jet flow: turbulence models

gforney commented 9 years ago

Application Version: 6.0.0
SVN Revision Number: 9688
Compile Date: 23 Dec 2011
Operating System: Linux

Last year (Nov 2011), i checked the jet flow case with FDS 5.5.3 (SVN 7031), FDS 5.5.3
FDS6=.TRUE. (SVN 7031) and FDS 5.5.3 DYNSMAG=.TRUE. (see image_SVN7031.png). The development
was gratifying. 

In the last few days i checked the same case with FDS 6 (SVN 9688) and the turbulence
models Deardorff, Vreman and Smagorinsky (see image_SVN9688.png). After the major change
of the turbulence model (SVN 8975) i can see some major differences. The same observations
can be made with different values for the grid size (5 cm, 20 cm, 40 cm).

There seems to be a problem.

information:
----------
grid size: 10 cm
u-volicity: mean for 30sec (delta_t = 150sec - 130sec of the simulation)

case FDS 5.5.3 default: F_10_SVN7031b.fds
case FDS 5.5.3 FDS6=.TRUE.: F_10_SVN7031.fds
case FDS 5.5.3 DYNSMAG=.TRUE.: F_10_SVN7031a.fds

case FDS 6 default - Deardorff: F_10_SVN9688b.fds
case FDS 6 Smagorinsky constant: F_10_SVN9688a.fds
case FDS 6 Smagorinsky dynamic: F_10_SVN9688.fds
case FDS 6 Vreman: FDS6_F_vrem_010.fds

Original issue reported on code.google.com by gregor.jaeger on 2011-12-28 13:36:28

_Attachment: image_SVN9688.png
_
_Attachment: F_10_SVN7031b.fds_
_Attachment: F_10_SVN7031.fds_
_Attachment: F_10_SVN7031a.fds_
_Attachment: F_10_SVN9688b.fds_
_Attachment: F_10_SVN9688a.fds_
_Attachment: F_10_SVN9688.fds_
_Attachment: FDS6_F_vrem_010.fds_

gforney commented 9 years ago

(No text was entered with this change)

Original issue reported on code.google.com by gregor.jaeger on 2011-12-28 13:37:39

_Attachment: image_SVN7031.png
_

gforney commented 9 years ago

Thanks for the information. I will ask Randy McDermott to take a look at this. Could
you post a reference to the "analytical" results. I assume that this is some sort of
centerline velocity correlation for a fan?

Original issue reported on code.google.com by mcgratta on 2011-12-28 17:36:47

gforney commented 9 years ago

I will post an abstract. Randy will get the hole reference by mail because there is
a copyright.

Original issue reported on code.google.com by gregor.jaeger on 2011-12-28 20:00:28

_Attachment: analytical_background.pdf_
_Attachment: image_analytical-background.png
_

gforney commented 9 years ago

Gregor,

Many thanks.  Your reference is sufficient.  No need to send a post.

Good catch on DYNSMAG.  I had indeed introduced a bug recently.  I am running all the
cases now with the fix and will report back soon.

Best,
Randy

Original issue reported on code.google.com by randy.mcdermott on 2011-12-28 20:12:55

gforney commented 9 years ago

Here are the latest results with dx = 10 cm.  Dynamic Smagorinsky seems to be working
again.  I am setting up 5 cm grid right now and will commit all these cases to the
repository.

Original issue reported on code.google.com by randy.mcdermott on 2011-12-28 21:56:33

_Attachment: jet_decay_dx10cm.pdf_

gforney commented 9 years ago

Latest results for two grid resolutions are attached.  I non-dimensionalized the velocity
and downstream distance, as well as the grid resolution.  We should be careful about
interpreting these results.  It would appear that dynamic Smagorinsky is the clear
winner.  But it is about 30% more expensive than the other models.  Also, the Reynolds
number for this case is 10^5, which is much higher than what we typically see in fires.
 The exception to this is near sprinkler nozzles.  And, in fact, Topi has noticed more
or less the same trend: that dynamic works better for getting good profiles near nozzles.

The dilemma is that dynamic becomes very erratic for buoyant plumes at low grid resolution
(D*/dx \approx 5).  Deardorff behaves much better for low resolution plumes, giving
a reasonable level of dynamics while still retaining some semblance of the fire shape.
 We would be asking a lot to have a single subgrid model that works perfectly at all
grid resolutions, for all Reynolds numbers, and for all Froude numbers.  So, I can
make my peace with saying that if the user wants to simulate a high Re jet, then dynamic
or Vreman may be the best option.  The last comment I'll make about Deardorff is that
I like its simplicity and the fact that it is based on an approximation to the subgrid
kinetic energy, k_sgs.  The important point is this: our approximation to k_sgs can
be improved!  I am especially thinking about the issues we will face when we start
development on adaptive mesh refinement (AMR).  Having direct control over the k_sgs
budget is very helpful in an AMR scheme.

Original issue reported on code.google.com by randy.mcdermott on 2011-12-29 14:08:08

_Attachment: jet_decay.pdf_

gforney commented 9 years ago

Thank you for correcting the bug and your explanations. I isn't my goal to say "model
A is always better than model B". In my opinion, it's important to know something about
strengths and weaknesses of the models. That was the goal for my test cases.

I'm pleased that the case takes its place in the Verification Guide. Thanks for this
honor.

Original issue reported on code.google.com by gregor.jaeger on 2011-12-29 15:08:54

gforney commented 9 years ago

Gregor,

I totally agree with you about understanding the models.  I just wanted to make the
point to others, who might look at this case in isolation, that there is more to the
story.  I thank you greatly for catching the bug.

Regarding the verification write up, your short description in "analytical_background.pdf"
is great.  But could you elaborate a bit on the definition of m and its physical meaning.
 I suppose it relates to the point at which the momentum mixes with the jet core and
we therefore lose the constant jet velocity.  But (without reading the German report)
it is not clear to me whether this range you selected for the test case m=[0.12,0.20]
has some physical relevance.  Was this the experimentally observed range of the core
breakup? 

Thanks!

Randy

Original issue reported on code.google.com by randy.mcdermott on 2011-12-29 15:23:21

gforney commented 9 years ago

I'll send you a summary for the definition of m and its physical meaning in the next
week. I need a few days.

Gregor

Original issue reported on code.google.com by gregor.jaeger on 2011-12-29 15:32:15

gforney commented 9 years ago

OK, thanks.  But I am really only looking for a sentence or two.

Original issue reported on code.google.com by randy.mcdermott on 2011-12-29 15:34:57

gforney commented 9 years ago

Randy, Gregor,
very interesting discussion.

Gregor,
I assume you did the analysis automated? Is it possible to redo the simulations of
one grid size with a lower RE-number? Lets say VEL=-1 m/s? The core length should be
more or less the same, but we could see how much the outcomes of the different models
depend on the RE-number.

Thanks 

Boris

Original issue reported on code.google.com by Info@F-Sim.de on 2011-12-30 19:55:25

gforney commented 9 years ago

Would not be a problem.  But we might as well get a thorough plan together and test
a broad range of Re.

I have added a section to the Verification Guide called "Jet Centerline Velocity Decay".
 Also, the cases are set up in the Validation/Turbulent_Jet directory in the repository.
 Because of the cpu requirements to run the high res cases, these will be processed
with the validation suite instead of the verification suite.  The Matlab script to
process the output is in Utilities/Matlab/scripts/jet_decay, which you can run from
master_verification_script.

Original issue reported on code.google.com by randy.mcdermott on 2011-12-30 20:15:15

gforney commented 9 years ago

Randy,

good idea! When back in the office next week, Gregor and I should have access to some
CPU-time. I am pretty curious about the outcomes.

Boris

Original issue reported on code.google.com by Info@F-Sim.de on 2011-12-30 22:16:13

gforney commented 9 years ago

Randy,

Gregor and I discussed the problem and right now I am not quite sure if we aren’t comparing
apples to peaches.
I would appreciate to hear your advice.

When the measurements were made, I assume there was a ventilation appliance pushing
air through a shaft/channel. The end of the shaft/channel is the beginning of the core
zone (x=5* d0), where the measurements start.

http://upload.wikimedia.org/wikipedia/de/1/19/FREISTRAHL.PNG

In channel flow, with Re becoming something between 2300 and 10000, the flow gets turbulent.
In fact we can assume, that the outflow of the end of the channel was a turbulent flow.
While not using the synthetic turbulence model you implemented in FDS, the outflow
of the air right at the VENT we used is a laminar flow. Right?
I am not quite sure how the different models DynSmag, Deardorff and Vreman might behave
if we 
a) give them a “Vorlaufzone”, means modelling the channel before the outlet to give
the fluid some space to switch turbulent, or 
b) use your synthetic turbulent boundary condition.

It might be interesting to compare this:

Const Smag, Dyn Smag, Vreman and Deardorf
Cell size 10 and 20 cm
VENT, VENT with synthetic turbulence and with “Vorlaufzone”
Re = 10^5, 5*10^4 and 10^4 (or something like that)

This may take us some time, so I would appreciate hearing your opinion on this…

Thanks 

Boris

Original issue reported on code.google.com by Info@F-Sim.de on 2012-01-05 17:01:12

gforney commented 9 years ago

Boris,

I would do the upstream channel first.  Use this to (a) evaluate the turbulence models
and (b) to gather the statistics you need to enter into the synthetic turbulent inflow.
 Then also try the synthetic turbulence.  It would be the first verification test for
that feature.

Thanks!
Randy

Original issue reported on code.google.com by randy.mcdermott on 2012-01-05 18:07:33

gforney commented 9 years ago

Hi Boris,

Where do we stand on this Issue.  I would like either to get this into the guide or
close it.  I need the write up from Andreas.

Thanks!
Randy

Original issue reported on code.google.com by randy.mcdermott on 2012-03-21 12:38:52

gforney commented 9 years ago

Randy,

I have been in holidays and I have to confess I neglected this issue...
We will work on this next week and send you the outcomes at least in 2 weeks...

Boris

Original issue reported on code.google.com by Info@F-Sim.de on 2012-03-25 12:56:16

gforney commented 9 years ago

Randy,

we have ran the first simulations and it seems that, as we assumed, there are large
differences between using a VENT and simulating an upstream channel. For example see
Deardorff with 20 cm.

Not all of the simulations are finished yet. We liked to analyse the outcomes, recheck
if there are no mistakes and compile the outcomes next week.

Before starting the simulations with the synthetic turbulent inflow:
is it possible to measure inputs like N_EDDY, L_EDDY or VEL_RMS or are there any sources
for reasonable assumptions for these inputs?

Boris

Original issue reported on code.google.com by Info@F-Sim.de on 2012-04-05 14:36:51

Attachment: Deardorff.png

gforney commented 9 years ago

Boris,

Thanks for this.  Interesting results.  And, I guess, good news for Deardorff.

Unless they are published in the experimental report on the jet decay, L_EDDY and VEL_RMS
are themselves parameters of the flow.  N_EDDY is a statistical parameter, as N_EDDY
gets large your statistical error goes down.  For this case, I can't give any hard
numbers on what you would need.  I would refer you to Jarrin's thesis.

In terms of evaluating the turbulence models, let's take the synthetic bc out of play
(this needs separate verification).  It is fine to use the upstream channel as you
have done.  If you wouldn't mind sending me the input file, I'll modify the cases in
the repository and rerun the cases for the guide.

Thanks!
Randy

Original issue reported on code.google.com by randy.mcdermott on 2012-04-05 14:48:11

gforney commented 9 years ago

Randy,

if you don"t mind a few more days, I would like to end all the simulations and recheck
that we did no errors in the  simulations.

Boris

Original issue reported on code.google.com by Info@F-Sim.de on 2012-04-06 21:31:41

gforney commented 9 years ago

Randy,

the upstream versions with 50% blockages in the channel were to much. We will repeat
the simulations without blockages in the channel, just upstream. I think the outcomes
will more fit our epectations...

Boris

Original issue reported on code.google.com by Info@F-Sim.de on 2012-04-23 13:58:31

_Attachment: FDS6_VREMAN_V_010_2-0_Vorlauf_devc.pdf_
_Attachment: FDS6_VREMAN_V_020_2-0_Vorlauf_devc.pdf_

gforney commented 9 years ago

Boris,

I would use a single mesh for the upstream channel at a high resolution.  This mesh
does not need to be as large in the y and z directions as the chamber you are using
for the jet decay region.  It only needs to be the width of the inlet channel.  You
can add turbulence at the inlet vent via Jarrin's method.  What we need is some indication
of the turbulence properties upstream of the jet exit from the experimental report.
 Else we are just guessing, and we can tune the results to match whatever we want.

R

Original issue reported on code.google.com by randy.mcdermott on 2012-04-23 14:04:32

gforney commented 9 years ago

I changed the input files like suggested. I think they will take 12-24 hours till finished.
I'll post the new outputs tomorrow.

Boris

Original issue reported on code.google.com by Info@F-Sim.de on 2012-04-23 15:45:05

gforney commented 9 years ago

Here are the latest results using the upstream turbulent channel at the inlet.  As you
can see, the boundary condition is critical.  All the different models are now within
reason, even constant Smagorinsky.  Note that I adjusted u_0 to 2.1 for the plot to
account for the profile at the entrance.  If I use the value of u_0=2, which is specified
at the flat profile VENT, then the initial u_max/u_0 is greater than 1.

The setup and processing tools for these cases can be found in:

FDS-SMV/Validation/Turbulent_Jet/

Original issue reported on code.google.com by randy.mcdermott on 2012-04-24 12:38:33

_Attachment: jet_decay.pdf_

gforney commented 9 years ago

Here is a link to a movie of a velocity slice for Deardorff:

https://docs.google.com/open?id=0B4528gcI9D3HRW1IQWdhTzNCSVE

Original issue reported on code.google.com by randy.mcdermott on 2012-04-24 12:55:08

gforney commented 9 years ago

Randy,

thanks. That was fast. Our PC has not even finished all of the simulations...
The outcomes (including the movie) look great.

Without wanting to expand this issue too much, I have one last question.
I compared 4 different simulations of the same geometry:

1. 1 MESH with upflowchannel, borders of the upflowchannel with full OBSTs 
2. 2 MESH "                                                              "
3. 1 MESH with upflowchannel, borders of the upflowchannel with OBSTs of 1 cell thickness
4. 1 MESH with upflowchannel, borders of the upflowchannel with OBSTs of 0 cell thickness

We are using SVN 10121 because of some problems with V11 of our compiler. Noise=.True.
The outcomes seem to differ although the boundary conditions should be largely identical.

Boris

Original issue reported on code.google.com by Info@F-Sim.de on 2012-04-24 13:51:39

_Attachment: Channel_1MESH.fds_
_Attachment: Channel_1MESH_0OBST.fds_
_Attachment: Channel_1MESH_1OBST.fds_
_Attachment: Channel_2MESH.fds_
Attachment: Outcomes.pdf

gforney commented 9 years ago

Boris,

I you are seeing different results, then you need to tighten your velocity tolerance
on PRES, e.g.,

PRES VELOCITY_TOLERANCE=0.001, MAX_PRESSURE_ITERATIONS=100/

But the cases I ran were using 2 meshes for the dx=10 cm case and 49 meshes for the
dx=5 cm case.  All looked fine with the lates code.  Let's put this issue to bed. 
The issues you are getting into now are more suited for the Pressure Solver development.

Best,
R

Original issue reported on code.google.com by randy.mcdermott on 2012-04-24 14:00:12

gforney commented 9 years ago

Randy,

thanks for your help.

Boris

Original issue reported on code.google.com by Info@F-Sim.de on 2012-04-24 14:31:43

gforney commented 9 years ago

(No text was entered with this change)

Original issue reported on code.google.com by randy.mcdermott on 2012-06-13 13:48:56

firemodels / fds

jet flow: turbulence models #1527