[PEDA] Octagonal Pads

[Geoff Harland]

That is an excellent procedure for board houses to engage in, and as such
there would be a lot to be said for *all* board houses to adapt it. (And
quite apart from improving the level of service provided to their customers,
they would also be doing *themselves* a favour, as requiring their customers
to "sign off" on the Acrobat files provided to them (before any PCBs are
actually manufactured) would reduce the likelihood of commercial
relationships turning acrimonious as a consequence of PCBs not being
manufactured in a manner matching what their customers envisaged.)

In my experience, the better board houses get in touch with their customers
whenever they discover any aspects of the (Gerber or NC Drill or other)
files provided to them which look "suspicious" in any way, so whenever it
would be appropriate, there would be merit in board houses providing two
copies of (Acrobat/PDF) "printouts" of any layer which looks "suspicious";
one of those "printouts" would be totally unembellished, while the other
incorporated annotations (as required and appropriate) to highlight the
suspicious aspects.

(Regrettably though, some board houses do leave a lot to be desired. I have
recently heard of a case when a board house failed to match the locations of
a PCB's boundary to the locations of the boundary specified within the PCB
file. And in other cases, board houses have failed to read all of the
documentation which has been provided to them.)

Something which I have been doing for a very long time, and which I would
strongly recommend that *everyone* designing PCBs also do, is to (*always*)
review all of the Gerber files and NC-Drill files created from a PCB file
prior to sending them to any board house. The CAMtastic server provided with
AD can be used for that purpose, but for increased peace of mind, there is a
lot to be said for using a "third party" application for that purpose
(instead/ as well). (I am not aware of any significant defects within the
CAMtastic server that would result in any aspect of Gerber files or NC-Drill
files being "mis-displayed", but I still think that the additional degree of
"independence" that is gained from using somebody else's application to
(also) preview those files has a lot to be said for it.)

As some members of this mailing list are probably aware, I use Graphicode's
GC-Prevue application for that purpose, but there are various other
applications which can be used instead, of which some are of a similarly
freeware nature.

While it does not hurt to have some understanding of the nature of Gerber
(and NC Drill) files, the most important thing is to actually preview those
files. So although using *just* the CAMtastic server for that purpose is
arguably not as reassuring as (also) using a third party application, it
would still be better than not previewing those files at all. The better
board houses have their customers' interests at heart (and ultimately their
own interests) by procedures such as providing Acrobat files depicting what
each layer will look like, and/or contacting their customers whenever they
discover anything suspicious, but because some board houses aren't as
professional in that regard as others, everyone should still preview their
files (and *always* do so) prior to despatching them.

If the GC-Prevue application is typical of such applications in this regard,
you will need to invest some time in acquainting yourself with how to use
such an application (to actually preview Gerber and NC-Drill files). (Even
the CAMtastic server needs some time to become familiar with, partly because
the source code for it was originally acquired by Altium, rather than being
totally written by Altium's programmers "from scratch". Some effort has
since been made to make it more "Protel-like" in nature, but it is probably
still not as easy to use as the other servers.) But I would still advocate
that everyone take the time to become familiar with at least one such
application (or "if all else fails", even just the CAMtastic server), as
previewing files can still prevent PCBs from being mis-manufactured. (The
staff working at board houses can't read your mind, so in some
circumstances, the files they receive might not look suspicious to them, but
their contents could still result in PCBs being manufactured whose details
differ from what you actually intended.)

And at the risk of being perceived by some members of this mailing list as
"Altium-bashing" again, there are still some aspects about Altium's software
that also strengthen the case for always previewing Gerber (and NC Drill)
files. Some of the properties of pads and vias are determined by Design
Rules, and specifically by the "dominant" Design Rule of the appropriate
type for each such object for each of the properties concerned (involving
how those objects are rendered on the Internal Plane, Paste Mask, and Solder
Mask layers). And what you might think is the dominant Design Rule for a
particular pad or via does not necessarily always "match" what the software
thinks is the dominant Design Rule. Such mismatches can often be attributed
to "user-error", but it is still not out of the question that such
mismatches could sometimes be attributed to "software error" instead. But
regardless of whether any such mismatch can be attributed to user error or
to software error, there is still a good case for previewing the contents of
output files, and especially the Gerber files specifying the details on the
Internal Plane, Paste Mask, and Solder Mask layers.

And while I am not currently aware of how things are looking in that regard
within AD6, there have definitely been various issues in previous (major)
versions which have had an impact upon the "contents" of those layers. At
one stage there were two distinct bugs within the AD 2004 version whose
interaction could (and in at least one case actually did) result in (bottom
side) solder paste stencils being mis-manufactured. One of those bugs was
rectified before the release of SP4, while the other bug was not rectified
until after SP4 had been released. As SP4 was the last SP to be released for
AD 2004 though, that other bug is still present within AD 2004, and in some
circumstances can still "bite" the unwary.

(For users of AD 2004 to avoid being bitten by that bug, they need to ensure
that *every* surface mount pad within a PCB file is *truly* "Simple" in
nature. And it is *not* suitable to invoke the properties dialog box for
each such pad to check whether they really are Simple; it is instead
necessary to display the properties of such pads while using the Inspector
Panel or List Panel instead. If they subsequently find any Bottom (copper)
Layer pads which are *not* Simple, the values of each such pad's X-Size,
Y-Size, and Shape properties on the Bottom layer need to be copied to the
corresponding properties on the Top layer *and* (very important) to the
corresponding properties on the Mid layer. And if they find any Top (copper)
Layer pads which are *not* Simple, those pads should be temporarily moved to
the MultiLayer layer, then their "Padstack Mode" property set to the
"Simple" value, then their Layer property restored to the Top Layer again;
doing that is actually more straightforward than copying (the X-Size,
Y-Size, and Shape) property values from the Top layer to the Mid and Bottom
layers.)

Regards,
Geoff Harland.


----- Original Message ----- 
From: "John Echols" <jechols at keyless.com>
To: "Protel EDA Discussion List" <PEDA at techservinc.com>
Sent: Wednesday, November 29, 2006 8:48 AM
Subject: Re: [PEDA] Octagonal Pads


> All of the board houses we use send me pdf files of each layer for an OK
> before they proceed.  I can look for any obvious D-code mistakes and any
> special shapes I made to see if they came through as expected.
>
> John Echols
>
> -----Original Message-----
> From: Terry Creer [mailto:tcreer at entechgroup.net]
> Sent: Tuesday, November 28, 2006 2:26 PM
> To: dan_enslen at ti.com; 'Protel EDA Discussion List'
> Subject: Re: [PEDA] Octagonal Pads
>
> In addition to this, as I work at a manufacturer, I'm sure we'd be
> more than happy to do a check-plot of the artwork onto film for
> the customer to check the outputs prior to manufacture.
>
> Far cheaper than 'suck it and see' board runs.
>
> -----Original Message-----
> From: PEDA-bounces at techservinc.com
> On Behalf Of Dan Enslen
> Sent: Wednesday, 29 November 2006 6:58 AM
> To: 'Protel EDA Discussion List'
> Subject: Re: [PEDA] Octagonal Pads
>
> Good Afternoon All,
> I am not in the same position here as most, and I have
> absolutely no experience with Gerber readers, but it
> seems to me that it would be quite easy these days to
> make a prototype run to check out any radically new
> or questionable PCB structures. Granted, the monetary
> resources may prohibit this in a lot of cases. Just my
> 2 cents worth.
>
> Dan Enslen
>
> The only reason time exists is so
> everything doesn't happen all at once.