Lesson 1 - PCB Design

Design Guidelines…

1)      Keep board design, component layout, and conductor traces as simple as possible. Avoid odd shaped boards, multi-axis component arrangements, and complicated conductor paths.

2)      Attempt to restrict the maximum board area to a size that will fit evenly into a 18 X 24 inch panel when manufactured and keep the board outline dimensions as nearly rectangular as possible. i.e. an 8X10 board will fit evenly 4 times into an 18X24 standard panel with the required clearances and tooling needs of the manufacturer being met.

3)      Use a standard grid as large as possible to define the locations of features and components.

4)      Keep conductor traces as short as possible.

5)      Use 45 degree angles where ever possible, Avoid 90 degree angles or Acute angles for traces.

6)      Run long conductors with the long dimension of the board.

7)      Keep conductors away from the edges of the board at least .025 inches.

8)      When wave soldering break up ground planes on the bottom side of the board to avoid warping or blistering of the board.

9)      Keep terminal pads a minimum of .05 away from board edges

10)  Keep the number of hole sizes to a minimum.

11)  Identify each layer of the board in the margins just outside the board outline.

12)  Indicate polarity and component orientation.

13)  Place components that have adjustable features like pots or switches or variable capacitors, in areas of the board that they can be accessed while mounted  in the equipment.

14)  Make sure that test points are accessible and on a .100 inch grid for automated bed of nails testers.

15)  All components dissipating more than 1 Watt of heat energy should be mounted in such a way as to not allow the body to come in contact with the board surface. This protects the epoxy laminate from degrading due to exposure to heat beyond it’s rated temperature specifications.

16)  Place components that must dissipate more than 2 Watts of energy directly on a heat sink or attached to the chassis to conduct the heat away from contact with the board.

17)  Take note of mechanical support for heavier components, placing them near the board supports.

18)  Be aware of the potential to entrap moisture under components and make provision for cleaning the boards after assembly.

19)  Use the minimum number of layers needed to make your printed circuit. Always use a symmetrical layer stack up with evenly distributed copper on the layers.

20)  Use standard board thicknesses where possible, beware of the costs involved in exotic designs.

21)  Components weighing more than ¼ oz. per component lead should be mounted with a clamp or some restraining device to prevent over stressing the solder joints under vibration. The solder joints should not be the sole support for heavier components.

22)  Do not rely on solder mask material as an insulation device.

Before the board outline can be defined, the following considerations must be taken into account:

1)      Type of housing the board will fit into

2)      Maximum 3 dimensional space available for the board

3)      Mounting, fastening, clamping method to be used

4)      Electrical cables, connectors, terminals, and adjustable components that need accessed

5)      Type, thickness, and material to be used

6)      Surfaces of the board to me used for component mounting

7)      Method of assembly to be employed,  Hand assembly, wave solder, reflow solder for surface mounting, through hole assembly with automated equipment… etc.

8)      Addition of any tooling holes

Before beginning a Printed Circuit board layout the end use of the product that the board must reside in must be known. What sort of environmental conditions will the assembly be exposed to? Conditions that can affect the performance of the design must be considered.

1)      Shock and Vibration

2)      Humidity

3)      Temperature

4)      EMI/EMC or electrical fields

5)      Chemicals or corrosives

The designer needs to have a schematic, a bill of materials or parts list, and all the specifications for the components to be mounted and connected on the board. From this information the designer will develop the layout and master pattern for the printed circuit board. The designer will compile the information on all components including the physical size, lead pattern and spacing, special mounting data required hole and terminal sizes and electrical and thermal limitations.

The following process  describes the sequence of events that must take place in order to develop a board layout.

1)      Study the final schematic diagram

2)      Understand all symbols, reference designations, and component specifications.

3)      Using the component specification sheet, determine component body configuration, size , mounting options, land pattern, and any other specific requirements for assembling and testing the part.

4)      Take note of any polarity requirements for polarized components. Identify the Cathode end of diodes,  emitter for transistors, and polarity for capacitors, Pin one for IC’s  and connectors, and polarity for windings of transformers, and wire wound chokes where required.

5)      Group components according to common connections, logical function or specific circuit function.

6)      Determine grounds and supply voltage requirements for components and IC’s and place decoupling caps near the voltage pins as required by the design. Observe the wattage requirements and if using distributed power and ground traces take note of the conductor widths and lengths to minimize voltage drop or noise or thermal heating of traces.

7)      Establish heat sinks, ground planes or other special conductor geometries as needed.

8)      Understand connection requirements, bus and high speed data needs, locations of clock lines, and terminating resistors, EMI/EMC requirements, isolation of susceptible circuits from noisy circuits, etc.

9)      Look for human engineering needs, accessibility of adjustments, connectors, switches, card guides, ejectors, protection from high voltages, indicators and lights located where they can be seen in the equipment, test points, probe points, and manufacturing registration guides and supports for tooling.

10)   Layouts should be viewed from the PRIMARY or COMPONENT side.

11)  Parts should be placed  by their level of critical importance in the circuit, fixed features that interface with the chassis, or enclosure first like connectors, switches, lights or LED’s, displays, mounting hardware, clamps, standoffs, screws, cables, etc. Next larger Integrated Circuits or IC’s with their associated decoupling capacitors located as close as possible to the power pins, or special high speed digital or analog or RF parts with special features that must be incorporated into the design copper for electrical or signal performance reasons. These are usually laid out in groups that can be associated with each other and moved as a unit to their location in the design keeping their important relationships established at all times.  If a particular component is connected to more components than any other component on the board, that is the best one to start with and build around.  Try not to use odd axis mounting of components unless absolutely necessary, as this may require hand assembly rather than machine assembly of those components.

12)  Component placement is everything! Good component placement will almost always result in good board performance.  There are four basic component placement strategies that can be used independently or in combination:

a.       Schematic orientation

b.      Peripheral placement

c.       Central component placement

d.      Fixed array placement

The most basic concept of schematic orientation is used on medium to low density analog boards. This works especially well when the input is at one end of the circuit and the output is at the opposite end. Peripheral placement is used when board edge connectors or off board mounting or components with a fixed board edge locations are employed. These components should be positioned first and then subsequent components can be placed radiating inwards towards the center of the board.  Central component placement  usually involves a one or more large BGA or FPGA components place centrally in the board with parts being places around their periphery in sequence until the board is placed. The Fixed array concept is used for large digital designs that use many large chips of the same style with an equal spacing on a grid pattern and are typically machine routed. DFM or design for Manufacturing is a set of guidelines that are used by designers to improve the machine assembly of designs. If the board is going to be a high volume product it is mandatory that the designer understand and employ these rules in their designs. Components must be oriented in like fashion with 90 degree two-axis locations relative to the board long dimensions… targets or fiducials are required to register the board with the pick and place machines or auto insertion machines that populate the board with components by robotic assembly. Lower volume products may be hand assembled and not require these features.

Typical applications for Printed Circuits are as follows:

Class 1 - General Electronics Products -

Class 2 - Dedicated Service Electronics -

Class 3 – High Reliability Electronics -

See if you can classify the following product categories:

Consumer Electronics – Digital Wrist Watch, CD Player, Am/FM/Radio/Alarm Clock, Television, Calculator, Digital Coffee Pot, Microwave Oven, Home Alarm Systems, Cellular Telephone, Home Computer, Home Theater/Stereo Surround Sound System, Cable Television Converter Box, Hand Held Video Games, Remote control electronic toys… LOJACK auto recovery system…etc.

Telecommunications – Point to Point Microwave Transceivers, Police/ Fire/ Rescue Radios, Digital Network Equipment, SatCom transceivers, Commercial and Private Aircraft Radios and Instrumentation, Cell Telephone Relay Stations, CB Radio/2 Way Walkie Talkies, etc…

Industrial Electronics and Instrumentation – Weather Radar and Weather related Telemetry, Oscilloscopes, Network Analyzers, Ohm Meters, Temperature meters, Strain Gauges, Environmental Chambers and Ovens, Spectrum Analyzers, Solar Photovoltaic Power Cogeneration equipment, DC to AC Power Inverters, Switcher Power Supplies, CCD Telescopes…

Military Electronics – IFF transponders, IR detectors, Night Vision Goggles, Military grade Computers with encryption, Fire Control circuits, Satellite Navigation instrumentation, Encrypted Frequency Hopping VHF Radios, Direction Finding Equipment, Missile Guidance Systems, FLIR Pod Test equipment, etc…

Aerospace Electronics – Satellite systems, Space Shuttle controls and system, Aircraft communications and controls, etc…

Automotive Electronics – Automotive Ignition Controls, Emission monitoring and controls, Fuel Air Mixture, Fuel Injection, Climate controls, Dash Instrumentation, Radio/TV entertainment accessories, etc…

Medical Electronics – Heart Monitors, Automated Medicine dispensing equipment, Breathing machine, Dialysis machine, Laser assisted tooth whitening machine, Laser optical corrective surgery machine LASIX, X-ray or CAT Scan equipment, MRI Imaging equipment, etc…

According to IPC-2221 1.6 Printed board assemblies are classified by intended end item use.  The Performance Classes are listed as follows:

Class 1 - General Electronics Products - Includes consumer products, some computer and computer peripherals, as well as general military hardware suitable for applications where cosmetic defects are not as important, and the major requirement of the board is its functionality.

Class 2 - Dedicated Service Electronics – Includes Communication Equipment, sophisticated business machines, instruments and military equipment where high performance and extended life are required, and for which uninterrupted service is desired but not critical. Certain Cosmetic imperfections are allowed.

Class 3 – High Reliability Electronics – Includes Military and Commercial equipment where continued performance or performance on demand is critical. Equipment failure or down time is not tolerated and must function when required in the case of life support systems, or critical weapons systems. For applications where high levels of assurance are required and service is essential.

Producibility Levels:

Level A – General Design Complexity - preferred

Level B – Moderate Design Complexity - standard

Level C – High Design Complexity – reduced producibility.

Board Type:

Type 1 – Single Sided PCB

Type 2 – Double sided PCB

Type 3 – Multilayer without Blind or Buried vias

Type 4 – Multilayer With Blind and/or Buried vias

Type 5 – Multilayer Metal Core board without blind and/or buried vias

Type 6 – Multilayer Metal Core board with blind and/or buried vias