Renesas VersaClock7 PCB Instruction Manual

Manual
V
ersaClock7 PCB Layout Guidelines
R31UH0017EU0100 Rev.1.00
Aug 4, 2022
Page 1
© 2022 Renesas Electronics
PCB layout is a physical realization of the circuit designs. Good board layout practices will improve the electrical
performance by controlling crosstalk and ensuring signal integrity. In addition, layout plays a fundamental role in
meeting EMC emissions and immunity requirements.
This document provides information and recommendations to aid in the design and layout of PCB circuitry using
VersaClock7 (VC7) devices. It contains information for generic PCB layout and some particular considerations
for VC7 devices.
Contents
1. Layer Stack-Up............................................................................................................................................... 2
2. Placement....................................................................................................................................................... 4
3. Crystal Placement and Handling.................................................................................................................. 4
4. VC7 Device Electrical and Thermal Pad Handling...................................................................................... 5
4.1 RC21008A/RC31008A – 40-LGA [3] ...................................................................................................... 5
4.2 RC21012A/RC21012A – QFN-48 [4]...................................................................................................... 7
4.3 RC21005A/RC21005AQ – 32-LGA [5].................................................................................................... 8
5. Trace Routing................................................................................................................................................. 9
5.1 Single-Ended Routing............................................................................................................................ 9
5.2 Differential (Clock) Pair Routing............................................................................................................ 9
6. Power Supply Trace and Power Filtering Layout..................................................................................... 12
7. References.................................................................................................................................................... 13
8. Revision History .......................................................................................................................................... 13

VC7 PCB Layout Guidelines Manual
R31UH0017EU0100 Rev.1.00
Aug 4, 2022
Page 2
1. Layer Stack-Up
A PCB consists of multiple layers of copper (foil) and isolation materials laminated together. PCB layer stack-up
design refers to the layer arrangement of copper and dielectric material layers with the total number of layers
and the thickness of each layer taking into considerations.
Planning optimal multilayer stack-up is one of the most critical factors in determining electromagnetic
compatibility performance of a PCB. A well-designed layer stack-up can both minimize the radiation and stay
robust from external noise sources.
The following two diagrams illustrate the significance and relationships of signal impedance and EMC control
with the PCB layer stack-up.
A signal trace that is suspended over a ground plane with a dielectric layer between them is call a microstrip. Its
impedance is determined by a number of factors in the PCB and its stack-up arrangement:
■Signal trace width
■Thickness of the trace (thickness of copper layer)
■Distance between the two traces if it is a differential pair
■Thickness of the dielectric layer between a microstrip and the ground plane under the dielectric layer
■Dielectric constant Er
The following figure shows the calculation of a differential pair’s impedance on the top layer of a PCB stack-up
[1].
Figure 1. Signal Impedance with Respect of PCB Stack-Up
When a signal trace changes layers, the above factors affecting trace impedance change as well. Caution must
be exercised in order to keep the signal impedance continuous to avoid signal integrity impairments.
Another signal type is called a stripline signal, which is one sandwiched between two dielectric material layers. A
stripline signal trace impedance is similarly related to these factors but with a different calculation formula (not
provided).
Figure 2. Stripline Signals Embedded in Dielectric Layer between Two GND Layers

VC7 PCB Layout Guidelines Manual
R31UH0017EU0100 Rev.1.00
Aug 4, 2022
Page 3
It is worth noting that stripline signals are in between two GND plane layers. This minimizes crosstalk between
the stripline signals and signals outside this layer. This is why an optimal stack-up design will enhance EMC
performance of a PCB design.
Layer stack-up is a universal requirement for any PCB design, not just for VC7 devices. The following stack-up
example is a board stack-up used for our VC7 Evaluation Board. The following comments are specific to this
board layer stack-up:
■A 10-layer board is planned
■6 layers are dedicated to copper planes – 4 ground planes and 2 power planes. This generous number of
ground and power planes will help the board’s EMC performance.
Note: Depending on signal density, not every PCB board can dedicate such an abundant number of copper
planes.
■Every signal layer must have an adjacent copper plane layer (ground or power plane) as return current paths
for the signals on that layer.
■Megtron-6 material of different thickness are chosen as the dielectric layers between copper layers. Megtron-6
material demonstrates a very low loss at signal frequency < 2GHz. Given the clock frequencies in VC7
devices, FR4 material should be adequate.
■Total board thinness is 62mil, which is the most common board thickness.
Figure 3. VC7 EVB Layer Stack-Up [2]
■From the above stack-up, Layer 3 (signal layer) is sandwiched between Layer 2 (GND plane) and Layer 4
(GND plane). Thus, Layer 3 is the preferred layer to route critical signals as noise and cross-talks are
minimalized. This is also true for Layer 8.
■Copper layer thickness is defined by weight of copper (e.g., ½ oz of copper, or 1oz of copper). The thickness
of copper layer of 1oz is the thickness of copper when 1oz of copper is spread evenly across a square foot,
which is 0.35mm or 350mil (see the following figure).

VC7 PCB Layout Guidelines Manual
R31UH0017EU0100 Rev.1.00
Aug 4, 2022
Page 4
Figure 4. Copper Weight (Foil Thickness)
2. Placement
The optimal placement of the VC7 device and its neighboring components is specific to each design. The
following general recommendations are provided for the designer to consider:
■Place the VC7 device/crystal away from switching power supply circuit.
■Place and orient the VC7 device for convenient routing of input and output clock traces.
■For crystal placement and routing recommendations, see “Crystal Placement and Handling”.
■For decoupling capacitor placement and routing recommendations, see “Power Supply Trace and Power
Filtering Layout”.
3. Crystal Placement and Handling
Xin/Xout are the crystal oscillator circuit interface pins. Consider the following recommendations when using a
crystal:
■Place the crystal as close to the IC pins as possible to minimize Xin/Xout trace length. The purpose of doing
so is to minimize parasitic capacitance and interference. For the same reason, avoid using vias in Xin/Xout
traces.
■When using capacitors on each crystal pin to set the load capacitance value, connect the ground side of the
two capacitors close together and close to the IC ground connection. The reason is to minimize noise coupling
from the ground plane. The VC7 devices have internal capacitors. It is preferred to use internal capacitance to
avoid using external capacitors. When doing so, configure the internal capacitance based on crystal’s load
capacitance (CL) in the spec. Avoid overloading or underloading the crystal.
■Treat the crystal component area as a “keep out area” for signal routing on other layers.
■Rout Xin and Xout traces as non-coupled high impedance traces. Separate them by at least 3x the trace
width.
■Xin can be overdriven by a single-ended LVCMOS signal, or an AC-coupled signal lead from a differential
pair, provided that the signal amplitude remain between 500mV and 1.2V and a slew rate of at least 0.2V/ns.
In this case, the VC7’s internal capacitance should be configured to a minimum value. In the following
schematics, place the signal termination resistor close to Xin pin.

VC7 PCB Layout Guidelines Manual
R31UH0017EU0100 Rev.1.00
Aug 4, 2022
Page 5
Figure 5. XIN Overdrive with an LVCMOS or an LVPECL Clock Source
4. VC7 Device Electrical and Thermal Pad Handling
VC7 devices come with an ePad – a ground island directly beneath the device on the same layer the IC is
soldered on the PCB. The ePad is both a grounding pad and a thermal relief pad for the device. ePad patterns
are different in different part numbers. Separate discussions on ePad handing are included in the following
sections.
4.1 RC21008A/RC31008A – 40-LGA [3]
■Device land pattern is shown below:
●PCB pad width: 0.20mm
●PCB pad length: 0.45mm
○Toe extension (beyond package edge): 0.05mm
○Heel extension (toward package center): 0mm
■Stencil recommendations (Unit: mm):
●Thickness: 0.125
●Aperture for thermal pads: 0.84 × 0.84 (x9, each aperture centered on corresponding land pattern of each
pad)
●Aperture for pins: 0.22 × 0.58 (x40, heel coincides with package pin heel)
■Via placement and connections:
●Place a thermal/ground via on each thermal pad.
●This implementation is called via-in-pad, which is the option for this package because there is no extra
space for the vias outside of pads.

VC7 PCB Layout Guidelines Manual
R31UH0017EU0100 Rev.1.00
Aug 4, 2022
Page 6
Figure 6. 40-LGA Land Pattern Dimensions
Figure 7. Layout Land Pattern Recommendations for RC21008AQ

VC7 PCB Layout Guidelines Manual
R31UH0017EU0100 Rev.1.00
Aug 4, 2022
Page 7
4.2 RC21012A/RC21012A – QFN-48 [4]
■Device land pattern is shown below
●PCB pad width: 0.20mm
●PCB pad length: 0.55mm
○Toe extension (beyond package edge): 0.05mm
○Heel extension (toward package center): 0mm
■Stencil recommendations (Unit: mm)
●Thickness: 0.125
●Aperture for thermal pads: 2.3 × 2.3 (x4, 200um gap between apertures; centered on land pad).
Note: We recommend 4x 2.3 × 2.3 mm solder paste pads instead of a big, single pad to avoid excessive
copper.
●Aperture for pins: 0.20 × 0.58 (x48, heel coincides with package pin heel)
■Via placement and connections:
●Place as many thermal/ground vias as fit in each of the 4 split pads.
●This implementation is called via-in-pad, which is the option for this package as there is no extra space for
the vias outside of pads.
Figure 8. QFN-48 Land Pattern Dimensions

VC7 PCB Layout Guidelines Manual
R31UH0017EU0100 Rev.1.00
Aug 4, 2022
Page 8
4.3 RC21005A/RC21005AQ – 32-LGA [5]
■Device land pattern is shown below.
■Stencil recommendations (Unit: mm)
●Thickness: 0.125
●Aperture for thermal pads: 0.60 × 0.55 (x4, each aperture vertex closes to the aggregate center of the
pattern. Four apertures should be aligned with the corresponding vertex of the land pad)
●Aperture for pins: 0.22 × 0.68 (x32, heel coincides with package pin heel)
■Via placement and connections:
●Place thermal/ground via in space close to each thermal pad.
●Connect each via with a thermal pattern with a trace for a low impedance connection. Via size and trace
width are per each design’s DCR.
Figure 9. 32-LGA Land Pattern Dimensions

VC7 PCB Layout Guidelines Manual
R31UH0017EU0100 Rev.1.00
Aug 4, 2022
Page 9
5. Trace Routing
Routing a PCB board with VC7 devices should follow the generic engineering practice of PCB routing rules.
Routing recommendations are summarized in the following sections.
5.1 Single-Ended Routing
■Keep clock traces as straight as possible. Use arc-shaped (or 45 degree) traces instead of right-angle or even
sharp-angle bending.
Figure 10. Trace Bending
■Do not use multiple signal layers for clock signals (i.e., to avoid changing layers).
■Do not use vias in clock transmission lines (i.e., to avoid changing layers). Vias can cause impedance
mismatch impairing signal integrity.
■Always route clock signals (and any signal in that matter) on a layer that has an immediately adjacent ground
layer as a return current path.
■As a classic routing pitfall, avoid routing a signal across a cut-out/slit on the reference plane. If unavoidable,
use a stitching capacitor (i.e., 0.1uF) to provide a return current path as follows.
Figure 11. Using a Stitching Capacitor Where Passing a Ground Plane Slit
5.2 Differential (Clock) Pair Routing
Differential traces should always be routed together (side-by-side). This keeps any noise injection into the signal
pair a true common-mode noise which gets rejected by the receiver. In a real PCB routing, consider the following
points as additional recommendations.

VC7 PCB Layout Guidelines Manual
R31UH0017EU0100 Rev.1.00
Aug 4, 2022
Page 10
■Keep both leads of a differential pair the same length so that signals arrive at the receiver at the same time.
Use “phase matching bumps” to the lead that is shorter than the other lead to make both signal leads the
same length. Remember to compensate at the end where length deficit takes place as shown below.
Figure 12. Adding Phase Compensation Bumps in a Differential Pair
■If ac-coupling capacitors are used, place the coupling capacitors in a way that the differential pair can be
routed symmetrically as shown below.
Figure 13. Symmetrical Placement of Series Components in a Differential Pair
■To avoid a non-related component on the board, avoid encompassing the component within the differential
pair. Rather route the differential pair away from the component together as in the following diagram.
Figure 14. Avoid Encompassing an Unrelated Component in a Differential Pair