At 12:35 PM 6/23/99 +0800, Lum Wee Mei wrote:
>  I have a question regarding Gerber output. Most of our designs are done
>with 6/6 (trace/spacing). One one occassion, our regular PCB vendor called
>us up and inform us that they found some 5/5 on a particular layout.
>However, when we call up the layout on our workstation with grid at 1mil
>setting, we found that the so-called problem area to be a perfect 6/6.

Perhaps you should send your workstation to the vendor! :-)

Seriously, what a CAD program shows is *theoretically* the same as what it
outputs as Gerber, but there are many pitfalls. I don't know Mentor, but I
know of only one way that a 6 mil trace can become a 5 mil one, and that is
the assignment of an incorrect aperture. Some CAD systems will accept an
aperture if it is within a certain tolerance of the exact size for the
primitive; this is one way that 6 could become 5; but it would be expected
to be 5 *everywhere*, not just in some places. As to 5 mil clearances, this
might be caused by roundoff error, either in the Gerber generation (perhaps
there is a resolution setting) or in the plotting. One clue is the comment
"at 1 mil setting." What does one find with the grid at 0.1 mil?

Another possibility is that the few traces that turn out to be 5 mils are
actually 5 mils, and roundoff is responsible for the belief that it is 6
mils. But I would assume that Mentor would be able to query the trace
directly to determine its size.

I'd look at the Gerber with a viewer; if you don't have one, there are a
number of free ones available for download. Graphicode gcprevue, Lavenir,
CAM350, CamCAD, CAMtastic may be names to look for.

If the viewer confirms what the CAD program shows, the problem is almost
certainly at the fabricator's end.

But to be absolutely sure, I would look at the gerber code itself. Gerber
is pretty easy to read with a text editor, and once one knows the
formatting which is being used in a particular file, it is pretty easy to
take the coordinates of a trace and find the trace even in a large file.
Looking at the aperture table (which will either be an external table or
will be embedded at the beginning of the Gerber file), one will know
exactly what aperture is being used and where the lines are being drawn. If
the traces are being drawn orthagonally, that is, either the x-coordinate
or the y-coordinate is the same for both ends, finding the separation
between two traces is just a matter of subtraction. Otherwise it may take a
little more calculation....

And measuring a non-orthagonal trace separation using a 1-mil grid may also
produce a round-off error of up to 1 mil.

If it is a vendor problem, it should be possible to isolate the problem
Gerber and send a file to the vendor containing only that little piece;
this would enable the vendor to better identify what is going wrong.


[log in to unmask]
Abdulrahman Lomax
P.O. Box 690
El Verano, CA 95433