Fullscreen HTML5Med Res (??MB)HTML4

FIRST LOOK: TIM BLYTHMAN REVIEWS THE ALL-NEW When we reviewed AD19, we found some handy new features like component re-routing, follow mode for track routing and an updated layer stack manager. The folks at Altium have not rested on their laurels and the new version, Altium Designer 20, should be available to the public at about the time this article goes to press. We got to try a beta version and here is what we found. I n case you aren’t familiar with it, Altium Designer is EDA (electronic design automation) software that traces its roots back to an early Australian PCB design tool, Protel PCB. We use Altium Designer at SILICON CHIP for all our PCB designs. We reviewed AD18 in August 2018 (siliconchip.com.au/Article/11189) and subsequently, AD19 in the April 2019 issue (siliconchip.com.au/ Article/11527). You may recall that AD18 was quite a revolutionary step from previous versions while AD19 continued to add features and iron out bugs. So we were keen to see what the latest version had to offer. The “Roadshow” In October this year, we were invited to Altium’s Roadshow 2019 event at Sydney’s Olympic Park, where they revealed (among other software), Altium Designer 20. The notion of continuous improvement was emphasised at the Roadshow. The folks at Altium are aware that Altium Designer is a leader in the EDA market. But they also note that they cannot stay in such a position without continually stepping up their offering. The Roadshow event also covered upcoming Altium products such as the Altium 365 platform. Altium 365 is a cloud-based platform that allows collaboration between the various stages of electronics design and manufacture. One benefit of being cloud-based, besides allowing users to roam easily, is that users not directly involved with PCB design (and who would not have the Altium application) can view and comment on designs. This could be handy for people involved in manufacturing or mechanical design, so they Screen1: the Schematic Editor looks much the same as in AD19, although you may notice some slight differences. This is due to the new DirectX rendering, and it is generally easier to see. Zooming and panning around the schematic is considerably smoother, too. 70 Silicon Chip Australia’s electronics magazine siliconchip.com.au Screen2: we created an exaggerated creepage rule to show how it works. Note how the indicated creepage path avoids the slot. AD20’s creepage rule can even handle paths crossing from one side of the board to the other, taking PCB thickness into account. This rule might catch situations which manual creepage checking could miss. can see details of the design without needing an Altium license. Since our team is small, with typically one or two people doing PCB and mechanical design and assembly on a given project, it’s hard for us to put something like Altium 365 through its paces. But we imagine it will be quite useful for larger teams, especially if they are geographically distributed. The Roadshow also took some time to explain some features which have been part of Altium Designer for a while. A quick poll of those at the Roadshow indicated that a good number are still using versions as old as AD14; it’s clear that the Altium team is aware of Screen3: the High Speed Return Path rule checks that a signal return path (such as a ground plane on another layer) is correctly placed along a highspeed signal line. If it is missing, as in the upper left corner shown here, or has less overlap than specified, a violation is generated. The Impedance Profile options come from the Advanced Layer Stack Manager. New features • Improved schematic editor • Dynamic schematic compilation • Any Angle Routing and improved trace editing • Creepage path Design Rule • And more... this and want to let users know about the benefits of using the newer versions, with their improved features. Altium Designer 20 Let’s start by looking at some of the newer features in AD20. We tested version 20.0.6; the final release version will almost certainly be different. We installed it alongside AD19 so we could make comparisons. ensure the PCB layout is correct. The Schematic Editor has been completely rewritten for AD20. It now makes use of DirectX for graphics rendering, so using it is much smoother. It has been sped up so much that ‘compilation’ happens in real time. The ‘Compile’ menu option is still there, but it just brings up the dialog box summarising the compilation results. (‘Compiling’ a schematic essentially checks that there are no glaring errors, like duplicate component designators or important unconnected pins.) As a result, the Schematic Editor now feels much more snappy. Screen1 shows its new appearance. As well as being faster, we think it is also much softer on the eyes. For example, when Installation Screen4: this dialog shows the new text justification options, below the font type selection. Existing projects without text justification set will remain unchanged until a justification setting is chosen. The location coordinates are automatically re-calculated when the justification is changed so that the text stays in the same place. siliconchip.com.au The install process for AD20 is relatively straightforward and similar to that for AD19. A small 23MB installer program downloads and installs the full program. In total, around 2GB was downloaded and the install took up around 5GB of storage space. After opening Altium Designer 20, we were given the option to import settings and had to select the license to use. After that, it opened the files we had open the last time we used AD19. The whole upgrade experience was quite seamless, and it felt very much like we were continuing where we left off with AD19. Schematic Editor While you might think that Altium Designer is focused on PCB editing, creating a schematic is essential to Australia’s electronics magazine Screen5: although the differences are quite subtle, if you look carefully, you will see that the labels next to CON1 are not aligned as well as for CON2. But placing the text for CON2 took a fraction of the time, because of the ability to right-justify the text and centre it vertically so each string lines up exactly with the pin centres. December 2019  71 Screen6: the new modal properties dialog box (at left) with the properties panel (in AD19 style) at right. While the default behaviour for AD20 has changed to be modal, the Preferences can be changed so it is not modal (PCB Editor -> General -> Double Click Runs Interactive Properties). A similar option for the Schematic Editor is under the Graphical Editing item. you zoom in and out, the font and line weight doesn’t ‘jump’ in steps like it used to, and you can read smaller text when zoomed out a bit more easily. It’s a subtle difference, but we feel that it’s an improvement. Laying traces There are still some times when we’re using AD19 that we go to move a track which isn’t quite in the right place and it doesn’t go where we want it to. As a result, it is often easier to ‘rip up’ the trace and lay it from scratch. But with AD20, this has improved immensely. Now, when moving a track, it also takes into consideration the connected traces (at each end). So the result of trying to move traces is now much more intuitive and obvious. Track laying has been improved too, with improved any-angle routing. This too feels smarter. We saw a demonstration of BGA (ball grid array) escape routing at the Roadshow. This was shown to be a lot more fluid and intuitive in AD20 than its predecessors. Fortunately for us (and you, dear reader, who may be assembling our projects), we have not used any BGA parts yet. But we did try routing one of our existing projects with the any-angle setting. The result is reminiscent of the 72 Silicon Chip carefully curved, hand-drawn PCB designs from the 1970s. Even if you don’t work with tiny chips, it’s a great option if you’re going for that retro look (Screens 7&8). It may also be a way to cram tracks into a small gap in your layout that would otherwise seem impossible! Design Rules Design rules allow a PCB design to be checked for validity and safety; the rules are set according to manufacturer specifications (eg, minimum trace width and spacing) and electrical standards and regulations (for example, high-voltage track clearance). The PCB Editor in AD20 has some new design rules. The most useful of these is creepage distance. Enforcing this is most important in mains-rated designs, where minimum creepage distances are specified in many standards. Creepage distance is slightly dif- ferent from clearance distance in that creepage is that path between two conductors along the surface of the PCB, while clearance is simply the straight line distance. This is because current may flow along a nominally insulating path (eg, the PCB substrate) in the presence of surface contaminants. One way of increasing creepage distances is to mill slots in the PCB, which removes a surface on which contaminants can collect and form a creepage path. You will have seen these slots on board designs we’ve previous published, such as the Opto-Isolated Mains Relay from October 2018 (siliconchip. com.au/Article/11267). Screen2 shows how the (exaggerated) creepage rule is applied. The online rule checking and violations display allows you to see immediately whether changes to the design will fix the problem. In the case shown, the design rule violation could be eliminatVias that are not covered in solder mask can cause problems; here’s an example where we forgot to tent them in an early prototype (for our Stackable Christmas Tree). They can easily be shorted accidentally and can corrode, plus they make it look like the board is missing some components. Australia’s electronics magazine siliconchip.com.au Screen8: the Interactive Routing Properties are shown by pressing the TAB key when routing; the Any Angle Routing option is shown under Corner Style, where the mouse pointer is located. Routing is resumed by pressing the ESC key. Screen7: we routed our Tiny LED Xmas Tree PCB from the November 2019 issue using any-angle routing. It was easy to achieve a working result, especially around the unusual board edge shape. The result looks less engineered and more organic; perhaps that’s appropriate for a tree… ed by lengthening the slot. Sometimes this creates an alternative creepage path, but this can now easily be seen and rectified. High-speed return paths In our review of AD19, we explained how the Advanced Layer Stack Manager could be used to calculate and set the impedance of paths in high-speed designs by using information about dielectric thickness, trace width and ground plane layers. This makes it easier to tune highspeed designs correctly. In practice, variations in the return path can compromise the assumptions made in these calculations. The new High Speed Return Path rule can be used to ensure that the return path (in the ground plane layer) is adequate. The selected impedance profile determines to which layer the high-speed signal is referred. The amount of overlap and whether voids due to pads or vias are included can also be selected. We’re unlikely to need this feature, especially since many of our boards only have two layers, but many other engineers will make good use of it (Screen3). Tented vias By default, vias placed in the PCB Editor are not ‘tented’, ie, placing them opens the surrounding solder mask. Unless you need a test point (and if you do, you should place one explicitly), it’s generally better to have the via covered in solder mask. There’s less chance of siliconchip.com.au short circuits that way. We generally place tented vias, but it’s quite easy to end up with untented ones in a design by accident. The new “SolderMaskExpansion” design rule allows all vias to be tented by default. The rule can be found under Design Rules -> Mask -> Solder Mask Expansion (see Screen9). Better text support Improvements have also been made to text objects in the PCB Editor. This is definitely something that we will use, especially as our designs have more text on the silkscreen (to assist with manual assembly) compared to designs opti- mised for machine assembly. We often have rows of pins with identifying text next to each one. Unless the text sits to the right of the pins, aligning it nicely was a tedious, manual job. Now there is the option to set the justification of each text object, so aligning by the top, bottom, left, right or centre is now possible. Screen4 shows the updated text object properties box. Screen5 shows the difference this makes. The text accompanying CON1 was laid out in the way have previously done this with Altium Designer 19. The snap grid causes a small amount of unevenness, and each item had to be placed by hand. Screen9: this shows the design rule to cover all vias in solder mask film automatically. Set both options to “Tented” and all your vias will almost disappear. Australia’s electronics magazine December 2019  73 Screen9: creating the symbol for an Arduino shield with the Symbol Wizard. You can use a spreadsheet to generate the pin names and then paste them back into the table. or perhaps due to a circuit revision to an already produced board. Sometimes components added to a PCB are stacked up haphazardly. There is an option to move these components to a selected area, under Tools -> Component Placement -> Arrange within Rectangle. After selecting the parts, choose this menu option and then drag a rectangle with your mouse pointer. All the components are placed neatly inside it. This is an efficient way of tidying the layout before starting the serious job of placing (or adjusting) components. Place components from file CON2 makes full use of the justification feature of AD20. We created the first text object and aligned it to the right (horizontally) and centre (vertically), so that it lined up with the pin centre. We then copied and pasted it for the other pins, then edited the text labels. As a result, all the text objects are aligned perfectly, in a fraction of the time. Panels and properties The default behaviour of the object property box has changed in AD20. Previously, you could double-click on a part to open its property dialog box and make changes. Alternatively, you could open the properties panel and make changes there. Now the property dialog box is modal by default, meaning that it must be closed before working in the main application window. The dialog box has been rearranged to make more settings visible without scrolling. See Screen6 for a comparison of the new dialog box against the older (but still available) panel. We’re slowly getting used to the idea of clicking on Panels -> Properties to bring up the panel for making changes to multiple parts. There is a setting to revert the behaviour to be more like AD19 if you find you don’t like this change. But we think many who were used to the pre-AD18 workflow will welcome it. A similar arrangement is found in the Schematic Editor. This is handy for choosing component footprints, as it 74 Silicon Chip involves less scrolling than in AD19. Tips and tricks Here are some things we learned at the Altium Roadshow which are not specific to the new version, AD20. There is a component footprint wizard in the PCB library editor which allows many common component footprints to be easily created by entering such figures as the pin count, pad size and spacing. Even non-standard footprints can be created by using the wizard and then modifying the result. There’s also a symbol wizard to ease the creation of schematic symbols. When editing a schematic library, this can be found under Tools -> Symbol Wizard. Although it only appears to generate square boxes with pins along the sides, it also allows the various pin types, designators and other data to be edited in a small spreadsheet. The real secret to this tool is that you can copy and paste data from a separate spreadsheet program, making automatic creation of families of parts much easier. Even existing parts can be edited with the symbol wizard; it’s probably the best way to make wholesale changes to a symbol. Component placement A critical step in the PCB design process is component placement; efficient trace routing is not possible without proper placement. We learned about two handy tricks for doing this. The first is simply a tool for tidying up your PCB as you transfer it from your schematic, either on the first pass Australia’s electronics magazine This feature is intended for use with automated component placement during manufacture, but it can come in handy for a variety of other tasks. You can generate a file containing a list of component identifiers, X/Y coordinates and rotations in a humanreadable (and editable) format. This is done via the File -> Assembly Outputs -> Generate pick and place files. This creates a file with a .TXT extension but you can edit it and then rename it to .PIK. This file can then be loaded via the Tools -> Component Placement -> Place and all the components will be moved into their new positions. This could be a speedy way to place components on a grid, without having to do it manually! Conclusion We have no hesitation in switching from AD19 to AD20. The speedups in the Schematic Editor alone are enough to convince us. The only other change in workflow is the new properties dialog behaviour – but as we explained, you can revert to the old behaviour if you prefer it. The big lesson we got out of the Altium Roadshow is that there are great features that we (and many other Altium users) are not yet aware of, which can be used to make PCB layout jobs even easier. SC Free trial of Altium Designer You can get a fully-featured 15day evaluation version of Altium Designer for free. If you haven’t yet tried the software, visit www.altium. com/free-trials/ for more information. This page also has information about free trials for other Altium products such as the Concord Pro Library Manager. siliconchip.com.au