Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronic 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.

Register Log in

What Is Recomended PCB StuckUP Layers For High Spedd Design

Status
Not open for further replies.

shawndaking

Full Member level 3
Joined
Jun 20, 2001
Messages
187
Helped
12
Reputation
24
Reaction score
6
Trophy points
1,298
Activity points
1,077
I'm Looking For You'r Opinion About The Ideal PCB Stackup Layers For Multilayer High Speed Design.

i Would like To use At Least Half Of The Layers For Signals, But I Would Also Would Like To Keep Clock Layer Isolated, I also Would Preffer To Locate Voltage Plane Near To GND Layer.

I'll Apretiate You'r Contribution !
 

hwswboy

Member level 4
Joined
Jul 2, 2001
Messages
75
Helped
4
Reputation
8
Reaction score
4
Trophy points
1,288
Activity points
605
There are not simple answer.

How many layers, impedance, buried resistors.....????

You need to be more specific... but perhaps this calculator helps you
 

flatulent

Advanced Member level 5
Joined
Jul 19, 2002
Messages
4,629
Helped
489
Reputation
980
Reaction score
150
Trophy points
1,343
Location
Middle Earth
Activity points
46,689
famous company guide lines

A famous company which has the experience of boards functioning properly and passing EMI measurements the first time has these guidelines:

1. Ground and power plane layers should be symetrically spaced relative to the stack center in the stackup. For example, if the third layer in from one side is ground, the third layer in from the other side should be ground.
2. The ground planes should be stitched together around the periphery with vias spaced 0.1 or 0.05 wavelengths apart relative to the highest EMI measurement frequency.
3. Higher speed signal routes should be on a single layer between two ground planes.
4. Lower speed signals can be on two layers between power and ground planes but biased in spacing to the planes and away from each other. The lines should cross at right angles.
5. The power planes should be bypassed to ground around the edges with capacitors spaced similarly to the ground stitch vias.
 

roli

Full Member level 5
Joined
Apr 29, 2001
Messages
246
Helped
9
Reputation
20
Reaction score
9
Trophy points
1,298
Location
'SiliconWafer' Island
Activity points
1,824
What about the Layes Stack-Up / Grounding rules for "Analog Islands" buried in High-Speed Noisy Digital regions ? (e.g. - Separation of Analog Power and Ground from Digital Power and Ground, Ground Escapes, Analog Caps Decouplings, and recommended location of the eventual Galvanic connection between Analog Ground and Digital Ground)
 

flatulent

Advanced Member level 5
Joined
Jul 19, 2002
Messages
4,629
Helped
489
Reputation
980
Reaction score
150
Trophy points
1,343
Location
Middle Earth
Activity points
46,689
digital rules

As you guessed, the famous company design rules were for microwave speed digital systems. For analog additions, keep the circuits on the edge of the board away from the rest. It has its own stackup of layers. The power is applied through its own cabling back to the power supply. The only trace or plane connections to the digital part are where it interfaces to the rest of the system. This is usually a ADC. The ADC stradels the two ground plane areas which are connected by a narrow trace which is under the analog trace going to the input of the ADC.

Digital circuitry can also have islands if the system has to meed very strict EMP or other induced currents. Many companies have internal requirements more strict than CE or military ones. In this case all of the externally induced currents will flow between the edge connectors. You design the layout like a floor plan for an office. There are clear paths between the connectors with "rooms" to the side formed by slits in the ground and power planes. The circuitry is put by function/subcircuit into the rooms and only the traces to the other rooms are brought out.
 

Status
Not open for further replies.
Toggle Sidebar

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top