[PCB_FORUM] Re: Planes: Negative vs. Positive?

Ed:
 
The positive plane clearance is going to be the DRC values from the pad, where 
negative thermal or clearance flashes are normally calculated from the drill 
size.  We looked at this extensively when we were deciding whether to to to 
positives, and found the swiss cheese effect on the positive planes under BGAs 
was much more noticeable on the gerbers than was the equivalent negative planes 
using thermal and clearance flashes.  I don't have the graphics available, nor 
do I have time to replicate them right now, maybe I will do this when I have 
more time, since this subject comes up every six months or so.  
 
For now, I am going to put this into the "Religious War" category, along with 
90° traces, vi or emacs,  and Windows/Linux/Mac.  We prefer negative planes and 
have no problem with them, others prefer positive planes.
 
It is moot with us anyway.  Until Cadence decides to allow us to define a 
thermal pad shape with a void in it so we can keep our SHF/EHF analog signals 
discontinuity free when we transition from the outside world to the board 
world,  we have to stay with negative planes and old-style flashes that could 
be defined with lines.
 
Until I can show y'all why it's better, I ain't going to be drawn into it again 
:)
 
-- 
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 Ed Caldwell
Sent: Thursday, July 19, 2007 10:07
To: icu-pcb-forum@xxxxxxxxxxxxx
Cc: icu-pcb-forum@xxxxxxxxxxxxx; icu-pcb-forum-bounce@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Planes: Negative vs. Positive?



Hi George, 

I may have misunderstood your statement... but doesn't the opening from pin to 
positive plane follow the DRC settings (or exception clearances)?  And doesn't 
the opening in a negative plane ignore the DRC settings and simply follow the 
anti-pad? 

Respectfully! 
Ed 

Ed Caldwell
PCB Designer
USA 678-473-8707
mailto:ed.caldwell@xxxxxxxxxx
EDS http://www.eds-pcb.com




<george.h.patrick@xxxxxxxxxxxxxx> 
Sent by: icu-pcb-forum-bounce@xxxxxxxxxxxxx 


07/19/2007 12:58 PM 


Please respond to
icu-pcb-forum@xxxxxxxxxxxxx



To
<icu-pcb-forum@xxxxxxxxxxxxx> 

cc

Subject
[PCB_FORUM] Re: Planes: Negative vs. Positive?

        




  
Positive plane layers have a much larger opening around pins.  This is fine if 
you are doing low to medium speed boards (roughly < 200 MHz clock speed), but 
on high-speed designs the impedance discontinuities created by the huge opening 
around the pins are significantly greater on a positive plane than on a 
negative plane. 
  
We use negative planes for this reason, and we always use Valor to check our 
artworks to make sure we haven't shot ourselves in the foot :) 
  
YMMV 
  
-- 
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 Bob McCreight
Sent: Thursday, July 19, 2007 06:51
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Planes: Negative vs. Positive?

The design team I work with is split one which to use, negative or  positive 
planes.
What are the pros and cons of each? What do most people prefer to  work with?
We are currently using 15.5.1 but evaluating 16.x for possible future  
migration.
  
 Thanks for your feedback.
  
 Bob McCreight, C.I.D.

Other related posts: