NXP Semiconductors QN9090 User manual

JN-RM-2079
QN9090 module development reference manual
Rev. 1.0 —17 Jan 2020
Reference manual
Document information
Info
Content
Keywords
QN9090, module
Abstract
Reference Manual for QN9090 modules and platform design.

NXP Semiconductors
JN-RM-2079
QN9090 module development reference manual
JN-RM-2079
All information provided in this document is subject to legal disclaimers.
© NXP Semiconductors N.V. 2020. All rights reserved.
Reference manual
Rev. 1.0 —17 Jan 2020
2 of 31
Contact information
For more information, please visit: http://www.nxp.com
Revision history
Rev
Date
Description
1.0
20200117
Creation

NXP Semiconductors
JN-RM-2079
QN9090 module development reference manual
JN-RM-2079
All information provided in this document is subject to legal disclaimers.
© NXP Semiconductors N.V. 2020. All rights reserved.
Reference manual
Rev. 1.0 —17 Jan 2020
3 of 31
1. Introduction
This manual describes the hardware for the reference designs for modules based around
the NXP QN9090 wireless microcontroller. The NXP QN9090 modules are small, low-
power and cost-effective evaluation and development board or application prototyping
and demonstration of the QN9090 device.
The QN9090 is an ultra-low-power, highly integrated single-chip device that enables
Standard Bluetooth Low Energy RF connectivity for portable, extremely low-power
embedded systems.
The QN9090 SoC integrates a radio transceiver operating in the 2.4 GHz ISM band
supporting BLE Radio, an ARM Cortex-M4 processor, up to 640 kB flash,152 kB SRAM
and 128 kB ROM, BLE Link layer processing hardware and peripherals optimized to
meet the requirements of the target applications.
The design considerations presented in this manual are equally valid for bespoke
solutions where the QN9090 device is placed directly onto the product PCB.
Three modules models are available:
•QN9090-001-M10
•QN9090-001-M13
The models available are described in Table 1.
In order to complete a successful PCB design by your own the hardware guidelines
described in this reference manual must be followed as strictly as possible. Further
information on the QN9090 characteristics are available in the “QN9090 Bluetooth Low
Energy 5.0 Wireless Microcontroller” datasheet.
The QN9090-001-M10 module has been fitted to a mezzanine board (OM15077) for use
on the QN9090 evaluation kits. The module is known as QN9090-001-T10.
1.1 Audience
This guide is intended for systems designers
1.2 Regulatory approvals
The QN9090-001-M10 and M13 are compliant with:
•RED 2014/53/EU
•CFR 47 FCC part 15

NXP Semiconductors
JN-RM-2079
QN9090 module development reference manual
JN-RM-2079
All information provided in this document is subject to legal disclaimers.
© NXP Semiconductors N.V. 2020. All rights reserved.
Reference manual
Rev. 1.0 —17 Jan 2020
4 of 31
2. Reference Design
The reference design package includes the following information for each module
variant:
•Reference manual: JN-RM-2079
•Schematics
•Layout
•Bill-of-Materials
Full design databases including schematics and layout source files are available on
request.
The following table provides a summary of the QN9090 Module Reference Design that is
available from the Wireless Connectivity area of the NXP web site.
Table 1. Modules references
Part number
Description
Content
Reference
Manual
JN-RD-6058
QN9090
Module
Reference
Design
Package
OM15069
Standard Power
PCB Antenna
QN9090-001-M10
JN-RM-2079
OM15069
Standard Power
Fl connector
QN9090-001-M13
Note: These reference designs are approved for the operating temperature range of
−40 ºC to +125 ºC.

NXP Semiconductors
JN-RM-2079
QN9090 module development reference manual
JN-RM-2079
All information provided in this document is subject to legal disclaimers.
© NXP Semiconductors N.V. 2020. All rights reserved.
Reference manual
Rev. 1.0 —17 Jan 2020
5 of 31
3. Block diagram
Fig 1. QN9090-001-M10 & M13 block diagrams
4. Design considerations
To have successful wireless hardware development, the proper device footprint, RF
layout, circuit matching, antenna design, and RF measurement capability are essential.
RF circuit design, layout, and antenna design are specialties requiring investment in tools
and experience. With available hardware reference designs from NXP, RF design
considerations, and the guidelines contained in this application note, hardware engineers
can successfully design BLE radio boards with good performance levels. The following
figures show the QN9090 M10 & M13 reference modules. They contain the QN9090
device and all necessary I/O connections.
QN9090
Matching
µ
Fl
connector
QN9090-001-M10
QN9090
Matching
Printed
antenna
QN9090-001-M13

NXP Semiconductors
JN-RM-2079
QN9090 module development reference manual
JN-RM-2079
All information provided in this document is subject to legal disclaimers.
© NXP Semiconductors N.V. 2020. All rights reserved.
Reference manual
Rev. 1.0 —17 Jan 2020
6 of 31
Fig 2. QN9090-001-M10 & M13
The device footprint and layout are critical as the RF performance is affected by the
design implementation. For these reasons, use of the NXP recommended RF hardware
reference designs are important for successful board performance. Additionally, the
reference platforms have been optimized for radio performance. Even small changes in
the location of components can mistune the circuit. If the recommended footprint and
design are followed exactly in the RF region of the board, sensitivity, output power,
harmonic and spurious radiation, and range will have a high likelihood of first-time
success.
The following subsections describe important considerations when implementing a
wireless hardware design starting with the device footprint, PCB stack-up, RF circuit
implementation, and antenna selection. The following figure shows an example of a
typical layout with the critical RF section which must be copied exactly for optimal radio
performance. The less critical layout area can be modified without reducing radio
performance.
NOTE:
Exact dimensions are not given in this document, but can be found in the manufacturing
files for the QN9090 modules
4.1 QN9090 device footprint
The performance of the wireless link is largely influenced by the device’s footprint. As a
result, a great deal of care has been put into creating a footprint so that receiver
sensitivity and output power are optimized to enable board matching and minimal
component count. NXP highly recommends copying the die flag exactly as it is shown in

NXP Semiconductors
JN-RM-2079
QN9090 module development reference manual
JN-RM-2079
All information provided in this document is subject to legal disclaimers.
© NXP Semiconductors N.V. 2020. All rights reserved.
Reference manual
Rev. 1.0 —17 Jan 2020
7 of 31
the following figure; this includes via locations as well. Deviation from these parameters
can cause performance degradation.
Fig 3. Critical Layout of die flag area
Fig 3 shows the critical areas of the device die flag. These are the following:
•Ground vias and locations
•RF output and ground traces
•Die flag shape
4.2 PCB Stack-Up
Complexity is the main factor that will determine whether the design of an application
board can be two-layer, four-layer, or more. From an RF point of view a 4 layers PCB
is preferred to a two layers PCB. Nevertheless, in a very simple application it should
be possible to use a 2 layers PCB.
The recommended board stack-up for either a four-layer or two-layer board design is
as follows:
•4-layer stack-up:
—Top: RF routing of transmission lines
—L2: RF reference ground
—L3: DC power
—Bottom: signal routing
•Two-layer stack-up:
—Top: RF routing of transmission lines, signals, and ground
—Bottom: RF reference ground, signal routing, and general ground
RFIO
GND vias
Die flag

NXP Semiconductors
JN-RM-2079
QN9090 module development reference manual
JN-RM-2079
All information provided in this document is subject to legal disclaimers.
© NXP Semiconductors N.V. 2020. All rights reserved.
Reference manual
Rev. 1.0 —17 Jan 2020
8 of 31
The QN9090-001-M10 and QN9090-001-M13 (OM15069) modules are built on a
standard 4–layer printed circuit board (PCB) with the individual layers organized as
shown in Fig 4.
Fig 4. PCB stack-up
Note: The NXP PCB layouts assume use of the layers defined above. If a different PCB
stack-up is used, then NXP does not guarantee performance.
NXP strongly recommends the use of the above stack-up.
As shown in Fig 4, regarding transmission lines, it is important to copy not just the
physical layout ofthe circuit, but also the PCB stack-up. Any small change in the
thickness of the dielectric substrate under the transmission line will have a significant
change in impedance; all this information can be found on the fabrication notes for
each board design. As an illustration, consider a 50-ohm microstriptrace that is 18-mils
wide over 10 mils of FR4. If that thickness of FR4 is changed from 10 to 6 mils, the
impedance will only be about 36 ohms.
In any case the width of the RF lines must be re-calculated according to the PCB
characteristics in order to ensure a 50-ohm characteristic impedance.
When the top layer dielectric becomes too thin, the layers will not act as a true
transmission line, even though all the dimensions are correct. There is not universal
industry agreement on which thickness at which this occurs, but NXP prefers to use a
top layer dielectric thickness of no less than 8-10 mils.
There is also a limit to the ability of PCB fabricators to control the minimum width of a
PCB trace and the minimum thickness of a dielectric layer. +/- 1 mil will have less
impact onan 18-mils wide trace and a 10-mil thick dielectric layer, than it will on a much
narrower trace and thinner top layer.
This can be an especially insidious problem. The design will appear to be optimized
with the limited quantityofprototypeandinitialproductionboards,inwhichthebare
PCB'swereallfabricatedinthesame lot.However,whenthe productgoesintomass

NXP Semiconductors
JN-RM-2079
QN9090 module development reference manual
JN-RM-2079
All information provided in this document is subject to legal disclaimers.
© NXP Semiconductors N.V. 2020. All rights reserved.
Reference manual
Rev. 1.0 —17 Jan 2020
9 of 31
productiontherecanbevariations in PCBfabricationfrom lot-to-lot which can degrade
performance.
The use of a correct substrate like the FR4 with a dielectric constant of 4.4 will assist you
in achieving a good RF design.
While no special measures are required for the board design, it is recommended that
Class 1 tolerances be used.
4.3 RF circuit topology and matching
NXP always recommends that designers start by copying the existing NXP reference
design. This applies to both the circuit portion (schematic) of the design, and the PCB
layout. For all RF designs, particularlyfor designs at frequencies as high as 2.4 GHz, the
PCB traces are a part of the design itself. Even a very short trace has a small amount of
parasitic impedance (usually inductive), which has to be compensated for in the
remainder of the circuit.
What may seem like a minor change to the layout, or what would certainly be a minor
change at a lower frequencyof operation,canactually bea significantchange at 2.4 GHz.
For example, we may consider that a metal trace on a PCB such as the QN9090-001M1x
modules is approximately 0.8 nH per mm. At lower frequencies, this would have no
impact, but at 2.4 GHz this would have a significant impact in any matching circuits.
The circuits used on the NXP reference designs are all tuned and optimized on the
actual layout of the reference design, such that the final component values take into
account the effects of the circuit board traces,andother parasiticeffectsintroducedby
thePCB.Thisincludessuchissuesasparasiticcapacitance between components,
traces, and/or board copper layers, inductance of traces and ground vias, the non-ideal
effects of components, and nearby physical objects.
The layout of the RF portions of QN9090 based modules is critical. It is important that the
reference designs are strictly adhered to, otherwise the following may occur:
•Reduction in RF output
•Excessive spurious RF outputs leading to RF compliance issues
•Unacceptable power slope across the full channel range
•Poor range
•Reduced Rx sensitivity
4.4 Transmission lines
Transmission lines have several shapes such as microstrip, coplanar waveguide,
and strip-line. For BLE applications built on FR4 substrates, the types of
transmission lines typically take the form of microstrip or coplanar waveguide
(CPW). These two structures are defined by the dielectric constant of the board
material, trace width, and the board thickness between the trace and the ground.

NXP Semiconductors
JN-RM-2079
QN9090 module development reference manual
JN-RM-2079
All information provided in this document is subject to legal disclaimers.
© NXP Semiconductors N.V. 2020. All rights reserved.
Reference manual
Rev. 1.0 —17 Jan 2020
10 of 31
Additionally, for CPW, the transmission line is defined by the gap between the trace
and the top edge ground plane. These parameters are used to define the
characteristic impedance of the transmission line (trace) that is used to convey the
RF energy between the radio and the antenna.
QN9090 has a single ended RF output with a 3-component matching network
composed of a shunt capacitor, a series inductor then another shunt capacitor. In
addition, a 0-ohm resistor has been placed between the RFIO port of the chip and
the first shunt capacitor. These elements transform the device impedance to 50
ohms. The value of these components may vary depending on your specific board
layout. The recommended RF matching network is shown in Fig 5.
Avoid routing traces near or parallel to RF transmission lines or crystal signals.
Maintaining a continuous ground under an RF trace is critical to maintaining the
characteristic impedance of that trace. Avoid any routing on the ground layer that
will result in disrupting the ground under the RF traces.
Keep the RF trace as short as possible.
Fig 5. RF Matching Network
4.5 Components
All electronic components have parasitic characteristics that cause the part to act in a
non-ideal way. Typically, these effects become worse as the frequency of operation is
increased.
Controlled impedance trace
(50 ohm microstrip)
RF Match
Printed antennaµFl connector