The NET_SHORT property mentioned by Vivekananda can be added to the pin of the connector inside the schematic as well. This will ensure connectivity without adding any dummy part. -- George Patrick Tektronix, Inc. Central Engineering, PCB Design Group P.O. Box 500, M/S 39-512 Beaverton, OR 97077-0001 Phone: 503-627-5272 Fax: 503-627-5587 <http://www.tektronix.com/> http://www.tektronix.com <http://www.pcb-designer.com/> http://www.pcb-designer.com It's my opinion, not Tektronix' -----Original Message----- From: icu-pcb-forum-bounce@xxxxxxxxxxxxx [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Vivekananda R K - CTD, Chennai Sent: Thursday, April 21, 2005 04:02 To: icu-pcb-forum@xxxxxxxxxxxxx Subject: [PCB_FORUM] Re: DGND/AGND merge point Hi William, I can understand your problem.I can suggest one more way to short agnd,dgnd . 1.Create PTH oblong shape(based your required length and width) 2.Create the pin as a .dra file. 3.Place that pin(Note:Very important that this pin should come through the Netlist and as a component you can assign net name as agnd or dgnd) between agnd,dgnd split point.(once it is placed the tool will take the clearance between pin to shape) 4.Edit /Property of the pin only 5.Select "Net_short" 6.Add the net names agnd(if the pin net name in the netlist is assigned dgnd) or (the pin net name in the netlist is dgnd than assign in the net short property agnd) This will avoid the drc . If any doubt pls mail me. Regards Vivek Pcb Designer HCL Technologies Chennai -----Original Message----- From: William Billereau [mailto:william.billereau@xxxxxxx] Sent: Thursday, April 21, 2005 4:02 PM To: icu-pcb-forum@xxxxxxxxxxxxx Subject: [PCB_FORUM] Re: DGND/AGND merge point Thanks for this tips, but it is a workaround. It avoids DRC but not future errors as it is not electrically controlled. In fact I forgot to tell that we used to do such methods but it can later on a new revision generate a short-circuit or something like. So we think it is not secure.. And then we would need something safer, if possible.... William ----- Original Message ----- From: Vivekananda R K - CTD, Chennai <mailto:vivekanandark@xxxxxxxxxxx> To: icu-pcb-forum@xxxxxxxxxxxxx <mailto:icu-pcb-forum@xxxxxxxxxxxxx> Sent: Thursday, April 21, 2005 12:22 PM Subject: [PCB_FORUM] Re: DGND/AGND merge point Hi William, In allegro menu 1.Setup/Subclass/Board geometry/ Create a layer called "GND_SHORT" 2.Add/line under Board geometry/Gnd_short layer(Here you need to add a line width of 50 mil with required length where the agnd and dgnd gnds generating point) 3.In the manufacturing /artwork/Film Control select your gnd layer.art (plane layer)film and add the subclass layer "gnd_short" under the class board geometry(Set it in the Gerber level) I hope this may help without generating DRC. Regards K.Vivek Pcb Designer Hcl Technologies Chennai. India. -----Original Message----- From: William Billereau [mailto:william.billereau@xxxxxxx] Sent: Thursday, April 21, 2005 2:03 PM To: icu-pcb-forum@xxxxxxxxxxxxx Subject: [PCB_FORUM] DGND/AGND merge point Hello All. Quite often, a board contains both AGND and DGND and the customer asks us to connect them together on a single point on the board, like GND pin of a connector. Does anybody know how to do it in Allegro without generating DRCs errors? Thanks in advance. William. DISCLAIMER: This message and any attachment(s) contained here are information that is confidential, proprietary to HCL Technologies and its customers. Contents may be privileged or otherwise protected by law. The information is solely intended for the individual or the entity it is addressed to. If you are not the intended recipient of this message, you are not authorized to read, forward, print, retain, copy or disseminate this message or any part of it. If you have received this e-mail in error, please notify the sender immediately by return e-mail and delete it from your computer