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

Hey Gary,

 

You may already know this but I figured it was worth saying to the
group; On positive plane layers you're plane void is based on a
clearance above the Regular pad size but on negative plane layers the
Anti-Pad is used to generate the void openings in the plane which is
normally based on the drill and can be smaller than the Regular pad.
So there could be a case where the void in the plane could be smaller on
negative planes compared to positive.  I think that is what George was
getting at.

Hope this helps,
Michael Catrambone
UTStarcom, Inc.

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Macindoe, Gary
Sent: Thursday, July 19, 2007 2:00 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: