[PROTEL EDA USERS]: Aperture definitions for (regular) octagonal pads

["Geoff Harland" <gharland@ingenico.com.au>]

Here's a potential "gotcha" that those using octagonal pads have to watch
out for (and which I discovered recently while inspecting some blank PCBs
after these had been manufactured).

The RS274X standard does not support octagonal apertures in which the width
and height differ (or at least not in any straightforward manner), but does
support octagonal apertures when the width and height are identical (as such
an octagon is a "regular" polygon, which is a shape that is supported by the
RS274X standard). However, I have long maintained (and continue to maintain)
that the angle of rotation specified within the associated (embedded)
aperture definition should be 22.5 (degrees) rather than zero, as the
specification for embedded aperture definitions stipulates that a polygon
having a rotation of zero (degrees) has a vertix on the X axis. As such, I
have long been in the habit of modifying the Gerber files produced from PCB
files created using Protel, so that the angle specified is 22.5 degrees (in
place of the 0 degrees specified within the Gerber files as these were
originally created).

My recent discovery concerns the *diameter* of octagonal pads (as opposed to
their angle of rotation), as inspection of a recent set of incoming PCBs
revealed that the octagonal pads within these did not seem to have much
"meat" around the outside of their associated (plated through) holes. In a
nutshell, the specification for describing polygonal apertures seems to
specify the *outer* diameter of the polygon concerned, or the vertix to
(opposite) vertix distance. (In the case of polygons with an odd number of
sides, I suspect that this distance is the diameter of the *circumcircle*,
and this specification would equal the vertix to vertix distance for
polygons with an even number of sides.) However, the distance that is
specified within the Gerber files produced by Protel is the edge to
(opposite) edge distance, which is smaller than the vertix to vertix
distance by a factor of cos(ine) 22.5 (degrees) (or ~ 0.92387953).

The moral of the story seems to be that not only should the angle of
rotation be changed from 0 degrees to 22.5 degrees, but that the specified
size of this should also be magnified by a factor of sec(ant) 22.5 (degrees)
( SQRT(4 - SQRT(2)), as a bit of algebra/trigonometry reveals, or ~
1.08239).

However, the PCB manufacturer should also be informed that both of these
modifications have been made to the embedded aperture definitions within the
Gerber files, as the possibility exists that the associated pads will be
produced oversized and/or with an incorrect orientation otherwise. (I have
previously advocated that the PCB manufacturer should be notified of the
changed angle within these aperture definitions, so in the event that the
associated size is also changed, then the PCB manufacturer should similarly
be alerted to this as well.)

A concrete example of an embedded aperture definition *before* this is
modified:

%ADD52P,0.070X8X0*%

{Aperture D52, Polygon shape, 0.070" size, 8 sides, rotational angle of 0
degrees}

and *after* this has been modifed:

%ADD52P,0.076X8X22.5*%

{Aperture D52, Polygon shape, 0.076" size, 8 sides, rotational angle of 22.5
degrees (70 * sec 22.5 degrees is ~ 75.767, but this has been rounded to the
nearest mil)}

It is not devoid of merit to avoid the use of octagonal pads entrely (and I
avoid the use of octagonal pads with differing widths and heights), but in
the event that you do want to use these, then there is a lot to be said for
making the modifications that I have described to the Gerber files (and of
notifying the PCB manufacturer of these changes).

And remember that octagonal pads with a rotation of 90, 180, or 270 degrees
are specifed as pads of circular shape with Protel 99 SE SP5. So don't
forget to rotate all such pads (within the PCB file) to an angle of 0
degrees before generating Gerber files... (Use of the global editing feature
can assist in this regard.)

Regards,
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.