Continue to Site

Welcome to

Welcome to our site! 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.

What Is Recomended PCB StuckUP Layers For High Spedd Design

Not open for further replies.


Full Member level 3
Jun 20, 2001
Reaction score
Trophy points
Activity points
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 !

There are not simple answer.

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

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

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.

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)

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.

Not open for further replies.

Part and Inventory Search

Welcome to