[PEDA] Tips on using Protel 99 SE (was: Advanced PCB V2.8 Libraries)

[Geoff Harland]

Hi Bob,

I'm glad to hear that you figured out how to open that Library file.

With hindsight, I could have informed you that you would need to either
"import" that file or define a "link" to it, but I have been so accustomed
to using Protel 99 SE that aspects like that are second nature to me, and at
that the time that I previously responded to this thread, I was unaware that
you had only started using Protel 99 SE recently.

Because many aspects of Protel 99 SE differ from version 2.8, you would be
well advised to read as much documentation as possible to familiarise
yourself with what has changed. I'm making no claims to provide an
exhaustive list of all of those changes, but here are *some* of the things
which have changed:

- PCB Library files can now be created or edited without having to have any
PCB (document) file also open at the same time.

- Instead of 16 Signal layers, 4 Internal Plane layers, and 4 Mechanical
layers, there are now 32 Signal layers, 16 Internal Plane layers, and 16
Mechanical layers. The Mechanical layers are only enabled if you
specifically enable them though, with the "Setup Mechanical Layers" dialog
box (menu entry of "Design >> Mechanical Layers...") being used to control
which of those layers are enabled, and the name assigned to each of those
layers. Similarly, with the exception of the two external layers, none of
the copper layers are "enabled" unless you specifically enable them; copper
layers are similarly "enabled" or "disabled" (and renamed) from the "Layer
Stack Manager" dialog (menu entry of "Design >> Layer Stack Manager...").

WARNING: it is not impossible to "mis-sequence" copper layers, and/or end up
with "missing" copper layers. (Example of first: a sequence of Top, Mid 2,
Mid 1, Bottom; example of second, a sequence of Top, Mid 2, Mid 3, Bottom,
which could be created be enabling the Mid 1, Mid 2, and Mid 3 layers, and
then disabling the Mid 1 layer again.) In order to minimise the probability
of a PCB not being manufactured properly, you should remain accordingly
vigilant about which layers are currently enabled, and their current
sequence.

- Vias can now connect to Internal Plane layers, and both vias and pads can
now *each* connect to more than one Internal Plane layer.

- Properties of pads and vias on the Internal Plane and (Paste and Solder)
Mask layers are now specified by the use of Design Rules. That has been the
case for all versions since version 2.8, though with Protel 99 SE,
properties of pads and vias on the Mask layers can be specified on a per-pad
or per-via basis ("over-riding" the value of the property that would
otherwise be defined by the appropriate type of "dominant" Design Rule for
that particular pad or via).

WARNING: the ("Design >> Make Library") command that creates a PCB Library
file from the components contained in a PCB (document) file is buggy, as the
values of some of properties are *not* always properly "copied" from the
"source" components to the "target" footprints. User-specified values for
Paste Mask Expansion and Solder Mask Expansion properties are amongst the
properties which are thus-afflicted.

- Printouts from PCB files are now created by the use of a "PCB
Printer/Previewer" server in conjunction with "PCB Printer" files (which
have an extension of .PPC), and there is a lot more control over exactly
what appears within each printout. And if you have installed SP6 for Protel
99 SE (which I would strongly recommend if you haven't already done so), a
new Special String of .Printout_Name is available for identifying the name
of each printout. (The .LayerName Special String is still provided, but it
always identifies the layer that it resides on within all printouts, thus
matching the behaviour of that string within "Composite Mode" printouts in
version 2.8.)

- Gerber files, NC Drill files, BOM files, Pick and Place files, and Test
Point Report files are now created by the use of a "CAM Manager" server in
conjunction with "CAM output configuration" files (which have an extension
of .CAM).

- It is no longer possible to create "plots" from PCB files.

- The details of thermal relief patterns which have *four* conductors
(rather than just *two* conductors) are now correctly defined within Gerber
files which incorporate embedded aperture definitions; that had *not* been
the case in version 2.8 (which you may or may not previously have been aware
of). However details of thermal relief patterns which have *two* conductors
(rather than *four* conductors) are *not* correctly defined within Gerber
files which incorporate embedded aperture definitions (and unless that has
been rectified in AD 2006, is *still* an outstanding bug involving Gerber
files). And like version 2.8, pads which have an Octagonal Shape are *never*
correctly defined within Gerber files which incorporate embedded aperture
definitions (and yet again, unless that has been rectified in AD 2006, is
yet another still outstanding bug involving Gerber files).

- It is possible for users to "customise" their "Resources", to wit, menu
entries, toolbar buttons, and shortcut keys. A tip from my personal
experience is that if you want to define shortcut keys which can start
commands in the middle of other commands, then *don't* define any such
shortcuts which (also) use the 'Alt' key, and *don't* define any such
shortcuts which use either the 'F9' or 'F10' key (and regardless of whether
or not any other keys, such as the 'Shift', 'Ctrl', or 'Alt' keys, are also
used at the same time).

- Users can also define and subsequently run "scripts" which can perform
various tasks on an "automated" basis. And at one time it was also possible
for users to be provided with "SDK" files (if they were prepared to agree to
a NDA) which permitted them to create their own addon servers (if they also
had a copy of Delphi 5) to provide yet more customised functionality. (I
don't know if you would ever be interested in doing that, and I also don't
know whether Altium would still be prepared to provide those files to
anyone. As far as I'm concerned though, they *should* still be prepared to
provide those files to "bona fide" owners of Protel 99 SE, even if they do
so without also providing any support to anyone actually using those files.)

It is not out of the question that you were already aware of at least some
of the items on the above list, but as Altium no longer provide support for
Protel 99 SE, *this* mailing list is effectively the predominant means of
ongoing support for that particular version.

There are assorted bugs in Protel 99 SE, some of which are of a "gotcha"
nature. To avoid one such "gotcha" which I am specifically aware of, *all*
pads which incorporate holes should reside on the MultiLayer layer, as any
such pads which are *not* on that layer do *not* "auto-generate" "blowouts"
(aka "antipads") on any of the Internal Plane layers.

And to avoid another not-unrelated "gotcha", it is also advisable to define
a "Power Plane Connect Style" Design Rule with a "No Connect" Rule Attribute
which specifically applies to *all* pads with a False Plated property,
because without such a Design Rule being defined, you risk an outcome in
which the software will attempt to "connect" some of those pads to Internal
Plane layers (by "Thermal Relief" and/or "Direct" connections). (You should
probably define a Pad Class whose members consist of all such pads, and then
specify that particular Pad Class as the set of objects which that
particular Design Rule then applies to.)

Also bear in mind that DRC (Design Rule Checking) procedures should not be
treated as "gospel", as aspects involving Internal Plane layers are not as
well analysed as they could be, and pads with a False Plated property are
regarded as "unroutable" (which can be a real pain if you ever really do
want to route connections to such pads).

There are many other things which I could say about Protel 99 SE, but
hopefully what I have said will still give you a good start, and don't
hesitate to ask if there are any aspects for which you would like to have
answers provided.

Regards,
Geoff Harland.


> Hi Geoff,
> I got this to work.   I had to "Import" the file.  Took me awhile to
figure
> out how to get a blank DDB set to accept it.  I think I have it now,
> in 99SE library format.
> Thanks,
>
> -Bob
>
> >Hi Bob,
> >
> >You *should* be able to open an AdvPcb 2.8 Pcb Library file in Protel 99
SE,
> >as I tried this just a minute ago, and had no problems.
> >
> >You might need to "specify", however, that the file concerned is a *PCB*
> >Library file, and *not* a *Schematic* Library file, as both types of
files
> >use the same extension (.LIB) in all versions of Protel up until Protel
99
> >SE. In the Explorer window, right click on the icon provided for the
file,
> >then select "Properties" from the popup menu. Then select the "PCB
Library
> >Document" item within the resulting "Properties" dialog.
> >
> >If you still have problems opening that file, I could have a go at
> >attempting to open/update it for you if you like, so you could attach a
copy
> >of the file concerned within a private message sent to me. (Naturally I
> >wouldn't disclose any details of the contents of that file to anyone
else.)
> >
> >Regards,
> >Geoff Harland.
> >g_harland at optusnet.com.au
> >
> > > Hi,
> > > Is there any way to read AdvPCB V2.8 libraries into 99SE?  The manual
> > > says you can add them but when I try I it says the format is
unrecognized.
> > > I would really like to acess these footprints.
> > > Thanks,
> > >
> > > -Bob