Chapter13 pcb design
Upcoming SlideShare
Loading in...5
×
 

Chapter13 pcb design

on

  • 3,234 views

 

Statistics

Views

Total Views
3,234
Views on SlideShare
3,231
Embed Views
3

Actions

Likes
4
Downloads
141
Comments
0

1 Embed 3

http://www.techgig.com 3

Accessibility

Categories

Upload Details

Uploaded via as Adobe PDF

Usage Rights

© All Rights Reserved

Report content

Flagged as inappropriate Flag as inappropriate
Flag as inappropriate

Select your reason for flagging this presentation as inappropriate.

Cancel
  • Full Name Full Name Comment goes here.
    Are you sure you want to
    Your message goes here
    Processing…
Post Comment
Edit your comment

Chapter13 pcb design Chapter13 pcb design Document Transcript

  • The University of New South Wales School of Electrical Engineering and Telecommunications ELEC3017 ELECTRICAL ENGINEERING DESIGN CHAPTER 13: PRINTED CIRCUIT BOARD DESIGN Lecture Notes Prepared by Mr Leon Dearden , Mr Don Williams2 and A/Prof. W.H. Holmes 1 (with minor edits by A/Prof. D. Taubman) 1 CLD Quality Services Pty Ltd 2 Associative Measurement Pty Ltd.ELEC3017 Electrical Engineering Design 1 Printed Circuit Board Design
  • PCB REQUIREMENTS SPECIFICATIONNormally when you contemplate designing a PCB for a particular project, there is theexpectation that there is a need for a number of identical items of product to meet acustomer’s requirements. The customer of course could be internal as well as external.Whether specified formally or not, there will be a set of requirements that the PCBassembly is expected to meet. These requirements often cover such things as: • Electrical/electronic performance ∗ Power output ∗ Frequency response ∗ Sensitivity ∗ Signal to noise ratio ∗ Etc. • Mechanical ∗ Volume, area or height constraints ∗ Weight constraints ∗ Special shapes to fit in with existing mechanical components ∗ Special packaging ∗ Etc. • Environmental ∗ Ambient temperature ranges ∗ Humidity ∗ Shock and vibration ∗ Altitude ∗ Etc.It is important to establish the requirements before circuit design commences, becauseoften the choice of circuit is very dependant on the type and availability of componentswhich can meet all of the required performance, mechanical and environmental factors.There may also be constraints imposed on the design process by the capability of theavailable production processes. For example, there may be constraints on the number oflayers 1 , the available hole sizes, the track spacings or finishes. Every effort should be madeto identify constraints on components or processes, including possible trade-offs.1 Thus, at UNSW only single or double sided boards without plated through holes may be made.ELEC3017 Electrical Engineering Design 2 Printed Circuit Board Design
  • COMPUTER-AIDED PCB DESIGN PROCEDUREWith the Requirements Specification defined and component and process limitationsunderstood, it is now time to complete the PCB design. It is assumed in the following thatthe electronic circuit design has already been carried out – i.e. the component types andvalues have been selected.PCB design was formerly done by applying opaque tape strips, representing the coppertracks on the finished PCB, onto a polyester (‘Mylar’) film to produce the ‘artwork’ for thecopper etching. However, nowadays PCBs are almost always designed using special CADsoftware packages such as Altiuml, Orcad, Daisy or Mentor, and the artwork is producedfrom the resulting computer file using a photoplotter (or perhaps a laser printer or plotter inless exacting designs).The steps in the design using PCB design software are generally as follows.Schematic EntryThe beginning of the design cycle that will result in a PCB is to enter the schematic circuitdesign into the CAD system. This process is called “schematic entry” or “schematiccapture”. While it is possible to proceed directly to PCB design without going through thefull schematic capture stage, it is definitely not recommended except for the very simplestof designs. It is just too easy for humans to fail to detect errors, even in simple PCBdesigns.The PCB schematic entry software has pinout libraries, schematic libraries and functionmodel libraries for the component parts. Also included is the ability to add your owncomponents into these libraries. Designs can be done in a hierarchical structure or ahorizontal structure. The hierarchical structure is the best for complicated systems,including boundaries for VLSI, hybrids (thin and thick film) and special artworkconstructions such as stripline layouts for high frequency work.There are two main outputs from the schematic entry part of the PCB design software: 1. The Netlist The CAD system will have the necessary connectivity data at the completion of the schematic entry process. The most important outcome of the schematic capture process is the netlist, which is a file defining the conducting tracks on the PCB and their connections to the components. This file is used later to check the accuracy of the wiring layout of your PCB, and is also the input to the layout stage of the PCB design. 2. The Parts List or BOM (Bill Of Materials) The CAD system will also output a parts list (or Bill of Materials, also known as a BOM) after the schematic entry has been completed. Ideally this will interface directly to a CAM system, but sometimes small conversion programs are needed to convert it into the correct part numbers for the manufacturing data base.ELEC3017 Electrical Engineering Design 3 Printed Circuit Board Design
  • Most schematic capture programs allow you to characterize each component with attributes such as component type, style, part number, ratings, supplier etc. This makes the production of an accurate parts list a straightforward matter, which is important in real-world production situations.Error Checking 1. Transcription Errors Error checking at this stage is a very important part of the process, as it is during the initial circuit entry stage that the greatest potential for human error arises. Any error made in transcribing your design will be present in all future stages of the process. So check, re-check and check again! If you can, get someone else to check your work at this stage to ensure that all circuit errors are eliminated. 2. Other Circuit Errors Modern design software tools, such as the Altium tools used in Elec3017, offer the facility of an electrical rules check. This check will typically detect shorts, inputs with no driving source, unconnected pins, bus contention and a number of other common errors. Also, the netlist can usually be exported to a circuit analysis program (e.g. SPICE or Micro-Cap) to verify the correct electrical operation of the circuit. In fact, the Altium software, used in this Elec3017, incorporates its own simulation tools. Simulation serves as a final design check, both on the circuit design itself and on the schematic entry into the CAD system. If the netlist is correct, the final PCB design will also be correct.Component PlacementThe netlist is the input for the actual physical PCB design. The first thing is to place thecomponents on the PCB. This is the most critical part of the PCB design process,especially at high frequencies or with high parts densities. Design engineers play a much bigger role in component placement than in any other aspect of the PCB manufacturing process.The first operation is to select a basic outline shape for the PCB, and then to manuallyplace those components whose position is externally constrained (e.g. because of front orback panel layouts). Other parts may also be placed manually because of designconsiderations such as critical track frequencies, bus layouts, thermal geometry, powersupply voltage drop, etc. It is also common to manually place certain major parts, such asvery large ICs. Features such as cut-outs, mounting holes, edge connectors andmechanical clearance areas are detailed at this stage of the layout.ELEC3017 Electrical Engineering Design 4 Printed Circuit Board Design
  • Many CAD systems can automatically place the remaining components using data fromthe netlist to place parts on the PCB outline. The program minimizes conductor lengths,thus being able to achieve greater parts densities by less track coverage of the availablePCB area. However, many designers prefer not to use automatic placement.Wiring Connections (Routing)The next operation is to position (or ‘route’) the conducting tracks between the componentpins. This can also be done automatically by most PCB design programs, but once againsome tracks may first be routed manually for the same reasons that certain componentsmay be manually placed. In particular, it is usually wise to place power traces and othercritical traces by hand first, especially for audio and RF circuits. Then auto-routing may beemployed if desired, though many designers prefer hand placement of circuit traces.Be prepared to re-locate components if the trace density is too high or is badly unbalancedacross the area of the board, or if critical leads become too long. The designer should beaware at all times, particularly with RF designs, that printed wiring has distributedresistance, inductance and capacitance. The effects of this may have to be allowed for inthe design.It is important that the manufacturing tolerances (line spacing, conductor width, etc.) aresatisfied – otherwise a PCB design may result that nobody can make. Hence the processspecification has to be known at the PCB layout stage. Most CAD systems differentiatebetween bus, track and power conductors. There are also options for minimizing definedtrack lengths and assigning connector pinouts to the rest of the system. Multi-PCBsandwiches (including daughter boards or piggy back boards) can be autorouted and theautorouter can ‘take over’ at any stage after manual placement and routing.Design Rule ChecksOnce you have completed your layout and interconnections, most PCB design programspermit you to run design rule checks to ensure that the manufacturing tolerances aresatisfied (e.g. the track width and spacing requirements) and that circuit and signalconnections are correct to the original circuit diagram. This is why the checking appliedto the original circuit schematic is so crucial.PlottingThe final task is to produce plotted artwork from which the PCBs can be manufactured.Nowadays it is usually not necessary for a designer to produce the original artwork, asdesign files can be transferred to PCB shops as disk files. The PCB shops generally preferto produce their own artwork directly from client disk files so that they can ensure thestandard of plotting meets their particular process requirements.For artwork to be produced, the PCB design has to be converted for photo-tooling. Thisimplies that the PCB design software must interface with a photoplotter, which is done bymeans of a so-called Gerber file. The layers of multilayer PCBs must be suitably definedas to order, and the dimensions must be defined in relation to a ‘datum point’ (where theELEC3017 Electrical Engineering Design 5 Printed Circuit Board Design
  • locator awl is later put for the ‘booking’). The details vary from plant to plant. Forexample some plants may require negative photo-tooling while others require positivephoto-tooling. The designer today typically produces plots of artwork only for checking orreference purposes, though in simple manufacturing processes the basic artwork for thecopper etching may be printed using a laser printer or a plotter.GENERAL PCB DESIGN PRINCIPLESDetermine Your Design StandardsIt is now time to determine and set down the design standards that you are going to applyto the PCB design. More details and options are given below, but an example set of designstandards for a digital logic design may be as follows: a) ICs will be logically laid out in an array fashion and oriented east-west on the PCB. b) Component side traces will run generally east-west with solder-side traces running north-south. c) IC pads will be oval in shape and 0.050” wide by 0.125” long and allow for pin-through connections (see diagram). This will allow one 0.015” wide conductor between pads with 0.017” track clearance on each side. d) Minimum track widths will be 0.015” and traces will be spaced on a basic 0.050” grid. e) Power and ground traces shall be 0.050” wide and run east-west between the IC pins on the component side of the PCB. These traces shall be connected in a grid fashion at the board edges to minimize lead inductances. f) 100 nF multilayer ceramic bypass capacitors shall be provided on the basis of one per IC package. These capacitors will be located close to each IC package. g) IC sockets shall be used and ICs shall be oriented in the same direction. h) etc ...Artwork Viewing ConventionThe usual design convention is that layouts are always viewed from the component side ofthe board. Adhering to this standard will avoid confusion and possible errors on the part ofboard manufacturers.Component OutlinesAt the start of the PCB layout design, select appropriate component outlines from thecomponent libraries supplied with the PCB design software. Be prepared to modify theseoutlines if necessary to conform to your basic design standards. For example, you mayneed to adjust the size and orientation of pads to suit non-plated-through designs.ELEC3017 Electrical Engineering Design 6 Printed Circuit Board Design
  • You may also need to create your own outlines if suitable components aren’t available inthe libraries supplied.Component PlacementComponents should always be mounted on the side of the PCB with the least amount ofconnecting tracks. If possible, they should be evenly distributed over the PCB. Heavycomponents should be placed near board supports whenever possible. The direction of air-flow and heat-sinking requirements will also influence component placement. Theplacement of some components may be externally constrained, e.g., because of front orback panel layouts. Placement techniques vary depending upon the nature of the circuitand the preferences or practices of individual designers, but mostly four basic componentplacement concepts are used, either independently or in combination: 1. Schematic Placement This is used primarily on low density analogue boards. Where the schematic has been drawn with a physical sense and has a minimum of interconnection crossovers, components can often be placed more or less as they are physically drawn on the circuit diagram. This scheme works particularly well where signal inputs can be placed along one edge of a board and the outputs along the opposite edge. 2. Peripheral Placement This method is appropriate when board edge connectors or other components that require a specific fixed location are used. These components are placed first and interconnecting components are placed radiating inwardly from the fixed component locations. 3. Central Placement This concept applies to boards that have complex multiple lead devices such as integrated circuits, relays or modules with supporting peripheral components. In this system, the multi-lead components are centrally placed with the supporting components placed radiating outwards from them. 4. Fixed Arrays This concept is typically used for straight digital logic boards comprising mainly integrated circuits. Here the ICs are logically placed in fixed patterns with a uniform space allotment relating to the number of leads per device.Wiring and Component OrientationIn general, when locating and orienting components and tracks, strive to achieve an orderlyappearance. The orientation should be made with an eye to logical and short connections.Components should be placed so that their major axis is parallel to a board edge and to theflow of cooling air where that is applicable. Also, to the extent that good functional designis not compromised, components should be placed either parallel (preferable) or at rightangles to each other, and with the same orientations for like components. In particular,ELEC3017 Electrical Engineering Design 7 Printed Circuit Board Design
  • polarized components should all be oriented in the same direction, and value codes andpolarity markings should be visible and readable from the same direction.On two-layer digital logic boards it is common practice to route all traces on one layer inone direction, and on the other layer to route all traces in the perpendicular direction. Thisscheme requires the use of more feedthroughs or “vias”, but in exchange will providemaximum routing flexibility, improve reliability, and usually increase circuit packingdensity.6. SOME PCB DESIGN GUIDELINESBoard SizeThere are a number of factors to consider in determining the size of a PCB. First toconsider are any mechanical constraints imposed by the Customer RequirementsSpecification – e.g. • Dimensional • Environmental (heat dissipation, sealing, etc) • Incorporation with other mechanical componentsNext to consider are any constraints imposed by the available manufacturing process – e.g. • Maximum blank sizes • Technology (single/double sided, multi-layer, plated-through or non-plated- through holes, etc.)Finally, estimate the area required by the components that have to be mounted, making areasonable allowance for the additional area required for connections around integratedcircuits and connectors. As a rule of thumb for a double-sided design, proceed as follows: • Compute the square area required for each type of component (including lead terminations) and multiply each type by the number of like components (square mils is often a convenient unit 2 ); • For integrated circuits and connectors, use the footprint area (including pins) + 50%; • Add the area required for board edges (clearances) and mounting hardware and/or heatsinks.If the area required from the above calculations is 80% or less of that available, then thelayout is most likely to be achievable. Anything more than 80% would require a carefulre-assessment and possibly would need a larger board size or a different approach such assplitting the design into two boards or going to multi-layers.Conductor Widths and Spacings2 1 square mil = 0.000001 in2 (i.e. 0.001 in × 0.001 in)ELEC3017 Electrical Engineering Design 8 Printed Circuit Board Design
  • There are a number of factors to be considered when specifying conductor trace widths andspacings. If a conductor width is too small, the track may become open circuit during orafter manufacture, or there may be heat problems if it carries too much current. However,it is advisable to avoid using conductors of larger than 0.5” width. If larger areas areneeded, such as for ground planes, then relieved areas should be incorporated to preventblistering and warpage during soldering.Conductor spacing is normally determined by considering peak voltage betweenconductors, the altitudes at which the circuit board will be in use, and the conformalcoatings to be applied to the board. Too narrow a spacing between conductors can giverise to voltage “arc over” or to short circuits due to solder bridging. Generally, excessivelywide widths and spacing can result in waste of space and material and hence unwarrantedcost. The golden rule is to maintain maximum size within the available area, consistentwith maximum trace widths and minimum spacing requirements, to achieve ease ofmanufacture and durability in usage.Conductor Cross SectionsWhere current carrying capacity is important, minimum conductor widths and thicknessesshould be checked. It is however often important that the inductance of power reticulationtraces be minimised, e.g., for digital circuit layouts, and this may dictate thicker traces thanthose chosen on the basis of current carrying capacity alone.Conductor Connections and RoutingThere are some “Dos” and “Don’ts” to be considered when joining traces and when joiningtraces to pads. A sample of these are shown in Figure 5.ELEC3017 Electrical Engineering Design 9 Printed Circuit Board Design
  • Figure 5. Connection Dos and Don’ts.Component Terminal HolesA printed circuit board should have a separate mounting hole for each component lead orterminal. The two basic types of terminal holes used are unplated holes and plated-throughholes (PTH). Un-plated or unsupported holes contain no conductive material, plating,solder or any type of reinforcement. They are usually drilled or punched into a PCB.Plated-through-holes begin as unsupported holes. Conductive material is then electricallydeposited or “plated” on the inside walls to form an electrical connection between thelayers of a board. The plating usually consists of tin-lead over electro-deposited copper.For the boards that you will be designing, you will be using unplated holes.As a guide, the following formula can be used to determine the minimum diameter of anunplated hole: Min. Hole Dia. = Max. Lead Dia. + Min. Drill Tolerance (adjusted to next larger standard drill size)Typically, minimum drill tolerances are ± 0.003” for holes up to 0.0226” dia. (23 AWG)and ± 0.004” for larger holes. Table 1 provides a convenient reference. In general,unplated holes should be no more than 0.020” greater than the minimum lead to beinserted.The number of different hole sizes on a circuit board should be kept to a minimum. As thenumber of different hole sizes increases, so does the cost and difficulty in manufacturingthe board.Terminal Areas and PadsA terminal area or pad is a portion of a printed circuit used for making electricalconnections between a component or wire and part of the conductive circuit pattern.Generally, pads completely surround and abut the mounting holes. Exceptions are whenELEC3017 Electrical Engineering Design 10 Printed Circuit Board Design
  • “flat pack” type components are to be mounted on the board surface. Terminal area shapesvary with designer preference, however there are specific advantages and disadvantages toeach particular shape. Square or rectangular shaped pads provide maximum adhesion ofthe copper pad to the circuit board and are useful when a large component hole is requiredwhere there is a minimum of useable terminal area space. However, these pads are moresusceptible to solder bridging when placed in close proximity to other pads or traces.Round or elliptical pads can be placed closer to other pads or traces with less risk of solderbridging. Terminal area size should be as large as practicable while maintaining minimumspacing requirements. The minimum pad area is based on: 1. The maximum hole size 2. Hole location tolerance 3. Pad area location tolerance 4. Conductor width tolerance 5. Minimum required annular ringTable 1 also shows suggested minimum pad area sizes for various conductor sizes forunplated holes. Note that these recommendations may need to be modified to suitparticular design requirements, such as running one or more traces between pads or wherea manufacturing process is used that is capable of finer lines and closer tolerances.Table 1. Hole Sizes and Terminal Areas for Unplated Holes Lead Size Rec. Hole Size Rec. Pad Size AWG Dia. Dia. Max. Pref. Standard Minimu Drill (mm) (mm) Tol. Pad Dia. Pad Dia. m (mm) Pad Dia. 34-29 .160-.287 0.368 0.076 #79 .100” .075” .0625” (0.7) * (0.7)* 28-23 .320-.574 0.71 0.076 #70 .115” .085” .075” (0.9)* (0.9)* 22-20 .634-.813 1.02 0.102 #60 .125” .100” .090” (1.0)* 19-17 .912-1.151 1.32 0.102 #55 .140” .110” .100” (1.3)* 16-15 1.29-1.45 1.59 0.102 #52 .150” .120” .110” (1.6)** Note that the metric sizes shown in brackets are more practical for single and double sided boards of the type made at UNSW.ELEC3017 Electrical Engineering Design 11 Printed Circuit Board Design
  • Dimensions and TolerancesFor more complete information on dimension and tolerance considerations for printedcircuit board design you are referred to the following publications: MIL-STD-275D MIL-P-13949E IPC-ML-910A IPC-D-300F IPC-D-320AGround PlanesA ground plane is a continuous conductive area used as a common reference point forcircuit returns, signal potentials, shielding or as a heat sink. Generally, to prevent blisteringand warping during soldering operations, any area larger than 0.5” diameter should bebroken up or relieved using some geometric pattern to achieve a non-conductive area equalto approximately 50% of the conductive area. An exception to this rule is where a shield isrequired for use with Radio Frequency designs. Provided the shield is on the componentsside, useful shielding can be obtained by employing the technique of providing a setminimum clearance around all pads and traces on the component side. Special treatment ofsoldered ground connections is required to avoid “heat sinking” of the terminal area duringsoldering with the ensuing risk of inferior soldered joints. Refer to Figure 6.Another special case often occurs with linear circuits such as opamps or audio circuitswhere particular ground configurations or “equipotential” or guard rails are required toprovide a shield between input and output circuits, particularly where high gain or lownoise operation is desired. Reference should be made to the manufacturer’s data sheetswhere often examples of suitable printed circuit layouts are given to suit the chip andapplication concerned. Figure 6. Ground Plane Considerations.When working with high frequency signals it is important to remember that tracks act likewaveguides. In this case, even the short connections between an IC and a ground planemay suffer from impedance mismatch effects. A shorted, near quarter wavelengthtransmission line has very large input impedance. This means that if your connection toELEC3017 Electrical Engineering Design 12 Printed Circuit Board Design
  • ground is on the order of λ/4, the connection will appear to be very poor indeed. To stayclear of such problems, it is recommended that connections be no more than λ/20 in length.At frequencies of 1 MHz, the wavelength is λ≈300 metres, so this is no problem. Atfrequencies of 1 GHz, however, the wavelength drops to 300 mm, meaning that you shouldtry to keep your connections to within about 15 mm in length!!Inter-Layer Connections in Two-Layer BoardsFor two-layer boards, there may not always be the facility for plated-through holes, so thatspecial consideration will be needed to effect connections between the solder andcomponent sides of the board. In this situation, the following techniques may be used: 1. Pin-Throughs Arrange opposing pads on both solder and component sides and solder together using a wire or special pin made for the purpose (e.g. Harwin pins). 2. Component Leads With forethought many of the component mounting leads can be utilized for interlayer connections by soldering the component lead on both sides of the board. 3. Links or Jumper Wires These are particularly useful to bridge data buses or densely populated wiring areas. Soldering both sides of the lead also offers interlayer connection possibilities. 4. IC Sockets While it is possible to solder both sides of IC pins to effect interlayer connections and mimic plated through boards, there is very little chance of successfully removing such an IC without damage to the board and the IC, if removal subsequently becomes necessary.For experimental or prototype boards where it is advantageous to be able to remove an ICfor testing or trouble-shooting, it is preferable to use IC sockets. To effect interconnectionsbetween solder and component layers using sockets it is possible to use a double-padarrangement, with one pad connected to the socket pin and the other nearby to allow for apin through to the other layer. This arrangement can mimic a proper double-sided plated-through-hole board design quite closely, with a small penalty to pay in terms of extra boardarea for pin-throughs.Component MountingUnless required by its function, no part of a component should protrude beyond the edge ofthe PCB. Usually a minimum clearance of say 0.062” should be maintained between boardedges and card guides or any other mounting hardware. Components weighing more than 7grams per lead should be supported by clamps or other means so that soldered joints arenot strained due to shock or vibration effects. All parts dissipating 1 watt or more shouldbe mounted away from the PCB so that no physical contact is made unless heat sinks areprovided. Any components with conductive cases should ideally be mounted at least0.062” away from conductive tracks (or more at high voltages or altitudes, or in theELEC3017 Electrical Engineering Design 13 Printed Circuit Board Design
  • absence of protective coatings). If minimal spacing must be used then some form ofadditional insulation is required. Horizontally mounted axial lead components should bemounted with the body of the part in contact with the PCB and clamped if the weight isabove that specified above. If axial components are to be mounted vertically then theyshould be spaced around 0.015” (min.) to 0.125” (max.) above the PCB to allow for goodsoldered joints and adequate cleaning. The highest point of the top lead should not extendmore than 0.550” above the board surface and may need to be insulated to prevent contactwith other components. The same comments regarding weight apply here.There are a number of recommendations from both IPC and MIL-STD about lead spacingof axial lead components. In general it is recommended that axial leads extend around0.060” straight out from the body of the component before the bend starts and that theminimum bend radius should be one to two times the wire diameter. To determine theminimum lead spacing, use the following formula: LSmin = CLmax + 2 × LE + 2 × BRmin + LDwhere: LS = Lead spacing (rounded up to the nearest standard grid increment). CLmax = Maximum component length (including coating meniscus or other excrescences). LE = Lead extension (0.030” min. to 0.060” preferred). LD = Lead diameter. BRmin = Minimum bend radius, calculated as follows: Condition BRmin LD < 0.027” 1 × LD 0.028” < LD < 0.047” 1.5 × LD 0.047” < LD 2 × LDAutomatic Component Insertion and Surface Mounted ComponentsMost of the foregoing is applicable for all types of PCBs, although the emphasis was onthrough-hole technology. However, there are additional factors to be considered when aboard is being designed for automatic (NC) component insertion and/or for use withsurface mounted components. We will not go into these here, but if this is contemplated infuture, then it would be advisable to obtain advice on layout requirements from theparticular board manufacturer before commencing the layout.ELEC3017 Electrical Engineering Design 14 Printed Circuit Board Design
  • REFERENCES[1] K. Brindley, Newnes Electronics Assembly Handbook, Butterworth-Heinemann, Oxford, 1993.[2] Printed Circuit Drafting Technical Manual and Catalog 107A, Bishop Graphics, 1985. This is unfortunately now out of print, but all the relevant information originated from the IPC and MIL references which follow.[3] Guide to Making Printed Circuit Boards, Dick Smith Electronics, Cat B-6005.[4] Definitions and Terms: MIL-STD-429 Printed Wiring and Printed Circuit Terms and Definitions. IPC-T-50 Terms and Definitions[5] Printed Circuit Design – Single-Sided and Two-Sided Boards: MIL-STD-275D, Printed Wiring. MIL-P-55110, Printed Wiring Boards. IPC-D-300, Printed Wiring Board Dimensions and Tolerances 3. IPC-CM-770, Guidelines for Printed Circuit Board Component Mounting.3 IPC stands for Institute for Interconnecting & Packaging Electronic Circuits, Evanston, IL USA.ELEC3017 Electrical Engineering Design 15 Printed Circuit Board Design