## PCB Design Guidelines ### PCB Footprint Design The QFN68L package dimensions of the SF32LB52X series chips are: 7 mm x 7 mm x 0.85 mm; number of pins: 68; pin pitch: 0.35 mm. Detailed dimensions are shown in Figure 5-1.

Figure 5-1 QFN68L Package Dimensions

Figure 5-2 QFN68L Package Outline

Figure 5-3 QFN68L Package PCB Pad Design Reference

### PCB Stackup Design The SF32LB52X series chips support single-sided and double-sided layouts. Components can be placed on one side, or capacitors and other components can be placed on the back side of the chip. The PCB supports a PTH through-hole design. A 4-layer PTH design is recommended, and the recommended reference stack-up structure is shown in Figure 5-4.

Figure 5-4 Reference Stack-up Structure

### General PCB Design Rules The general PCB design rules for a PTH board are shown in Figure 5-5.

Figure 5-5 General Design Rules

### PCB Trace Fanout For QFN package signal fanout, all pins are fanned out through the top layer, as shown in Figure 5-6.

Figure 5-6 Top-Layer Fanout Reference

### Clock Interface Routing The crystal must be placed inside the shielding can, with a clearance of more than 1 mm from the PCB outline. Keep it as far away as possible from components that generate significant heat, such as PA, Charge, PMU, and other circuit components. The distance should preferably be greater than 5 mm to avoid affecting the crystal frequency offset. The crystal circuit keep-out area should have a clearance greater than 0.25 mm to avoid other metals and components, as shown in Figure 5-7.

Figure 5-7 Crystal Layout

It is recommended to route the 48 MHz crystal traces on the top layer, with the length controlled within the range of 3–10 mm and the trace width 0.1 mm. Three-dimensional ground shielding is required, and the traces must be kept away from VBAT, DC/DC, and high-speed signal lines. No plane voids or copper cutouts are allowed on the top layer under the 48 MHz crystal area or on adjacent layers. Other traces are prohibited from passing through this area, as shown in Figures 5-8, 5-9, and 5-10.

Figure 5-8 48MHz Crystal Schematic

Figure 5-9 48MHz Crystal Routing Model

Figure 5-10 48MHz Crystal Routing Reference

It is recommended to route the 32.768 kHz crystal traces on the top layer, with the length controlled to ≤10 mm and a trace width of 0.1 mm. The spacing between the parallel 32K_XI/32_XO traces must be ≥0.15 mm, and three-dimensional ground shielding is required. No plane voids or copper cutouts are allowed on the top layer under the crystal area or on adjacent layers, and no other traces are allowed to pass through this area, as shown in Figures 5-11, 5-12, and 5-13.

Figure 5-11 32.768KHz Crystal Schematic

Figure 5-12 32.768KHz Crystal Routing Model

Figure 5-13 32.768KHz Crystal Routing Reference

### RF Interface Routing The RF matching circuit should be placed as close as possible to the chip side, not near the antenna side. The filter capacitor for the AVDD_BRF RF power supply should be placed as close as possible to the chip pin, and the capacitor ground pin should be connected directly to the main ground through a via. The schematic and PCB layout of the π-type network for the RF signal are shown in Figures 5-14 and 5-15, respectively.

Figure 5-14 π-Type Network and Power Circuit Schematic

Figure 5-15 π-Type Network and Power PCB Layout

It is recommended to route RF traces on the top layer to avoid vias and layer transitions that may affect RF performance. The trace width should preferably be greater than 10 mil. Three-dimensional ground shielding is required, and acute-angle and right-angle routing should be avoided. RF traces should be controlled to 50 Ω impedance, with plenty of shielding ground vias placed on both sides, as shown in Figures 5-16 and 5-17.

Figure 5-16 RF Signal Circuit Schematic

Figure 5-17 RF Signal PCB Routing Diagram

### Audio Interface Routing AVDD33_AUD is the audio power supply pin, and its filter capacitor should be placed close to the corresponding pin so that the ground pin of the filter capacitor has a solid connection to the PCB main ground. MIC_BIAS is the power output pin that supplies power to the microphone peripheral, and its corresponding filter capacitor should be placed close to the corresponding pin. Similarly, the filter capacitor for the AUD_VREF pin should also be placed close to the pin, as shown in Figures 5-18a and 5-18b.

Figure 5-18a Audio-Related Power Filtering Circuit

Figure 5-18b PCB Reference Routing for the Audio-Related Power Filtering Circuit

For the analog signal input ADCP pin, place the corresponding circuit components as close as possible to the chip pin, keep the trace length as short as possible, apply three-dimensional ground shielding, and keep it away from other strong interference signals, as shown in Figures 5-19a and 5-19b.

Figure 5-19a Analog Audio Input Schematic

Figure 5-19b Analog Audio Input PCB Design

For the analog signal output DACP/DACN pins, place the corresponding circuit components as close as possible to the chip pins. Each P/N pair must be routed as differential traces, with trace lengths kept as short as possible and parasitic capacitance less than 10 pF. Three-dimensional ground shielding is required, and the traces should be kept away from other strong interference signals, as shown in Figures 5-20a and 5-20b.

Figure 5-20a Analog Audio Output Schematic

Figure 5-20b Analog Audio Output PCB Design

### USB Interface Routing The USB traces PA35(USB DP)/PA36(USB_DN) must first pass through the ESD device pins and then go to the chip side. Ensure that the ESD device ground pins are properly connected to the main ground. The traces must be routed as differential traces with 90-ohm differential impedance control, and three-dimensional ground shielding must be applied, as shown in Figures 5-21a and 5-21b.

5-21a USB Signal Schematic

5-21b USB Signal PCB Design

Figure 5-22a is a reference diagram for the component layout of USB signals, and Figure 5-22b is the PCB routing model.

Figure 5-22a USB Signal Component Placement Reference

Figure 5-22b USB Signal Routing Model

### SDIO Interface Routing SDIO signal traces should be routed together as much as possible and should not be routed separately. The total trace length should be ≤50 mm, and the length matching within the group should be controlled to ≤6 mm. The clock signal of the SDIO interface requires three-dimensional ground shielding, and the DATA and CMD signals also require ground shielding, as shown in Figures 5-23a and 5-23b.

Figure 5-23a SDIO Interface Circuit Diagram

Figure 5-23b SDIO PCB Routing Model

### DCDC Circuit Routing The power inductor and filter capacitors of the DC-DC circuit must be placed close to the chip pins. The BUCK_LX trace should be as short and wide as possible to ensure low loop inductance for the entire DC-DC circuit. The feedback trace for the BUCK_FB pin must not be too narrow and must be greater than 0.25 mm. The ground pins of all DC-DC output filter capacitors should be connected to the main ground plane with multiple vias. Copper pouring is prohibited on the top layer in the power inductor area, and the adjacent layer must be a complete reference ground. Avoid routing other traces through the inductor area, as shown in Figures 5-24a and 5-24b.

Figure 5-24a DC-DC Key Component Circuit Diagram

Figure 5-24b DC-DC Key Component PCB Layout

### Power Supply Routing PVDD is the power input pin for the chip's built-in PMU module. The corresponding capacitor must be placed close to the pin, and the trace should be as wide as possible and must not be less than 0.4 mm, as shown in Figure 5-25.

Figure 5-25 PVDD Power Routing Diagram

The filter capacitors for pins such as AVDD33, VDDIOA, VDD_SIP, AVDD33_AUD, and AVDD_BRF should be placed close to the corresponding pins. Their trace widths must meet the input current requirements, and the traces should be as short and wide as possible to reduce power supply ripple and improve system stability. ### Other Interface Routing When a pin is configured as a GPADC signal pin, three-dimensional ground shielding is required, and it must be kept away from other interfering signals, such as the battery level circuit and temperature check circuit. ### EMI&ESD - Avoid long-distance routing on the outer layer outside the shielding can. In particular, interfering signals such as clocks and power should be routed on inner layers as much as possible and must not be routed on the outer layer. - ESD protection devices must be placed close to the corresponding connector pins. Signal traces should first pass through the ESD protection device pins to avoid signal branches that bypass the ESD protection pins. - The ground pins of ESD devices must be connected to the main ground through vias. Ensure that the ground pad traces are short and wide to reduce impedance and improve ESD device performance.