Fullscreen HTML5Med Res (??MB)HTML4

“Hands on” review by Tim Blythman Altium Designer 19 is the latest incarnation of the PCB design software that we’ve been using at SILICON CHIP, in one form or another, for over 20 years. While the changes are more evolutionary than revolutionary (compared to the big step that was Altium Designer 18), there are definitely some great new features to discover. I t’s now 2019, and that means that Altium Designer 19 is available. If you were on the ball, you might have even noticed that it was released in mid-December last year, less than a year after Altium Designer 18. You can see our comprehensive review of Altium Designer 18 in the August 2018 issue of SILICON CHIP (siliconchip. com.au/Article/11189). Altium Designer 19 is the latest generation of EDA (electronic design automation) software that began over 30 years ago as the Australian product, Protel PCB. Effectively a tool for turning a circuit idea into a finished PCB, Altium Designer is the tool we use at SILICON CHIP to design PCBs for all our projects. We’ve now been using Altium Designer 19 for around a month and are quite happy with the improvements we have seen in that time. Installation AD19 is a 1.9GB download which uses up about 4.9GB of storage space after installation. To install it, you first download a small (~20MB) program which then downloads and installs the rest by itself. There was an option to transfer our settings from a pre70 Silicon Chip vious version of Altium Designer, which we took, and it did transfer all our settings across, although it didn’t bring over our recently used documents list. This review is of version 19.0.10, which was the latest version available at the time of testing. Altium usually releases a few updates to each major version of Designer over the year, presumably to fix bugs that were reported or discovered during that time. Component re-route feature This is one of the new features that many people are sure to make good use of. In practice, it’s certainly not perfect, but it’s worth using. The situation is this: you have placed and routed a small group of components, perhaps an IC and its associated passives, but then you realise that the entire group needs to be moved for whatever reason. Previously, you would have to do a fair bit of track rerouting. At the very least, you would move the group of primitives, including the parts and their interconnecting tracks, and then try to fix up the now mangled external connecting tracks, getting them to where they need to go without short circuits or clearance violations. In the worst case, Australia’s electronics magazine siliconchip.com.au Fig.1: a section of a PCB we are currently working on, where we want to move a large group of components to the right. Fig.2: AD19’s Component reroute feature has been enabled, so after moving them, most of the external tracks are still connected correctly, and there are no apparent design rule violations as a result of the move. you may have to reroute all the tracks around those parts. Component re-route is the solution to this. As the name suggests, when this feature is enabled, tracks are re-routed whenever components (or a group of components) are moved, reducing the need to do this manually. Fig.1 shows a PCB we’re working on while Fig.2 shows the result of moving a large group of components 5.08mm to the right, with this feature enabled. You can see that many of the tracks connecting these components to other parts of the circuit have changed shape to preserve those connections and prevent overlaps and short circuits. Some of these tracks would need to be manually cleaned up as they have become unnecessarily ‘loopy’, but it’s a lot less work than re-routing all the tracks manually. Fig.3 further demonstrates how re-laid tracks do not always end up finding the obvious paths. But the resulting layout is still valid, even if non-optimal. When this feature is enabled, there’s a brief pause after each movement, while the track paths are recalculated according to the current design rules. So you certainly don’t want to have it switched on all the time. There are times when you may even need to move a component out of the way temporarily, in which case you don’t want the connected tracks to follow. This feature can be switched on and off via the Preferences dialog box (available either from the Tools menu or the gear icon on the menu bar), under PCB Editor → Interactive Routing → Component re-route (see Fig.4). Follow Mode for track placement. You might notice that our PCB design for the Stackable LED Christmas Tree published in the November 2018 issue (siliconchip.com.au/ Article/11297) has some curved tracks that gently follow the contours of the board. This was painstakingly done by creating an arc, assigning it to a net, then adjusting it for the correct radius, and finally connecting the tracks at each end. Both sides of the PCB have a pair of stacked arcs, for a total of four, so this took some time to accomplish. AD19’s Follow Mode allows the interactive routing to follow the contours of an object (which may be composed of several smaller primitives such as lines and arcs). The new version would have allowed us to simply start the track, switch to Follow Mode to create a gentle arc along the board edge, and then resume normal routing. To activate Follow Mode, start routing a track as usual, and then when you have reached the obstruction, move the mouse pointer over the obstruction and press Ctrl-F. The track will now consist of arcs and line segments following the contour of the obstruction until the left mouse button is clicked, after which normal routing resumes. Interactive routing design rules are obeyed during Follow Mode, of course, and the results can be seen in Fig.5. In addition to this new feature, the routing algorithm has been generally improved and seems to be slightly smarter Follow Mode for routing tracks One routing feature which we would have certainly used in the past, had it been available at the time, is the Fig.3: here we tried to move CON2 with Component re-route turned on; the tracks were originally parallel. This only happened very occasionally, but it was quite surprising when it did happen. siliconchip.com.au Fig.4: this shows where the Component re-route option can be enabled or disabled in the Preferences. Click OK after changing the setting for it to take effect. Australia’s electronics magazine April 2019  71 Fig.5: using Follow Mode on the lower track produces a neater result and allows better use of board space. than before. It will now more reliably detect if the track has looped back upon itself, and close the loop to shorten the track. Sometimes you don’t want that, though, so that feature can also be turned off in Preferences. Advanced Layer Stack Manager We do not use the Layer Stack Manager to any great extent as our designs typically have only two layers on standard FR4 substrate (with a couple of four-layer exceptions), and usually don’t have any special requirements regarding high-frequency operation. But this new feature would be useful for those that do have such special requirements, such as with many RF boards. The new version of the Layer Stack Manager uses a material library to keep track of which material characteristics (such as copper weight and dielectric thickness and other properties) can be used on a given PCB. The layer stack can then be assembled from the library of known materials. This allows customisation of the board’s impedance characteristics, for both single conductors and differential pairs. Given accurate material information, the Impedance tab allows quantities such as impedance, propagation delay, track inductance and track capacitance to be easily calculated. An example of the result of these calculations being displayed is shown in Fig.6. This dialog also shows how Fig.7: the Dielectric Shapes Generator dialog box gives an idea of how some types of printed electronics can be fabricated, using minimal areas of dielectric material which are used to separate conductors that would otherwise produce a short circuit. 72 Silicon Chip Fig.6: the Impedance tab of the advanced Layer Stack Manager provides the option to fine-tune track impedance and other characteristics for both single-ended and differential tracks. the software uses the stack material data to calculate the dimensions for laying tracks with a controlled impedance for differential signalling. Printed electronics support One of the more unusual ways of creating circuits is the use of printed electronics. This involves printing conductive layers on an insulating substrate to build up the circuit, rather than the more traditional method of removing Fig.8: the Multi-Board Assembly tool can be used to see how a design composed of multiple components, including PCBs and other parts, comes together as a whole. Here we have combined four copies of our Stackable LED Christmas Tree with the USB Digital Interface board. Australia’s electronics magazine siliconchip.com.au Fig.9: using the Multi-Board Assembly feature, we have placed the PCB for the Opto-Isolated Relay into a UB3 jiffy box. If we then added 3D footprints for the relay and capacitor, a relatively simple job, we could then check that the assembled PCB fits in the enclosure before even having the boards manufactured. copper in unwanted areas which were pre-laminated onto the substrate. Multiple circuit layers can be added by placing insulating or dielectric material between the conducting layers. As such, the PCB layout process is much the same in principle, except that the shapes for the intervening dielectric layers need to be generated, not just those for the conducting tracks. Altium Designer 19 can work with such designs and generate the dielectric shapes. This is controlled through the Layer Stack Manager, where the Features option is set to “Printed Electronics”. The layer stack itself should be modified to suit the design; typically, there is no bottom silkscreen as there is no easy way to print it onto the bottom layer due to the order of printing. With printed electronics, the conducting layers are generally not made of copper; normally a conducting polymer is used, with significantly more resistance. Its properties can be set in the Layer Stack Manager too. An AD add-on is required to generate the shapes on the insulating layers, and this can be installed by finding the “Dielectric Shapes Generator” in the Extensions and Updates tab. Once the tracks have been laid, the Dielectric Shapes Generator is run from the Tools → Printed Electronics → Dielectric Shapes Generator menu. The dialog box which appears is shown in Fig.7. This will give you an idea of how the various layers pile up, and how the dielectric shapes create the necessary separation. Some emerging PCB prototyping technologies will use printed electronics techniques. There are even some people modifying 3D printers to extrude conductive filament or modifying ink-jet printers to lay down conductive ink at the moment. The output of the Printed Electronics mode is standard Gerber files as per a regular PCB design, and these files could even be a handy option for anyone who develops a method of printing in conductive inks at home. Multi-board assemblies We noted in our review of Altium Designer 18 that it introduced better integration of multi-board designs, and it made the creation of flexible designs easier too. In fact, practically any rigid design could be made into flexible versiliconchip.com.au sion by substituting a flexible dielectric layer for the rigid fibreglass layer (and many PCB manufacturers can do this for you, for a price!) But this becomes more difficult when you need to combine both types of board in a design. Not only do you need to visualise how the boards themselves come together but you must also determine how they fit together with other parts such as enclosures. To test this out these multi-board assemblies, we created an assembly of a few of our Stackable LED Christmas Tree boards, mentioned earlier, along with the compatible USB Digital Interface board that was published in the same issue (siliconchip.com.au/Article/11299). The resulting assembly can be in Fig.8. This would have come in handy while we were designing that project, as we had to resort to printing the PCB pattern and making paper cutouts to check that the boards would stack and fan out neatly. The steps required to implement muti-board assemblies involve creating the various PCBs and, if you wish to include enclosures, 3D STEP file representations of them. A “Multi-Board Assembly” is created, and the various parts added and moved into place in a 3D view, not unlike the 3D view accessible from the PCB layout tab. As we noted, it is possible to incorporate enclosures into a multi-board design to be able to see how the entire product fits together. We think that this is actually the most useful aspect (for us, anyway) of the Multi-board feature; to see how complete assemblies fit in enclosures. That would be true whether we are trying to fit one board or several into an enclosure; we do the latter from time to time, with more complex designs. As an example, Fig.9 shows a mock-up of the 230V Opto-Isolated Relay board (October 2018; siliconchip.com.au/Article/11267) fitting inside a UB3 jiffy box. When you bring the various parts of the project together, you will then be able to see whether there are any conflicts, for example, components that would foul parts of the case, such as the lid. If you find such a problem and need to modify one of the PCBs (or even the case) to fix it, once the source files are changed, the complete assembly can be refreshed with the modified parts to confirm that the changes fix the problem. When using off-the-shelf enclosures, it is easy to do a real-world test fit, but there would be many companies (and even individuals with 3D printers) who are designing their own enclosures, making this a bit more difficult. This feature gives the option of being able to test fit many parts without waiting weeks for samples to be manufactured for test fitting. Another potential use for the multi-board assemblies feature is using the 3D renderings and visualisation to demonstrate to potential customers or others what a product under development will look like when complete. 3D Export Completed multi-board assemblies (and even plain PCBs) can now be exported as 3D STEP files too, allowing 3D representations of the assembly to be used in other applications. You could, for example, use a 3D printer to print dummy versions of the PCB for mechanical testing, or import the 3D object into another application that is not able to accept Altium’s normal file format. Australia’s electronics magazine April 2019  73 Fig.10: this shows some of the representations that can be created using the Draftsman feature. The top layer view and drill drawing view could be used by the PCB manufacturer to confirm the PCB design and the lower views can be used to confirm that the final assembly is correct. Draftsman tool While the Multi-Board and Assembly feature allows the finished product to be visualised, there is also the Draftsman tool to help communicate how the product should look at various stages of manufacture, and to assist those involved in manufacturing. It is a way to quickly create several smart-looking diagrams and tables to help communicate the intent of the design. We tried it out, again using the Stackable LED Christmas Tree design, and in a few minutes, we were able to create what can be seen in Fig.10. You would have to agree that the result looks pretty spiffy! In use The change from Altium Designer 18 to Altium Designer 19 is not a big as the step up to Altium Designer 18 was, from previous versions. Ignoring the added and improved features, nothing appears to have moved from where we expected to find it. So workflow is unaffected. That’s important since you build a lot of “muscle memory” using software like this long-term and breaking old habits can take months, and can slow you down initially. While we ultimately like many of the changes introduced with AD18, it did take some time to get used to them! Of course, finding and activating some of the new features will involve knowing where to find the setting in the first place, but a quick web search to figure that out (or the time taken to read this article) is certainly worth the time saved by a really useful and time-saving feature like Component re-route. Altium 365 Another tool has been announced in conjunction with Altium Designer 19 is Altium 365. It is touted as a cloudbased tool for collaboration, and will also allow access to projects by stakeholders via a browser, as well as from within the Altium Designer application. 74 Silicon Chip It appears that Altium 365 will allow people to contribute to and be updated on projects without needing the full Altium Designer application. Users of Altium Designer 18 or older will need to upgrade to Altium Designer 19 to make use of Altium 365. At the time of writing, Altium 365 is undergoing beta-testing and we have not tried using it. The verdict We have not looked back at Altium Designer 18 since installing Altium Designer 19. Now that we have settled into how the newer versions (18 and 19) work compared to the older versions (17 and older), Altium Designer 19 appears to provide the small, but useful improvements that we expect from a newer version. As noted, some of the new tools appeared to be something we would not necessarily make use of, but we certainly can see the utility. These are not useless “bells & whistles” as you sometimes find in other software. For example, using the Multi-board Assembly to check how an enclosure fits would be handy if we did not have the time to wait for prototypes to be manufactured. Altium gives the option of installing the two versions alongside each other, so that if you have any doubts about how the newer version works, you can always try Altium Designer 19 on a trial basis. But we think that, like us, you will be happy to make the switch. We have installed new versions side-by-side with older versions in the past, only to find that the old version gathers dust (so to speak), and is eventually removed to save some storage space. More details? You’ll find much more information about Altium 10’s many features (more than we had space for here), free trial software, SC etc on Altium’s website: www.altium.com.au Australia’s electronics magazine siliconchip.com.au