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

Austin,

 

Yes, positive planes can have larger, same or smaller clears than what a
negative plane will use from the padstack.

Also, on either positive or negative, you can manually void larger any
thru pin or via individually.

 

Have 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 Austin Franklin
Sent: Thursday, July 19, 2007 1:18 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Planes: Negative vs. Positive?

 

Hi Gary,

 

No problem.  Long time PADS, shorter time Allegro user (about four
years?).  Long time ago...long time SciCards user.  Long time high speed
digital designer.

 

Am I right that positive planes can also have a larger, same or even
smaller opening than negative planes, depending on how you set it up?

 

This is great info, at least for me, thanks!  Sometimes the subtleties
of things like this across different tools escape me until I bump my
head.

 

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 3:00 PM
        To: icu-pcb-forum@xxxxxxxxxxxxx
        Subject: [PCB_FORUM] Re: Planes: Negative vs. Positive?

        Hey Austin,

         

        Sorry, I guess I got the impression that you were also a long
time Allegro user.

         

        George mistakenly said "Positive plane layers have a much larger
opening around pins."

         

        With positive planes, when the shape is created, all clearances,
thermal ties and more is determined by your setup in the Global Dynamic
Shape Parameters form.  After the shape is created, you can change all
of this for each shape separately with the shapes individual Dynamic
Shape Instance Parameters form.

         

        Starting to make sense yet?

         

        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 Austin Franklin
        Sent: Thursday, July 19, 2007 12:15 PM
        To: icu-pcb-forum@xxxxxxxxxxxxx
        Subject: [PCB_FORUM] Re: Planes: Negative vs. Positive?

         

        Hi Gary,

         

        I understand why they *could* be different, but...given your
explanation, and more to my confusion, your explanation doesn't say why
positive planes would *always* (which is what was said) have a larger
opening.  They could be configured to be smaller couldn't they?  It's
all in how you set it up?

         

        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: