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.

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.

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.

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

>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
P.O. Box 690
El Verano, CA 95433

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To join or leave this list visit:
*                      - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
* Contact the list manager:
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to