At 01:32 PM 6/21/01 -0500, David Cary wrote:
>Here's some stuff on my wish list. (Please tell me if Protel already does
>any of
>this stuff).
>
>---
>Make vias identical.
>Normally I want every via to be identical hole size, identical annular ring,
>etc. (but different x,y locations and nets, of course).
>Can I set up a design rule to warn me about accidentally modified vias ?
> (If I wanted something different, I could work around that design rule by
>converting it into a pad).
The Routing Via design rule seems to be intended for the autorouter, as has
been noted by Mr. Velander, it is not a rule check.
There is, however, a manufacturing rule for annular ring. This will detect
if any via has been modified such that it has insufficient annular ring. If
the via has sufficient ring, I might suggest that "fixing" it so that it is
the same as all the others might be intellectually satisfying but is
unlikely to improve the manufacturability of the board except under certain
conditions:
(1) The annular ring rule has been set too small. To control this, the rule
should be set to the actual size desired for all vias. Thus if a via ring
is different from the desired size, it will be larger and thus will either
have no effect on manufacturability or will improve it.
(2) The via is an odd hole size which creates an extra drill size. It
should be routine to review hole sizes on a board and eliminate unnecessary
variations. If one has some 32 mil holes and some 35 mil holes, usually it
would be appropriate to pick one size and use that for both original sizes.
There is a report option under Report/BoardInformation/Report, Net Via
Size. It is unclear to me what it does. It provides what appears to be a
report of via outer diameter, but the information as to diameter seems to
come from the Routing Via rule rather than from the vias themselves.
However, there are other report options which would identify wayward vias.
Assuming that hole size variations have been eliminated, any variation in
size will be a variation in annular ring. By selecting all vias and running
an annular ring report (say, top layer annular ring -- check the "selected"
box), you will get a list of vias with their annular rings.
Of course, you could simply double-click on a via, make it the size you
want, press the global button, check Copy Attributes for diameter and hole
size, and OK the global edit. You don't need a report if you simply *make*
all vias identical in this way.
>Is there a way to jump to each selected component one at a time ? I'm
>imagining
>another option under ``Browse PCB | Browse | Selected'' to list all the
>selected
>stuff, and then I could (one at a time) pick one from a list and hit ``Jump''.
It's easier than that, but less flexible. If you select the relevant
components, you can look at them one at a time with Jump Selected. You
don't have control over the sequence. Jump Selected will probably jump to
the first selected pad it finds, you may need to zoom out to see the whole
component.
>Sometimes I wish there were a way to select and delete ``unused stubs''. Say I
>move a component to the opposite side of the board. That usually leaves a
>lot of
>tracks that run to where the pads used to be. I don't need them any more.
>(Sometimes those stubs get deleted by Automatic Loop Removal when I re-route
>something nearby, but I can't seem to repeat that when I want to).
Good idea, but it's not in Protel at the present. Maybe the autorouter
would do it, but I hesitate to suggest tossing the board into such a
meatgrinder. The new autorouter *might* be usable for this. And it might
not. As far as I know, the only way to find these stubs, short of someone
writing a utility (the algorithm is simple), is to inspect the board layer
by layer; using single-layer display will make this quicker.
>Automatic unused via removal:
>Somehow I end up with a lot of vias that don't ``do anything''. They might be
>connected to copper on the top layer, but they do not connect to any of the
>power planes or to any copper on any other layer. I want to select them and
>delete them.
Ditto as with stubs. Highlighting all vias and inspecting layer by layer is
reasonably easy.
>--
>Redundant via removal:
>The autorouter likes to pile several identical vias at the same x,y
>location. It
>looks OK on the screen, but some board houses complain about ``multiple drill
>hits''. I don't see any reason not to automatically delete identical vias when
>they're at the same x,y location.
There is a tool for this from Premier EDA, I think. I don't know if it is
up-to-date. I'm not entirely convinced that automatic delection is a good
idea, but certainly the drill plots and drill output routines should
consider coincident holes as a single hole. This would eliminate multiple hits.
[EMAIL PROTECTED]
Abdulrahman Lomax
P.O. Box 690
El Verano, CA 95433
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/subscrib.html
* - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/[email protected]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
