I previously used a Cadstar for windows EDA software that supported slot/pads and it also showed the pad dimensions in the drill chart. This data was is the Gerber data. We also gave decisions of each slot to help the MFG recognize these pad definitions. This seems to be different and more room for error in P99SE because the pad will show up as a drill hit in the Gerber data and if they do not look at the extra slot definition for that pad on one of your mechanical layers that you have dientioned then your not going to get a plated slot for that pad. I have to do this for a RCD ceramic 25W PWLL resistor footprint. Also just noticed DXP is the same as P99SE they give a good description and suggestion on their connector footprint in the connector library part called "050DSUB0.762-4H15".
-----Original Message----- From: Dennis Saputelli [mailto:[EMAIL PROTECTED] Sent: Friday, October 10, 2003 10:28 AM To: Protel EDA Forum Subject: Re: [PEDA] oblong Pads/Slots (plated) in P99SE we have done it most of the different ways you have outlined it hasn't seemed to have mattered much which methond we use, if the notes are clear it comes out ok by almost whatever method you use but one time it didn't ... we just got a hole instead of a plated slot and all of the quick turn multilayer bds were ruined, they couldn't be grunched (and time lost which was even more valuable) our notes and methods were clear and the same shop followed them correctly on previous orders when i complained they launched an 'investigation' after a day or so they called and said they found out what the problem was "what?" i ask "we make mistake" they said they replaced all the boards so the bottom line is that it would be nice if there were some 'standard' way to have this in the electronic file that did not rely so much on operator skills and reading ability both of which are on downward trends doesn't the excellon format support slots? Dennis Saputelli "John A. Ross [Design]" wrote: > > > -----Original Message----- > > From: Michael Biggs [mailto:[EMAIL PROTECTED] > > Sent: Thursday, October 09, 2003 6:48 PM > > To: 'Protel EDA Forum' > > Subject: [PEDA] oblong Pads/Slots (plated) in P99SE > > > > I have noticed in P99SE component library that you cannot > > change the hole size to be a oblong or plated slot for > > footprints. I know there are alternative ways to call out > > these drill holes to be plated slots within the pad, but what > > is the proper or favorable way to do this in P99SE? Thank You > > in advance for responses. > > Michael > > My favoured way for definition of a cut out (plated or otherwise) within > a pad is as follows. > > Create pad as a rectangular shape and define pad stack ensuring the pad > dimensions have allowed for enough free land around the slot. > > In the centre of the pad I make the hole size the same as the width of > the slot (rout) that is needed within the pad. > > If the slot is to be plated, then mark the hold plated, if not plated > then mark it as such. > > So up to now we have the pad defined, plating status and slot width as > well as the centre of the slot. > > I usually define Mech layer 1 as a board outline and use Mech layer 2 > for board dimensions. > > On mech layer 1 & 2 I draw an outline of the slot I need the same as the > hole diameter in the pad and using arcs with the same radius of the pad > hole to terminate the slot ends. > > On layer 2 I add the overall dimensions so that the fab shop can see > where to draw the drill/rout path. I also make a small annotation here > as well to indicate plated status as the pad definition seems to be too > subtle for some fabs, :-( even although it is documented in the release > notes. > > Sometimes I also place 2 x co-ordinates at the centre of the opposite > arcs within the slot on layer 3, as some front end systems allow for the > start/end points of the slot to be typed in instead of drawn. But these > are useless if the same origin is not used after import to the usable > film box within the CAM tools the fab shop uses. > > I prefer to use a single pad for this, I have seen other suggestions > using 2 to mark the rout start/end, same idea as my co-ords above so > that the CAM guys can just draw/snap between the 2 but this has other > issues. > > Best Regards > > John A. Ross > > RSD Communications ltd > Email [EMAIL PROTECTED] > WWW http://www.rsd.tv > ================================== -- Dennis Saputelli ========= send only plain text please! - no HTML ========== _______________________________________________________________________ Integrated Controls, Inc. www.integratedcontrolsinc.com 2851 21st Street tel: 415-647-0480 San Francisco, CA 94110 fax: 415-647-3003 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *