicit
Runge Kutta schemes), but I'm finding the solution still
diverges after the first solution file is output. I have also
removed the inadvertent extra line space within the initial
conditions block of my *.ini file which Peter pointed out.
Could the issue be somewhere else, or is the mesh in this case
still too coarse? Are there other relaxation controls that I'm
overlooking? I'm not sure the characteristic boundary
conditions in this case provide any advantage over the
sub-in-fpttang and sub-out-fp boundary conditions I'm using.
Again, any input would be appreciated.
Best Regards,
Zach
On Tuesday, June 10, 2014 6:04:38 PM UTC-7, Vincent, Peter E
wrote:
Hi Zach,
For characteristic BCs I believe the syntax in 2D is:
[soln-bcs-$name]
type = char-riem-inv
rho = ...
u = ...
v = ...
p = ...
Whether you go non-dimensional or not is largely down
to personal preference - for me it simplifies things.
I would certainly try reducing the time step -
however I am pretty certain you will also need to run on
a finer mesh than the one you attached here initially.
Cheers
Peter
Hi Peter,
Thanks for getting to this for me. Would you
be able to describe for me the requisite input
parameters for these characteristic boundary
conditions? It sounds like I may prefer to
utilize those. When using the non-dimensional
form, are you indicating it is easier for the
solver or from a user-perspective. I don’t have a
preference whether the variables are
dimensionalized prior to the simulation running or
during post-processing; though, at some point
along the way I will need to do it. Although, I
guess I prefer to see the output already in
metrics to which I’m accustomed, so maybe I lied
in my previous statement. I’ll try reducing the
time step further as well to cover all of my
bases.
Best Regards,
Zach
Hi Zach,
Thanks for your interest in PyFR. A few
comments:
1.) The initial condition should be set
according to:
[soln-ics]
rho = (psp*32.174)/(r*tsp)
; Freestream Density (lbm/ft^3)
u = 558.166
; X Component Velocity (ft/s)
v = 9.743
; Y Component Velocity (ft/s)
w = 0.0
p = r*tsp*rey*mu/usp
; Freestream Pressure (lbf/ft^2)
from within your .ini file.
2.)
The following may be the cause of
the solution blowup:
-
The mesh is very coarse for a p = 3
run, and hence you are likely
dramatically under resolving the
flow
-
Your time step may be too big, and
hence violating the CFL limit (PyFR
is explicit in time)
3.)
Other comments:
-
It may be easier to do everything in
non-dimensional form (i.e. chord of
1, inflow speed of 1, free stream
density of 1, then set Mach number
with the free stream pressure and
set the Reynolds number with the
viscosity.
-
You may want to try using our new
characteristic BCs
(type=char-riem-inv) for this case
(available in v0.2.1). They are not
currently documented, but require
specification of the full free
stream state.
Hope
this is of some help. Others may
have more detailed comments.
Cheers
Peter
All,
I've
posted this enquiry to both
Freddie and Peter already, but
perhaps others would be able to
contribute or be interested in its
resolution. I've made a couple
initial attempts to try to setup
and run a simulation around a 2D
NACA 0012 series airfoil with
conditions set at mach = 0.5, aoa
= 1 deg, rey = 5000 (ref length =
1ft) at SLS (or tsp = 518.688 deg
R). I've generated a few meshes
of varying mesh density. The
latest of which I've shared here
is my first attempt at generating
a very coarse curvilinear mesh via
Gmsh. After inspecting the
initial flow solution, it appears
that the fields for pressure,
density, and velocity are set
according to those prescribed by
the boundary conditions. It
appears that the solution diverges
very quickly after beginning the
run, and I'm trying to better
understand why this occurs as I
attempt to become more familiar
with PyFR and its options.
Best
Regards,
Zach
Davis
enc
--
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
pyfrmailingli...@googlegroups.com.
To post to this group, send email to
pyfrmai...@googlegroups.com.
Visit this group at http://groups.google.com/group/pyfrmailinglist.
For more options, visit https://groups.google.com/d/optout.
<naca_0012_coarse.msh><naca_0012_2d.ini>
--
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 email to [email protected].
Visit this group at http://groups.google.com/group/pyfrmailinglist.
For more options, visit https://groups.google.com/d/optout.
--
You received this message because you are subscribed to a topic in the Google Groups "PyFR Mailing List" group.
To unsubscribe from this topic, visit https://groups.google.com/d/topic/pyfrmailinglist/MOyz1XeEIb0/unsubscribe.
To unsubscribe from this group and all its topics, send an email to [email protected].
To post to this group, send email to [email protected].
Visit this group at http://groups.google.com/group/pyfrmailinglist.
For more options, visit https://groups.google.com/d/optout.
|
naca_0012_2d.ini