> Beware the octagon pads! Protel does not define them properly in the
> gerbers. My experience has been that, with a separate aperture file, it's
> treated as a rectangular pad with chamfered corners, and the gerber file
> doesn't carry enough info as to how far the chamfer cuts back. Embedded
> apertures are even worse; Protel treats an octagon pad as having faces at
> the four points of the compass, whereas every board shop I've dealt with
> (and apparently the Gerber 274X standard as well) treats it as having
> points at the compass points, thus fouling up all the clearances. I just
> got back a board with all the octagons rotated 22.5  compared to the
> appearance in the original file. Hence I no longer use octagon pads for
> routine stuff, though I may occasionally use one to flag a special test
> point, out in wide-open country where no interference is possible.
> Steve Hendrix

I sometimes use octagonal pads (each having equal width and height), though
with care. When I do use them, I use embedded aperture definitions (the
RS274X standard), and I actually modify these (the embedded aperture
definitions), to make them comply with the RS274X standard.

In that regard, I change the rotational angle specified from 0 degrees to
22.5 degrees. I *also* change the diameter that is specified; I scale this
up by a factor of the secant of 22.5 degrees. A rotational angle of 0
degrees puts vertices on the X and Y axes; changing that angle to 22.5
degrees results in octagons with (road side) STOP sign orientation (which
matches what is depicted within a Protel PCB file).

Scaling the diameter upwards is based on experience. One PCB I received late
last year contained an octagonal pad that looked "anaemic"; there was far
less copper between the outside edge of the pad and the outside edge of its
associated hole than I expected. Re-examining the RS274X standard at that
time suggested that the diameter specified (within the embedded aperture
definition) actually specifies the diameter of the polygon's *circumcircle*,
or the vertix to (opposite) vertix distance (given that a regular octagon
has an even number of edges/vertices). Protel's software sets a distance
equal to the pad's edge to (opposite) edge distance, which is smaller than
the vertix to (opposite) vertix distance, and by a factor of the cosine of
22.5 degrees. As such, the distance specified within the Gerber files
created by Protel has to be scaled upwards to compensate (by a factor of the
secant of 22.5 degrees, which is the reciprocal of the cosine of 22.5

I also include a note in the readme.txt file (sent with the Gerber files and
NC Drill files), in which I explain what modifications I have made to the
Gerber files, and the reason for making these. And I also place text strings
on a Mechanical layer advising of the orientation and sizes of octagonal
pads, and include the contents of that (Mechanical) layer in the Gerber
files, so that when the PCB manufacturer views the Gerber files, the
resulting enclosed text should ensure that the octagonal pads will be
interpreted correctly. (It is not safe to assume that the PCB manufacturer
will necessarily read the contents of any readme.txt file that is sent with
the Gerber files.)

However, I never use octagonal pads where the width and height differ; such
pads are not really supported by the RS274X standard (or at least not in a
straight forward manner). *If* I had reason to believe that a PCB
manufacturer would accept PCB specifications in the form of a GC-Prevue file
(which supports apertures having a chamfered rectangular shape), I would
then consider using such pads, but otherwise I concur that the potential
exists for the pads concerned to be mis-manufactured.

Back on the original topic for this thread, a complex pad shape can be
supported by surrounding a supported pad shape by primitives as required
(arcs, fills, tracks, pads). However, when arcs, fills, or tracks are used,
these do not acquire the net assigned to the connected pad by default. It is
possible to assign this net to these primitives, but it is still an extra
step to achieve that outcome (recent contributions to this thread explain
how). As such, it is preferable to implement a complex pad shape by the use
of *just* pad primtives. And in the corresponding component in the schematic
library file, multiple pins should be located in the same location, so that
when the user connects a wire to that point (in the schematic file), he or
she connects to both/all of the pads concerned at the same time.

In previous posts, I have long advocated that each pin that is part of a
component should have an unique number/designator. So, for example, you
might have a "flag-ship" pin "2", and supplementary pins "2A", "2B" (, etc,
as required). The names and numbers of all supplementary pins should be set
to a hidden state within the component within the schematic library file, so
that within the schematic file, only the "2", of the "flag-ship" pin, is
displayed (and not the "2A", "2B", etc, as well, which would occupy similar
locations as the "2" text, and thus render printouts of the schematic file
as less readible, not to mention less agreeable from an aesthetic and
professional perspective as well).

Adopting this procedure means that when a netlist file is produced, the
supplementary pins will all be assigned to the appropriate net, i.e. the
same net that is assigned to their corresponding "flag-ship" pins. That way,
DRC errors are not generated, and no separate step is required to assign the
appropriate net to the supplementary primitives that make up each complex
pad shape.

Protel is supposed to be working on supporting multiple pins/pads having the
same designator/name (within the same component). IME, that state has yet to
be fully achieved. A such, adopting my policy of unique designators/names
for each pin/pad keeps you out of the pooh.

I would like to say more, but I have work to return to. If some of the above
is not clear, I and/or others can assist as required.

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.

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To join or leave this list visit:
* http://www.techservinc.com/protelusers/subscrib.html
*                      - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
* Contact the list manager:
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to