> Another option is to use a through-hole "component". The schematic symbol
> has 2 pins, one connected to each net. The footprint has two
(through-hole)
> pads that are close enough to short (as described earlier). Place the
> footprint stradling the boundary between the planes, so each thru-hole
will
> connect to one plane.
>
> Dwight Harm
>
> Agreed. This would be acceptable in many (if not all) situations, and if
> appropriately implemented (by setting the pads' X-Size and Y-Size to zero
on
> Mid layers, and ditto on one of the outside layers (which is possible by
> using the Padstacks feature), thus confining the (linking) copper
connection
> to just *one* of the external copper layers), could even permit the nets
to
> be disconnected (relatively easily) if so required, which could be useful
> for testing or trouble-shooting purposes.
<snip>
> Geoff Harland.
Thinking about my previous posting (above), concerning the possible usage of
the padstacks feature, it would in fact be a bad idea to set the pads'
X-Size and Y-Size to *zero* on Mid layers and one of the outside layers, as
that would have undesirable implications from the perspectives of PCB
manufacture and net-connecting quality.
As such, if users really did want to link two nets on *just* *one* of the
outside copper layers (to facilitate disconnecting these nets if so desired,
whether for testing/trouble-shooting purposes or otherwise), the Padstacks
feature should be used, but the pads' X-Size and Y-Size on the Mid layers
and *other* outside (copper) layer should be set to some larger value
(greater than zero). Values should be chosen to ensure a minimal thickness
of copper between the edge of the hole and the edge of the pad (on that
layer), with such a distance being something like 5mil to 10mil. As such,
the pads' X-Size and Y-Size (on those layers) should be 10mil to 20mil
larger than the pads' hole diameter (as there is copper on both (/opposite)
sides of the hole).
And whereas a rectangular shape should be selected for (both pads on) the
outside copper layer being used to connect the nets, a circular shape should
be selected instead for (both pads on) the Mid layers and other external
copper layer.
The distance between the centres of the (two) pads should of course be great
enough to ensure that these pads are satisfactorily separated on all the
layers where the pad diameter is smaller (and the pad shape is circular).
And on the layer where the pads are to come in (very) close contact, the
pads' X-Size and Y-Size should be set to both achieve this (very) close
contact, and to implement the required thickness of the "link" between the
different nets.
On a different note, I have not made extensive use of polygons on Power
Plane layers. That said, I am not unaware of the limitations on the
locations of polygons' boundaries (relative to one another); it is not
(currently) possible to place one polygon *totally* inside another. As such,
one improvement for Protel to look at is aspiring to an objective of
supporting any combination of polygon boundaries which is topologically
"kosher". (In the case of one polygon inside the other, the region within
the *inner* polygon should be regarded as being part of that polygon, while
the *remainder* of the region within the *outer* polygon should be regarded
as being part of that polygon instead. In general (always?), if the
boundaries of different polygons never touch/cross one another, a
topologically "kosher" situation exists.)
Although implementing this may seem straightforward and obvious, I strongly
suspect that to actually implement this would be easier said than done, and
that probably is in fact the reason why it hasn't been implemented to date.
That said, there must be times when the (current) inability to place any
polygon entirely within another is an unwelcome and undesirable shortcoming.
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]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
