Reference circuitry

To ensure good RF performance when designing PCBs, it is highly recommended to use the PCB layouts and component values provided by Nordic Semiconductor.

Documentation for the different package reference circuits, including Altium Designer files, PCB layout files, and PCB production files can be downloaded from the product page for the nRF52805 on www.nordicsemi.com.

Schematic CAAA WLCSP with internal LDO regulator setup

In addition to the schematic, the bill of material (BOM) is also provided.

Figure 1. CAAA WLCSP with internal LDO regulator setup

Schematic: CAAA WLCSP with internal LDO regulator setup

Note: For PCB reference layouts, see the product page for the nRF52805 on www.nordicsemi.com.

Table 1. Bill of material for CAAA WLCSP with internal LDO regulator setup
Designator	Value	Description	Footprint
C1, C2, C9, C10	12 pF	Capacitor, NP0, ±2 %	0201
C3	1.2 pF	Capacitor, NP0, ±5 %	0201
C4, C5	100 nF	Capacitor, X5R, ±10 %	0201
C6	100 pF	Capacitor, NP0, ±2 %	0201
C7	2.2 µF	Capacitor, X5R, ±20 %	0402
C8	1.0 µF	Capacitor, X5R, ±5 %	0402
L1	2.2 nH	High frequency chip inductor ±5 %	0201
L2	3.3 nH	High frequency chip inductor ±5 %	0201
U1	nRF52805-CAAA	Multiprotocol Bluetooth® low energy, and 2.4 GHz proprietary system-on-chip	WLCSP-28
X1	32 MHz	XTAL SMD 2016, 32 MHz, Cl = 8 pF, Total Tol: ±40 ppm	XTAL_2016
X2	32.768 kHz	XTAL SMD 2012, 32.768 kHz, Cl = 9 pF, Total Tol: ±50 ppm	XTAL_2012

Schematic CAAA WLCSP with DC/DC regulator setup

In addition to the schematic, the bill of material (BOM) is also provided.

Figure 2. CAAA WLCSP with DC/DC regulator setup

Schematic: CAAA WLCSP with DC/DC regulator setup

Note: For PCB reference layouts, see the product page for the nRF52805 on www.nordicsemi.com.

Table 2. Bill of material for CAAA WLCSP with DC/DC regulator setup
Designator	Value	Description	Footprint
C1, C2, C9, C10	12 pF	Capacitor, NP0, ±2 %	0201
C3	1.2 pF	Capacitor, NP0, ±5 %	0201
C4, C5	100 nF	Capacitor, X5R, ±10 %	0201
C6	100 pF	Capacitor, NP0, ±2 %	0201
C7	2.2 µF	Capacitor, X5R, ±10 %	0402
C8	1.0 µF	Capacitor, X5R, ±5 %	0402
L1	2.2 nH	High frequency chip inductor ±5 %	0201
L2	3.3 nH	High frequency chip inductor ±5 %	0201
L3	10 µH	Chip inductor, IDC,min = 50 mA, ±20 %	0603
L4	15 nH	High frequency chip inductor ±10 %	0402
U1	nRF52805-CAAA	Multiprotocol Bluetooth® low energy, and 2.4 GHz proprietary system-on-chip	WLCSP-28
X1	32 MHz	XTAL SMD 2016, 32 MHz, Cl = 8 pF, Total Tol: ±40 ppm	XTAL_2016
X2	32.768 kHz	XTAL SMD 2012, 32.768 kHz, Cl = 9 pF, Total Tol: ±50 ppm	XTAL_2012

PCB guidelines

A well designed PCB is necessary to achieve good RF performance. Poor layout can lead to loss in performance or functionality.

A qualified RF layout for the IC and its surrounding components, including matching networks, can be downloaded from www.nordicsemi.com.

To ensure optimal performance it is essential that you follow the schematics and layout references closely. Especially in the case of the antenna matching circuitry (components between device pin ANT and the antenna), any changes to the layout can change the behavior, resulting in degradation of RF performance or a need to change component values. All reference circuits are designed for use with a 50 Ω single-ended antenna.

A PCB with a minimum of two layers, including a ground plane, is recommended for optimal performance. The distance between the ground plane and the top layer should be less than or equal to 0.8 mm. On PCBs with more than two layers, put a keep-out area on the inner layers directly below the antenna matching circuitry (components between device pin ANT and the antenna) to reduce the stray capacitances that influence RF performance.

A matching network is needed between the RF pin ANT and the antenna, to match the antenna impedance (normally 50 Ω) to the optimum RF load impedance for the chip. For optimum performance, the impedance for the matching network should be set as described in the recommended package reference circuitry in Reference circuitry.

The DC supply voltage should be decoupled as close as possible to the VDD pins with high performance RF capacitors. See the schematics for recommended decoupling capacitor values. The supply voltage for the chip should be filtered and routed separately from the supply voltages of any digital circuitry.

Long power supply lines on the PCB should be avoided. All device grounds, VDD connections, and VDD bypass capacitors must be connected as close as possible to the IC. For a PCB with a topside RF ground plane, the VSS pins should be connected directly to the ground plane. For a PCB with a bottom ground plane, the best technique is to have via holes as close as possible to the VSS pads. A minimum of one via hole should be used for each VSS pin.

Fast switching digital signals should not be routed close to the crystal or the power supply lines. Capacitive loading of fast switching digital output lines should be minimized in order to avoid radio interference.

Note: The distance between the ground plane and the top layer should be less than or equal to 0.8 mm. If this design rule is not followed, Radio parameters may not meet specification.

PCB layout example

The two-layer PCB layout shown in the following figures is a reference layout for the WLCSP package with internal LDO setup.

For all available reference layouts, see the product page for the nRF52805 on www.nordicsemi.com.

Figure 3. Top silk layer

Figure 4. Top layer

Figure 5. Bottom layer

Important: No components in bottom layer.

PMIC support

The nRF52 Series is comprehensively supported by Nordic Semiconductor's own range of PMICs (Power Management Integrated Circuits). These PMICs are meticulously designed to enhance the performance and efficiency of the nRF52 Series devices. This integration ensures the longest battery life and the highest reliability for the end application. The synergy between the nRF52 Series and the Nordic PMICs highlights Nordic Semiconductor's commitment to providing a complete and cohesive solution for their customers' needs in wireless technology applications.