3.1 Reference PCB Stack-Up
This section provides the reference PCB stack-up for a 4-layer design with 0.8 mm as PCB thickness. The reference design provided is based on the module design.
Note: If a different PCB stack-up with a different PCB thickness
is required to meet the end design constraints, be sure to meet the required
controlled impedance for the RF trace by maintaining the same height between layer-1
(Top layer) and layer-2 (Inner layer 1) to maintain the same trace width and spacing
requirements.
Following the guidelines below is recommended for achieving the best performance:
- Top layer – Used for RF traces and signal routing
- Inner layer 1 – Used for ground plane. Ensure this ground plane is not broken by any signal traces. This ground layer must be selected immediately below the layer containing the RF traces routed from the PIC32CX1012BZ24032 device to the antenna.
- Inner layer 2 – Used for routing power traces and signal traces. Instead of using the entire plane, power traces must be routed as thick trace sufficient (around 20 mil) to minimize IR drop. The remaining part of the plane must be filled with ground polygon pour.
- Bottom layer – Used for power and signal traces
| Layer Name | Layer Type | Stack-Up Details | |||
|---|---|---|---|---|---|
| Materials (um) | Finished (um) | Tolerance (um) | DK | ||
| S/M | Solder mask | — | 10 | — | — |
| TOP signal | Copper(T oz+plating) | 12 | 35.00 | ±15 | — |
| — | 2116 RC55 | 120 | 220.00 | ±22 | 4.3 |
| — | 2116 RC55 | 120 | |||
| L2 gnd | Copper(1 oz) | 35 | 30.00 | ±10 | — |
| — | Core 130 mm | 130 | 130.00 | ±10 | 4.3 |
| — | Copper(1 oz) | 35 | 30.00 | ±10 | — |
| — | 2116 RC55 | 120 | 220.00 | ±22 | 4.3 |
| — | 2116 RC55 | 120 | |||
| Bottom signal | Copper(T oz+plating) | 12 | 35.00 | ±15 | — |
| S/M | Solder mask | — | 10 | — | — |
| Laminated thickness | — | — | 700 | ±10% | — |
| Overall thickness | — | — | 800 | ±100 | — |