> What is the best way to put a mounting hole in a PCB?
> I had a CAM HOLD put on a job I sent to Advanced Circuits.  They said all
> the holes, which I defined as pads with zero X and Y size and the
> appropriate hole size, shorted out the two inner planes.
> I want a simple hole, not connected to any net.
> Should I make the X and Y size the same as the hole size?  Which layer
> should I put the pad on?
> Andy Sybrandy

The following is a repeat of a posting I made not that long ago (on 2 Feb
this year):

> Does anyone know how to make non plated holes without a pad show up when
> you print?
> Ron Tupa

When I want a pure hole on a PCB, i.e. no copper within the hole and no
copper around the outside of it on any layer, I place a pad in the
appropriate location, set its Plated property as False, and, *initially*,
set its width (X-Size) and height (Y-Size) equal to its hole size.

This width and height (equal to hole size) are sustained when preparing
printouts; the locations (and diameters) of such holes are subsequently
displayed. But when I prepare Gerber files from the PCB file though, I
(previously) set the width and height of all such pads to *zero*. That way,
the associated pads will not be "flashed" at all within the Gerber files.

The Global editing feature can be used to "zero" all such pads prior to
producing Gerber files; the selection/qualification criterion is pads with
the *same* Plated property (given that you would select one of the unplated
pads when making such a change), and the properties to be copied (which
would be selected by default) are the X-Size and Y-Size. (The "All
primitives" item should also be selected instead of the "All FREE
primitives" item within the "Change Scope" ListBox, unless none of the
components in the PCB file incorporate such holes/pads.)

A Design Rule, or Design Rules, should be set up so that the Solder Mask
Expansion distance for all such pads is zero. And if/when you want the
soldermask film to end clear of such holes (by 5mil, say, or perhaps even
more, if the underside of the head of a screw will be sitting on the surface
of the PCB), separate pad(s) of the appropriate diameter should be placed on
the Top Solder Mask and/or Bottom Solder Mask layers (in the same location
as the hole/pad on the MultiLayer layer). (Speaking personally, I normally
don't add such pads on these layers myself, but there could be situations
where a "flash" is required in the Gerber file(s) for the Top Solder Mask
and/or Bottom Solder Mask (plot)layers.)

I have previously released an addon Server for use with Protel 99 SE which
incorporates a Process which will either "zero" all such pads (so avoiding
the need to use the Global editing feature, as described above) or "unzero"
these (restoring the width and height of each such pad equal to its hole
diameter). As explained, such pads would be "zeroed" before generating
Gerber files, and "unzeroed" before producing printouts (in the event that
you wanting to produce printouts *after* producing Gerber files). However,
while the Processes within this Sever (a number of other Processes are also
provided) will work if SP5 is installed, these Processes will *not* work
when SP6 is installed (because Protel has updated some of the files
associated with using addon Servers, as well as requiring such Servers to be
compiled using Delphi 5, instead of either Delphi 5 or Delphi 3, as was
previously the case). As such, I will be providing an updated version of my
addon Server at the earliest opportunity, and members of this forum will be
notified at the time that I do so. (So watch this space.)


If it is not clear from that posting, the pads concerned are on the
MultiLayer layer. And as far as the updated Servers go, I have visions of
uploading these to the egroups/Yahoo website before I finish work today
(conditional upon finding the time to complete the associated tasks). I will
post again advising when these Servers have been so uploaded.

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.

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
*  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 http://www.techservinc.com/protelusers/subscrib.html
*  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 : http://www.dolist.net

Reply via email to