[PCB_FORUM] Re: DGND/AGND merge point
- From: "Gerry Meier" <gerry.meier@xxxxxxxxxxxxxx>
- To: <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Thu, 21 Apr 2005 07:32:20 -0700
Yves
Also if you use 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 Yves Cantraine
Sent: Thursday, April 21, 2005 9:48 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: DGND/AGND merge point
You can short two dynamic shapes together by using the DYN_DO_NOT_VOID property
on the shape with the higher priority.
Just have them overlap at somne point and apply the property.
Yves
-----Oorspronkelijk bericht-----
Van: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx]Namens Ritter, Alan
Verzonden: Thursday, 21 April, 2005 15:35
Aan: icu-pcb-forum@xxxxxxxxxxxxx
Onderwerp: [PCB_FORUM] Re: DGND/AGND merge point
This is one of the classic problems...our local workaround is fine if you use
negative plane layers, and goes something like this:
The negative plane consists of two classes, one etch (call it subclass
"GND") and one anti-etch (call it "GNDSEP").
On the etch, create your shapes for GND and AGND, attach them to the respective
nets and let Allegro generate the thermal reliefs, antipads, etc., as
appropriate. Leave a 25-mil or so gap between the GND and AGND shapes.
On the anti-etch, lay down a 25-mil (or narrower if you prefer) LINE (not
CLINE) that traces the boundary between your GND and AGND shapes. We also add
a 50-mil line just inside the perimeter of the board, as well, to keep copper
planes away from the cut edge.
Now, for the trick: LEAVE A GAP in the AGND/DGND separation line. Pick the
location per your customer's requirements (usually either at the A/D converter,
or at the power connector). When you create artwork for the plane layer, make
sure that you have it set up as a NEGATIVE layer. Turn on the pads and shapes
for the etch class, and the lines for the anti-etch class. Click the "suppress
shape fill" option and generate artwork. This will generate the antipads and
thermals for pins/vias and the separation barriers.
We have used this workaround (and it IS a workaround) for quite a while. It
keeps good track of AGND/DGND connectivity but does NOT guarantee that the
separation/junction between the two is correct...you, as designer, have to
verify that by viewing the Gerber files out the far end of the process.
Yes, it's a kludge...but it works...
/s/jar (alan.ritter@xxxxxxxxxx)
http://www.mtritter.org
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?
EMAIL DISCLAIMER
Please Note: The information contained in this message may be privileged and
confidential, protected from disclosure, and/or intended only for the use of
the individual or entity named above. If the reader of this message is not the
intended recipient, or an employee or agent responsible for delivering this
message to the intended recipient, you are hereby notified that any disclosure,
distribution, copying or other dissemination of this communication is strictly
prohibited. If you received this communication in error, please immediately
reply to the sender, delete the message and destroy all copies of it.
Thank You
-----------------------------------------------------------
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:
