> It's useful to have a pad of finite size so that it'll be visible as a
> reminder in case you have "(Show) Pad Holes" turned off on
> the Design\Options panel. Best to make an NPT pad up as a
> single-layer pad on the Drill Drawing Layer; this avoids creating
> objects on the Mask Layers during Gerber generation, and
> eliminates error messages during DRC. I use 10mil diameter
> pad for standard boards, with the hole size adjusted to suit.
>
> Brian

While I appreciate that using pads on the Drill Drawing Layer avoids
creating images on the Solder Mask layers, printouts of the Drill Drawing
layer are problematic for such pads; only those pads which are located on
the MultiLayer layer, and external copper layers (I think), have their
associated hole diameters depicted, and counted, in printouts of the Drill
Drawing layer. (However, these holes *are* listed and counted in the NC
Drill files.)

As such, I confine all pads having an associated hole to the MultiLayer
layer (see below for more details).

> I make the pad and the hole size the same and tick off the "Plated" box in
> the Pad->Advanced menu. It works fine with the Print Preview and my PCB
> manufacturer doesn't complain.
>
> Igor
>
> > Do I need to have a pad size greater than zero for a NPT hole (mounting)
> > or should I make it equal to zero.
> >
> > Jerry Gierach

Personal preference to some extent, but I set each such pad's pad diameter
equal to its hole diameter when saving the PCB file, and when generating
printouts. And when I want to generate Gerber files, I set the pad diameter
of all such pads equal to zero.

I have created a process within my PcbAddon server which facilitates either
"zeroing" all such pad diameters (for pads having unplated holes) or setting
the pad diameter of each such pad equal to its hole diameter.

Setting the pad diameter equal to hole diameter when producing printouts
means that the associated hole gets to be depicted in the printouts; OTOH,
there is no merit in "flashing" such pads within Gerber files (because any
copper within the associated hole's boundary does not end up within the
final PCB). While it arguably doesn't hurt to have such pads "flashed" (as
long as the diameter of the flash is less than the diameter of the pad's
hole), eliminating a "flash" all together results in smaller Gerber files.

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