[PCB_FORUM] Re: DGND/AGND merge point
- From: "Gary MacIndoe" <gary.macindoe@xxxxxxx>
- To: icu-pcb-forum@xxxxxxxxxxxxx
- Date: Thu, 21 Apr 2005 09:15:55 -0600
William,
Quite a few responses, all of them basically workarounds, for good reason.
You want to short together two differently named nets, YOU ARE NOT SUPPOSE
TO DO THAT!! No matter how you choose to short the two nets together (and
there are lots of ways to do it), you are more or less tricking the system.
When we have gnd and gndaud (audio ground), we create the separate planes,
and have a 0603 resistor to tie them together. This way gives you the most
flexibility: you can just put in a zero ohm to short them, you can put in
any value of resistance, short the 0603 pads with a wire or solder blob etc.
Ok, here's another way, a little bit different. Throughout your schematic,
you have lots of GND and AGND connections (probably two different ground
symbols). Somewhere in your schematics, put a resistor with GND on one side
and AGND on the other. After the design is placed/routed and you are ready
to create planes, define the separation between the two grounds with anti
etch (if your plane will be negative) or a reference line.
Next, in the schematics, remove the resistor between the two different
ground symbols and connect them together with just a wire. Since GND
probably has more connections than AGND (at least in our designs it does)
Concept will put all of the AGND connections on the GND net. Now you create
your GND plane leaving about a 50 mil or so gap somewhere along the
separation line. It is quite easy to undo if you want, just put the
resistor back in between the two ground symbols and you are back to GND and
AGND nets.
Good luck!
Gary E. MacIndoe
PCB Design Engineer
Advanced Micro Devices, Inc.
Longmont, Colorado
U2 at the Denver Pepsi Center were incredible!
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx]On Behalf Of William Billereau
Sent: Thursday, April 21, 2005 2:33 AM
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.
Other related posts: