Natural smoke venting and efficiency coefficient through open vents

[John]

Dear all
I have made an FDS model to simulate natural smoke venting, using OPEN
VENTs. After varying input, I have found a total of 27 m2 vent area to
be adequate. The smoke lid’s efficiency is given by the manufacturer,
but what kind of efficiency is presupposed in FDS? Reading the slice
files, I notice some variation in the airflow through the open vent
(which of course is natural due to drag along the rim). In this case,
however, I would like to find the efficient vent area.

[Kevin]

Do you mean "effective" vent area? In any case, an OPEN vent is just a
constant pressure boundary. If you are concerned about the flow
through a particular vent, do not use an OPEN boundary because the
constant pressure assumption is just that -- an approximation. You
should extend your computational domain beyond the vent and build it
out of obstructions. The flow in and out will then be treated
naturally as part of the solution of the governing equations.

[John]

I see. I will extend my computational domain, but I believe my
question remains. I have had a look in the manual and technical
reference guide, but have not found the equation for this phenomenon.
What I am looking for is the EFFECTIVE vent area in my simulations,
which enables me to choose the right type of smoke lid for my client.
Hope someone can lead me to this equation.

Thanks
John

> > however, I would like to find the efficient vent area.- Hide quoted text -
>
> - Show quoted text -

[iker23]

Hi John!

I am trying a similar simulation, I think that the vent area that you
have to use is de effective area. For examle: if the geometry area of
your vents is 6.25m2 and the and the efficiency coefficient is
0.65(this is given by the manufacturer) the effective area is 4.06m2,
you have to use this area in FDS. But you have to be careful with the
adjust of the gird, the vents have to coincide with the gird, or else
FDS can make a reduction of vent area.

I hope this help you. if yo need help my e-mail is:
ikfer...@yahoo.es

thanks!!

> > - Show quoted text -- Ocultar texto de la cita -
>
> - Mostrar texto de la cita -

[dr_jfloyd]

FDS is a computational fluid dynamics code. It does not impose a flow
loss coefficient at an orifice like one would do with a hand
calculation or with CFAST. It is up to you, the user, to do a grid
study to determine if your grid is fine enough to resolve the flow
through your opening.

On Jun 13, 4:47 am, iker23 <ikke...@gmail.com> wrote:
> Hi John!
>
>  I am trying a similar simulation, I think that the vent area that you
> have to use is de effective area. For examle: if the geometry area of
> your vents is 6.25m2 and the and the efficiency coefficient is
> 0.65(this is given by the manufacturer) the effective area is 4.06m2,
> you have to use this area in FDS. But you have to be careful with the
> adjust of the gird, the vents have to coincide with the gird, or else
> FDS can make a reduction of vent area.
>
> I hope this help you. if yo need help my e-mail is:

> ikferpr...@yahoo.es

> > - Mostrar texto de la cita -- Hide quoted text -

[John]

iker23,
In your example you are assuming 100 % efficiency in the simulated
vents. If you study a slice file or a vector slice through a vent/
hole, you will find that the air speed velocity is declining in the
outer edges of the vent. Hence the simulated vent has an efficiency of
less than 1, and you end up with larger venting area than you actually
need.

On Jun 13, 10:47 am, iker23 <ikke...@gmail.com> wrote:
> Hi John!
>
>  I am trying a similar simulation, I think that the vent area that you
> have to use is de effective area. For examle: if the geometry area of
> your vents is 6.25m2 and the and the efficiency coefficient is
> 0.65(this is given by the manufacturer) the effective area is 4.06m2,
> you have to use this area in FDS. But you have to be careful with the
> adjust of the gird, the vents have to coincide with the gird, or else
> FDS can make a reduction of vent area.
>
> I hope this help you. if yo need help my e-mail is:

> ikferpr...@yahoo.es

> > - Mostrar texto de la cita -- Hide quoted text -

[Kevin]

The declining air speed near the edge of a vent could be an artifact
of Smokeview. Velocity components are computed at grid cell faces and
then interpolated at cell corners for presentation in Smokeview. Thus,
near the edge of the vent, you see what appears to be a lower velocity
because the solid cell velocity of zero is averaged with the vent cell
velocity of some positive value. In fact, if you resolve the grid well
enough, you should see faster flow speeds at the vent edges, as is
predicted by potential flow theory and measurements of Steckler et al.
at NIST 20 years ago.

> > - Show quoted text -- Hide quoted text -

[JWilliamson]

In an under-resolved vent, the wall boundary slip conditions can play
a role (ie. if your vent area is 2x2 grid cells). In a fully-resolved
vent, the effect of the slip condition is small, but it can
arbitrarily reduce your vent flow in a coarse mesh. This reduction
will depend on your grid, and your prescribed slip condition. I'm not
certain if this effect is present if you use an OPEN boundary to
simulate your vent, but it should have an effect if your vent flow
path (normal direction) is greater than 1 grid cell.

Prescribing free-slip should eliminate the effect.

[Martin]

Is there any validation work with FDS that compares velocities, mass
flow or volume flow through natural vents? My experience with FDS,
using a relatively coarse mesh ( about 10 grid cells across the
natural vent) is an over prediction of the volume- and mass flow
compared to a simple hand calculation( Bernoulli).
I use the pressure across the vent (some horizontal distance from the
vent), actual vent area (number of cells) and temperature from FDS.
The flow coefficient for the hand calculation is obtained from the
literature (0,6-0,7). The volume- or mass flow from FDS is obtained
with the volume- or mass flow function in FDS. Has anyone experienced
similar trends? I am using a HOLE by the way.

On Jun 13, 4:03 pm, JWilliamson <williamson.justin.w...@gmail.com>
wrote:

[Kevin]

I think it would be better to compare against actual measurements.
Many have used Steckler's data from NIST, for example. I should think
there are plenty of other datasets with door flow data.

[Roth]

Many commerical CFD codes e.g. Fluent have the ability to apply an
additional pressure loss across an opening via a specification of a
pressure loss coefficient (dP = K * 0.5 * rho * V^2). This is
especially useful if one wants e.g. a uniform exhaust velocity across
a pressure-specified boundary (say K \approx 10). This same mechanism
can be applied to interior faces in the domain to parametrize e.g. the
flow through a grill without explicitly resolving the grill.

Any desire to implement such a feature in FDS?

[Kevin]

We currently have a POROUS obstruction that allows us to impose a
specified velocity via a pressure drop normal to a plane in the middle
of the computational domain. I suspect that this is just a slight
variation on this idea. Is there a simple description in terms of a
pressure gradient. We deal with dp/dx, not just dp.

[John]

Thank you all for your useful comments!

John