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.

PCB Stack-Up for 4-Layer Boards

Status
Not open for further replies.

checkmate

Advanced Member level 3
Joined
Feb 25, 2004
Messages
833
Helped
178
Reputation
356
Reaction score
125
Trophy points
1,323
Location
Toilet Seat
Activity points
7,815
4 layer pcb stack up

I've read recommended stack-up configurations, mostly using S-G-P-S configurations. There are some which use the more unconventional S-P-G-S stack-up, the reason being components have taken up much of the routing space on the toplayer.

Am I right to say that the ground plane should be closest to the signal plane with a higher routing density?

Another question unrelated to stack-ups. Given the choice, is it better to "snake" a route through IC pads, or switch layers and route through another plane? Is there a general guideline on which option to choose?
 

House_Cat

Advanced Member level 4
Joined
Feb 21, 2002
Messages
1,371
Helped
406
Reputation
812
Reaction score
98
Trophy points
1,328
Location
USA
Activity points
16,422
4 layer pcb stackup

The placement of planes is determined by which arrangement will give you the shortest return path for the signal. You have remember that a signal path is not one sided - it is a loop. In general, the smaller the signal loop, the less crosstalk and noise coupling there will be.

You are correct that, in general, placing a continuous ground plane closest to the more dense signal routing layer will provide the best oveall results. In a properly bypassed board, the power plane can also act as a return layer - but the ground plane is generally the preferred return layer.

Recalling what I said in the first paragraph, the best signal routing is the most direct path - including the most direct return path. Routing through IC pins often gives the most direct signal path - provided the return path (on a plane) is free to follow directly under the signal trace. This is because the path of least inductance for the signal is for the return current to flow on the copper layer directly under the signal trace. If, for some reason, the ground plane cannot be continuous under the signal trace, then the signal trace should be routed such that it has the most direct path over the continuous ground copper. That way, the return current doesn't create a loop through the return path(s) of other signals. Such a loop acts as a coupler from one signal path to another and causes what we call 'noise'.

So... a short answer is - yes, the ground next to the bottom layer for your example seems to be the best choice, and routing though the IC pins would probably be the best choice. There is no rule of thumb - each routing case has to be analyzed for the best solution.

There is an advanced discussion of signal return paths in a presentation at:
https://www.national.com/appinfo/adc/files/controlling_noise.pdf
 

    checkmate

    Points: 2
    Helpful Answer Positive Rating

jdhar

Full Member level 5
Joined
Aug 16, 2004
Messages
258
Helped
16
Reputation
32
Reaction score
2
Trophy points
1,298
Activity points
2,753
pcb stack 4 layer

I think it would depend on what is on the layer also.. for eg, if you have a clock signal, you would want that on the layer closest to GND, correct?
 

House_Cat

Advanced Member level 4
Joined
Feb 21, 2002
Messages
1,371
Helped
406
Reputation
812
Reaction score
98
Trophy points
1,328
Location
USA
Activity points
16,422
4-layer pcb stackup

I think it would depend on what is on the layer also.. for eg, if you have a clock signal, you would want that on the layer closest to GND, correct?

In general, that would be correct. It does depend on the type of clock generator in use, and which edge of the clock is used. You are correct that a rule of thumb for a hobby project could be to put the higher speed signals adjacent to ground. In more advanced applications, each signal return has to be considered individually with regard to source and load. In some high frequency cases, neither plane would be preferrable over a separate return trace, or perhaps a coplanar waveguide structure with the plane voided under the waveguide.

So.. the short answer is - it depends. For general hobby use, ground plane is good. For more advanced applications, there may be a better way to return the signal.
 

tux

Member level 4
Joined
Sep 6, 2005
Messages
71
Helped
5
Reputation
10
Reaction score
3
Trophy points
1,288
Activity points
1,832
4 layer pcb stack up structure

best layerstacking is
Signal 1
GND 2
Power 3
Signal 4

u can swap GND/Power depending upon the critical signal routing and on which area more component placed
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top