> I have just noticed (after my client told me!) that Protel gerbers of
> octagonal pads end up as rounded pads. Is this just a configuration
> problem or does Protel not like octagonal pads or is there some
> other good reason for this behaviour? The actual problem is that the
> PCB manufacturer reproduced the octagonal pads somehow but
> the paste screen made from Protel gerbers has rounded holes
> which, apparently, causes some minor problems...
> Les Grant

This has been a problem from SP5 (and earlier?), and which has not been
fixed in SP6.

Octagonal pads with *differing* width (X-Size) and height (Y-Size) are
*always* "flashed" within RS274X (embedded aperture definitions provided)
Gerber files as obround (oval) shapes. That has always been the case for as
long as Protel has supported the production of RS274X files. (And that state
of affairs can be attributed to such shapes not being supported by the
RS274X standard, or at least not in a straightforward manner.)

When the width and height *are* identical though, it has been "traditional"
for such pads to be be "flashed" as (eight sided) (regular) polygonal
shapes. However, with SP5 and SP6 (and earlier SPs as well?), the only such
pads to be "flashed" in this manner are those whose rotational angle is zero
degrees (or 360 degrees). Pads with a rotational angle of 90 degrees, 180
degrees, or 270 degrees, are "flashed" as circular shapes instead.

My PcbAddon Server includes a Process which sets the rotational angle of all
pads having a rotational angle of 90, 180, or 270 degrees to zero degrees.
(For pads having a rotational angle of 90 or 270 degrees, the X-Size and
Y-Size distance properties are also transposed.) My experimentation has
suggested that there is merit in doing this for all pads, rather than just
those of octagonal shape; pads with a non-zero degree rotational angle are
apparently not always "flashed" as a single shape.

It is another long-standing contention of mine that the manner of defining
octagonal pad apertures within the embedded aperture defintions is not
compliant with how these should be specified. I believe that each of these
definitions should specify a rotational angle of 22.5 degrees rather than 0
degrees. And because the definition for these definitions appears to
stipulate that the distance specified in the specification is the vertix to
(opposite) vertix distance, and *not* the edge to (opposite) edge distance,
then the distance actually specified in each aperture definition should be
larger by a factor of the secant of 22.5 degrees.

I have created a Perl script which rectifies these embedded aperture
definitions, and I use this whenever I have a PCB file that incorporates
octagonal pads. I would be happy to provide a copy of this to any user who
is interested in using this. (At some stage I might even port the source
code to Delphi and so create an executable file, so that users won't need to
install Perl files on their PC.)

And by the way, you really should seriously consider previewing all Gerber
files (and NC Drill files) before despatching these to a PCB manufacturer.
The Camtastic 2000 Designer's Edition provided by Protel can do this. There
are other utilities available which can also do the same job, such as
Graphicode's (freeware) GC-Prevue. Doing this will pick up things such as
octagonal pads in the PCB file being depicted as circular pads in the Gerber

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