Drill hole to etch/Shape clearance (DRC)

Currently there is no Drill Hole to Etch/Shape clearance checks in Allegro available. Normally the only time this comes up is when you have Non-Plated holes that need to be kept clear and in those cases I add Route Keepouts to library symbol to prevent any problems. I know that there has been some talk about supporting Drill to Pin/Via/Etch checks but there has been no commitment at this point.

Mike Catrambone
UTStarcom, Inc.

Thank You,
SATYA
ATS ECAD Tech pvt ltd

With the emerging of high speed signals there will be a need to eliminate via pads in internal layers - to reduce capacitance/match via impedance.
in my design i need to remove via pads for specific nets type in specific layers.
after changing the via defenition to pad smaller then hole
i get traces hug the via hole.
as i know it is not possible to add a keepout to via defenition.
a poor work around is to eliminate the via pads as last action before gerbers.
when the PCB will come back for Rev Upgrade we will have to restore the via pad size before routing.

Roby Drath
MEMTEK Ltd.

In the Artwork Control Form, Film Control section you can use the option, Suppress Unconnected Pad. You can set this option individually for each layer. It does not remove the pads from the Allegro data base, it only removes them from the Gerber artwork. There is no need to restore the via pad because it is never removed from the Allegro database. For additional control you can take advantage of the Optional/Fixed switches in Pad Designer. Choosing the Fixed setting in Pad Designer prevents suppression of the pad in the Gerber data even if Suppress Unconnected Pad is turned on in the Artwork Control Form. Randy

hi randy

I'm aware of this function
BUT, the Padstack library has not been built with this in mind.
any way one may want to remove pads of only particular vias without the need to built new via type and replace the desired vias
Roby