> Can anyone tell me if it is possible make a via or pad that is connected
to
> the Vcc net on the top and bottom layers only. TI do not want to connect
it
> to the inner Vcc plane as the decoupling caps are on the secondary side of
> the pcb and I want the voltage to see them before the leg of the IC.
>
> I tried making a pad and using the padstack to not connect to the middle
> layers but was not sucessful.
>
> Wesley Webb

As others have suggested, use a (MultiLayer) pad instead of a via, and
define a Design Rule so that there are no connections to that pad on any
internal Power Plane layers.

A possible problem with using pads (instead of vias) is that
non-single-layer pads are always through-hole in nature (whereas vias can
also be "blind" or "buried" in nature). As such, if a "blind" or "buried"
via is desired, *and* it is desirable to have this *not* connect to one or
more internal Power Plane layers (that are amongst those layers "occupied"
by the via), I would then go for adding pads on those internal Power Plane
layers as required (in the same location as the via concerned). (And if the
via is moved, these pads should also be moved at the same time.)

I previously mentioned that I would provide a post on the MultiLayer layer,
pads, and vias. I have not forgotten about that intention, and I still
intend to do so. At this stage though, with pads and vias having reared
their head again, I will mention that I see merit in retaining the
distinction between pads and vias. When Pad Master printouts or Gerber files
are produced, vias are *not* included in these, and that aspect would be
lost if vias ceased to be a distinct type of object.

As such, this thread suggests that there is merit in the concept of being
able to assign names/designators to vias. If implemented, Design Rules could
then be defined to control assorted properties of individual vias, with the
application of such Design Rules then being selectable by the
name/designator assigned to each via. (The "(AdvPcb) 2.8" (i.e. dialog box
determined) approach would avoid the requirement to assign names to vias,
but that would rule out the possibility of being able to set the properties
of vias on a selective basis by the use of Design Rules, as well as making
it more difficult to determine which vias have particular properties.)

Another difference between pads and vias is that (unlike vias) pads can not
be "blind" or "buried" in nature, i.e. occupy more than one copper layer,
but not *all* of those layers. Off-hand, I do not see any merit in being
able to define *pads* (as opposed to vias) that have a "blind" or "buried"
nature, but if anyone thinks differently, then let us all know, and why.

Does anyone see merit in being able to define *vias* with
obround/rectangular/octagonal shape (rather than just circular shape), or
with different shapes and/or dimensions on different layers? (At present
that can be accomplished for "through hole" connections, by using pad
objects instead of via objects, but not for "blind" or "buried"
connections.) My view is that the purpose of vias is to provide connections
between different copper layers, and as such, a circular shape does the job
just fine, as the associated *hole* is also circular in shape (and also has
the same diameter for each copper layer it encounters). But given that I
think that there is a case for being able to control *other* properties of
vias, such as internal Power Plane layer connection details, polygon
connection details, and Solder Mask layer properties (including the ability
to set these properties for *each* of those layers), maybe "padstacks"
properties are yet another aspect of vias that could also be
user-controllable.

More in another post (next week I hope, and maybe I can find time this
weekend to write some of the details). For the time being, I am ambivalent
about the MultiLayer layer. I suspect that this could be totally eliminated
from future (major) versions of Protel, but I am not at all convinced that
this would necessarily be a good idea. That is not to say that this layer is
devoid of shortcomings, but I currently lean to the view that totally
dumping that layer would be somewhat akin to throwing out the baby with the
bathwater...

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/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