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

Title: Message
Hi all,

I fully agree with George that negative planes give better results than positive ones in terms of Swiss cheese effect under BGAs. I also have to admit that  Michael 's way to use planes in my opinion is very effective. In general both positive dynamic shapes and negative planes work good and give almost the same results. A differences are seen in special cases. Quite recently I wanted to achieve results possible with negative planes using positive dynamic shapes and I found a dangerous trap described in my mail "Via to shape clearance" from 27-04-2007. As far as I know at present only using negative planes could in a safe way solve such problem just because antipads are defined from hole edges. Other possibility for such problem would be to create very wide split moats to guarantee that any via placed in the moat area is isolated from either island on the split plane.

Maybe somebody can solve such problem without using negative planes, it would be an interesting lesson.

cheers,
Robert

Michael Catrambone wrote:

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
Å 503-627-5272 (voice)     Æ 503-627-5587 (fax)
http://www.tektronix.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: