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

Hi Robert,

I am wrong a lot of the time... but in my experience, the Swiss cheese 
effect can be avoided using a constraint exception area under the BGA if 
you have the Performance or Expert level tool.  If you are limited to the 
Studio tool you can use overlapping but separate planes with different 
clearance parameters to achieve the different clearances from one area to 
another.  Only thing with overlapping planes is that crossing voids must 
be avoided.

Regarding the Via to shape problem... maybe I am under stating the problem 
you outlined but cannot the Via to shape clearance be corrected by 
reshaping the plane/gap to encompass/avoid the via?

(This is not a promo for positive planes... just hoping to help)

Regards,
Ed

In search of truth... grasping for sanity




Robert Szumowicz <robert.szumowicz@xxxxxxxxxx> 
Sent by: icu-pcb-forum-bounce@xxxxxxxxxxxxx
07/20/2007 05:35 AM
Please respond to
icu-pcb-forum@xxxxxxxxxxxxx


To
icu-pcb-forum@xxxxxxxxxxxxx
cc

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






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.

GIF image

GIF image

Other related posts: