<snip>
> As to microvias, if that only meant "small vias," there would obviously be
> no special support needed. But I think that some extra film may need to be
> generated for laser drilled vias-in-pad: no-copper areas where the hole is
> to be burned through. Once again, I'd ask the fabricator what was needed.
> Protel will not directly generate no-copper zones within pads, but it
would
> be easy enough to generate a film with flashes of the appropriate size
> where the holes were to be, and then the photoplotters could be instructed
> to subtract that film from the normal film for the layer.
>
> The other day, I was trying to remember why I wanted Protel to support
> anti-copper; I kept thinking that keepouts accomplish this for polygons.
> Here is the reason: anti-copper pads placed in a regular pad would create
a
> no-copper hole in the pad.
>
> (If all one wants is a small hole in the center of the pad, the donut
> capabilities of gerber could be used. Use manual apertures (not RS274-x)
> and specify the hole size. If one wants holes in other locations, one
could
> build up pads with the *real* pad has a hole and the other pads or fills
> extended the pad, but anti-copper would be a lot easier to use.)
>
> Abdulrahman Lomax
>From the point of view of producing Gerber files, defining an "anti-copper"
region within a larger region otherwise fully occupied by copper (for a
Gerber file of a "positive" nature) is not too difficult; a line of:
%LPC*%
could be added to a Gerber file, which indicates that following data is
"clear" rather than "dark".
The flashes for the microvias, which would be within the anti-copper areas
consequently defined (probably circular flashes with an appropriate
diameter), could in turn be preceeded by a line of
%LPD*%
which would indicate that the following data is "dark" again (rather than
"clear").
So the Gerber file for a "standard"/"signal" layer would have an '%LPD*%'
line near its start, then commands for most of the flashes and draws, then a
'%LPC*%' line, then flashes for "anti-copper" areas (typically within the
areas occupied by flashes which define pads), then another '%LPD*%' line,
then (last of all) flashes for the microvias (within the "anti-copper"
areas).
However, ... adding support for a general anti-copper feature within Protel
*itself* would be new, and past experience suggests that it takes a while
for Protel to produce debugged code after a new feature are added. That
said, if microvias are going to catch on, Protel is going to have to do what
needs to be done to support the use of these, and if that means adding
support for an anti-copper feature, I guess they, and us as the users, will
have to bite the bullet.
Then again, if microvias could *only* reside *precisely* at the geometric
centre of a pad, then the need for a general-purpose anti-copper feature
could be avoided; instead, the Pad Class could be enhanced to support an
(optional) (circular shaped) "no-copper" region whose centre coincides with
the pad's centre. The resulting Gerber files could then contain aperture
definitions in which some of the defined apertures are donut shaped rather
than solid, as Abdulrahman Lomax alluded to above. (By the way, I apologise
for not properly reading his relatively recent posting on multiple-section
schematic components; I acknowledge that he did mention that the 27th
section could have a suffix of AA, etc.) A small via (to wit the microvia)
could then be placed within this "no-copper" region.
All other things being equal, I suspect that it would be far easier for
Protel to enhance the Pad Class than to add support for a general-purpose
anti-copper feature. But I have no experience with using microvias, and I
suspect that it is not out of the question that routing considerations could
sometimes dictate that it would be preferable to locate a microvia within a
pad whose centre does *not* coincide with the pad's centre.
Another possibility be to enhance the Pad Class so that a "no-copper" region
could optionally be defined, with which the user could both specify the
diameter of this *and* its offset from the pad's centre. (The Gerber files
would be more complex, but the commands described above could be used to
achieve the desired result.) My gut feeling is that this would still be far
preferable to attempting to add a general-purpose anti-copper feature.
(Updated DRC procedure: check that a microvia's centre co-incides with the
centre of the "no-copper" region within the pad surrounding the microvia,
and that there is sufficient clearance between the microvia and the
surrounding pad. With a general-purpose anti-copper feature though,
<shudder>.)
Regards,
Geoff Harland.
-----------------------------
E-Mail Disclaimer
The Information in this e-mail is confidential and may be legally
privileged. It is intended solely for the addressee. Access to this
e-mail by anyone else is unauthorised. If you are not the intended
recipient, any disclosure, copying, distribution or any action taken
or omitted to be taken in reliance on it, is prohibited and may be
unlawful. Any opinions or advice contained in this e-mail are
confidential and not for public display.
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
