I'll comment on the original and, a bit, on Mr. Wiseman's reply.

At 04:57 AM 10/2/2003, Steve Wiseman wrote:
02/10/2003 09:26:45, "Ryan Koh" <[EMAIL PROTECTED]>

>To ensure that all my vias are not exposed after fabrication
(masked), is it
>that "Tented" should be selected under the via properties?


That is now the simplest and most flexible way to do it. So you will just do a Global Edit on the vias you want tented. The older way, before Protel gave us the Tent checkbox, was to define the solder mask clearance for the vias, in the Manufacturing Rules, as a negative number greater than the radius of the via pad.

>I am trying to created Gnd border along the perimeter of my
rectangular pcb
>board, which should be masked (just like thick traces). If I were
to use
>"place trace", the cornerings would be round - not what I want to
>It is required that the cornerings be sharp right angles.

I might ask, "Why?" Sharp right angles in copper at the edge of the board are somewhat of an invitation for something to peel up the copper. Not a big likelihood of it happening, but if the engineer made this requirement, I *would* want to know why. More usually, *if* there is a real requirement, it would not be "sharp" but rather a maximum radius. In some applications a sharp point like that has .... effects. I'd ask the function of this ring of copper.

The simplest way to put copper around the board is, in fact, to draw it with track. It's more trouble to do it any other way, so there ought to be a reason!

If it's rihgt at th edge of teh board, then the router (whirling-blade
thing, not autorouter) will make sure that the edges follow the
edge of teh PCB (but board houses don;t like routing through
copper, since they get little slivers that can end up in teh wrong

Generally speaking, you don't want copper to the edge not only because of that, but because it will end up being exposed, unprotected by solder mask, and possibly not with solder either, so it would be quite vulnerable to corrosion.

>Can I use "place Fill" or "Place Pads" to create the GND border? If
so, what
>can I do to ensure that my GND border would not be exposed
(masked like
>copper traces) after fabrication?

You don't want to use pads, per se, because of the solder mask complication. You could, of course, tent the pads with a Mfg. Rule, but this is unnecessarily complex since there is a better way.

I'd go for a fill (and lock it down, or Protel will perpetually assume
you'd much rather be editing the fill than anything else...)
If you go for pads, you'll have to mess around with editing them,
whereas fill, you can just drag. Pads will by default be exposed (
no soldermask), fills are just copper features. If you want them
exposed, drpo a fill on the soldermask layer in the same place.

One more comment about fills. Protel generally will photoplot them with a flash, i.e., as if they were pads. It creates an aperture definition for the flash. Just as good practice, One might create a fill that is the shape of an already used square pad. This will avoid the creation of an extra aperture. Not a huge issue, just a detail. If I wanted a 100 mil border, with square edges, I'd probably just create a 100x100 mil fill and put one in each corner of the board, with 100 mil track between them.

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

Reply via email to