[PEDA] Many similar Sheet Symbols

[Phillip Stevens]

Hi Geoff,

As a user of AD,  I'd first like to say "Thank You" for "fighting the
good fight" on our behalf,  while you were there.

I'm currently reading Beginning Python, by Magnus Lie Hetland,  Apress.
There is a nice quote from page 343 that I thought you might appreciate:

"...it can be useful to adopt the attitude that a feature doesn't really
exist (or isn't really a feature) until you have a test for it."

Friday, November 3, 2006, 4:16:10 AM, you wrote:

> 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



>  
> ____________________________________________________________
> You are subscribed to the PEDA discussion forum

> To Post messages:
> mailto:PEDA at techservinc.com

> Unsubscribe and Other Options:
> http://techservinc.com/mailman/listinfo/peda_techservinc.com

> Browse or Search Old Archives (2001-2004):
> http://www.mail-archive.com/proteledaforum@techservinc.com
>  
> Browse or Search Current Archives (2004-Current):
> http://www.mail-archive.com/peda@techservinc.com