Fullscreen HTML5Med Res (??MB)HTML4

By NICHOLAS VINEN Lots of new features in . . . Altium Designer 2013 PCB layout software Altium Designer is the successor to the popular Autotrax and Protel ECAD (Electronic Computer-Aided Design) programs but it has a lot more features and capabilities than its predecessors. We take a look at the latest version and detail some of its best features for circuit design and PCB layout. I N THE NOVEMBER 2010 issue of SILICON CHIP, we reviewed Altium Designer Summer ’09, along with the NanoBoard 3000 hardware. At the time, we had had about a month to try out Altium Designer but hadn’t done a lot of serious work with it. Since then, the software has gone through a number of revisions and we have used it extensively for PCB layout. While it has a lot more capabilities than just PCB layout – including circuit simulation and microcontroller/FPGA programming – we tend to mostly use it for drawing up circuits and subsequently laying out PCBs to implement them. We recently decided to take another look at Altium Designer, for two reasons. Firstly, because a number of new features and improvements have been made in the last three years and secondly, because we now have more experience with Altium and this has 82  Silicon Chip given us further insight into its particular strengths and weaknesses. To recap briefly, for those who are unfamiliar with Altium, it is a high-end piece of electronics design software which runs exclusively on Windows computers and is used by many businesses and individuals to design products ranging from a single component on a small board up to monsters with thousands of components and many layers. It is the successor to Protel and inherits much of its predecessor’s design philosophy while adding a lot more. New features While there have been many updates to Altium Designer since we originally looked at it, AD13 is the first major update in a few years. It is installed as a new piece of software, rather than just updating the previous version and it introduces a number of new features. But upon investigation, we realised that most of the improvements since AD09 have been introduced incrementally over the intervening time and these in total have resulted in an overall substantial improvement in Altium Designer. One feature missing from Altium Designer that has finally been added in the latest update is layer transparency (see Fig.1). You can now set the transparency for any visible layer as a percentage, allowing layers beneath to be seen through it rather than obscured by it. This has a couple of important benefits. Firstly, when doing tricky routing jobs, it’s helpful to be able to see all the layers at once so that you can figure out whether a complex route (possibly involving multiple vias and tracks on many different layers) will work or whether there are too many obstacles in the way. Previously, this siliconchip.com.au required flipping between these layers to make each in turn the top-most, so you could see them in their entirety. The transparency also allows you to better see just how multiple track segments in a single layer overlap. This can be important since Altium can automatically move and re-route tracks but only as long as they are continuous and it’s quite easy to get into a situation where two tracks appear to be joined but there is a small gap or overlap in the middle so they are considered separate. With transparent tracks, it’s easier to find such situations and fix them. Active Bill of Materials This feature has just been introduced with AD version 13.3 and ties in with the existing Vault and Bill of Materials systems, which were already quite powerful. Basically, what it lets you do is shop for components for your design from within Altium and then associate a given component in your design to the model and get supplier information such as price and stock as well as specifications, images, etc (see Fig.2). This can be used to fill in data on Fig.1: close-up of a mixed throughhole/surface mount PCB design with the new layer transparency feature enabled. Tracks on all layers can be seen, through pads or tracks on the currently selected layer. the schematic, generate a total cost for the project and ultimately produce a list of parts to order. The latest update also improves the very useful PDF export feature, which we’ll explain briefly below. Other useful features Over the years of using Altium Designer, we’ve found some things that it is particularly good at doing. In many cases, these features are not available with other ECAD (Electronics Computer Aided Design) packages. Here is a list of those we consider most useful, in no particular order (we won’t go into much detail on basic tasks such as placing components – those are things that just about any ECAD package can do and haven’t changed much since our last review): • The ability to push tracks and vias, during and after track routing: this has come in very handy on a number of occasions. Compare Figs.1 & 3. All we did to change the PCB was click on the lower via to the left of Q28 (labelled “PIN10”) and drag it up and to the right. If there’s room, Altium will then re-route tracks around it and even push some aside (eg, the blue track labelled “PIN2”) but only as much as Fig.2: Active Bill of Materials links your design to part suppliers, giving access to real-time data on pricing and stock. This data can then be used to generate an overall price for manufacturing the design, as well as making sure that all the parts you need are available in sufficient quantities. siliconchip.com.au September 2013  83 Fig.3: the same PCB as shown in Fig.1 but here we have dragged the “PIN10” via up and to the right. Note how nearby tracks have been automatically moved to make room for it. Doing this manually can be time-consuming on a large, complex design. necessary. We cleaned up the result a bit to remove unnecessary wiggles in the track but that was only a few seconds of extra work. You can do something similar with tracks too; simply select one and then drag it and it will move adjacent tracks as it is dragged, if necessary. You can even re-order tracks like this in some cases, eg, when the other track emerges from a via and the track you are dragging can go around either side. Of course, you could do this all manually but it would be quite a lot of work; PCB layout is an iterative process for all but the simplest designs and when using other ECAD packages, we’ve spent hours ripping up and relaying tracks before we found the best routing solution. With Altium, this same job can take minutes if you take advantage of its ability to push and re-route tracks for you. Altium can also potentially move tracks while you are placing a new one, as long as you are using the “HugNPush” mode. In this mode, as you move the mouse alongside another track, it will place the new one at a safe distance (ie, adhering to your minimum clearance rules) but if you try to move the new track through a gap that is too small, Altium will move tracks that are in the way (if possible) to make room. • Searching for items on the PCB based on their characteristics and doing mass changes. Again, this is a real time-saver in some situations compared to other packages which require you to manually and laboriously change every single one. For example, let’s say you design a PCB to be manufactured in a particular factory then you move production to another factory which has a larger minimum via size. Your design may have hundreds or even thousands of vias. With Altium you can right-click on one, select “Find Similar Objects” and you are then presented with a dialog which allows you to choose which criteria to select – object type, layer, hole size and so on. Upon clicking “OK”, all matching objects are selected. You can then use the PCB Inspector (see Fig.4) to alter their properties en masse. In this case, you would simply type a new value into the “Hole Size” input box and press Enter and the hole size of all selected vias would change to the new value. You could also change the via pad size at the same time, if necessary. Any clearance violations which result from this are then highlighted and you can then fix them by, say, moving the vias (Fig.5). This same process can be used to change text label fonts, line widths, pad shapes – all manner of object properties. • TrueType fonts on PCBs: this is a simple feature (to use, anyway) but can make your PCBs look a lot more classy. We still tend to use the default vector font for component values and so on as it keeps file sizes small and it’s relatively easy to read. TrueType fonts are great for labelling the board with its product name, company logo and so on, for a really professional presentation. • 3D view: not as pointless a feature as it may at first seem. You need to use components with 3D models (or make your own) but once you do, all Fig.4: a “zoomedout” view of the same PCB as shown in the earlier figures with all vias selected, using the “Find Similar Objects” dialog. The properties of the objects can then all be changed at once using the PCB Inspector dialog, shown here. In this case, we can change the via drill size, copper diameter, tenting (whether or not they are covered with solder mask), net membership and other properties. 84  Silicon Chip siliconchip.com.au Fig.5: after increasing the hole size and diameter for all vias, some are now too close to adjacent tracks or pads so these have been highlighted in green. This is the “online design rule check” feature in operation. You can also get a list of violations and zoom in to see each one in detail. Each individual violation can be fixed by moving one or more of the components which are too close together, as set by your chosen design rules. you need to render your board in 3D is a single key press. This can be used to check component fit, especially for those which have an overhang. It can also be used to make sure that the board and its components will fit in a specific case, with the shafts and LEDs lining up with the appropriate holes and so on. It’s also a great tool to show clients what a design will look like before it has actually been built. Compare the 3D rendering of our CLASSiC DAC board (Fig.6) to the adjacent photo we published from a similar angle. It’s a pretty good match. Note that we built all the 3D models ourselves, as we are using a custom library. These are all built from vertical extrusions, cylin- ders and spheres. More advanced 3D models are possible if you have access to 3D “STEP” models (Standard for the Exchange of Product model data). • Complex design rules: design rules (minimum clearance, minimum track width, minimum hole size, etc) can depend on object attributes such as net membership. For example, say you are laying out a PCB with high-voltage and low-voltage sections. You need different track clearance rules depending on whether the two tracks in proximity are low-voltage, high-voltage or one of each. In many PCB layout programs, you have to check this manually, eg, set the track clearance to the minimum for the low-voltage section and then check each high-voltage track in turn to ensure it is far enough away from any low-voltage tracks. But in Altium you can set up multiple rules so that this happens automatically and you will be alerted if any given pair of tracks are too close for safety. For those who aren’t familiar with the terminology, we should point out that a “net” is a collection of component pins and tracks which are electrically connected. An Altium schematic drawing can be used to automatically generate a list of nets (“netlist”) and this is brought into the PCB layout, both to act as a guide during layout and in order to perform the Design Rule Check (DRC) which alerts you to short circuits between nets, nets which Radio, Television & Hobbies: the COMPLETE archive on DVD YES! A MORE THAN URY NT QUARTER CE ICS ON OF ELECTR HISTORY! This remarkable collection of PDFs covers every issue of R & H, as it was known from the beginning (April 1939 – price sixpence!) right through to the final edition of R, TV & H in March 1965, before it disappeared forever with the change of name to EA. For the first time ever, complete and in one handy DVD, every article and every issue is covered. If you’re an old timer (or even young timer!) into vintage radio, it doesn’t get much more vintage than this. If you’re a student of history, this archive gives an extraordinary insight into the amazing breakthroughs made in radio and electronics technology following the war years. And speaking of the war years, R & H had some of the best propaganda imaginable! ONLY Even if you’re just an electronics dabbler, there’s something here to interest you. 62 $ Please note: this archive is in PDF format on DVD for PC. Your computer will need a DVD-ROM or DVD-recorder (not a CD!) and Acrobat Reader 6 or above (free download) to enable you to view this archive. This DVD is NOT playable through a standard A/V-type DVD player. 00 +$10.00 P&P Exclusive to: HERE’S HOW TO ORDER YOUR COPY: SILICON CHIP siliconchip.com.au BY PHONE:* (02) 9939 3295 9-4 Mon-Fri BY FAX:# (02) 9939 2648 24 Hours 7 Days <at> BY EMAIL:# silchip<at>siliconchip.com.au 24 Hours 7 Days BY MAIL:# PO Box 139, Collaroy NSW 2097 * Please have your credit card handy! # Don’t forget to include your name, address, phone no and credit card details. BY INTERNET:^ siliconchip.com.au 24 Hours 7 Days ^ You will be prompted for required information September 2013  85 Fig.6: a 3D view of our CLASSiC DAC design, using simple 3D models we built ourself using the 3D tools Altium provides. These are vertical shape extrusions, cylinders and spheres. As you can see, despite the simplicity of this approach, the result looks quite realistic and can be used both to visualise the design and to check the mechanical fit of components and overall assemblies before a prototype is built. are too close to each other (clearance violations) and so on. We used net-specific clearance rules to help lay out the Soft Starter for Power Tools PCB (published in July 2012). Once the net classes and design rules are defined, you can lay tracks in the low voltage section and they will automatically stay away from the high-voltage tracks. Fig.7 shows an extra track added to this design, between the low-voltage section at right and the incoming mains Active track at left. Note that it is flagged as violating the clearance rules with the Active track even though it is further away from this than it is from the low-voltage ground track at right. In fact, Altium has a very powerful design rule system which allows you to set up many different custom rules depending on requirements, eg, some areas of the PCB can have different track clearance or width rules and so on. Design rules are assigned an order of priority so that you can set up exceptions to rules and you can even have rules which are based on boolean expressions. It’s a powerful system. • Ability to “tent” individual pads/ vias, change individual hole sizes, 86  Silicon Chip pad sizes, shapes and component outlines: normally, you define component characteristics in your PCB library and them simply place them on a board. But there are many times when a component on the PCB must vary from the default. For example, you may need to make the pads of a particular component thinner to make enough room for a track to pass through the middle while in other cases, you want them to remain larger to minimise the chance of tracks being lifted during soldering. With some PCB layout programs, in this situation you are forced to create a new library element with a different pad arrangement and you quickly end up with many variations of each component to suit different situations – it’s messy. With Altium, you can simply edit the component on the PCB by “unlocking” it and then making changes. You can re-lock it when you are finished. This isn’t without its drawbacks – for example, if you later change the base component in the library and then update the PCB with this new configuration, any changes to components which have been varied are lost and must be re-applied. So this is a feature to be used with caution but it can still be a real time-saver. We also like the fact that we can selectively “tent” vias and pads on either or both sides of the PCB, so that they are covered with solder mask during the manufacturing process. Some layout programs force you to do all-or-nothing tenting and by making this part of the manufacturing export step, you can easily forget to do it, eg, when re-ordering a board you have had made previously. • Interactive routing: while other PCB layout packages have interactive routing, Altium’s version works particularly well. We described the most useful modes, “Walkaround” and “HugNPush”, in our last review. One useful feature we didn’t ment­ ion is the ability to press the backspace key while laying a multi-segment track to go back a step if the last segment didn’t get placed quite where you wanted it to. It’s also quite easy to move track segments after laying them without having to re-do the connecting segments. Also, because Altium picks up the initial track size from the pad/track which you click on to start placing, you siliconchip.com.au This is the fully-assembled CLASSiC DAC PCB. It clearly demonstrates the realistic appearance of the Altium 3D model. Silicon Chip Binders REAL VALUE AT $14.95 * PLUS P &P don’t have to constantly go changing the current track size while doing a layout with a variety of different track widths, eg, 10 thou/0.25mm wide for signals and 40 thou/1mm for power. This may seem like a small point but it saves a lot of fiddling and frustration. Also, when a new component or via is placed, if it is in contact with an existing track, it is automatically added to the same net. You have to be careful since that may not always be what you want but it’s very handy for example when placing vias on a ground or power plane – although there is also an automatic via stitching feature which can do this for you. • Polygon pours: while this is a common feature of PCB layout programs, Altium’s handling of it works particularly well. For a start, after placing a polygon, you can easily move its corners and edges, add vertices and so on. It’s also easy to re-pour a polygon (around tracks, pads and other polygons) and to “shelve” it, which Are your copies of SILICON CHIP getting damaged or dog-eared just lying around in a cupboard or on a shelf? Can you quickly find a particular issue that you need to refer to? Keep your copies safe, secure and always available with these handy binders These binders will protect your copies of SILICON CHIP. They feature heavy-board covers & are made from a dis­tinctive 2-tone green vinyl. They hold 12 issues & will look great on your bookshelf. H 80mm internal width H SILICON CHIP logo printed in gold-coloured lettering on spine & cover Silicon Chip Publications PO Box 139 Collaroy Beach 2097 Fig.7: Altium’s powerful Design Rule Checking system has several benefits for PCB design and layout. This demonstration shows how tracks assigned to nets in various “net classes” can have different clearance rules. The track at left carries 230VAC mains voltage (≥100 thou clearance) while the track at right is low voltage (≥20 thou clearance) and hence the added track in the middle causes a rule violation for one but not the other. siliconchip.com.au Order online from www. siliconchip.com.au/Shop/4 or call (02) 9939 3295 and quote your credit card number or mail the handy order form in this issue. *See website for overseas prices. September 2013  87 How Multi-Layer PCBs Are Designed & Made I N THIS ARTICLE, we have referred to “tented vias” and “polygon pours” but readers may not be familiar with these terms. Making double-sided and multi-layer PCBs is quite complex so we won’t give the full details here but the following information should go some way towards explaining these terms. As with a single-sided PCB, double-sided PCBs are generally made using a sheet of fibreglass as a substrate but with copper foil laminated on both sides and then etched. The problem is how to connect the tracks on the top of the board to those on the bottom. The simplest method is to drill a hole through both and then solder a wire or component lead on both sides. But this is virtually impossible for components that sit right on the PCB surface and soldering feed-through wires is expensive and time-consuming. Vias Vias are used to perform the same function. To create a via, a hole must still be drilled but it can be quite small; they are typically around 20 thou or 0.5mm in diameter although larger/multiple vias are used for high-current tracks. Copper is then plated onto the cylindrical fibreglass surface of the hole, forming a hollow wire which joins the two tracks. In fact, a modern double-sided board will have all or most of the holes plated, including those for component leads. This means that component leads are held into their mounting holes more strongly than they would be if temporarily removes it from the design as this makes it easier to edit tracks which intersect with it. You can define the polygon pour order which is important for deterministic results when polygons overlap. You can also determine whether copper is poured directly into contact with pads or if they are instead connected with (thermal) “reliefs” which are basically short sections of track. This is important to avoid dry joints for components connected to large copper planes which can otherwise act as a heatsink during soldering. The polygon-pad connection style can be defined on a per-PCB or per88  Silicon Chip they were just soldered to the copper tracks, even if soldered on both sides. It’s also easier to just plate all the holes although exceptions can be made if necessary. Most modern PCBs also have a “solder mask” layer applied as one of the final steps. This is a polymer film which covers the copper tracks but leaves the pads exposed, making accidental track-to-track, track-topad or pad-to-pad bridges much less likely when soldering. It also greatly reduces the amount of solder required when using wave soldering and helps improve the reliability of reflow soldering. Since the holes drilled in a PCB aren’t necessarily perfectly aligned with the tracks, vias require a certain amount of copper around them on both sides to make sure the hole is touching copper and thus the through-plating makes the required connection. But it isn’t necessary to solder anything to these vias and often they are placed under components, making it impossible. So it’s common to have the solder mask completely cover a via. This is known as “tenting”. Through-hole pads may also be tented on one side of the board, which we find helps with soldering (less solder wickthrough). with just the two layers becomes excessive. ICs in packages with very closely spaced pins or lands (ie, those in BGA or LGA packages) generally require at least four layers to “break out” all the connections from the IC to tracks leading away from it. Multi-layer boards are fabricated as multiple thin double-sided boards which are then laminated together. Clearly, alignment in this process is very important. Additional steps are required to allow vias to pass through multiple layers. The simplest form of via on a multi-layer board is one which goes all the way from the top layer to the bottom layer, joining all the layers between. However it is also possible to have a “blind via”, which starts at either the top or bottom layer but terminates at some intermediate layer, leaving the remaining copper layers above or below it electrically isolated. Similarly, it is possible to have “buried vias” which are only between two or more internal layers and not visible from the outside at all, once the PCB has been completed. Altium has comprehensive support for multi-layer boards and allows each via to have a unique profile, connecting to some or all of the layers with different-sized pads on each layer if necessary. Polygon pours & thermal reliefs Sometimes, having just two layers isn’t enough; vias take up space on the board and at some point a design becomes so complex that the number of vias required to lay it out The copper tracks used to join components are usually formed from line segments; curves are also possible and for radio-frequency signals may be required. But sometimes you need to join many pads and vias together and the easiest way is to do a “flood fill”, where all the otherwise unoccupied areas on a particular layer are filled with a continuous island of copper and this island is then connected to each point as required. polygon basis, which is useful because for high-power tracks you may need the direct connection whereas components connected to a signal ground plane can do so via reliefs. You also get several options for each polygon pour, for example, whether to remove “dead” copper, ie, copper islands with no actual electrical connection. • Net & layer highlighting: when you move a mouse over a track or pad in Altium, the connected net is automatically highlighted. But more importantly, you can hold down Control and click a net and the rest will dim. These two effects can be used in combination to see where various tracks cross over on different layers and so on. A feature we find even more useful – even vital in some cases – is the ability to view and edit a single layer of a PCB at one time which is accessed via the Shift + S keyboard shortcut. This is a great way to remove the clutter from the display when working on a complex layout and it’s also incredibly useful when you are trying to select a group of tracks but not the components or other objects that connect to them. One could get a similar effect by manually disabling all but one layer and then re-enabling them later but that would be a lot of work. With this shortcut, you can easily flip between Multi-layer boards siliconchip.com.au This is a common way to make ground connections but can also be used for power distribution on multi-layer boards. On a four-layer board, it may be the case that one layer is used for ground (bottom, say), one for power (top) and two for signal routing. This means that wherever ground or power is required – and for some designs, that may be at hundreds of different points – you just need to place a via at that point from the appropriate power plane layer. Any through-hole pads must be on the top or bottom layer, to allow components to be soldered to it after the PCB has been made, so in this case you need a “hole” in the power or ground plane so it isn’t shorted to one of those. Most PCB layout programs therefore provide an automated polygon pour feature. You specify a layer and an outline (which may be the whole PCB or a section of the PCB) and assign it to a particular net. Within that outline, all blank spaces (or depending on settings, contiguous blank spaces) are filled with copper, with an appropriate clearance to all adjacent tracks and pads. Tracks or pads within this area that are assigned to the same net are joined to or merged with this copper fill. Fig.9 on the following page shows a portion of the CLASSiC DAC PCB which has ground planes on both the top and bottom layers formed by “polygon pours”. As you can see, it is automatically poured around the vias that are under IC5. Also note the “via stitching” joining the two ground layers for a low impedance at upper left. Thermal reliefs The vias between the top and bottom ground planes in Fig.9 use the “direct connect” style where a hole is simply drilled through the two planes and plated though, top and bottom layers (or on a multilayer board, inner layers) to follow what is going on. • Layer sets: a quick and easy way of showing or hiding groups of layers at once. For example, you can have a minimal layer set (top and bottom copper plus pads, say) and a more complete layer set for when you need to see everything (including mechanical layers) and quickly switch to the minimal layer set while doing routing. • PDF export: this is a great way to show schematics to co-workers or create documentation for clients. Larger designs will normally take up multiple schematic sheets and these siliconchip.com.au giving the lowest possible resistance for the connection. However, the pads joining to this ground plane (ie, the pin of each component that’s connected to ground) are joined using “thermal reliefs”. This is true for both through-hole and SMD components. For example, look at the two capacitors to the left of IC5. The left-most pad of each is isolated from the ground plane by a narrow ring where the copper has been etched away, except in four places, 90° apart. The idea here is that the electrical resistance of the connection is still very low because although the sections joining the pad to the ground plane may be narrow, they are also very short. This usefully raises the thermal resistance between the pad and ground plane. The ground plane, being a large sheet of copper foil, has a fairly low thermal resistance to the ambient air surrounding the board. As a result, trying to solder any components directly to the ground plane is going to be more difficult as it will draw heat away from the joint. Molten solder applied to the PCB that is hot enough to solder a component joined to a thin track (eg, during wave soldering) may solidify on a ground-connected pad before a proper joint has been formed. But the relief-connected pads have an intermediate thermal resistance to ambient, ie, lower than other pads but not much lower and so only a small amount of extra heat is required when soldering. The thermal reliefs may seem too small to make a noticeable difference but if you try soldering to pads with both connection styles you will find that the difference is quite significant. And when using automated assembly techniques, relief connections may be required to get consistent results. can be exported in a single action to a multi-page PDF. With the latest version of Altium, you can even click on components in the PDF schematic to see the component attributes (type, voltage, power rating, tolerance etc). You can also export the PCB to a PDF but this is less useful for a variety of reasons, including low contrast with red/blue on white (for some reason it’s much easier to see on black). We prefer exporting PCBs to Gerber files, which can also be sent off for manufacture. Advanced features Altium also has a number of features which we do use but rarely. Many of these are important for designing commercial equipment, especially high-speed digital circuits. For example, when laying out boards with fast memory (eg, DDR) or high-speed buses, you want to keep each track in the bus to much the same length, so that the signals arrive at the other end simultaneously. Altium provides a few ways of doing this which really make it easy. In a recent design, we used the Interactive Length Tuning feature to lengthen individual tracks in a bus until they were all the same (Fig.8). With this tool, all you do is set up the parameters and “wipe over” a track and zig-zags are automatically added until its length has increased to the set maximum. A similar effect can be achieved using the “Equalise Net Lengths” menu option. There’s also an option for tuning differential pairs, which are normally routed together but may need to be modified to have the same length, depending on the details of the route. Once you’ve finished routing tracks, you can then use the Signal Integrity checker (also visible in Fig.9) to check that all the tracks meet your various requirements for overshoot, undershoot and so on. Potential improvements With such a large piece of software, it’s inevitable that there would be some things we don’t like. And while there are a few, generally they are more minor annoyances than serious problems. Probably the most obvious limitation is that you need to keep your computer hardware up to date to get decent performance. Having said that, fast computers are really quite cheap these days and the hardware cost is a pretty insignificant cost of running the software – the license itself being far more expensive. Altium’s disk footprint has been somewhat reduced by recent updates, from multiple gigabytes down to about 1GB if you are mainly doing PCB layout work, which shows that they have a desire to optimise the software rather than just adding more “bloat”. We do occasionally run into bugs but generally these do not result in any lost work – Altium has a pretty good system for automatically handling “exceptions” gracefully. But on occasion, it can go into an endless loop and it has to be terminated. Normally though, this only happens when using September 2013  89 Fig.8: Altium has a number of advanced design features for modern, highspeed digital/ analog PCB designs. Here we are showing two – Interactive Length Tuning (to add the “wiggles” to the tracks in the bus at left) and the Signal Integrity dialog which performs analysis of the design to ensure it meets design specifications. one of the newer features; the basic PCB layout portion of the software itself is quite reliable. We have also run into some fussiness importing and exporting certain types of file, such as old Protel PCB files and Gerber files. PCB files generally import correctly except that sometimes text is misplaced or rotated. PCB files are sometimes not exported correctly though – for example, if you export a PCB with a polygon fill to a format that doesn’t support polygons, they are silently dropped from the design. We should probably consider ourselves lucky that Altium still supports such an ancient file format at all – in a similar situation, many other vendors would forget it entirely. As for Gerber files, the format is notoriously poorly standardised so it isn’t surprising that we have to fiddle with the file headers to get Altium to successfully import a file produced in another ECAD package. With a modified header, it processes the file correctly. Some areas of the user interface which we previously would have criticised have been improved with updates over the last few months. It’s somewhat unusual when a software company brings out frequent updates to their product and they actually make it noticeably better! For example, certain menus which appear during PCB editing now pop up more quickly, resulting in a smoother work flow. Conclusion Fig.9: close-up of a PCB design (the CLASSiC DAC) showing copper ground planes on both top and bottom layers made using polygon pours. Note how the “poured” copper “flows” around vias, tracks and any other areas of copper that belong to different nets. Component pads joined to the ground plane are via “thermal reliefs” while vias are joined directly to both planes. 90  Silicon Chip Altium Designer is a very powerful tool for PCB layout, especially for demanding designs. That comes at a price though: $A7245 + GST initially and $A1750 + GST per year for updates after the first year. That’s not an unreasonable amount to pay for such a powerful tool if it’s used every day in a commercial environment but it’s certainly out of the reach of amateurs; there is a (much cheaper) student version though. We would certainly recommend Altium as a circuit and PCB design and layout tool, if you can afford it. It has so many useful features that users will need to attend some of their training seminars before they will have a chance to use its full potential. For further information, contact Altium on +61 2 9410 1005 or email SC sales.au<at>altium.com siliconchip.com.au