Re: [PROTEL EDA USERS]: Drill Drawing

[Jon Elson <jmelson@artsci.wustl.edu>]

Hans wrote:

> Hi Group,
>
>  The time has come to submit my design and one of the things that was
> requested was a drill drawing. I'm having somewhat of a probelm doing
> this. I generate the NC Drill output using the CAM manager. Up to here
> all works fine. Once I want to look at the file, say by importing it
> through CAMtastic, I can't get it in there. All the sudden, there are
> entries for tool numbers and things alike. So, my question is ... once I
> have a design on Protel (with through vias only) I generate the Gerber
> files for the masks, but what do I have to do in order to get the
> appropriate Drill code? Any help will be greatly appreciated,

I do this on all my boards.  The drill drawing (NOT the drill GUIDE!)
has little symbols that are different for each hole size.  Generally this
entire file uses only one aperture, except that the board outline from
a mechanical layer and any text either directly on that layer or from
a mechanical layer could be drawn in another aperture.

The NC Drill file (ASCII file extension .TXT, EIA extension .NCD)
is a totally different thing from the drill DRAWING - with the
extension .GD1     The .TXT file is generally preferred, as the old
EIA paper tape codes are officially obsolete.  The .TXT file
specifies the hole locations, and nothing else.

The .GD1 file is a DRAWING, to be plotted by a Gerber-compatible
photoplotter or just examined on the screen.  If you include the
...LEGEND text on that layer, a drill legend with the associated
symbol will be part of the drawing.

Don't try to look at the .TXT file with a gerber file viewer.  Although
these files are both variants of RS-274D (or X) syntax, the Gerber
files are generally created with leading zeroes suppressed and no
decimal points, and the drill files are generally created with TRAILING
zeroes suppressed, and no decimal points.  For this reason, the files
will massively corrupt the interpretation of coordinates.  Drill files
select tools with commands like T03, while the gerber files select
apertures with commands like D14.  So, these files are effectively
incompatible.

As for describing tools to the fab house, the drill report, .DRR,
should be sent to them, as a human-readable file listing the
drill sizes and tool numbers.  The tool sizes are actually listed in
the .TXT file as commands that would be ignored by many drill
controllers.

Jon