Rf design and review guidelines

RF DESIGN AND REVIEW GUIDE LINES
Monday, FEBRUARY 15, 2016
Contact Name: T Y JOSE
Telephone:+91 9952967626/949276116
Email:tyjose@gmail.com,tyjose@live.com

of 21
Contents
1. Scope of the Document ..................................................................... 4
2. Documents for Design reviews............................................................ 4
3. RF GUIDELINES ............................................................................. 5
3.1 Power Supply Regulation and specifications........................................ 5
3.2 Decoupling especially for Tx Power supply.......................................... 5
3.3 Power Supply and ground pad distribution ......................................... 6
3.4 Split ground topology Digital /Analogue/ RF ..................................... 6
3.5 Supply crosstalk ............................................................................ 6
3.6 Supply switches............................................................................. 6
3.7 Antenna Placement, Enclosure, and Ground Plane ............................... 6
3.8 Matching Network for Antenna ......................................................... 7
3.9 Cross talk and tracks with λ/4 length ................................................ 7
3.10 Un terminated copper shapes lengths............................................. 8
3.11 All long traces should be with Controlled Impedance traces................ 8
3.12 Minimize Vias in High frequency paths ............................................ 8
3.13 Xtal Osc spec. stability harmonics . ................................................ 8
3.14 SPI/I2C communication track lengths ............................................. 9
3.15 Verify general fulfilment of all regional regulations GSM/GPRS/LTE...... 9
3.16 RF traces bending radius .............................................................. 9
3.17 TDD/FDD switching circuits ....................................................... 9
3.18 Presence of shield, mounting and general profile ............................. 10
4. DFM/DFT GUIDE LINES................................................................. 10
4.1 Component to component spacing ................................................... 10
4.2 Component to board out line and fasteners spacing.......................... 10
4.3 Test points availability size and spacing............................................ 11
4.4 Spacing of Vias and general features................................................ 11
4.5 Trace to trace spacing in all routing layers ........................................ 11
4.6 Fiducial and tooling holes ............................................................... 11
4.7 Solder mask................................................................................. 12
4.8 Assembly and fabrication drawings .................................................. 12
4.9 Stencils, any other tooling.............................................................. 13
4.10 BOM to NM verification................................................................ 13
4.11 PCB Size and Mechanical Fit......................................................... 14
4.12 Panel /single - drawing, V Grove /routing..................................... 14
4.13 Thru hole component lead diameter .............................................. 15
4.14 Tooling holes four corners non plated ............................................ 15
4.15 Reduce number of thru hole components as possible ....................... 15
4.16 No Component legend falling on component pad ............................. 16
4.17 Component orientation, Solder thief .............................................. 16

of 21
5. EMI/EMC GUIDE LINES ................................................................. 16
5.1 Ground System ............................................................................ 16
5.2 Power supply Considerations .......................................................... 16
5.3 Isolated DC-DC Converters............................................................. 16
5.4 Segregation of components ............................................................ 17
5.5 PCB Considerations ....................................................................... 17
5.6 Board Layers................................................................................ 17
5.7 Signal Line considerations .............................................................. 17
5.8 Terminate lines with HF and RF signals............................................. 18
5.9 Digital Circuits.............................................................................. 18
5.10 Clock Termination ...................................................................... 18
5.11 Analogue Circuits ....................................................................... 18
5.12 Decoupling Capacitor .................................................................. 18
5.13 Cables...................................................................................... 18
5.14 Crosstalk .................................................................................. 19
5.15 Shielding .................................................................................. 19
5.16 Component Considerations .......................................................... 19
5.17 Component Placement ................................................................ 20
6. REFERENCES .................................................................................. 20

of 21
1. Scope of the Document
This document gives guidelines for RF, DFM/DFT and EMI/EMC Design, Review and Verification of
designs based on most of the wireless control integrated circuits. It covers all application segments
such as automotive, telecom, industrial, IoT and consumer electronics and provides best-practice
aspects and checklists for exhaustive system verification in the customer application. Even if some
of the hints may sound like common sense or just a good engineering practice, they are still
included as reminder.
This document has applications of Wireless Control Wireless IC products in its focus: receivers (RX),
transmitters (TX) and transceivers (TRX) – some of them with integrated temperature, acceleration
and pressure sensors and microcontrollers – however, current guideline version is narrowed to
general and RF, DFM/DFT, EMI/EMC aspects .
This document can help us in following design phases:
Verification plan definition
Schematics design and review
PCB layout design and review
Firmware/Software/Hardware co-verification and Design-For-Test and manufacturing (DFT
and DFM)
System verification, validation and sign-off
Design issue/problem detection, localization, debugging and fixing
Definition of production test
Disclaimer & Limitations: This document is provided on an “as-is/best-effort” basis and contains
detailed, but still generic and design-independent guidelines, thus it can only extend and by no
means replace an obligatory design-specific customer-defined verification plan. Thus there is no
liability resulting from following these guidelines whatsoever.
2. Documents for Design reviews
[1].Schematics with revision details
[2].PCB LAYOUT with revision details
[3].Bill of Materials
[4].Data sheets for the components used

of 21
3. RF GUIDELINES
3.1 Power Supply Regulation and specifications
Clean and stable power supply is essential for good RF applications. Following characteristics must
be specified, designed and verified in the application over the full specified range of environmental
and operating conditions. Sufficient margin should be provided while designing the power
circuits.
 Supply voltage: Check all supply & regulated voltages in all functional modes (variation vs.
temperature and application supply voltage). Supply voltage must remain within the specified
(min-max) range for all devices under all circumstances. Lower operating voltage than “min”
may cause performance loss (blocking, linearity, phase noise, output power) or even overall
malfunction (due to analog operating point or logic threshold shift). Higher operating voltage
than “max” may cause an overall malfunction (due to analog operating point or logic threshold
shift), electrical breakdown or product lifetime impact due to higher currents (electro
migration), higher dissipation (thermal stress) or overvoltage stress (VT drift over lifetime) – the
list of effects being not exhaustive.
 Supply voltage stability: Consider and check load and line regulation of all regulators (external
and internal). Do not load on-chip regulators with external loads, except explicitly allowed.
3.2 Decoupling especially for Tx Power supply
Bypassing is essential to high speed and RF circuit performance. It provides low impedance source
and return paths to high frequency changes in load current. Capacitors as close as possible to the
supply pins of each IC provide localized bypassing.
 Regulator stability: Take care about capacitive (decoupling caps!) and inductive (wiring!) loads
when designing supply circuitry. Use only recommended capacitor values and types for regulator
decoupling and place capacitors as close as possible to input/output pins. Violation of these
rules may cause regulator instability (=oscillations with arbitrary load-dependent amplitude and
frequency) causing in turn probably sensitivity loss and blocking performance loss (LO spurious
mixing) for RX circuits and unwanted TX spurious emissions.
• Supply RF and noise decoupling: DC power supply must be ripple-free. Take care and verify that
no external RF and noise sources (EMC) can penetrate into the DC supply network i.e. use
feed-through capacitors and ferrite beads. Specifically for TX circuits generating on-board RF
currents, voltages and fields make sure there is no “backscatter” from RF output matching or
antenna circuits to supply distribution network. Design for low-ohmic and Wideband-low-
impedance supply network and test that. To achieve wideband low-impedance behavior use
different capacitor values in parallel (high-C || low-L= 100nF || 1 nF || 100 pF). All circuitry
generating large current surges (CMOS digital, line drivers) must be locally decoupled to reduce
switching noise on supply. Avoid switching regulators – if required in the application, try to
implement types with constant switching frequency or apply linear regulators at the output. In
that case check explicitly in the application behavior of RX and TX at RF + around the designed
switching frequency and its harmonics.

of 21
3.3 Power Supply and ground pad distribution
Power supply and ground lines must be low-ohmic and have low-impedance (low L), i.e.
corresponding PCB track width. Use large ground planes and - if possible – inner layers. Avoid ground
loops, i.e. contamination of sensitive (input) ground nodes with shared return path for high-current
(RF or switching) outputs. Use star topology (common ground) for ground and supply line
connection. Use split ground (digital + analog + RF) topology in general. Provide galvanic isolation
where feasible. Avoid using PCB Vias in supply and ground distribution – if you must have them, use
several multiple Vias in parallel to reduce the parasitic R an L.
3.4 Split ground topology Digital /Analogue/ RF
Grounding and routing are also critical steps in Radio board layout and fabrication. These steps will
directly impact board parasitic parameters that sometimes result in undesirable system
performance. There are no unique solutions to ground distribution in RF board design; several
approaches can achieve satisfactory system performance. Split ground planes or split traces can be
utilized to separate analog and digital signals or to isolate high-current or high-heat-generating
sections. Based on previous experience with RF board design, however, a single solid ground plane
in a four-layer stack-up board works well. The general rule is to avoid cross-interference by using a
ground plane to shield the RF section from other circuitry in the board.
3.5 Supply crosstalk
Take care that any wire or PCB trace approaching λ/4 length, independently of its original
“purpose” (i.e. even GND or supply), starts to behave like antenna and either emit or receive the RF
signal over large distances with high efficiency. Also pure capacitive or inductive crosstalk may
contaminate either supply, if routed in parallel with large signal tracks, or sensitive input (RX
antenna) or reference (XOSC) signals may become contaminated from a noisy supply line.
3.6 Supply switches
In many applications, it is required to cut-off the supply lines to sub circuits using discrete supply
switches. Take care to design for low-ohmic and low-impedance solution (Rds_on) over all supply,
temperature and load conditions and verify that.
3.7 Antenna Placement, Enclosure, and Ground Plane
 Always place the antenna in a corner of the PCB with sufficient clearance from the rest of
the circuit.( For patch antenna give minimum 10 mm clearance from the main PCB)
 Always follow the antenna designer’s/manufacturer’s recommended ground pattern for the
antenna.
 PCB antennas are variants of a monopole antenna. Monopole antennas need solid ground for
proper operation.
 Never place any component, planes, mounting screws, or traces in the antenna keep-out
area across all layers.

of 21
 The actual keep-out area depends on the antenna used.
 Do not place the antenna close to the plastic in the industrial design. Plastic has a higher
dielectric constant than air. Proximity of the plastic to the antenna results in the antenna’s
seeing a higher effective dielectric constant. This increases the electrical length of the
antenna trace and reduces the resonant frequency.
 The battery cable or mic cable must not cross the antenna trace on the PCB on the same side
of the antenna.
 The antenna must not be covered by a metallic enclosure completely. If the product has a
metallic casing or a shield, the casing must not cover the antenna. No metal is allowed in the
antenna near-field.
 The orientation of the antenna should be in line with the final product orientation so that
the radiation is maximized in the desired direction.
 There must not be any ground directly below the antenna. There must be enough ground at
a distance (ground clearance) from the antenna and this ground plane must have a minimum
width.
3.8 Matching Network for Antenna
Antenna is resonant circuit, the most important parameters for the antenna resonance is the length,
capacitance and inductor. The capacitance and inductance will be affected by external
components, ground plane, enclosures etc. For a perfect matching of the antenna need to tune for
these external effects.
 Plan to have a provision for an antenna matching network because a lot of parameters in the
antenna’s proximity (plastic, ground variation, substrate differences, and other components)
can vary its impedance, and therefore, the antenna may need retuning. If the impedance of
the antenna is unknown, it is preferable to have a provision for a PI or T network of three
components, with 0 ohms populated in series components and no load for shunt components.
This helps you to populate any topology needed for a matching network later.
 When using the matching network values provided by the antenna manufacturer, ensure that
you use the trace length from the antenna to the matching network specified in the
manufacturer datasheet or reference design.
 Always verify the antenna matching network with the final plastic enclosure in place and
the product placed in typical use case scenarios. For example, verify a wireless mouse with
its plastic held on the hand and placed on a mouse pad, plastic, wood, metal, or floor
3.9 Cross talk and tracks with λ/4 length
Capacitive and inductive crosstalk occurs between traces that run parallel for even a short distance.
In capacitive coupling, a rising edge on the source causes a rising edge on the victim. In inductive
coupling, the voltage change on the victim is in the opposite direction as the changing edge on the
source. Most instances of crosstalk are capacitive. The amount of noise on the victim is proportional
to the parallel distance, the frequency, the amplitude of the voltage swing on the source, and the
impedance of the victim, and inversely proportional to the separation distance.
Measures that reduce crosstalk are:
 Keeping RF-noise-carrying traces that are connected to the microcomputer away from other
signals so they do not pick up noise.
 Signals that may become victims of noise should have their return ground run underneath
them, which serves to reduce their impedance, thus reducing the noise voltage and any
radiating area.

of 21
 Never run noisy traces on the outside edge of the board.
 If possible, group a number of noisy traces together surrounded by ground traces.
 Keep non-noisy traces away from areas on the board were they could pick up noise, such as
connectors, oscillator circuits, relays, and relay drivers.
Antenna Factor Length Rules: Normally, trace length becomes important when it is greater than
1/10 of the wavelength. For professional applications, that number becomes 1/20 to 1/30 of the
wavelength. For automotive and consumer two-layer boards, 1/50 of the wavelength begins to be
critical, particularly in unshielded applications. Traces longer than 4 inches can be a problem with
noise. In these cases, some form of termination is recommended to prevent ringing.
3.10 Un terminated copper shapes lengths
Open copper shapes form un terminated transmission line. This will results in capacitance and or
Inductance, which will degrade the signal integrity.
So keep all un terminated copper shapes as short as possible and design pads as small as possible.
3.11 All long traces should be with Controlled Impedance traces
Telecommunications and computing equipment are operating at high frequencies have to be given
serious consideration. At high frequency PCB traces act as transmission lines and the energy can
reflect back and forth similar to a wave on a lake when it meets an obstruction. Controlled
impedance traces are designed to minimize electrical reflections and ensure an error free transition
between the PCB track and interconnections.
Do not use right-angle bends on traces with controlled impedance.
3.12 Minimize Vias in High frequency paths
Vias will introduce capacitance in high frequency traces, Short RF Traces should be on Component
Side of Board, Routed to Eliminate Vias. Minimizing Vias in RF Path Minimizes Breaks in Ground
Planes- Minimizes Inductance. Helps Contain Stray Electric & Magnetic Fields. Use as few Vias as
possible to avoid adding extra capacitance loading to the trace.
3.13 Xtal Osc spec. stability harmonics in RF board and closely
nearby boards.
Crystal oscillators (XOSC) are used in applications as:
 RF reference sources for RX (for local oscillator) and TX (for modulator) PLLs and
clock sources for digital circuits.
It is thus essential for a XOSC to provide:
 fast startup behavior
 clean signal: no spurious discrete single-line spectrum & low phase noise
 frequency accuracy and stability
As every oscillator, it consists of resonator circuitry and an on-chip amplifier for energy loss
compensation to fulfill and sustain the oscillation criteria. However, the resonator circuitry includes
not only the quartz crystal itself, but also possible external and on-chip pulling (tuning) capacitors
and unavoidable LC parasitic (L and C of PCB tracks, pins, IC, XTAL, caps etc). It is thus essential to
verify all XOSC parameters in the final design, since there is large influence of all components on
the final performance. Additionally, crosstalk via supply, ground or surrounding signal lines, as well

of 21
as intercepted RF fields from outside will contaminate the XOSC output signal, which might cause no
troubles for digital circuits, but become critical for output PLL signals.
Verify crystal oscillator startup time and oscillation margin in the final design. Take care that
oscillation margin depends on complete circuit incl. PCB. Too low oscillation margin can cause XOSC
malfunction with marginal crystals (higher R), leading to no oscillation or parasitic oscillation at
some arbitrary frequency.
3.14 SPI/I2C communication track lengths
The integrity of the chip configuration and thus your design’s functionality and performance
depends on error-free SPI or I2C communication between the host μC and IC.
Keep the bus length as short as possible: long bus lines will induce substantial capacitive load (high
current spikes in the drivers high digital noise, higher current consumption and lower max. data
rate) and increase the crosstalk probability.
Bus communication routines (SPI, I2C) and data transfer (Tx Host) are verified during this phase, as
well as timing.
Use SPI tracking or checksum registers (not available in all products) in your application and in the
verification test to validate the bus implementation (FW and electrical) in an endurance (loop) test.
You may want to apply EMC stress during this test.
Implement bus communication timing compliant with datasheet requirements and verify that.
3.15 Verify general fulfilment of all regional regulations
GSM/GPRS/LTE
GSM/GPRS/and LTE operating bands and frequency varies from country to country. While designing
and validating country specific parameters should be considered.
3.16 RF traces bending radius
When transmission lines are required to bend (change direction) due to routing constraints, use a
bend radius that is at least 3 or 4 times the center conductor width. In other words:
This will minimize any characteristic impedance changes moving through the bend.
In cases where a gradually curved bend is not possible, the transmission line can undergo a right-
angle bend (non curved). However, this must be compensated to reduce the impedance
discontinuity caused by the local increase in effective line width going through the bend. A standard
compensation method is the angled miter
Similar methods can be employed for other transmission lines. If there is any uncertainty as to the
correct compensation, the bend should be modeled using an electromagnetic simulator if the design
requires high-performance transmission lines.
3.17 TDD/FDD switching circuits
Guard time is required between Tx and Rx and vice versa. The guard time is equal to a unit A’s
turnaround time plus the round trip delay. A unit A’s turnaround time is in the order of 50 us. The
round trip delay is in the order of 66 us. Thus the round trip delay can absorb the transmitter A’s

of 21
turnaround time whenever the direction of traffic switches. The loss in throughput due to guard
time for a 5 ms frame is about 2%.
3.18 Presence of shield, mounting and general profile
 Proper shielding is required using ground Vias/ planes to reduce EMI.
 Decouple the RF parts of the circuit from the DC parts of the circuit.
 Inputs and outputs should be far apart, so that RF energy does not reflect back from output
to input.
 Isolation and return losses should be at least greater than -10dbm.
 Shield IF components from RF components.
 Decoupling capacitors should be used between an IC and a high speed RF track to avoid
signal transference to IC.
4. DFM/DFT GUIDE LINES
4.1 Component to component spacing
The land pattern design and component spacing affect the reliability, manufacturability, testability
and repairability of surface mount assemblies. A minimum inter-package spacing is required to
satisfy all these manufacturing requirements. Maximum inter-package spacing is limited by several
factors, such as available board space, equipment, weight considerations, and circuit operating
speed requirements. Some designs require that surface mount components be positioned as close to
one another as possible. Recommended minimum spacing is 25Mil.
4.2 Component to board out line and fasteners spacing
Keep the clearance of any copper to the edge of the board as large as possible. Routed edges should
have at least 50 Mils clearance. If the copper is too close to the edge, the circuit may be

of 21
manufactured with an exposed copper track, which could lead to corrosion. Also Component to
board out line and Fasteners spacing suggested is minimum 100 mils.
4.3 Test points availability size and spacing
Clear access to test point is vital. Ideally, test pads should be provided on each node. If possible,
always place test pads on one side of the board to minimize the likelihood of more expensive
double-sided test fixtures. Test pads should be round and nominally 35 mils in diameter with pad-to-
pad accuracy of ±0.003". Test pads should also be located at least 125 mils from the board edge
because; pick and place systems and handlers require access to the board edges. Test pad spacing
should be 100 mils whenever possible, 50 mils at a minimum. Test Electronics can probe centers as
close as 15 mils , but these small probes are expensive and do not have the durability of the larger
probes. Test pads on the component side of the board should have at least 40 mils clearance from
components to avoid damage to either the probe or the part.
4.4 Spacing of Vias and general features
Increased component density on SMT designs has mandated the use of thinner copper, narrower
conductor width and spacing. Higher component density may increase PCB layer counts as well,
requiring the use of more Vias to make the necessary connections between layers.
The minimum spacing is 0.1524 mm or 6 mils. For four-layer inner trace/Vias/pads spacing, the
minimum spacing is 0.254mm or 10 mils.
Traces and Vias should be a minimum of 50 mils away from routed/scored edge.
The traces that connect Vias to BGA pads need to be masked off as a minimum to prevent solder
from scavenging into the Vias. The BGA pads are non-solder masked defined (i.e. solder mask
opening is larger than the metal pad).
For RF boards the space for ground Vias at 1/8 of a wavelength or less your ground plane will look
like a solid ground. For a 1-GHz RF circuits that have via spacing of 250 mils
4.5 Trace to trace spacing in all routing layers
Copper spacing is the minimum air gap between any two adjacent copper features. Trace width is
the minimum width of a copper feature, usually traces.
To minimize crosstalk in high-speed interface implementations, the spacing between the signal pairs
must be a minimum of 5 times the width of the trace. This spacing is referred to as the 5W rule. A
PCB design with a calculated trace width of 6 mils requires a minimum of 30 mils spacing between
high-speed differential pairs. Also, maintain a minimum keep-out area of 30 mils to any other signal
throughout the length of the trace. Where the high-speed differential pairs abut a clock or a
periodic signal, increase this keep-out to a minimum of 50 mils to ensure proper isolation.
4.6 Fiducial and tooling holes
A fiducial mark is a printed artwork feature created in the same process as the circuit artwork
for optical recognition systems. The fiducial and a circuit pattern artwork must be etched in the
same step. The fiducial marks provide common datum points for all steps in the assembly process.
This allows each piece of equipment used for assembly to accurately locate the circuit pattern.
There are two types of fiducial marks.
Global fiducial marks are used to locate the position of all circuit features on an individual board.
When a multi-image circuit is processed in panel form, the global fiducials are referred to as panel

of 21
fiducials. A minimum of two global fiducial marks is required for correction of offsets (x and y
position) and rotational offsets (theta position). These should be located diagonally opposite and as
far apart as possible on the circuit or panel. A minimum of three fiducial marks is required for
correction of nonlinear distortions (scaling, stretch and twist). These should be located in a
triangular position as far apart as possible on the circuit or panel.
Local fiducial marks are used to Locate the position of an individual component requiring more
precise placement. A minimum of two local fiducial marks are required for correction of
translational offsets (x and y position) and rotational offsets (theta position). This can be two marks
located diagonally opposed within or outside the perimeter of the land pattern.
The optimum fiducial mark is a solid filled circle. The preferred diameter of the fiducial mark is 1.0
mm. The maximum diameter of the mark is 3.0 mm. Fiducial marks should not vary in size on the
same PCB more than 25 μm. A clear area devoid of any other circuit features or
Markings shall exist around the fiducial mark. The minimum size of the clear area shall be equal to
twice the radius of the mark.
4.7 Solder mask
Solder Mask Finishes: Solder mask coatings are used to protect the circuitry on the printed board.
Solder mask coatings are available in two forms, liquid and dry film. The polymer mask material is
applied using several process methods and is furnished in varying thicknesses.
As an example, liquid materials will have a finished thickness of 0.02 mm [0.0079 in] to 0.025 mm
[0.00984 in] while the dry film products are supplied in thicknesses of 0.04 mm [0.016 in], 0.08 mm
[0.0315 in], and 0.10 mm [0.0394 in]. Although screen type printing for solder mask is available,
photo-imaged solder mask is recommended for surface mount applications.
The photo process provides a precise pattern image and when properly developed eliminates mask
residue from land pattern surfaces. The mask thickness may not be a factor on most surface mount
assemblies but, when fine pitch (0.63 mm [0.0248 in] or less) IC devices are mounted on the printed
boards, the lower profile solder mask will provide better solder printing control.
Solder Mask Clearances: A solder mask may be used to isolate the land pattern from other
conductive features on the board such as Vias, lands or conductors. Where no conductors run
between lands, a simple gang mask opening can be used .For land pattern designs with routed
conductors between lands, the solder mask pattern must completely cover the conductor. A more
precise registration is necessary because of the tight tolerance needed to cover
the conductors without encroaching on the land area. PCB manufacturers are required to keep the
solder mask material off the land. Clearance conditions can vary from 0.0 mm [0.0 in] to 0.1 mm
[0.0040 in].
4.8 Assembly and fabrication drawings
Gerber files are created to enable plotting of the individual design file elements. Depending on
their function, each Gerber file is compiled as an individual electrical layer, process or design
reference.
Gerber File Structure:
 Electrical Design Layers - These Gerber files are processed to create each electrical layer
(internal and external) that will ultimately be finished in copper on the PCB.

of 21
 Silkscreen - This file will create the stencil that will be used to apply the silkscreen (ink) to
the PCB. The Silkscreen is for component reference, identification and labeling. The
Silkscreen exists on the outer layers.
 Solder Mask - The solder mask will expose solderable areas and protect the PCB by covering
all copper elements. The Solder Mask minimizes solder bridges. In this
Example, the Gerber file was created as a negative. Areas in red will not be covered with
mask. The solder mask exists on the outer layers.
 Solder Paste - This file will be used to create a solder paste stencil. Prior to the board
assembly, the stencil will be used to apply solder paste directly to the pads on the PCB
(Areas in yellow). Once the solder paste is applied, surface mount components can be placed
and soldered.
 Fabrication Drawings - This file will be created to display all mechanical and fabrication
design parameters of the PCB. Parameters include layer stack up, board thickness,
tolerance, drill file, copper weight, dimensioning, and applicable design standards. PCB
manufacturing details include drill size, plating, and drill location information, electrical
layer stack up, board thickness, slots, cutouts and tolerance.
 Assembly Drawings – Identifies location and orientation of the electronic components to be
placed.
 Aperture Files - This listing defines the shape of individual elements on the PCB.
 Drill Files - CNC drill parameters used on the PCB fabricators system to drill and route the
PCB.
 Net list - The net list is typically an ASCII format generated from the schematic. It contains
all components (*part*) and connections (*net*) required for the PCB design.
 X-Y Placement Data - Components are placed within the PCB board outline. Keep outs,
cutouts and holes must be avoided.
4.9 Stencils, any other tooling
Solder paste plays an important role in reflow soldering. The paste tacks the component before
reflow. It contains flux, solvent, suspending agent, and alloy of the desired composition. Solder
Paste is applied on the lands before component placement either by screening, stenciling, or
syringe. Screens are made from stainless steel or polyester wire mesh, and stencils are etched
stainless steel, brass, and other stable alloys. Stencils are preferred for high-volume applications.
They are more durable than screens, easier to align, and can be used to apply a thicker layer of
solder paste, and, where narrow, point apertures are required for example, for fine pitch lands.
Electroformed stencils may be required for very small components such as 0201 capacitors and
resistors. The goal of the technology that’s employed to make the stencil is to ensure that this
transfer is as efficient and complete as possible. There are several post processes that enhance the
stencil’s performance, including electro polishing and trapezoidal section apertures that are created
with laser cut technology.
4.10 BOM to NM verification
Verify manufacturing part number for each and every item on the BOM.
Review end of life, lead-times and availability of components selected. Select the best component
that is not near its end-of-life, the component whose lead-time is within your delivery window and
the component that is widely available in distribution. All too often it is only after the design is

of 21
completed and implemented do you realize a difficult or long lead-time item has been unnecessarily
designed in the product.
Select components with machine placeable features and packaging options. This will avoid driving
additional cost at manufacturing phase by incurring additional manual handling of components.
When possible, list alternate components to allow manufacturing process to find the best price/lead
time part.
For specialized components (e.g. ICs) or high dollar items, register the parts with the manufacturer
and negotiate special pricing upfront.
Select components where the required Minimum Purchase Quantity best matches your annual
demand. Expected demand of 1000 units of a component that is only offered in 2500 unit reels
multiples creates obsolescence and waste.
On SMT assemblies use headers that can be placed with automatic pick & place equipment. Many
manufacturers do not offer pick caps for their SMT headers. Avoid selecting components that need
to be hand placed as this increases costs and the opportunity for errors.
Select parts that can withstand the temperatures of the reflow ovens and wave solder equipment.
Restrictions on Hazardous Substances (RoHS) parts need to withstand 260 Celsius as a maximum
temperature.
It is unadvisable for Ball Grid Arrays (BGA) RoHS components to undergo the traditional Tin-Lead
process; however, they can be processed but with higher reflow oven temperature profile. The key
is temperature; the temperature must be high enough to allow the balls to fully melt.
Verify Non mount parts in final BOM and confirm for smooth assembly for the board.
Wires need to be specified for Gauge, Length, Color, and UL rating. Remember to include
manufacturer’s part number.
4.11 PCB Size and Mechanical Fit
PCB Size should match for the equipments in assembly house, used for production. The key is that
size does matter and bigger is not always better. The larger the panel, typically the more difficult it
will be to process.
PCB Shape must have two parallel sides (longest sides) to process through automation.
0.125” keep out area along board edges or rails/break off tabs is required.
0.250” rail/break off tab minimum size.
4.12 Panel /single - drawing, V Grove /routing
With the assembly house and PCB fabricator need to optimize for lowest cost by having flexibility on
panelization.
Panels become less stable as the array size increases. Include information about overhanging parts
(outline & keep out areas)
V-Groove scoring is applied to both sides of the board. It is a “V” shaped groove leaving a 0.015”
web of material to support the board. Components or other features should not be too close to the
edge or damage may occur.
Typically 0.035” – 0.050” should be allowed. - 45 deg .015" V-Groove scoring guidelines.
Routing & Perforated Tabs refer to IPC-700. Perforated tabs are made up of 3 holes 0.040” in
diameter. Indent holes by 0.025” to avoid a manual operation after depanelization PCB edge .025"
Routing Perforated Tab guidelines
The location of the cut tab shall be specified, if critical as it may cause interference upon assembly
into the application box or hardware.

of 21
4.13 Thru hole component lead diameter
Firstly we should find out the maximum lead diameter. It is present in the datasheet or package
drawing of the component. The maximum lead diameters for all shape types of holes, Round hole
shape is used for Round PTH Lead. Rectangle holes shape is used for Rectangle PTH Lead. Square
holes shape is used for Square PTH Lead.
Minimum Hole Size is calculated as Minimum Hole Size = Maximum Lead Diameter + 0.25mm to
0.15mm, depending on the component classification.
If it’s a standard component from data base (ERP) the diameter and pad size will be taken care by
the system.
4.14 Tooling holes four corners non plated
Tooling holes are added to boards for a variety of reasons. PCB fabricators use them for aligning the
board during drilling and routing. Assemblers use them for alignment with stencils during solder
paste printing, and for location on pick-and-place machines. They are used for alignment on
electrical test fixtures. They may also be used as alignment holes in the final enclosure, often
mating with small molded plastic posts. For some of these purposes tooling holes can be placed in
the overall panel, but for activities that occur after de-paneling, or for boards that are not
panelized, tooling holes are required within the board outline. Tooling holes are often standard
sizes, for compatibility with commonly used locating pins. Common imperial sizes are 0.062", 0.093"
and 0.125". Common metric sizes are 1.0mm, 1.5mm, 2.0mm, 2.5mm and 3.0mm. Tooling holes are
always un-plated. This gives better accuracy since plating thickness is not well controlled. Putting
the holes near the outer edges of the board helps ensure that the board will be stable when it is
supported on the locating probes before the fixture closes. The centre of gravity of the board should
be inside the polygon described by the support locations.
4.15 Reduce number of thru hole components as possible
Even though THM provides stronger mechanical bonds than SMT, making through-hole ideal for
components that might undergo mechanical stress, such as connectors or transformers. Good for
test and prototyping. But THM has many drawbacks on the bare PCB side; THM requires the drilling
holes, which is expensive and time consuming. THM also limits the available routing area on any
multilayer boards, because the drilled holes must pass through all the PCB’s layers. On the assembly
side, component placement rates for THM are a fraction of surface mount placement rates, making
THM prohibitively expensive. Further, THM requires the use of wave, selective, or hand-soldering
techniques, which are much less reliable and repeatable than reflow ovens used for surface mount.
Most of all, through-hole technology requires soldering on both sides of the board, as opposed to
surface-mounts, which only -- for the most part -- require attention to one side of the board.
SMT allows for smaller PCB size, higher component density, and more real estate to work with.
Because fewer drilling holes are required, SMT allows for lower cost and faster production time.
During assembly, SMT components can be placed at rates of thousands—even tens of thousands—of
placements per hour, versus less than a thousand for THM. Solder joint formation is much more
reliable and repeatable using programmed reflow ovens versus through techniques. SMT has proven
to be more stable and better performing in shake and vibration conditions.

of 21
4.16 No Component legend falling on component pad
A legend is often printed on one or both sides of the PCB. It contains the component designators,
switch settings, test points and other indications helpful in assembling, testing and servicing the
circuit board.
All legends should be visible, should not fall on components or pad.
4.17 Component orientation, Solder thief
On any printed board assembly where surface mount devices are to be wave soldered, the
orientation of devices in respect to the solder wave can contribute to excessive solder process
defects. The preferred orientation compared optimizes the solder process, minimizing solder
bridging on the trailing or shadowed contacts as the assembly exits the solder wave. All polarized
surface mount components should be placed in the same orientation when possible. The following
additional conditions apply:
1 All passive components should be parallel to each other.
2 The longer axis of SOICs and the longer axis of passive components shall be perpendicular to
each other.
3 The long axis of passive components shall be perpendicular to the direction of travel of the
board along the conveyer of the wave solder machine.
5. EMI/EMC GUIDE LINES
5.1 Ground System
Low inductance ground System, Maximizing ground plane reduces inductance and capacitance
reduces EM emission and Cross talk. Distributed ground system reduces return currents.
5.2 Power supply Considerations
Eliminate Loops in power supply Lines.
Decouple Power supply in local boundaries.
Place High Speed lines close to power supply section and low speed away from power supply
5.3 Isolated DC-DC Converters
An isolated DC-DC converter can provide a significant benefit to reducing susceptibility and
conducted emission due to isolating both power rail and ground from the system supply
Isolated DC-DC converters are switching devices and as such have a characteristic switching
frequency which may need some additional filtering.

of 21
5.4 Segregation of components
Components need to be segregated with functionality – Analog Digital. High speed digital, RF and so
on. The tracks for each group should stay in their designated area. For a signal to flow from one
subsystem to another, a filter should be used at subsystem boundaries
5.5 PCB Considerations
Avoid slit apertures in PCB layout, particularly in ground planes or near current paths.
Areas of high impedance give rise to high EMI, use wide tracks for power lines on the trace side.
Make signal tracks strip line and include a ground plane and power plane whenever possible.
Keep HF and RF tracks as short as possible, lay out the HF tracks first
Avoid track stubs, these cause reflection and harmonics
On sensitive components and terminations use surrounding guard ring and ground fill where possible
A guard ring around trace layers reduces emission out of the board, only connect to ground at single
point and make no other use of the guard ring (i.e. do not use to carry ground return from a circuit).
Avoid overlapping power planes, keep separate over common ground (reduces system noise and
power coupling.
Power plane conductivity should be high, therefore avoid localized concentrations of via and
through hole pads (surface mount is the preferred assembly technology)
Track smoothening at the edges (non perpendicular edges at corners) reduces field concentration
If possible make tracks run orthogonally between adjacent layers
Do not loop tracks, even between layers; this forms a receiving or radiating antenna.
Do not leave any floating conductor areas, these act as EMI radiators, if possible connect to ground
plane (often these sections are placed for thermal dissipation, hence polarity should be unimportant
but check component data sheet.
5.6 Board Layers
Care must be taken that the ground layer should always be between high-frequency signal traces
and the power plane. If a two-layer board is used and a complete layer of ground is not possible,
then ground grids should be used. If a separate power plane is not used, then ground traces should
run in parallel with power traces to keep the supply clean.
5.7 Signal Line considerations
Use low pass High pass and band pass filters wherever applicable to limit the band width to
optimum.

of 21
Keep Feed and return paths as close as possible in wide band signal lines
5.8 Terminate lines with HF and RF signals
Terminate lines carrying signals external to the board at the board edge.
Avoid cables and tracks close to quarter wave length of signal frequency.
Track all signals on the board to avoid flying leads.
Minimize rise and fall time on signals and clock edges, slew rate limiting also reduces cross talk
5.9 Digital Circuits
When dealing with digital circuits, extra attention must be given to clocks and other high-speed
signals. Traces connecting such signals should be kept as short as possible and be adjacent to the
ground plane to keep radiation and crosstalk under control. With such signals, engineers should
avoid using Vias or routing traces on the PCB edge or near connectors. These signals must also be
kept away from the power plane since they are capable of inducing noise on the power plane as
well. While routing traces for an oscillator, apart from ground no other trace should run in parallel
or below the oscillator or its traces. The crystal should also be kept close to the appropriate chips.
5.10 Clock Termination
Traces carrying clock signals from a source to a device must have matching terminations because
whenever there is an impedance mismatch, a part of the signal gets reflected. If proper care is not
provided to handle this reflected signal, large amount of energy will be radiated. There are multiple
forms of effective termination, including source termination, end termination, AC termination, etc.
5.11 Analogue Circuits
Traces carrying analog signals should be kept away from high-speed or switching signals and must
always be guarded with a ground signal. A low pass filter should always be used to get rid of high-
frequency noise coupled from surrounding analog traces. In addition, it is important that the ground
plane of analog and digital subsystems not be shared.
5.12 Decoupling Capacitor
Any noise on the power supply tends to alter the functionality of a device under operation.
Generally, noise coupled on the power supply is of a high frequency, thus a bypass capacitor or
decoupling capacitor is required to filter out this noise.
5.13 Cables
Most EMC-related problems are caused by cables carrying digital signals that effectively act as an
efficient antenna. Ideally, the current entering a cable leaves it at the other end. In reality,
parasitic capacitance and inductance emit radiation. Using a twisted pair cable helps keep coupling
to a low level by cancelling any induced magnetic fields. When a ribbon cable is used, multiple
ground return paths must be provided. For high-frequency signals, shielded cable must be used
where the shielding is connected to ground both at the beginning and at the end of the cable.

of 21
5.14 Crosstalk
Crosstalk can exist between any two traces on a PCB and is a function of mutual inductance and
mutual capacitance proportional to the distance between the two traces, the edge rate, and the
impedance of the traces. In digital systems, crosstalk caused by mutual inductance is typically
larger than the crosstalk caused by mutual capacitance. Mutual inductance can be reduced by
increasing the spacing between the two traces or by reducing the distance from the ground plane.
5.15 Shielding
Shielding is not an electrical solution but a mechanical approach to reducing EMC. Metallic packages
(conductive and/or magnetic materials) are used to prevent EMI from escaping the system. A shield
may be used either to cover the whole system or a part of it, depending upon the requirements. A
shield is like a closed conductive container connected to ground which effectively reduces the size
of loop antennas by absorbing and reflecting a part of their radiation. In this way, a shield also acts
as a partition between two regions of space by attenuating the radiated EM energy from one region
to another. A shield reduces the EMI by attenuating both the E-Field and H-field component of
radiating wave.
5.16 Component Considerations
Locate biasing and pull up/down components close to driver/bias points.
Minimize output drive from clock circuits.
Use common mode chokes between current carrying and signal lines to increase coupling and cancel
stray fields.
Decouple close to chip supply lines, reduces component noise and power line transients.
Use low impedance capacitors for decoupling and bypassing (ceramic multilayer types are preferred
due to high resonant frequency and stability).
Use discrete components for filters where possible (surface mount is preferable due to lower
parasitic and aerial effects of terminations on through hole parts).
Ensure filtering of cables and over voltage protection at the terminations (this is especially true of
cabling that is external to the system, if possible all external cabling should be isolated at the
equipment boundary).
Minimize capacitive loading on digital output by minimizing fan-out, especially on CMOS ICs (this
reduces current loading and surge per IC).
If available, use shielding on fast switching circuits, mains power supply components and low power
circuitry (shielding is expensive and should be a ’last resort’ option).
In general, keeping the bandwidth of all parts of the system to minimum and isolating circuits where
possible reduces susceptibility and emissions. Considerations which are applicable to reducing noise
levels are equally applicable to EMC compliance, EMC compliant circuits should obviously exhibit
low noise levels.

of 21
5.17 Component Placement
 Connectors should be placed on side or corner of the board-Locating the connectors on one
edge of the board makes it much easier to hold them all to the same reference potential.
This is extremely important for boards with high-frequency components that will not be
housed in a shielded enclosure. Some designs require that connectors be located on different
sides of the board. In these cases, every effort should be made to avoid placing high-
frequency circuits between any two connectors. When placing high-frequency circuits
between connectors is unavoidable, a metal enclosure and filtering to chassis ground is
generally necessary to keep the board from being able to drive common-mode currents on to
the attached cables.
 A device on the board that communicates with a device off the board through a connector
should be located as close as possible (e.g. within 2 cm) to that connector.
 All off-board communication from a single device should be routed through the same
connector.
 Components not connected to an I/O net should be located at least 2 cm away from I/O nets
and connectors.
6. REFERENCES
[1].Standards document: IPC-7351 February 2005
[2].Application Notes on RF design and EMI EMC guidelines from major Chip vendors like
TI, Infineon and more.

of 21
END OF THE DOCUMENT
For further information, please contact
tyjose@gmail.com +91 9952967262/9496276116

Rf design and review guidelines

More Related Content

What's hot

Viewers also liked

Similar to Rf design and review guidelines

Recently uploaded

Rf design and review guidelines