> > I still have a one question:
> >
> > 1. Why is it important to change the X and Y size to zero before
> > It was said this prevents "flashing" from within the Gerber file, but I
> > don't know what that means.
> >
> > Andrew Lowy Sybrandy
> IMHO, it is important _not_ to reduce the pad size to zero - if you do,
> you'll have shorts between the inner layers.
> You must keep pads on the inner layers that are larger than the hole
> size, to keep the hole plating (or mounting screw, if the hole is
> unplated) from contacting the inner layers.
> If you really don't want copper pads on the top and bottom, you have to
> define a pad stack with the surface pads smaller than the hole size.
> Peter Bennett

I was the poster who originally suggested changing the X Size and Y Size to
zero before producing Gerber files. However, that advice was for the
situation where the user wanted a hole in the PCB which was not to be
through hole plated, *and* which was not to be (immediately) surrounded by
copper on any layer. Such holes might be wanted in certain situations, such
as the two mounting holes for the plastic mounting lugs of an RJ-45
connector, for instance. (Another example is the small holes associated with
"breakout" patterns in panellised PCBs; you do not want pieces of copper
from *plated* holes lurking about to create potential mischief, so such
holes should be *unplated*.)

Regardless of the X-Size and Y-Size of a pad, the pad's *hole* diameter has
a bearing upon the diameter of any circular shape "flashed" on internal
power plane layers in the same location. (The other contributing factor is
the dominant design rule for the Power Plane Clearance distance for the pad
concerned.) So reducing the pad's X-Size and Y-Size to zero will *not*
result in shorts on internal power plane layers (as long as the dominant
design rule for the Power Plane Clearance distance for the pad concerned
results in a sensible *positive* distance, which is customarily the case).

For *other* internal layers (i.e. "standard" signal/copper layers), running
a DRC on the PCB file concerned will result in an error being reported if
any track (or arc, fill, etc) passes through the area occupied by the pad's
*hole*, as defined by the pad's hole diameter property. (An error will also
be reported if such a primitive passes through the area occupied by the pad
itself, as defined by its X-Size and Y-Size, unless both of these items have
an identical Net property.)

And as to what is meant by "flashing" in Gerber files, Gerber files are
created with the use of a set of apertures, or shapes. When a particular
aperture is used, it can either be used in a "draw" or "flash" mode. When
"drawing" occurs, the aperture is activated in one location, and remains
activated until after it has moved to some other location. "Flashing" occurs
when the aperture is activated in one location, and is then de-activated
again before that location has been changed. As such, fills, pads and vias
are customarily "flashed", while arcs, tracks and strings are customarily
"drawn". So what I was referring to was a situation where a hole was *not*
to be surrounded by copper, so reducing the associated pad's X-Size and
Y-Size to zero will subsequently result in that pad not being depicted at
all in the Gerber files produced for the "standard" copper layers. (But as I
explained, those pads *will* customarily be "flashed" in the Gerber files
for any internal power plane layers (which are *negative* layers in nature),
so that there will subsequently be no connections between the surface of
those holes and any copper on those layers.)

I hope I have made myself reasonably clear in the above explanations.

Geoff Harland.
E-Mail Disclaimer
The Information in this e-mail is confidential and may be legally
privileged. It is intended solely for the addressee. Access to this
e-mail by anyone else is unauthorised. If you are not the intended
recipient, any disclosure, copying, distribution or any action taken
or omitted to be taken in reliance on it, is prohibited and may be
unlawful. Any opinions or advice contained in this e-mail are
confidential and not for public display.

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
*  This message sent by: PROTEL EDA USERS MAILING LIST
*  Use the "reply" command in your email program to
*  respond to this message.
*  To unsubscribe from this mailing list use the form at
*  the Association web site. You will need to give the same
*  email address you originally used to subscribe (do not
*  give an alias unless it was used to subscribe).
*  Visit http://www.techservinc.com/protelusers/subscrib.html
*  to unsubscribe or to subscribe a new email address.
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *


To leave the EDAFORUM discussion list, send a email with
'leave edaforum' in the body to '[EMAIL PROTECTED]'

More Information : http://www.dolist.net

Reply via email to