There are two options:
1) Leave your PCB manufacturer to design PCB stackup for you (Recommended)
- You don’t need to spend your time by designing stackup. Leave it on PCB manufacturer – they are professionals. They do it every day. Also, by doing it this way, you can work on design in parallel of handling issues with PCB stackup.
- Many times PCB manufacturer is not able to build PCB stackup designed by other company or a person outside their company. The main reason is unavailability of material used in some PCB stackups. Selection of material is the best to leave on them – they will choose stocked material.
- PCB manufacturers use different track geometry calculators and they will not guarantee track impedance if track geometry is calculated by someone else. Many times their calculated numbers and your calculated numbers will be different.
An example of email to PCB manufacturer with request for PCB stackup and track geometry
Please suggest PCB stackup and track geometry for PCB with following parameters:
– 12 Layers:
L1 – Signal
L2 – GND
L3 – Signal
L4 – Signal
L5 – GND
L6 – Powers
L7 – Powers
L8 – GND
L9 – Signal
L10 – Signal
L11 – GND
L12 – Signal
Please suggest stackup.
– Required impedances:
Single ended: 50 OHMs (L1 (Ref: L2); L3, L4 (Ref: L2, L5); L9, L10 (Ref: L8, L11); L12 (Ref: L11))
Differential: 70, 90, 100 OHMs (L1 (Ref: L2); L3, L4 (Ref: L2, L5); L9, L10 (Ref: L8, L11); L12 (Ref: L11))
Please suggest geometry for impedance controlled tracks: Track width / Gap
– Used VIAs:
Through hole VIA: 0.45mm (pad) / 0.2mm (drill),
Start layer: L1, End layer: L12
Start layer: L1, End layer: L2; 0.27mm (pad) / 0.1mm (laser drilled hole)
Start layer: L2, End layer: L3; 0.27mm (pad) / 0.1mm (laser drilled hole)
Start layer: L10, End layer: L11; 0.27mm (pad) / 0.1mm (laser drilled hole)
Start layer: L11, End layer: L12; 0.27mm (pad) / 0.1mm (laser drilled hole)
Start Layer: L3, End layer: L10; 0.45mm (pad) / 0.2mm (drill)
Minimum track: 0.1mm / Minimum gap: 0.1mm
Board thickness: approximately 1.6mm
Board size: 40x80mm
2) Design PCB stackup by yourself
Basic information about PCB stackups:
- PCB is build from three basic materials: Copper foil, Prepreg, Core
- Standard Copper foil thickness: 5um, 12um, 18um, 35um, 70um
- Standard prepreg thickness: 65um, 100um, 180um
- Standard core thickness: 0.15mm, 0.20mm, 0.36mm, 0.46mm, 0.56mm, 0.71mm, 1mm, 1.2mm, 1.5mm, 2.0mm, 2.4mm, 3.2mm. Core is supplied with copper foil on both sides. For some cores you need to add copper foil thickness (18um or 35um) to the core thickness.
PCB stackup examples
|Standard 4 Layer PCB stackup [mm]||Standard 6 Layer PCB stackup [mm]||Standard 8 Layer PCB stackup [mm]|
There are some rules how to build your stackup. Not every combination is possible. Check it out with your PCB manufacturer.
Note: If you calculate impedances for your own stackup, don’t forget about PLATING. Plating process add an additional copper (e.g. 20um) to top and bottom layer (or if you use uVIAs and buried VIAs, then also to some of the inner layers).
PCB impedance calculation and Track geometry design
Example of Microstrip (the tracks on TOP and BOTTOM layers) impedance calculation
90 Ohms Differential / 55 Ohm Single ended for:
Track width: 11mil / Copper foil 18um (0.7mil) / Track Gap 8 mil / Dielectric thickness 2x 0.1 prepreg = 0.2mm (7.8mil) / material FR-4 (dielectric constant 4.8)
PCB impedance calculator – Single ended / Differential pair
Tip: It’s easy to convert between mm and mils. Use google and look for: “10mil to mm” or “0.2mm to mil”
Please Comment, LIKE, Share, ReTweet. Thank you.
5 thoughts on “How to design PCB stackup”
Good choice of words brother Robert. “Leave it to the professionals, they do it every day.” Besides, they are the ones who were forged to do this job.
PCB 4 Layers
allow for signals to run on the inside of your board, you have the ability to
pack more components within closer tolerances allowing for a more compact
design. Multilayer boards will always be offered with an even number of layers
on the PCB. The most common and practical are boards with layers of 4, 6, or 8.
A common approach to Multilayer is to dedicate one layer to the ground plane
while another is focused on power.
Great stackup article. I also found it helpful to reference this article for more info on the pcb layers you discussed.