[PCB_FORUM] Re: DGND/AGND merge point
- From: chris.ball@xxxxxxxxx
- To: icu-pcb-forum@xxxxxxxxxxxxx
- Date: Mon, 25 Apr 2005 10:04:19 -0400
I think the reason there are many solutions is that the 'best' solution
depends on the many things, some of which are the product, the designer and
engineer's personal preference, the company environment (workflow, library,
output, relationship with fab, CEM, etc....), etc...
There is no one answer that is 'best' for everyone, and as with any ECAD
system, there are many ways of handling the situation. I was thrilled to
find that Cadence has some options (like NET_SHORT) so that I can handle it
without additional 'kluge' parts in the schematic and layout, after years
of that....
-Chris
"Watts III, Nolan"
<nolan.watts.iii@xxxxxxxx> To:
icu-pcb-forum@xxxxxxxxxxxxx
Sent by: cc:
icu-pcb-forum-bounce@freel Subject:
[PCB_FORUM] Re: DGND/AGND merge point
ists.org
04/25/2005 09:42 AM
Please respond to
icu-pcb-forum
I agree. No DRC's, and you don't have to explain that you have two nets
shorted on the Gerber that are not connected in the netlist. Less
confusion for the downstream process.
Nolan
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Mike Golding
Sent: Friday, April 22, 2005 2:24 AM
To: 'icu-pcb-forum@xxxxxxxxxxxxx'
Subject: [PCB_FORUM] Re: DGND/AGND merge point
So it sounds like the only good answer that would satisfy the problem is
the
0 ohm resistor. I've done a lot of the suggestions from this thread in
the
past and personally like the 0 ohm solution the best.
Pros
It doesn't cause DRCs, it's driven by the schematic, no manual
alterations.
Cons
Takes up board space(there's always room for one more!), added item(s)
to
the BOM
-Mike
(Feel free to deprecate)
-----Original Message-----
From: Budathoki, Trilok (GE Consumer & Industrial)
[mailto:trilok.budathoki@xxxxxx]
Sent: Friday, April 22, 2005 3:14 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Cc: Paul Bradshaw
Subject: [PCB_FORUM] Re: DGND/AGND merge point
Paul,
With Due respect, I disagree with you. We talking about shorting two
nets
AGND & DGND. The method you suggesting just clears DRC but it leaves
serious
question unanswered.
1> How will you differentiate AGND & DGND nets.
2> Component Placement, deciding on split Gnd planes is difficult. This
is
gray area where you can go wrong.
3> If your board has only one net AGND/DGND, Signal Integrity Analysis
3> for entire design is not possible.
4> At PCB vendor's end,it might not pass BBT.
Trilok Budathoki
G.E- India Business Center
Email : trilok.budathoki@xxxxxx
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx]On Behalf Of Paul Bradshaw
Sent: Thursday, April 21, 2005 8:57 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: DGND/AGND merge point
If you short together two signals in ConceptHDL, it picks the
alphabetically
first one. So in this case, as far as Allegro is concerned, everything
becomes AGND. But this method does work. It's what we do.
Paul Bradshaw
Symbol Technologies, Inc
6480 Via Del Oro Drive
Mail Stop 14
San Jose, CA 95119
(408) 528-2606
>>> gary.macindoe@xxxxxxx 04/21/05 08:15AM >>>
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.
________________________________________________________________________
This email has been scanned for computer viruses.
________________________________________________________________________
This email has been scanned for computer viruses.
-----------------------------------------------------------
To subscribe/unsubscribe:
Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx
with a subject of subscribe or unsubscribe
To view the archives of this list please login at
//www.freelists.org.
Our list name is icu-pcb-forum or go to
//www.freelists.org/archives/icu-pcb-forum/
Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
Want to post a job listing ? DON'T DO IT HERE!
Better yet, join our jobs listing forum.
SUBSCRIBE: icu-jobs-forum-subscribe@xxxxxxxxxx
POST: icu-jobs-forum@xxxxxxxxxx
-----------------------------------------------------------
-----------------------------------------------------------
To subscribe/unsubscribe:
Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx
with a subject of subscribe or unsubscribe
To view the archives of this list please login at
//www.freelists.org.
Our list name is icu-pcb-forum or go to
//www.freelists.org/archives/icu-pcb-forum/
Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
Want to post a job listing ? DON'T DO IT HERE!
Better yet, join our jobs listing forum.
SUBSCRIBE: icu-jobs-forum-subscribe@xxxxxxxxxx
POST: icu-jobs-forum@xxxxxxxxxx
-----------------------------------------------------------
-----------------------------------------------------------
To subscribe/unsubscribe:
Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx
with a subject of subscribe or unsubscribe
To view the archives of this list please login at
//www.freelists.org. Our list name is icu-pcb-forum
or go to //www.freelists.org/archives/icu-pcb-forum/
Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
Want to post a job listing ? DON'T DO IT HERE!
Better yet, join our jobs listing forum.
SUBSCRIBE: icu-jobs-forum-subscribe@xxxxxxxxxx
POST: icu-jobs-forum@xxxxxxxxxx
-----------------------------------------------------------
-----------------------------------------------------------
To subscribe/unsubscribe:
Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx
with a subject of subscribe or unsubscribe
To view the archives of this list please login at
//www.freelists.org. Our list name is icu-pcb-forum
or go to //www.freelists.org/archives/icu-pcb-forum/
Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
Want to post a job listing ? DON'T DO IT HERE!
Better yet, join our jobs listing forum.
SUBSCRIBE: icu-jobs-forum-subscribe@xxxxxxxxxx
POST: icu-jobs-forum@xxxxxxxxxx
-----------------------------------------------------------
-----------------------------------------------------------
To subscribe/unsubscribe:
Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx
with a subject of subscribe or unsubscribe
To view the archives of this list please login at
//www.freelists.org. Our list name is icu-pcb-forum
or go to //www.freelists.org/archives/icu-pcb-forum/
Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
Want to post a job listing ? DON'T DO IT HERE!
Better yet, join our jobs listing forum.
SUBSCRIBE: icu-jobs-forum-subscribe@xxxxxxxxxx
POST: icu-jobs-forum@xxxxxxxxxx
-----------------------------------------------------------
Other related posts:
