At 01:50 PM 11/9/01 +1100, Geoff Harland wrote:

>However, I also consider that efforts to change or enhance pad and via
>objects would open a very large can of worms. Amongst the issues to consider
>(but certainly not the only issues concerned) are whether properties
>associated with the Solder Mask layers, Paste Mask layers, and Power Plane
>layers should be set by Design Rules, or by dialog boxes, or by either of
>those options. (I have spoken on that matter previously; at present,
>listings of Design Rules do not "report" settings which have been customised
>by usage of dialog boxes.)

I'd think that a bug because a user might rely on the design rule believing 
that it is of universal application. But I have not researched this.

In talking about the potential elimination of the "Multilayer" layer, 
however, no change is contemplated, per se, in how the calculated layers 
(solder mask, paste mask, inner planes, drill drawing) are handled.

The actual utility of the Multilayer layer is quite limited. Almost never 
would one want to draw a track on that layer. It appears in plots of all 
copper layers, yet it does not DRC, as I recall. Right now, there are two 
uses: through pads and vias. A "multilayer" pad is one which appears on all 
copper layers. This, right away, is problematic, since the layer appearance 
of pads is customizable; it is the *hole* which definitely appears on all 
layers, *if* it is a through hole. Pads, however, may be placed on any 
layer individually. Protel gets drill-drawing indigestion if such 
single-layer pads have holes, as I recall.

Vias, at present, can only be placed on the "multilayer" layer. Since vias 
can be blind or buried, the true display of a copper layer could be 
different depending on the layer. So a via is not really "multilayer." Once 
upon a time it was, and Protel's implementation was reasonable, if not the 
best.

(Basically, the difference between pads and vias has become academic.)

There are certain functions of the multilayer layer, I suspect, that are 
used by various designers. It would be useful to enumerate those uses, so 
that we could suggest how to provide the same or better functionality while 
fixing the problems created by the "multilayer" concept.

The *original* multilayer concept was that of an object that appeared the 
*same* on all copper layers. Thus a multilayer object could be displayed 
simply as it was, if and only if the multilayer layer was enabled, no 
problem. But that went out the door, first with surface mount, and then 
with blind and buried vias.

>Abd ul-Rahman Lomax has also recently mentioned that "blind" and "buried"
>vias are sometimes inappropriately displayed.

Actually, they are *always* inappropriately displayed. Either you have 
multilayer turned off, in which case no vias are displayed at all, or you 
have it turned on, in which case vias are displayed unconditionally, 
whether or not they exist on the enabled layers. This is really a major 
shortcoming at the point, actually one of the worst of which I know.

>  I concur that this could be
>regarded as a bug, but apart from that, I personally don't regard the
>MultiLayer layer as being "bad" in nature. It is a "special" layer, like the
>Drill Draw, Drill Guide and Keep Out layers, but PCB applications differ
>from general purpose CAD applications (such as Autocad) in that there is a
>good case for "special" layers to be provided.

I have not heard, yet, any good argument for the maintenance of this layer 
as a "layer." It is a "concept" more than it is a layer. A button that, in 
Display setup, turns on all copper layers would be useful. But a via is a 
via, it does not need a special layer!

[EMAIL PROTECTED]
Abdulrahman Lomax
Easthampton, Massachusetts USA

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to