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

Jerry,

 

Yeah, that's pretty much how I have it set up.

My default Shape to Pin is 5 mil, and that's at least the smallest
spacing in any of my padstacks.

 

Boy, shapes sure are loads of fun!

 

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 Schwartz,
Jerome
Sent: Thursday, July 19, 2007 12:16 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Planes: Negative vs. Positive?

 

Gary,

 

    Regardless of  using static or dynamic planes you can control how
the voids are made.

I define mine in the padstack. If the shape to pad DRC is smaller than
the antipad you will get a DRC.

I make my shape to pad DRC the same as my smallest antipad definition
therefore eliminating DRC's

and maintaining larger spacing's on my other padstack definitions. This
way I can use dynamic planes

and vary my clearances by padstack rather than having one clearance for
all pads. Different drills

sizes can have different GD&T criteria.

 

Jerry 

 

 

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Austin Franklin
Sent: Thursday, July 19, 2007 2:06 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Planes: Negative vs. Positive?

Hi Gary,

 

No, I'm not kidding.  I wasn't aware that the two were determined by
entirely different criteria.  To me, that is not intuitive, and
certainly isn't the same with other tools I've used.  IMO, they both
should give the same results ultimately, or at least should be able to
be configured so that they do.  But, thanks for the explanation.  I use
positive planes now, I used negatives in the past, but in other tools I
used them in, they didn't DRC correctly.

 

Regards,

 

Austin

 

        -----Original Message-----
        From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx]On Behalf Of Macindoe, Gary
        Sent: Thursday, July 19, 2007 1:52 PM
        To: icu-pcb-forum@xxxxxxxxxxxxx
        Subject: [PCB_FORUM] Re: Planes: Negative vs. Positive?

        You're kidding, right Austin?

         

        With negative planes, the clearance is determined by the
padstack and with positive planes, the clearance is determined by the
shape parameters (changeable on a shape by shape basis).

         

         

        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 Austin Franklin
        Sent: Thursday, July 19, 2007 11:20 AM
        To: icu-pcb-forum@xxxxxxxxxxxxx
        Subject: [PCB_FORUM] Re: Planes: Negative vs. Positive?

         

        Hi George,

         

        Why would the openings around pins be any different between
positive and negative planes?

         

        Regards,

         

        Austin

                -----Original Message-----
                From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx]On Behalf Of
george.h.patrick@xxxxxxxxxxxxxx
                Sent: Thursday, July 19, 2007 12:58 PM
                To: icu-pcb-forum@xxxxxxxxxxxxx
                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: