[PCB_FORUM] Re: nets shorted to gnd plane

Hi All,
For the most part I agree with George's response... that loose nut part
sounds familiar but I wont admit to it.... :-) We run valor on every board
and it will find most shorts that allegro wont. Things like someone
accidentally routing on a negative plane. Allegro sees this as connected but
obviously in the gerber you will get a void rather than a trace this way. Or
perhaps the previous designer shorted two shapes together with a shape or
line on a non-etch layer so as to avoid drc's... and the new designer
doesn't realize this and leaves the artwork control as is....  this would
again have a similar result where allegro would not see the problem but
valor (or other cam tool or ipc356 netlist compare) would. I also agree that
valor does throw a lot of false positives out there but I would rather
examine a few ( or not so few) false positives than miss a "false negative'.
:-) There is nothing more irksome than a tight timeline board put "on hold"
for a simple error that could have been caught with a quick IPC netlist
compare... 
Thanks,
Dharma
 

KAW/USA Ltd. 
39 Simon Street, #4 
Nashua, NH 03060 
603-886-8711 x212 
603-881-8763 fax 

Confidentiality Notice: This email and any accompanying documents contain
information that is confidential, privileged or exempt from disclosure under
applicable law and is intended for the exclusive use of the addressee. This
information is private and protected by law. If you are not the intended
recipient, or have received this email in error, you are hereby notified
that any disclosure, copying, distribution or use of the contents of this
document in any manner is strictly prohibited.

 

  _____  

From: george.h.patrick@xxxxxxxxxxxxx [mailto:george.h.patrick@xxxxxxxxxxxxx]

Sent: Monday, July 20, 2009 7:42 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: nets shorted to gnd plane


 
Oh, geeezzzz....  Next thing you know, the "Use positive planes" crowd will
be rolling out, warning everyone that them newfangled negative planes just
don't work  :)  If you don't use a feature you are never going to work the
bugs out of your process.
 
In 12+ years working with RS274X, I have never seen a short in the board
that wasn't caused by a loose nut on the keyboard (often the one I see in
the mirror).  Look carefully and I'll bet you find a bad thermal size,
vector based pad behavior turned off, or one of the things the others were
talking about.
 
While we are on it, beware of Valor.  It sometimes gives you false shorts
and brokens (usually brokens) when you run the netlist analyzer.  When you
dig in and really look at them, you find they are bogus or (again) loose nut
on the keyboard stuff (damn, forgot to set those drill depths again).  This
happens much more with the direct extract from Allegro, much less often when
importing gerbers.
 
-- 
George Patrick
Tektronix, Inc.
Central Engineering, EDS Applications Support
P.O. Box 500, M/S 39-512
Beaverton, OR 97077-0001
* 503-627-5272 (voice)     * 503-627-5587 (fax) <http://www.tektronix.com/> 
http://www.tektronix.com     <http://www.pcb-designer.com/>
http://www.pcb-designer.com
 
"Off-Grid and Proud of it!"

-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Dale Rasmusen
Sent: Monday, July 20, 2009 16:17
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: nets shorted to gnd plane



Hi Sam,

 

We have had problems in the past with 274X formats where they will have nets
shorted to planes.  You won't see the short in Allegro, but you can
definitely view it in a gerber viewer and it is very random.  We currently
use the 274D format and that works just fine, we just don't have the
embedded apertures.  It is no big thing to the board house, they will use
the photoplot.log that is generated for apertures.  

 

Dale Rasmusen

CAD Manager

TEKNOVUS


  _____

Other related posts: