Fullscreen HTML5Med Res (??MB)HTML4

In this third part of our short PC board design feature, we look at the “other layers” which make up a PC board, along with more advanced layouts and ways to make your board acceptable to manufacturers. Part 3 – by David L. Jones I f you ask most hobbyists and even many professionals what constitutes a PC board, they’d probably say the copper tracks and the base on which they are etched. But there is often much more to a PC board than that. For a start, there are other layers. And we are not just talking about double-sided or multi-layer boards, either. Silk screen The “silk screen” layer is also known as the “component overlay” or “component layer”. It is the layer on the top of your board (and bottom if needed) that contains the component outlines, designators (C1, R1 etc) and free text. This is printed on your board using a silk screening process. White is a standard colour but other colours are available upon request. You can even mix and match colours on the one board but that usually costs extra. When designing your board, make sure that you keep all your component designators the same text (font) size and oriented in the same direction. When laying out your own component footprints, where possible, make sure that you add a component overlay that reflects the actual size of your component. This way you will be able to tell at a glance how close you can physically position your components. Ensure that 60  Silicon Chip all polarised components are marked and that pin 1 is identified. Your silk screen layer will be the most inaccurately aligned of all your layers, so don’t rely on it for any positional accuracy. Ensure that no part of the silk screen overlaps a bare pad. Apart from printing limitations and readability, there is no minimum width requirement for lines on the component overlay, so feel free to use smaller lines and text sizes to fit things in. If parts of the text or lines don’t turn out perfectly on your board then it does not affect your design, unlike tracks and pads. To avoid clutter, some designers don’t put component values on the silk screen, just the component designator. SILICON CHIP takes the opposite approach and uses the component values, not designators. This latter approach means that anyone checking the board does not have to refer back to the circuit or parts list to find the component values. Solder Mask A solder mask is a thin polymer coating on the board which covers everything except the pads. and helps prevent solder from bridging between pins and tracks. This is essential for surface mount and fine pitch devices. Your PC board program will automatically remove solder mask from the pads. The gap it leaves between the pad and the solder mask is known as the “mask expansion”. The mask expansion should usually be set to at least a few thou. Be careful not to make it too big or there might be no solder mask between very fine pitch devices. Your solder mask is displayed in your PC board package as a negative image, just like the power plane. Under normal circumstances you don’t “Inside” a multilayer PC board – in this case, four layers. Note the “vias” which connect all the layers together. www.siliconchip.com.au need to put anything on your solder mask layer. But if you want to leave the solder mask off a certain part of your board, you can place tracks and fills on your solder mask layer. Solder masks come in two types, silk screen or “photo imageable”. Photo imageable masks provide better resolution and alignment and are preferred over silk-screened. You can get different colour solder masks but the standard colour is green. On most standard quality boards, the solder mask is laid directly over the bare copper tracks. This is known as Solder Mask Over Bare Copper or SMOBC. You can get other coatings over your tracks in addition to the solder mask but these are usually for fairly exotic applications. Mechanical Layer The mechanical layer (which may go under other names depending on the package) is used to provide an outline for your board and other manufacturing instructions. It is not part of your actual PC board design but is very useful to tell the PC board manufacturer how you want your board assembled. There are no hard and fast rules for this layer. Use it however you like; just make sure www.siliconchip.com.au you tell your PC board manufacturer. Keepout The keepout layer generally defines areas on your board that you don’t want auto or manually routed. This can include clearance areas around mounting hole pads or high voltage components, for instance. Layer Alignment When the PC board manufacturer makes your board, there will be alignment tolerances on the artwork film for each layer. This includes track, plane, silkscreen, solder mask and drilling. If you don’t allow for this in your design and make your tolerances too fine, you can end up in big trouble. Consult the manufacturer for what alignment tolerances they can achieve, and also what alignment tolerance you are paying for! Netlists A netlist is essentially a list of connections (“nets”) which correspond to your schematic. It also contains the list of components, component designators, component footprints and other information related to your schematic. The netlist file can be generated by your schematic package. Generating a netlist is also called “schematic capture”. Your PC board package can then import this netlist file and do many things. It can automatically load all the required components onto your blank board. It can also assign a “net” name to each of your component pins. With nets assigned to your PC board components, it is now possible to Auto Route, do Design Rule Checking and display component connectivity. This is the fundamental concept behind modern Schematic and PC board CAD packages. Rat’s Nest Your job of component placement will be made infinitely easier by having a “rats nest” display enabled. If there is one reason for going to the trouble of drawing up an accurate schematic and importing a netlist, this is surely it. For large designs, a rat’s nest display is essential. A rat’s nest display is one where the program will draw a straight line (not a track) between the pads of components which are connected on the schematic. In effect, it shows the connectivity of your circuit before you start laying out tracks. At the start of your board layout, with all your components placed down randomly, this will appear as a huge and complicated random maze of lines. December 2003  61 Hence the name “rat’s nest”. The rat’s nest may look very daunting at first but when you move each component the lines will automatically move with them. In this way you can see instantly which components are connected to which, without having to refer back to the schematic and constantly cross-reference component designators. Once you have used this feature, you won’t want to live without it With the rat’s nest display enabled, it will be almost possible to lay out all of your components optimally in no time, without having to lay down one single track. The rat’s nest display will effectively show you what your tracks will connect to. The rat’s nest lines should disappear when you route your tracks between components, so your design will get less and less “complicated looking” as you go along. When all the rat’s nest lines disappear, your board is fully routed. make changes to your existing PC board layout via the schematic editor. The program will take your schematic netlist and component designators and import them into your PC board design and make any relevant changes. Some packages will also automatically remove old PC board tracks that are no longer connected. You can do this at any time during your PC board layout. If you update your schematic, then you must forward annotate into your PC board design. You can do edits like this manually but forward annotation automates the process. Back Annotation is when you change one of the component designators (eg, C1 to C2) on your PC board and then automatically update this information back into your Schematic. More advanced back annotation features allow you to swap gates on chips and perform other electrical changes. There should never be much real need to use back annotation. Design rule checking Multi-layer PC board design Design Rule Checking (DRC) allows you to automatically check your PC board design for connectivity, clearance and other manufacturing errors. With the large and complex PC boards being designed today, it is impractical to manually check a PC board design. This is where the DRC comes into its own; it is an absolutely essential step in professional PC board design. Examples of what you can check with a DRC are: - Circuit connectivity. It checks that every track on your board matches the connectivity of your schematic. - Electrical clearance. You can check the clearance between tracks, pads and components. - Manufacturing tolerances like min/max hole sizes, track widths, via widths, annulus sizes and short circuits. A complete DRC is usually performed after you have finished your PC board. Some packages even have the ability to do “real time” (or “online”) DRC checking as you create your board. For instance, it won’t let you connect a track to a pad it shouldn’t go to, or violate a clearance between track and pad. If you have real-time DRC capability, use it; it’s an invaluable tool. A multi-layer PC board is much more expensive and difficult to manufacture than a single or double-sided board but it really does give a lot of extra density to route power and signal tracks. By having signals running on the inside layers of the board, you can pack components more tightly to give a more compact design. Deciding to go from double-sided to multi-layer can be a big decision, so make sure that a multi-layer board is warranted on the grounds of board size and complexity. You can forget about making multi-layer boards yourself - it requires a commercial manufacturer. Most of the hobby board suppliers will not do multi-layer boards. Multi-layer boards come in even numbers of layers, with 4, 6 and 8-layer being the most common. With a multi-layer board, you would typically dedicate one layer to a ground plane and another to your power, with perhaps a few signal tracks thrown on the power layer if you need to. If you have a digital-only board, then you’d often dedicate the entire power layer also. If you have room on the top or bottom layer, you can route any additional power rail tracks on there. Power layers are almost always in the middle of the board, with the ground closer to the top layer. Once you have your power taken care of on the inner layers, you’ll be Forward and back annotation Forward Annotation is when you 62  Silicon Chip surprised at the room you now have available for your signal tracks. It really does open up a whole new dimension to routing. If power planes are vital and you have a lot of connections to route, then you may have to move from four to six layers. Six layers will give you four full signal routing layers and two layers dedicated to power. You can really do some advanced routing with six layers. Eight layers and above is basically more of the same. Multi-layer design brings the options of using different types of vias to improve your routing density. There are three types of vias - standard, blind and buried. Standard vias go through the whole board and can connect any of the top, bottom or inner layers. These can be wasteful of space on layers which aren’t connected. “Blind” vias go from the outside surface to one of the inner layers only. The hole does not protrude through the other side of the board. The via is in effect “blind” from the other side of the board. “Buried” vias only connect two or more inner layers, with no hole being visible on the outside of the board. So the hole is completely buried inside your board. Blind and buried vias cost more to manufacture than standard vias. But they are very useful and almost mandatory for very high-density designs like those involving Ball Grid Array (BGA) components. Power planes It is good practice to use “power planes” to distribute power across your board. Using power planes can drastically reduce the power wiring inductance and impedance to your components. This can be vital for high-speed digital design, for instance. It is good design practice to use power planes whenever possible. They can even be used on double-sided boards, if most of your signal tracks are on the top layer. A power plane is basically one solid copper layer of board dedicated to either the Ground or Power rails, or both. Power planes go in the middle layers of the board, usually on the layers closest to the outer surfaces. On a 4-layer board with complex power requirements, it is common to dedicate one layer to the ground plane and another layer to various positive and negative power tracks. The ground rail www.siliconchip.com.au is usually your signal reference line, so a ground plane is first preference before a power plane is considered. Many PC board packages have special Power Plane layers that are designed and laid out in reverse to the other normal tracking layers. On a normal tracking layer, your board is assumed to be blank and you then lay down tracks which will become your actual copper tracks. On a power plane however, your board is assumed to be covered with copper. Laying down tracks on a power plane actually removes the copper. This concept can take some getting used to. A simple power plane will not have any “tracks” (or removed copper bits) at all on it but will just be one solid layer of copper. In which case you don’t need to lay down any tracks to remove any copper. However, it is common practice on more complex boards to “split” the power plane by laying down tracks. This may be done to separate an analog and a digital ground, which will reduce the amount of digital ground noise which is coupled into the more sensitive analog circuitry. A typical split power plane would involve a “track” being placed from near your input power connector or main filter capacitors and the opposite edge of the board. Be careful not to accidentally cause a power “loop” on your board by inadvertently connecting the two halves of your plane on the other side of the board. As a matter of course, you should place “tracks” completely around the outer edge of your board. This will ensure that the power planes do not extend right to the edge of the board. Power planes on the edges of your board can not only short to one another but also to any guide rails or mounting hardware. You don’t have to use the actual Power Plane layer on your PC board package if you don’t want to. You can use a regular signal layer and lay down copper fills and tracks yourself. Power Planes layers though often have some advantages that will vary from one PC board package another. practices to incorporate into any design. • Use copper, and lots of it. The more copper you have in your ground path, the lower the impedance. This is highly desirable for many electrical reasons. Use polygon fills and planes where possible. • Always dedicate one of your planes to ground on multi-layer boards. Make it the layer closest to the top layer. • Run separate ground paths for critical parts of your circuit, back to the main filter capacitor(s). This is known as “star” grounding, because the ground tracks all run out from a central point, often looking like a star. In fact, try and do this as matter of course, even if your components aren’t critical. Separate ground lines keep current and noise from one component from affecting other components. • If using a ground plane, utilise “split” plane techniques to give effective star grounding. • “stitch” required points straight through to your ground plane; don’t use any more track length than you need. • Use multiple vias to decrease your trace impedance to ground. Good bypassing Active components and points in your circuit which draw significant switching current should always be “bypassed”. This is to “smooth” out your power rail going to a particular device. “Bypassing” is using a capacitor across your power rails as physically and electrically close to the desired component or point in your circuit as possible. A typical bypass capacitor value is 100nF (0.1uF), although other values such as 1uF, 10nF and 1nF are often used to bypass different frequen- cies. You can even have two or three different value capacitors in parallel. When bypassing, you CANNOT replace multiple capacitors with one single capacitor; it defeats the entire purpose of bypassing! It is not uncommon for a large design to have hundreds of bypass capacitors. As a general rule, you should use at least one bypass capacitor per IC or other switching component if possible. Common values of bypass capacitors are 100nF for general purpose use, 10nF or 1nF for higher frequencies, and 1uF or 10uF for low frequencies. Special low Equivalent Series Resistance (ESR) capacitors are sometimes used on critical designs such as switch mode power supplies. HF design techniques High frequency design is where you really need to consider the effects of parasitic inductance, capacitance and impedance of your PC board layout. If your signal is too fast, and your track is too long, then the track can take on the properties of a transmission line. If you don’t use proper transmission line techniques in these situations then you can start to get reflections and other signal integrity problems. A “critical length” track is one in which the propagation time of the signal starts to get close to the length of the track. On standard FR4 copper boards, a signal will travel roughly 15cm every nanosecond. A rule of thumb states that you need to get really concerned when your track length approaches half of this figure. But in reality it can actually be much less than this. Remember that digital square wave signals have a harmonic content, so a 100MHz square wave has harmonic Good grounding Grounding (or earthing) is fundamental to the operation of many circuits. Good or bad grounding techniques can make or break your design. There are several grounding techniques which are always good www.siliconchip.com.au December 2003  63 components extending into the GHz region. In high-speed design, the ground plane is fundamental to preserving the integrity of your signals and also to reducing EMI emissions. It allows you to create “controlled impedance” traces, which match your electrical source and load. It also allows you to keep signals coupled “tight” to their return path (ground). There are many ways to create controlled impedance “transmission” lines on a PC board. But the two most basic and popular ways are called Microstrip and Stripline. A Microstrip is simply a trace on the top layer, with a ground plane below. The calculation involved to find the characteristic impedance of a Microstrip is relatively complex. It is based on the width and thickness of the trace, the height above the ground plane and the relative permittivity of the PC board material. This is why it is important to keep the ground plane as close as possible to (usually) the top layer. A Stripline is similar to the Microstrip, but it has an additional ground plane on top of the trace. So in this case, the trace would have to be on one of the inner layers. The advantage of stripline over microstrip is that most of the EMI radiation will be contained within the ground planes. There are many free programs and spreadsheets available that will calculate all the variations of Microstrip and Stripline for you. Some useful information and rules of thumb for high frequency design are: • Keep your high frequency signal tracks as short as possible. • Avoid running critical high frequency signal tracks over any cutout in your ground plane. This causes discontinuity in the signal return path, and can lead to EMI problems. Avoid cutouts in your ground plane wherever possible. A cutout is different to a split plane, which is fine, provided you keep your high frequency signal tracks over the relevant continuous plane. • Have one decoupling capacitor per power pin. • If possible, track the IC power pin to the bypass capacitor first, and then to the power plane. This will reduce switching noise on your power plane. For very high frequency designs, taking your power pin directly to the 64  Silicon Chip power plane provides lower inductance, which may be more beneficial than lower noise on your plane. • Be aware that vias will cause discontinuities in the characteristic impedance of a transmission line. • To minimise crosstalk between two traces above a ground plane, minimise the distance between the plane and trace and maximise the distance between traces. The coefficient of coupling between two traces is given by 1/(1+(Distance between traces / height from plane)2). • Smaller diameter vias have lower parasitic inductance and are thus preferred for higher frequency circuits. • Do not connect your main power input connector directly to your power planes; take it via your main filter capacitor(s). Double-sided loading Loading components on both sides of a PC board can have many benefits. Indeed, it is becoming an increasingly popular and necessary option when laying out a board. There are two main driving factors behind a decision to go with doublesided loading. The first is that of board size. If you require a particular board size and all your components won’t fit on one side, then double-sided loading is an obvious way to go. The second reason is that it is required to meet certain electrical requirements. Often these days, with dense high speed surface mount devices packed onto a board, there is either no room for the many bypass capacitors required or they cannot be placed close enough to the device to be effective. Ball Grid Array (BGA) devices, for example, benefit from having the bypass capacitors on the bottom of the board. Indeed, it is common to find double-sided loaded boards with nothing but bypass capacitors mounted on the back. This allows the bypass capacitor to be as close to the physical device power pin as possible. Be sure to involve your PC board assembler in discussions during the layout of your board. There are many things you can and can’t do with double-sided loading. Auto routing “Real PC board designers don’t auto route!” is an age-old war cry. While many will claim this is true, reality may often kick in and there certainly are times when you do need to consider the use of an auto router. Auto routing is the process of getting the PC board software to route the tracks for you. It will even attempt to route your entire board if you let it. Most of the medium to top range PC board packages will do this and the technology and theory behind autorouting techniques can be mind-boggling. Artificial intelligence and neural-based technology are some of the marketing buzz words used. If the PC board program can route the board for you, why not always use it? Doesn’t it just automate a mundane process like laying down tracks? The answers can be complicated and many but no matter how “smart” an auto-router is, it simply cannot replace a good human PC board designer. It is like trying to ask a computer program to paint a picture for you. If you give it enough information it may to able to produce something legible but it won’t be artistic and certainly won’t be a Mona Lisa. Many people think that auto-routers are a tool to help not-so-experienced PC board designers. In fact, the opposite is true! In the hands of an inexperienced designer, an auto router will produce a complete mess. But in the hands of a very experienced designer, an auto router can produce excellent results much quicker than the human designer could do. Auto routers come in handy when you have complex boards with not much routing space, on non-critical parts of your layout. Non-critical parts of a board might include low frequency or static control signals to components like LED displays, switches and relays. Advanced auto-routers do come with tools to let you specify exactly how you want electrically important tracks laid out. But by the time you have told it in excruciating detail what to do with every track, you could have laid it out yourself! Never use an auto-router to do your complete board; it will be a mess. But if you let it loose on a very specific non-critical area of your board, you can get some excellent results, sometimes indistinguishable from manual routing. You can even auto-route a single connection, and this is sometimes handy when you are having trouble finding routing space in the final phase of your layout. www.siliconchip.com.au 100 95 experienced at PC board design, Unless you are very simply stay away from auto-routers. This cannot be stressed 75 enough. Off the shelf and custom embedded controllers for OEMs Auto Placement Design for manufacturing 25 www.siliconchip.com.au 5 0 for the real world SPLat is the innovative Australian programmable controller system that’s been adopted by major OEMs world-wide. The SPLat MMi99DK216 combines a powerful controller and an operator interface into a single cost-effective package. The operator interface consist of 5 push buttons, 7 LEDs, a beeper and a 2 line by 16 character LCD. The polyester overlay is easily tailored with your own legends. The controller function has 8 digital inputs, 8 digital outputs, 2 analog inputs and 2 analog outputs. If you need more I/O we have a range of matching add-on and expansion boards, giving you a potential capacity of over 40 inputs and 40 outputs. All I/O is fully “real world” interfaced. MMi99DK216: MMi99DK: MMi99OEM: $395 (As described above) $329 (Without LCD) $186 (Board only, 100+) Quoted prices include GST. We accept all major cards. S&H $15 Made in Australia by SPLat Controls Pty Ltd 2/12 Peninsula Blvd Seaford VIC 3198 Ph 03 9773 5082 Fax 03 9773 5091 in ussie nova A t tion Panelisation: If you are looking at getting your board automatically assembled with a pick-and-place machine, then it pays you to get as many boards onto the one “panel” as you can. A panel is simply a large PC board containing many identical copies of your board. It takes time to place a board into position on a pick and place machine, so the more boards you can load at once, the more cost effective your manufacturing will be. A panel will also contain tooling strips on the top and bottom, to allow for automated handling of the panel. Different manufacturers may have different maximum panel sizes they can produce. Each individual board can be “routed out” and joined with “breakout tabs” or simply butted together and scoured out with a “V groove”. A V groove is a score mark placed on your board that allows you to easily “snap” the board along the groove. A breakout tab is a small strip of board perhaps 5-10mm long joining your board to your panel. Small non-plated holes are also drilled along this strip which allows the board to be snapped or cut out of the panel after assembly. You will need to consult your board loader to determine optimum panelisation size and requirements. Tooling Strips: Tooling strips are strips of blank board down the top and bottom side of your board. They contain tooling holes, fiducial marks and other manufacturing information if required. Standard tooling holes are required for automated handling of your board. 2.4mm and 3.2mm are two standard hole sizes. Four tooling holes per panel is sufficient, one in each corner. The tooling trips connect to your board(s) with breakout tabs or V Grooves. Fiducial Marks: Fiducial marks are visual alignment aids placed on your PC board. They are used by automated pick and place machines to align your board and find reference points. A video camera on the machine can identify the centre of 100 fiducial marks and use these points as a reference. On a panel there should be three fiducial marks, known 95 as global fiducials. Bottom left/right and top left corners. They should be at least 5mm away from the board edges. 75 They can be mounted on the tooling strips. The fiducial mark should be a circular pad on the copper layer of diameter 1.5mm typically. The fiducial should not Programmable controllers Gre a Auto Placement tools are available in many higher end 25 PC board packages. Professional PC board designers do not use Auto Placement 5tools; it’s that simple. Don’t rely on the Auto Place feature to select the most optimum layout for you. It will never 0work (unless it’s an extremely simple board), regardless of what the program makers claim. These tools do have one useful function however. They give you an easy way to get your components initially spread across your board. Visit our website for free software, our renowned training ecemberdocumentation 2003  65 course and complete onlineDproduct www.splatco.com.au be covered with solder mask and the mask should be removed for a clearance of at least 3mm around. The pad can be bare copper or coated like a regular pad. Two local fiducial marks (in opposite corners) are also required next to each large fine-pitch surface mount device package on your board. Thermal Relief: If you solidly connect a surface mount pad to a large copper area, the copper area will act as a very effective heat sink. This will conduct heat away from your pad while soldering. This can encourage dry joints and other soldering related problems. In these situations a thermal relief connection, which comprises several (usually four) smaller tracks connecting the pad to the copper plane. Thermal relief options can be set automatically in many packages. Soldering: Soldering considerations need to be taken into account when laying out your board. There are three basic soldering techniques: hand, wave, and reflow. Hand soldering is the traditional method typically used for prototypes and small production runs. Major impacts when laying out your board include suitable access for the iron and thermal relief for pads. Non-plated through double-sided boards should allow for ample room to get the soldering iron onto the top-side pads. Wave soldering is a common process used for surface-mount and throughhole production soldering. It involves passing the entire board over a molten bath of solder. Solder masks are absolutely essential here to prevent bridging. The major thing to watch out for when designing is ensuring that small components are not in the wave solder “shadow” of larger components. The board travels through the wave solder machine in one direction, so there will be a lack of solder trailing behind larger components. Surface mount devices are fixed to the board with an adhesive before wave soldering. Reflow soldering is the latest technique and is suitable for all surface mount components. The blank board is first coated with a mask of solder paste over the pads (solder “stencils” are used for this). Then each component is placed, and is sometimes held in place by an adhesive. The entire board is then loaded into an infrared or 66  Silicon Chip nitrogen oven and “baked”. The solder paste melts (reflows) on the pads and component leads to make the joint. A newer reflow method called pin-inpaste or intrusive reflow is available for through-hole devices. Combinations of wave and reflow soldering can be used for mixed through-hole and surface-mount boards. Wave soldering has the advantage of being cheap but the disadvantage of imposing placement limits on your components. Reflow soldering is more complex and expensive but it allows for very dense surface mount packing. consumer products due to their low cost. They are not suitable for plated-through holes or fine tolerance designs. A blank base material coated with copper is known as a copper clad board. A multi-layer board is made up of various individual boards separated by Pre-impregnated Bonding Layers, also known as “prepreg”. There are different ways to stack these board layers up and this will dictate what you can do with planes and blind/ buried vias. Consult the manufacturer for their recommendations on this. Basic PC board manufacture Surface finishes A PC board usually consists of a blank fibreglass substrate (“the board”), which is usually 1.6mm thick. Other common thicknesses are 0.8mm and 2.4mm. There are many types of PC board substrate material but by far the most common is a standard woven epoxy glass material known as FR4. This material has standard known properties, typical values of which are shown in the accompanying table. The most often-used parameter is probably the dielectric constant. This figure is important for calculating high-speed transmission line parameters and other effects. An FR4 PC board is made up of glass and resin. Glass has a dielectric constant of approximately 6, and the resin has a dielectric constant of approximately 3. So an FR4 PC board can typically have a figure ranging from under 4, to almost 5. If you need an exact figure you will have to consult with your PC board manufacturer. You can get your PC board manufactured with several different types of pad and track surface finish. Low cost single and double-sided boards without a solder mask typically have a roll solder finish on the copper tracks (commonly referred to as “tinned”). Beware of potential shorts between tracks with this method. More expensive boards will typically have solder mask over bare copper (SMOBC) tracks and rolled solder (tinned) on the pads and vias which is Hot Air Leveled (HAL). Hot air leveling helps surface-mount components to sit flat on the board. For large and critical surface mount components, a gold “flash” finish is used on the pads. This gives an extremely flat surface finish for dense fine pitch devices. Peelable solder masks are available and are handy for temporary masking of areas on your board during wave soldering or conformal coating. Typical FR4 Properties Dielectric Constant...... 3.9 to 4.8 Dielectric Breakdown.. 39kV/mm Water Absorption........ <1.3% Dissipation Factor........ 0.022 Thermal Expansion..... 16-19ppm/°C NOTE: These values can vary with manufacturers; check with your supplier for exact figures. Other exotic base materials like Teflon are also available but are only used for special designs that require a higher grade base material for a specific reason. There are cheaper materials than FR4, like phenolic base and CEM-1. These are hobbyist-grade boards but are also often used in some mass Electrical testing You can have your finished PC board checked for electrical continuity and shorts at the time of manufacture. This is done with a automated “flying probe” or “bed of nails” test machine. It checks that the continuity of the tracks matches your PC board file. It may cost a fair bit extra but this is mandatory for multi-layer boards. If you have a manufacturing error on one of your inner layers, it can be very difficult to fix. Signature Like any work of art, no board is complete without adding your name or signature to it! The signature can take any form your like. Some people put www.siliconchip.com.au their name, initials or a fancy symbol. Whatever it is, just make sure you add something. A signature can be placed on any of the copper layers or on the component overlay. Submitting your design for manufacture The first thing to know is which format to send your PC board file in. In Australia the standard format is any version of Protel (AutoTrax, PFW2.8, 99SE, DXP etc). Every manufacturer in Australia will happily take a Protel file. In fact, Protel format is their preferred way to receive a file. Many will also take other proprietary formats as well but you’ll have to check with them first. Supplying the original PC board package file will ensure that what you see on the screen is what you will get when your board is delivered. Unless you have a good reason to do so, don’t supply your file in any other format. Gerber plot files are the traditional and industry recognised file format and all major manufacturers will accept them. Many PC board designers still insist on generating and supplying Gerber files themselves, in order to have total control over the manufacturing process. In all but a few cases, generating Gerber files is not necessary and a thing of he past. Generating Gerbers adds an extra step of complexity to the PC board process where errors can creep in. So avoid the use of Gerber files where possible; they can be troublesome unless you know exactly how to generate them correctly. The manufacturer will ask for a lot of information before they quote. Ask them what you need to provide with your file. Here is a basic checklist: • A reference code and revision for your board. This makes it easy for both parties to track the progress of it. • Desired manufacturing time, known as the “turn-around”. 24 www.siliconchip.com.au hours will cost a LOT more than 2 weeks! • Quantity of boards required • Board thickness (1.6mm, 0.8mm, 2.4mm etc). 1.6mm is standard • Type of board (FR4, Teflon etc). FR4 is standard Number of layers • • Surface finish (SMOBC, HAL, Gold Flash etc). SMOBC and HAL is standard. • What colour you want your solder mask and component overlay. • Copper weight (1oz, 2oz etc). 1oz is standard. Whether or not you want electrical • testing. • The Track/Space clearance of your board • How your board dimensions are defined, eg, on the mechanical layer. • Whether you want boards “panelised” or individually cut. Many manufacturers will have “prototype” services where they fit as many of your boards onto a standard “panel” as they can, all for one fixed price. In most cases you will be charged a “tooling” cost. This is the cost of printing the photo masks for your board and also setting up their machines. This is usually a one-off cost, so if you get the same board manufactured again, you won’t have to pay the tooling charge. Do you believe that is all there is to know about PC board design? If you answered no, then you’d be right! Good PC board design takes lots Ozitronics www.ozitronics.com Tel: (03) 9434 3806 Fax: (03) 9434 3847 Email: sales<at>ozitronics.com USB 'Flash-Only' PIC Programmer For 'Flash' type PIC devices only. Truly portable - powered from USB port. Box supplied. USB type A connector. ZIF socket not included. K128 - $68.20 USB & Serial Port PIC Programmer USB/Serial connection makes it ideal for field use. Supports ICSP. USB type A connector. ZIF socket not included. 17VDC K149 - $68.20 USB only PIC Programmer Similar to K149 but without serial connection. Supports Low-Voltage ICSP. USB type B connector. ZIF socket not included. 17VDC K150 - $68.20 ATMEL 89xxx Programmer Uses serial port. No special programming software required. 4 status LEDs. ZIF sockets not included. 16VDC. K123 - $75.90 Programmer Accessories: 40-pin Wide ZIF socket (Z6) - $33.00 20-pin ZIF socket (Z5) - $22.00 USB cables (2M) - $11.00 Prices include GST - shipping extra. Full documentation available from website. of experience, so go get started on your next board using our tips. Next month, we’ll look at using the popular “Autotrax” and “Easytrax” PC SC board software. December 2003  67