[PEDA] Many similar Sheet Symbols

[Geoff Harland]

I'm *not* advocating that users *don't* use the Multi-Channel feature in
Altium Designer - but I *am* recommending that users should exercise
prudence whenever they do use it.

There are a number of options which can be selected when that feature is
used, ... and some of them might not work as well as others. For instance,
if an Alphabetical option is selected instead of a Numeric option, there
could be problems if the design incorporates more than 26 channels. With a
26th channel identified as "Z", the best outcome would be for a 27th channel
to be identified as "AA" (using a "numbering" scheme like that used to
identify the columns within spreadsheet files), and *maybe* that has now
been implemented, ... but in all of the versions of AD which I have seen,
the 27th channel is identified as "[" instead (with that character being the
character that immediately follows the "Z" character within the ASCII set of
characters). (As such, a 63th channel could be identified by the "DEL"
("Delete") character, which could really cause some grief.)

And while it is possible to define "bussed" netlist labels of a "one
dimensional" nature (e.g. D[0..7] for D0 .. D7), it is not implausible that
"multi-dimensional" netlist labels are still sitting in the "too-hard"
basket (as they certainly weren't implemented in the first instance). I also
recall that the "variable" part of netlist labels had to be at the very
*end* of each label, so while D0 .. D7 can be "bussed" (in the form of
D[0..7]), there were (and still are?) problems with attempting to "bus"
netlist labels such as D0B, D1B, ... , D7B - as D[0..7]B did not work as
envisaged.

Another thing which I found, while experimenting with the feature, was that
if I had a "Top" sheet, a "Row" sheet, a "Column" sheet, and a "Cell" sheet
(with the number of manifested instances of each type of sheet being 1, N,
M, and N*M respectively), then some options would work as envisaged, while
others were "dysfunctional". Furthermore, I can't recall off-hand whether
any of the "dysfunctional" options were totally warning-free when I
attempted to compile the project - but I do specifically recall that *none*
of the working options were *totally* warning-free. When I subsequently
reported those findings to one of Altium's programmers, I was informed that
the Multi-Channel feature was not intended to implement that type of
functionality. That would doubtless largely explain the outcomes I
encountered, but it still doesn't change the fact that it's not inherently
obvious that that type of functionality was not intended to be supported.

Moral of the story: if you want to use the feature, I would suggest looking
at the netlist file and the set of components created from the project, and
checking that all of the associated details are fully compliant with what
you intended.

As I have mentioned in other messages, there are many issues with Altium
Designer concerning features and functionality which have not been fully
thought through, and testing of the application is nowhere near as
comprehensive as it should be. And of course there are so many bugs which
have either only been fixed many *years* after they were first reported or
which have *yet* to be fixed (yet again many years after first being
reported).

I fully appreciate that it would not be appropriate for *all* bugs to be
fixed *only* when they reach the "front" of the queue, as some bugs are more
serious than others. That said, many of the bugs which are still
outstanding, or which were only fixed many years after first being reported,
are still bugs which *should* have been fixed in relatively short order,
either because they are of a "gotcha" nature, or because they force users to
jump through multiple hoops to get a job done, or because they otherwise
severely undermine user-productivity.

We really should be complaining about this situation to a much larger extent
than has been the case to date. Altium's corporate culture is not conducive
to raising the quality of its software through its own efforts, so unless
the level of complaining is distinctly escalated, we are going to keep on
getting more and more of the same.

When a new major version of software is released, the only reason why users
should feel ambivalent about it is the possible requirement to install it on
a PC with a higher running speed / yet more RAM / yet more hard disk
capacity. (I don't know why "bloat" is so much of an issue, but Altium is
certainly not the only offender in this regard).

With Altium Designer though, we are "treated" to new features which haven't
been fully thought through and which are still buggy, and it is a lottery as
to whether functionality which had been provided in previous versions is
still retained. (One example: until the ".PrintoutName" Special String was
eventually provided, the functionality previously provided by the
".LayerName" Special String, in identifying the nature of each ("Final
Mode") printout, had been lost. Another example: until relatively recently,
all versions following SP6 for Protel 99 SE did not permit users to
re-sequence the sequence of printouts within a set of printouts, which was
painful if you wanted to create a PDF file within which the sequence of all
layers (including non-copper layers) matched the sequence of layers within
the PCB file (as resequencing the sequence of printouts within a set of
printouts *was* possible in Protel 99 SE). And yet another example: the
"Find Similar Objects" feature was (and still is?) less user-friendly in
implementing "global" editing (than with the previously provided "expanded"
dialog boxes), as it didn't (and still doesn't?) provide users with the
ability to specify that only "free" primitives should be selected by that
feature, while excluding primitives which are child objects of components or
polygons.)

Almost enough for a day. One last thing though: Is Altium Designer still
"polluting" the RS-274X standard? In one of the SPs released for AD6 (which
I don't have a copy of, so I can't answer this myself), the release note
claimed that octagonal pads are now correctly depicted within Gerber files
for all angles. My experience has been that octagonal pads have *never* been
correctly depicted within Gerber files for *any* angle, so my initial
inclination was to say "oh oh". To test whether the "pollution" is still
occurring, place just one pad in a PCB file, with an Angle (Rotation)
property of zero degrees, equal X-Size and Y-Size values (e.g. 60mil), and
an Octagonal Shape property. Generate a Gerber file from that PCB file, and
check whether the pad which is depicted within the Gerber file appears the
same as the pad within the PCB file. If the RS-274X standard is still being
"polluted", the pad depicted within the Gerber file will have two vertices
on the X axis and another two vertices on the Y axis, so *none* of its
(eight) edges will be either horizontal or vertical. (OTOH, the pad in the
PCB file will have two horizontal edges and two vertical edges.)

While enquiring whether Altium Designer still "polluting" the RS-274X
standard could sound like I am asking whether somebody is still beating
their wife, the fact remains that Altium Designer *has* been "polluting" the
RS-274X standard in at least the past, even if it is not still doing so.
Maybe things really have improved in that regard, but I first reported that
there was an issue in this regard back in 1997, so *if* that issue has since
been rectified, it has *only* been rectified some time this year.

(Class performance, eh?)

Regards,
Geoff Harland.


> Hi Jakub,
>
> It's too bad that AD6 isn't a possibility for you,  as a multi-channel
design is
> *much* easier with AD6.  Otherwise a lot of manual intervention is
> required.  You might check out the multi-channel design demo's just to see
> what AD6 could do for you in this area:
> http://www.altium.com/webdemos/?p=10
>
http://www.altium.com/Evaluate/DEMOcenter/AltiumDesigneroverview/Multichanneldesign/
>
> I don't recall 99SE auto-generating the sheets for you here,  I think you
had to
> copy/paste a sheet to make the new sheets.  Then manually edit all of the
ref
> des so there were no duplicates.
>
> Somewhat painful in 99SE.  A piece of cake in AD.
>
> ---Phil Stevens
>
> >> GET AD6
> >> :)
> >> it really handles this pretty well
> >>
> >> in 99SE there are methods but at the end of the day i found that you
> >> really needed the 20 separate sheets
> >> and getting them to all annotate nicely was a major pain
> >>
> >> the 'repeat' feature was what finally drove me to AD6
> >>
> >> Dennis Saputelli