Recommended PCB Design Guideline for QSFP+/zQSFP/QSFP28 Channels
The yellow portions indicate GND2/GND4 cutout dimensions under the connector pads on the 1st and 2nd reference planes, respectively.
- Rectangular (W x H) cutout on the GN02 2 layer (recommended for data rates up to 17 Gbps) under the QSFP+ pads. For data rates up to 28 Gbps, add one additional GND layer cutout (GND04). W = 100 mil, H = 210 mil.
- Signal and GND vias, finished drill diameter = 10 mil, Via pad diameter = 20 mil
- All signal vias are back-drilled
- Each signal via must have one single GND via
- If the stack-up height is less than 1:12, you can also use an 8-mil finished via drill and an 18 mil via pad instead.
- P (signal-to-signal via pitch) = 40 mil
- Signal anti-pads: T = 90 mil, D = 45 mil
- G (signal-to-GND via pitch) = 30 mil
- 95 Ω differential PCB routing
Intel recommends that you have both the signal via and GND via located close enough to the connectors' signal and GND pads, respectively, to avoid cavity resonance at higher frequencies.
Did you find the information on this page useful?