Mark,

 You can also have problems like this with the 274D format.
A few things you might try:

1) Make sure your Allegro Accuracy [under Drawing Parameters]
and your Gerber Format line up, e.g. if you work in mils [.001"]
and your accuracy is 1, you're at .0001" accuracy in Allegro.
If your Format is 5.3 [Integer places.Decimal places] then the plotter
resolution is only to .001", +/- .0005" and it may not be able to
plot your shapes and cut outs. Try to set you Gerber Format to one place
beyond your Allegro accuracy [current limit of Gerber Format in Allegro
Ver 13.6 is X.5].

2) If your shapes have a lot of fine detail, you may be running out
of memory when your plot file is being built and Allegro may not warn
you. Try building the plot in a directory where you have more memory
available.

3) Make sure your shapes pass the Allegro Shape Check. If they don't,
fix the problems before plotting.

4) Get a Gerber Viewer besides Allegro & use it to check your plots.
Usually, Allegro is right on but when it's wrong it's really wrong
and the internal viewer won't always show the problem.A FREE viewer
is available from Lavenir (Windows/NT) @ :
http://www.Lavenir.com/Download/download.html  and it seems to work well.
We liked it enough we bought a copy so we could save job files for
reference. Other viewers, some free or with demo versions, are available.

5) Try the Cadence Users Group for more help. Details @
 http://www.dacafe.com/USERSGROUPS/Cadence/pcb.html

Tom Martin

At 02:38 PM 7/17/00 -0500, Mark Walter wrote:
>Has anyone seen problems with generating artwork files
>using the Gerber RS274x Format on Cadence?  We are
>running version PE13 still and I recently sent out a board
>using this "new" Gerber only to find out that one of the
>shapes on the top layer did not plot- No errors nor warnings
>regarding this were given and the boards will have to be
>reworked at a considerable cost and loss of time in the factory.