Bingo!!  Thanks Dwight, and everyone else that replied.

Now I understand why they said the inner planes were shorted.  I assigned
the pad to the top layer, and it was plated.  Duh!!

>From what I've gathered in all the responses, I can summarize what I've

1. Mounting holes should be multilayered.  This prevents shorting to inner
power layers.
2. Don't forget about additional mounting screw clearances!!  Do something
to prevent traces from being routed beneath the head of the screw, as
tightening the screw may scrape off the solder mask and cause a short.  This
can be accomplished by defining the X and Y size larger than the OD of the
head of the screw.
3. Define a large enough pad to provide for imprecise drills.  If the drill
is too large on a small pad, this may also cause shorts between layers.
4. Of course when one defines a pad, one must also choose a net on which to
place that pad.  I believe this should be "No Net"

I still have a one question:

1. Why is it important to change the X and Y size to zero before production.
It was said this prevents "flashing" from within the Gerber file, but I
don't know what that means.

> Andy,
> As far as why AC said the holes shorted, I'll take a guess:  If
> you made the pads single-layer (e.g., Top Layer) instead of
> MultiLayer, that's why.  If you look at the PCB in single-layer
> mode (Shift-S), for a single layer pad there won't be 'negative
> copper' on the inner planes to keep the planes away from the hole
> edges.  So if the hole is plated, you've got a definite short.  If
> unplated, your mounting screw could still easily short the planes.

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
*  This message sent by: PROTEL EDA USERS MAILING LIST
*  Use the "reply" command in your email program to
*  respond to this message.
*  To unsubscribe from this mailing list use the form at
*  the Association web site. You will need to give the same
*  email address you originally used to subscribe (do not
*  give an alias unless it was used to subscribe).
*  Visit
*  to unsubscribe or to subscribe a new email address.
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *


To leave the EDAFORUM discussion list, send a email with
'leave edaforum' in the body to '[EMAIL PROTECTED]'

More Information :

Reply via email to