[PEDA] Tips on using Protel 99 SE

[Geoff Harland]

> Hi Geoff,
> WOW, thanks for all this.  I know I way behind the curve here but I just
> have not had to move up and I can do my boards so much faster in 2.8
> since I knew it so well.  I never really could afford the time to go
through
> the learning curve but I now have some extra time.
>
> -Bob


Glad I could be of some help. There are a considerable number of yet other
aspects which have also changed, though I'm not sure if I could recall all
of them (and I also have other demands upon my time).

Another change which I didn't mention in my previous message is that there
have been substantial changes when it comes to manually routing connections.
My recollection of version 2.8 was that you had to route from pad to pad, as
I definitely recall a number of PCBs within which I had to place two or more
tracks in the same locations because of that. (And I also recall that the
netlisting "intelligence" had a tendency to be "frail", and even when I was
accordingly very careful, the netlisting details could still get stuffed up.
There was one occasion when I was directed to "clean up" the netlisting
details within a PCB file, and it took me quite some time to do that, as I
had to save the PCB file in ASCII format, then delve through the associated
data, then make changes as required, and then confirm that I could reopen
that file and that the netlisting details were then fully rectified. In
short, really horrible...)

In Protel 99 SE (as was also the case with Versions 3, 98, the original 99,
and all versions following 99 SE), routing consists of placing tracks that
interconnect *any*  objects that have the same Net property, so it is no
longer necessary to have to route multiple tracks in any locations. You can,
if you want to, terminate a (manually placed) track at either end, *or* at
*any* intermediate location, of a (previously placed) track (which has the
same Net property). In addition to that, netlisting "intelligence" is
substantially more robust than what it was in version 2.8.

(Because of the netlisting and manual routing considerations, and the
inability to customise any of the menu entries, toolbar buttons, or shortcut
key assignments, I positively loathed using version 2.8. Before an initial
SP was subsequently released for it, the very first fully "public" version
of AdvPCB 3.0 had an assortment of reasonably serious bugs, with just one
example being that hidden (Designator or Comment) strings were depicted
within Composite Mode Printouts - but for all that, I still considered it to
be bliss when I finally actually got to use it.)

Another change is that the L key is now used (rather than the S key) to move
a component to the opposite side of the PCB (and components now have a
specific Layer property in their own right, whereas in version 2.8, which
side of the PCB that each component resides on is inferred from the layers
that its Designator and Comment strings are placed on). The L key can also
be used to "swap" the Layer property of other types of objects (in the cases
of layers which really are paired, to wit, the Overlay, Paste Mask, Solder
Mask, and external Signal (copper) layers), but (unlike in the versions
which follow Protel 99 SE), the outcome of "swapping" (the layers of) a
number of objects at the same time won't necessarily give you the outcome
which you might expect (vis-a-vis where each of the objects concerned ends
up relative to all of the other objects concerned), so keep that in mind
whenever you do use the L key.

Something else to keep in mind is that in version 2.8, the dialog box
listing a pad's properties *always* lists the properties of the pad on (all
of) the Top, Middle, and Bottom layers. In all of the following versions up
until Protel 99 SE though, that dialog box incorporates a "Uses Padstacks"
checkbox whose state determines whether a similar set of (9) controls for
listing the properties on each of those layers are enabled, or whether a
*different* set of (3) controls are enabled which specify the X-Size,
Y-Size, and Shape properties for *all* of those layers.

However there is a bug in that the values which are listed in the latter set
of controls *always* match the values which are specified for the *Top*
layer in the former set of controls. That is indeed appropriate for pads
residing on a "Top Side" layer (i.e. on either the Top Overlay, Top Paste
Mask, Top Solder Mask, or  Top Signal layers), but is *not* appropriate for
pads residing on a "Bottom Side" layer instead (i.e. on either the Bottom
Overlay, Bottom Paste Mask, Bottom Solder Mask, or  Bottom Signal layers),
when the values listed in the latter set of controls *should* match the
values which are specified for the *Bottom* layer in the former set of
controls. It is also *not* appropriate for pads residing on any of the
remaining layers, when the values listed in the latter set of controls
*should* match the values which are specified for the *Middle* layer in the
former set of controls.

As such, it is definitely preferable to keep all pads which are *not* on the
MultiLayer layer to be of a "Simple" nature (i.e. to have the "Uses
Padstacks" checkbox *not* checked),  as/but extra care and work is required
to "rectify" any such pads which are *not* on a "Top Side" layer.

And unless you specifically want different properties on different layers,
pads on the MultiLayer layer should also similarly be made "Simple". I have
determined relatively recently that there is a bug in how MultiLayer pads
are depicted within printouts within which you want the properties of such
pads on the Top layer or Bottom layer to be depicted, as the properties of
such pads on the *Middle* layer are *always* depicted instead...

There are still many other aspects where there are differences between the
2.8 and 99 SE versions, but I would now be struggling to recall them and/or
to find the time to describe them. However I have an idea that one of the
other members of this mailing list has prepared a FAQ which can be
downloaded from somewhere, and while it wasn't specifically written with the
objective of advising users moving from version 2.8 to 99 SE, the
information within it could still be of interest and value to you. Hopefully
whoever did prepare that FAQ is *still* a member of this mailing list, and
can either advise you of where to download it from or else provide you with
a copy, but otherwise maybe some other member of this list might be able to
assist in that regard.

I have also created two addon servers which provide additional functionality
for the Schematic and PCB servers, which can be downloaded from the
"protel-users" mailing list hosted by Yahoo Groups. Only members of that
mailing list can download those files though, but if you are not a member of
that list and are still interested, I could send you copies of those
servers. (I would also like to update those servers to provide yet more
functionality, but it is a case of finding the time to do so, and especially
to update and provide the associated documentation.)

Regards,
Geoff Harland.