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

 

Ed,



You are right on.  When you create a positive plane, it follows the
Global Parameters (Shape -> Global Dynamic Params...).

 

On a shape by shape basis, you can then edit each shape's parameters,
creating a smaller or larger clearance around thru pins, SMD pins, vias
etc., larger or smaller thermal connects etc. (Shape -> Select Shape or
Void, RMB on highlighted shape to Parameters...).

 

I still use negative planes, as our padstacks have been proven to work
just fine.  I read the gerbers into an Allegro database for checking.

Positive planes use to be a real pain (do you remember "problem
points"?), and create so large gerber files that the fab houses would
complain.

I think they are ok with them now, but I still prefer negative.

 

Gary

  

Gary E. MacIndoe
PCB Design Engineer
Fort Collins, Colorado

amd.com

gary.macindoe@xxxxxxx

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Ed Caldwell
Sent: Thursday, July 19, 2007 11:07 AM
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.

GIF image

Other related posts: