[PCB_FORUM] Re: DGND/AGND merge point
- From: "Ritter, Alan" <Alan.Ritter@xxxxxxxxxx>
- To: icu-pcb-forum@xxxxxxxxxxxxx
- Date: Thu, 21 Apr 2005 09:34:47 -0400
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
-----------------------------------------------------------
Other related posts:
