Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Layer stackup for a 6 layer board

Status
Not open for further replies.

TommyR

Newbie level 4
Joined
May 1, 2015
Messages
5
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
30
I always felt it was necessary to place the gnd and pwr in the middle of the stackup.
For some reason an engineer said that isn't necessary now and he wanted them placed elsewhere.

Do users still do it the old way?
 

ads-ee

Super Moderator
Staff member
Joined
Sep 10, 2013
Messages
7,906
Helped
1,821
Reputation
3,652
Reaction score
1,799
Trophy points
1,393
Location
USA
Activity points
59,784
Since when has that changed? The adjacent pwr-grn plane stackup is good for high frequency bypass of high speed digital designs.

Either this isn't a digital board (RF guys tend to do things differently) or the engineer needs to read something like
 

TommyR

Newbie level 4
Joined
May 1, 2015
Messages
5
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
30
Well that's good to hear. I was told a long time ago doing it that way effectively created a big "capacitor".
 

ads-ee

Super Moderator
Staff member
Joined
Sep 10, 2013
Messages
7,906
Helped
1,821
Reputation
3,652
Reaction score
1,799
Trophy points
1,393
Location
USA
Activity points
59,784
Well that's good to hear. I was told a long time ago doing it that way effectively created a big "capacitor".

Well I would consider it more of a distributed high frequency capacitor, big would imply something with a large value of capacitance. ;-)
 

TommyR

Newbie level 4
Joined
May 1, 2015
Messages
5
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
30
Point well taken.
 

andre_luis

Super Moderator
Staff member
Joined
Nov 7, 2006
Messages
9,377
Helped
1,171
Reputation
2,361
Reaction score
1,164
Trophy points
1,403
Location
Brazil
Activity points
54,593
At page 10 of the document bellow, there is a table showing the expected performance of some stacking variants:

**broken link removed**
 

D.A.(Tony)Stewart

Advanced Member level 5
Joined
Sep 26, 2007
Messages
7,067
Helped
1,721
Reputation
3,441
Reaction score
1,725
Trophy points
1,413
Location
Richmond Hill, ON, Canada
Activity points
51,856
For large digital TTL design's it was common to use one decoupling cap on each IC. Then with 50 IC's it was preferred to use a thin dielectric between the +5V and Gnd for a distributed decoupling design, where the smallest reliable gap was chosen to give the largest capacitance per sq cm. But TTL had higher impedance for Voh, and lower impedance than CMOS for Vol, so conducted noise decoupling was a little more demanding than CMOS. With CMOS, the layout of high step current into capacitive loads can be important to isolate but low ESR bulk caps can do the job with a few well placed ceramic caps per small group of ICs.

So, no need to keep Vcc/Vdd layers together, unless there are special reasons, then you would use a very thin high quality pre-preg or solid laminate to avoid shorts, much thinner than standard layers. Imagine that a track width is equal to the dielectric gap is around 50 Ohms, and CMOS drivers are as low as 25 Ohms, so if you wanted to decouple the conducted noise, the dielectric gap of the pwr/gnd layers would have to be a very small fraction of the width of the IC to get under say 0.1 Ohm.
 

TommyR

Newbie level 4
Joined
May 1, 2015
Messages
5
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
30
I just printed it and am going to study it.
Thank you for your help -- it's appreciated.
 

marce

Advanced Member level 5
Joined
Feb 23, 2010
Messages
2,020
Helped
623
Reputation
1,246
Reaction score
611
Trophy points
1,393
Location
UNITED KINGDOM
Activity points
13,985
Don't forget loop area, if they are next to each other you do get some capacitance, but another advantage is similar loop areas down to the planes...
Re-read that Ti data sheet, interesting as it mentions 90 degree corners, which don't actually cause any problems till you get to GHz designs.
Look at other information as well from the likes of Henry Ott, Rlaph Morrison, Howard Johnson, Eric Bogatin etc. that is an old documents now and there is a lot around regarding this and since 2006 rise times have got faster, plus there are numerous variations on a theme... you may need to split the power layers to provide return layers for signals or to provide some capacitive screening between signal layers. The choices are endless and will be design dependant, though centre placement is a well tested basic.
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top