[PCB_FORUM] Re: DGND/AGND merge point
- From: "Gerry Meier" <gerry.meier@xxxxxxxxxxxxxx>
- To: <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Mon, 25 Apr 2005 06:52:59 -0700
Look at the net_short property in Allegro V15.2 it will include
information about the short in the comment section of the IPC-356A
netlist. So even if your sending valor data to your vendor export and
send the ipc netlist from Allegro. You may have to play with which net
is first:second to get it to work property.
The syntax of the NET_SHORT property is:
<net 1>:<net 2>:....
For example:
NET_SHORT = GND1 : GND2 : GND3
Gerry Meier
Sr. PCB Designer
Freedom CAD Services, Inc.
Voice: (603) 864-1300 x1350
Alt. Voice: (386) 753-0048
Email: gerry.meier@xxxxxxxxxxxxxx
visit our website at<http://www.freedomcad.com
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Kevin McCowan
Sent: Monday, April 25, 2005 9:49 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: DGND/AGND merge point
We did a version of this at my last job.
Placed a 0 ohmer and added a line/shape between the pads that was not on
a metal layer but was included in the gerber. It allowed us to have the
part and everything worked ok but we did not need to place the part.
The software did not complain and the schematic made sense (we used a
"do not place" part).
Still got a call from the board house because of a short, but after a
few times they came to understand it was intended.
Kevin McCowan
Sr. PCB Designer
TSI Telsys
Watts III, Nolan wrote:
> 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.
> 2> 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
-----------------------------------------------------------
-----------------------------------------------------------
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:
