> At 11:17 AM 3/14/01 +1100, Geoff Harland wrote:
>
> >Out of curiosity, what do you suggest should be done in a situation where
> >someone wants an unplated hole through a PCB, and this hole is to pass
> >through the middle of a pad on the bottom (copper) layer?
>
> Before making a suggestion, I would preferably want to know *why* the user
> wanted such a feature. It might affect the answer.
>
> But let me imagine one. One needs to solder a wire or part to the board
> and needs the hole to mount the part, but other constraints, perhaps very
> tight trace density in the area, only allows a minimal hole to be placed
> in the area, and there is no room for a pad on any other layer than, say,
> the bottom.

I did describe a scenario myself, further on in my previous post, in which
the designer might want such a feature. This scenario concerned the pads
used in a footprint for a through-hole crystal, where pads on the top side
of the PCB (were these to be provided) could short with the body of the
crystal, or at least if these were of the same diameter as the pads on the
bottom side of the PCB. (I also said that I use plated pads on the
MultiLayer layer myself, and use the padstacks feature so that the pads on
the top side of the PCB are much smaller in diameter then the pads on the
bottom side (and middle layers) of the PCB.)

> First of all, it should be noted that such a structure could be quite
> weak. This is effectively a single-sided PCB, as far as that part is
> concerned, and pad sizes for single-side PCBs are typically made quite a
> bit larger in order to provide better adhesion of the pad to the board.
> Even then, failure rates where there is any stress on the lead at all will
> be very high. I've  had a number of consumer audio products fail because
> the adhesive did not hold and ultimately the pad or the track attaching to
> the pad (more likely) cracked. Clinched leads can help, but if there is
> room for a clinched lead there is probably room for a pad. It is not the
> plating that is so important, but having a pad/solder fillet on both
> sides, which, with the lead itself, makes a rivet that is not easily
> dislodged.

The observation that the presense of a pad/solder fillet on both sides of
the PCB makes a rivet of robust nature is very pertinent in the
circumstances. It definitely vindicates my usage of plated through pads that
use the padstack feature (over the alternative option of using bottom side
only pads with unplated holes).

Other things being equal, plated-through pads should be used in preference
to single layer pads with unplated holes; the former are more reliable for
the reason described. But my experience with de-soldering through-hole
components from PCBs using plated-through multilayer pads indicates that the
superiority of this type of pad is not unconditional. (That is an
observation rather than an attempt to advocate that single layer unplated
pads be used instead. If you have the right equipment, and keep it in proper
order, de-soldering such components is less of a hassle than is otherwise
the case.)

> Having said that it is probably foolish, I would then go ahead and suggest
> there are a number of ways to accomplish the matter. Putting a hole in an
> SMT pad, as I recall, can confuse Protel in a number of ways, I'm not sure
> it works. Obviously, one might use a padstack and define the pad as
> non-plated, but there are complications with that as well.
>
> I'd be tempted to place a surface pad and an additional pad in the same
> location which would be through-hole, nonplated. I'm not sure what pad
> size I would use. Zero is too small; it is tempting to make the pad size
> the same size as the hole, but this has a reputation of generating little
> slivers of copper, not from the hole drilling, since the holes are
> generally drilled first, before any pattern has been established, but from
> misregister between the hole and the film. Perhaps it might be better to
> make the pad 5 mils smaller than the hole (10 mils diametric). With
> appropriate clearance rules it would serve as a routing obstacle. Because
> the hole is non-plated, it could come very close to a track without harm,
> perhaps as close as a mil or two, I don't know how close I would want to
> push it.

I concur that this method should work, but my sentiment is that it should
not be necessary to have to use two pads; I would prefer that I could
configure just *one* pad as required.

> Or one could use a single padstack with pads defined in a similar way.

If the pad's plated property is set false, I think that there would be
problems with routing to it. And if its plated property is set true instead,
you would have a plated through hole which would have no copper surrounding
it on the internal and top layers. That would be undesirable (as the rivet
aspect of a multilayer pad would be lost, amongst other things). Of course,
if the hole is surrounded by a minimal amount of copper on those layers,
then you would have a multilayer pad using the padstacks feature, which is
what I do in practice. But such a pad is multilayer and plated-through in
nature, rather than of a single layer and unplated nature. (And as this
thread has disclosed, this is in fact the preferable thing to do.)

> >My understanding is that whenever a hole in a PCB *is* through-plated,
> >then it is always advisable to have a minimal width of copper surrounding
> >the hole on each copper layer. As an example, if there should be at least
> >5mil of copper surrounding each hole, and a hole's diameter is 20mil,
> >then the minimum width and height of the associated pad on any layer
> >(Top, Bottom, or (intermediate) Middle) is 30mil (allowing 20mil for the
> >hole and 5mil on *each* side of this).
>
> To put this in perspective, you will have 1.4 mils of copper on the wall,
> so, effectively, with a plated through hole, you have a minimum pad size 3
> mils diametric larger than the hole. Considering drill tolerance and hole
> position tolerance, 5 mils radial is about as small as one would want to
> go.
>
> Abdulrahman Lomax

Thank you for responding to my enquiry. I would hope that all of those
following this thread now appreciate the superiority, from at least a
reliability perspective, of using plated-through multilayer pads, over the
alternative option of using single layer unplated pads.

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 join or 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]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to