[PROTEL EDA USERS]: Pad Master (plot)layers (ex Re: More trouble with P99SESP5 and gerber read back)

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

> At 12:40 AM 10/18/00 -0500, Jon Elson wrote:
>
> >Well, a pad master is not really a PC board layer, it is just a drawing.
>
> Drawing isn't the best word, but yes. And, in fact, Protel's "padmaster"
is
> not really a padmaster.
>
> >I turn all these unneeded plots off to reduce confusion.
>
> Absolutely a good idea.
>
> However, I have found one use for the top and bottom padmasters: In making
> an assembly drawing, I write gerber for, say, the top overlay and top
> padmaster. Then I bring these gerbers back in to the mechanical layer I am
> using for the assembly drawing. The padmaster includes only component
pads,
> whether they be surface mount or through-hole. Thus the pads together with
> the overlay usually make a good picture of the components, much better
than
> one will get from the overlay alone.
>
> This film is not what we used to call a padmaster -- which goes back to
the
> days of tape and mylar --, because the old padmasters also included vias.
>
> Padmasters were used, sometimes, for bombsighting as well as to generate
> solder masks
<snip>
> I did not invent padmaster artwork, but I did start using the technique
> before I learned that others were doing the same. I had been a printer and
> graphic artist, and printers also had a need for good layer register; the
> register pins I bought were made for use in the graphic arts.
>
> Abdulrahman Lomax

A trip down memory lane, with no objections from me on that count, and even
helpful in that I had forgotten, to some extent, that through hole pads and
vias (which were even more nearly always through hole in nature in those
days) were placed on their own, Pad Master, (mylar) layer, or at least when
you wanted the best possible registration of pads on different (copper)
layers (for the reasons described).

Although it was not unheard of for PCB designers to prepare and provide (to
the PCB manufacturer) a mylar sheet for the Solder Mask layer (or *two* such
sheets if the contents of the Top Solder Mask layer and Bottom Solder Mask
layer differed from one another), this was not universal practise. In the
event that *no* such sheets were created, the PCB manufacturer would
customarily prepare filmwork for a (common, i.e. top side and bottom side)
Solder Mask layer from an out-of-focus image of the Pad Master layer. The
consequence of the film being out of focus was that the diameters of the
resulting pad patterns were slightly larger than the *real* diameters of
these pads. (And this is precisely what is required for most pads on the
Solder Mask layers, *but* in the event that such layers are specifically
provided, then the contents of these can always be made to match *exactly*
what is required, including such details as the exact expansion value for
each pad and via, or whether each pad or via is "tented".)

The initial (DOS) versions of Protel were released in an era when the usage
of through hole components was still the norm, and one of the plotlayers
provided at that time (for producing printouts and Gerber files) was the Pad
Master plotlayer. (In due course, the Bottom Silkscreen layer and the two
Paste Mask layers were also provided, along with support for switching which
side of the PCB that each component was placed on.)

However, it could have been argued that the provision of the Pad Master
plotlayer was not absolutely necessary at that time, as the Gerber files
produced from each copper layer included the contents of the through hole
pads and vias, and the provision of Solder Mask layers (and plotlayers)
meant that the PCB manufacturer could also be provided with Gerber files for
the Solder Mask layer(s). I surmise that the Pad Master plotlayer could have
been provided for legacy reasons, which is arguably why the Drill Guide
layer (and associated plotlayers) were (and continue to be) provided. (Also
true, to some extent, for the Drill Drawing layer, but I for one *still*
produce printouts from this layer for checking and documentation purposes,
and as such, value the continued provision of this layer.)

At some stage, the previously provided Pad Master plotlayer was replaced by
Top Pad Master and Bottom Pad Master plotlayers. (Was there ever a time when
there were Top Pad Master and Bottom Pad Master plotlayers, *and* a (common)
Pad Master plotlayer?) As is reasonably well known, the Top Pad Master
plotlayer includes pad (primitives) from the Top Signal (copper) and
MultiLayer layers, and the Bottom Pad Master plotlayer similarly includes
pad (primitives) from the Top Signal (copper) and MultiLayer layers (and in
each case, they also include non-pad primitives from each Mechanical layer
which has been specified for inclusion in all (plot)layers). However, yet
again, it could be argued that the provision of these plotlayers is not
absolutely necessary. It remains possible to produce Gerber files for the
Solder Mask layers, and the Gerber files produced from each of the copper
layers specify where copper should be retained on each copper layer of the
PCB.

I suspect that legacy considerations are once again behind the reasoning to
provide these plotlayers. But as Abdulrahman Lomax and myself (and others?)
have mentioned in recent times, the provision of these plotlayers permits
(Top and Bottom) Assembly printouts to be created (from composite printouts
from Gerber files) *without* having to use the Power Print Server for this
purpose. As such, the (continued) provision of these plotlayers can be
regarded as highly desirable (just as I regard the (continued) provision of
the Drill Drawing layer as beneficial, as explained earlier in this
posting), even if the PCB manufacturer is not provided with the Gerber files
produced from these plotlayers (and ditto for Gerber files from the Drill
Drawing and Drill Guide plotlayers). (I have never provided Gerber files
produced from these plotlayers to any PCB manufacturer myself, and neither
have I ever been requested to provide such Gerber files.)

So please don't drop support for these plotlayers, Protel! (Going off-topic
to some extent, but please also give some consideration to re-providing a
Composite plotlayer, which was provided in early versions of Protel, but
which has since been withdrawn. Or even better, support for *multiple*
Composite plotlayers, with the ability for the user to designate *each* of
these. Or even better again, provide support for control over which
primitives from each layer end up in these files (in other words,
duplicating many of the capabilities of the Power Print Server when it comes
to generating Gerber files; it could be thought of as/called the Power
Gerber Server).)

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.