Fullscreen HTML5Med Res (??MB)HTML4

Altium Designer 22 Review by Tim Blythman We use Altium Designer to design all our project PCBs and have done so for many years. New versions and updates are released regularly, with new releases coming yearly for some time now. Therefore, 2022 sees the release of Altium Designer 22, and we installed it immediately to see what new features are available. Y ou might not think that there is much need for PCB software to change. While it is true that some people continue to use older versions of Altium Designer, there are good reasons to stay up to date, as improvements and new features appear with each version. Altium Designer 20 (reviewed December 2019; siliconchip.com.au/ Article/12176) was a significant milestone. There were substantial improvements from Altium Designer 19 for users, such as the Schematic Editor being completely rewritten to make it quite a bit faster. In fact, the entire suite was rewritten, with numerous features and enhancements. Notably, the new software base allowed integration with the then-upcoming Altium 365 ‘cloud’ software. We reviewed Altium 365 and Altium Designer 21 in January 2021 (siliconchip.com.au/Article/14705). Altium 365 is an online platform to allow shared access to projects and libraries and includes a version control system. We weren’t sure that our small team at Silicon Chip would use this sort of feature, but it has been a handy tool, especially with work-from-home now being common. In particular, we have found it a great way to keep our component libraries consistent and up to date. We expect that it is even more helpful for larger workplaces. Even through 2021 and after the release of Altium Designer 21, they brought out multiple updates and minor releases, so some of the features we mention here might have been seen in previous updates. It’s also worth noting that Altium provides numerous training and development webinars to ensure that its users are making the most of the software. For those readers who do not have an Altium subscription, it’s possible to use some of the online features of Altium365 by simply visiting the web page at www.altium.com/viewer/ The YouTube channel “Altium Academy” (www.youtube.com/c/ AltiumAcademy) is another good way to get a glimpse at Altium Designer and pick up some PCB design tips too. Altium Designer 22 Screen 1: here’s where you’ll find the setting to enable Automatic Cross References at the bottom of the Options tab (highlighted in yellow). The dialog window can be easily be reached by right-clicking on a sheet and selecting “Sheet Actions → Automatic Cross Reference Settings”. 84 Silicon Chip Australia's electronics magazine Altium Designer 22 was released in February and was followed closely by the Altium Roadshow, an online event that consisted of a series of technical sessions over two days. Importantly, siliconchip.com.au this included a guided overview of Altium Designer 22’s new features. We always find the Roadshow to be a great way to learn the best way to use Altium Designer and stay up to date with the newest features. We’re currently using Altium Designer version 22.2.1, the most recent release available at the time of the Roadshow. You might find some changes or improvements if you install a later version. Schematic Editor One feature that was added to the Schematic Editor in Altium Designer 22 appears minor. Still, we think it is quite handy and indicates the broad range of incremental improvements Altium provides. This is the Automatic Sheet Cross Referencing setting. You can enable it with a right-click on a schematic, then “Sheet Actions → Automatic Cross Reference” settings, as shown in Screen 1. When Automatic Cross References are enabled, references are shown on the schematic as seen in Screen 2. Note the grid coordinates on the sheet (3B and 3C) identifying the location within the target sheet. A right-click on the reference allows the reference to be followed like a hyperlink. Exporting such a schematic sheet as a PDF will include the cross-references as hyperlinks, allowing signals to be followed throughout the design, even if they aren’t on the same sheet. As it can be pretty frustrating trying to track signals otherwise when using ports, this is a powerful feature. They do tend to clutter the schematic a bit during the design stage, but it was handy to turn this setting on during the later verification stages to simplify broad checking of the design and also when PDFs are generated. PCB counterholes The PCB editor now allows counterholes to be added to a pad or hole. A counterhole is a machining process that does not extend through the full depth of the PCB laminate. A typical example would be a countersunk hole to allow a countersunk screw to be recessed into the laminate. The remaining laminate allows the board to be secured by the screw, but the recess means that the head of the screw does not protrude as much. As well as countersunk holes, which have an angled wall, counterbores siliconchip.com.au Screen 2: the automatically-generated Cross References include the sheet name and a grid reference that indicates the X/Y location of the object on that sheet. The Port Actions menu option also provides selections to jump to the location of any of the Cross References. Screen 3: counterhole settings are found under Pad properties in the Pad Features section. Here, a 90° countersunk hole is specified (45° per side), with the adjacent 3D view showing what it would look like. Screen 4: the same countersunk hole in the Draftsman view shows several dimensional callouts. You can place just about any linear, angular or diameter dimension on any part with such properties, so it is not limited to counterholes. with straight sides can be added to pads or holes on the PCB. Of course, the ability to implement such features will depend on your board manufacturer’s capabilities. Countersinks have the advantage that the bevel of the screw against the hole will positively locate the PCB at its mounting point. However, that may not always be required, especially if movement is expected or needs to be accounted for. Counterbores allow simple panhead screws to be recessed, among other jobs. When the design is exported, it will Australia's electronics magazine create separate files for counterholes on the top and bottom of the board. Screen 3 shows the appearance of a 90° (45° slope on each side) countersunk hole in the 3D view and its corresponding size and angle properties adjacent in the Pad Features section. A counterbore has a diameter (size) and depth properties. Screen 4 shows the same countersunk hole in a Draftsman view. This view was quickly and easily created by adding a new counterhole view to a Draftsman document and then adding some diametrical, linear and angular measurements. June 2022  85 IPC 4761 Screen 5: IPC 4761 Via Types can be found under Via Properties; a drop-down menu lists the types available according to the standard. These types can also be set as templates. Screen 6: an IPC 4761 Type 1A via on a four-layer PCB is shown here in the Draftsman view. This makes it clear that it consists of a simple solder mask on the top side of the PCB. Other types have different degrees of filling, plugging and covering. IPC 4761 is a standard created by the IPC (founded as the Institute for Printed Circuits) regarding the protection of vias (connections through the PCB) on printed circuit boards. Without delving too deeply into the specifics of the standard, it specifies seven different levels of treatment that can be applied to a via to protect it and the PCB. We alluded to the tenting of vias in our review of Altium Designer 20. This involves covering the bare metal of the via with a plastic solder mask layer. That is equivalent to the lowest (Type I and Type II) of the seven levels covered by the IPC 4761 standard. Other levels include various coverings and degrees of plugging (to cover or fully seal the hole left by the via). These may be needed to protect the vias from contact, moisture, corrosion or even to ensure that there are no holes to allow anything to pass through the PCB. Many specialised designs demand higher levels of protection than what our readers and we generally require. For example, boards that operate in very humid environments and with rapid temperature changes could be subject to condensation, and vias are often the first parts of a board to corrode away. So Altium Designer 22 now allows the IPC standard types to be directly chosen from a Via Types & Features section of the via properties. This is shown in Screen 5, a menu that lists the IPC 4761 types with a brief description of each. Those types with an “a” suffix have the treatment applied to one side only (it appears to be the top side), while the “b” suffixes have the covering applied to both sides of the via. The various types can also be chosen as via templates to streamline via placement. You can also add via layout views to a Draftsman document, as seen in Screen 6. The upshot of all this is that the design intent can be better communicated to the PCB manufacturer, and more consistent results can be achieved. PCB design Screen 7: Gloss and Retrace settings now have their own panel, which can be opened from the Panels button. This makes it simple to quickly adjust these settings while tweaking the final location of the PCB tracks. Other improvements to the PCB editor include more flexibility in the Pad properties editor when using top-­ middle-bottom or full-stack views. Each layer now has its own options Australia's electronics magazine siliconchip.com.au 86 Silicon Chip relating to things like corner radius and thermal relief, and they can now be set for each individual layer. A Gloss and Retrace panel has been added (accessible from the Panels button) to allow finer control of the options that are used for the “Route → Gloss Selected” and “Route → Retrace Selected” actions. The panel can be seen in Screen 7. (Glossing is where the routing of the track is automatically ‘fixed up’ to be as clean and direct as possible.) Bringing up this panel allows the glossing and retracing settings to be tweaked interactively as the track layout is finalised. There is also a new routing algorithm that now prevents loops from forming if a trace is brought back on itself. They also added design rules for SMD pad entry location and angle, which make it easier to produce neat designs by keeping SMD pads consistent. Since these are usually not critical criteria, there is also the option to disable the rules if they cannot be met. Screen 8: the Mixed Simulation extension is not installed by default, but can be added from the Extensions and Updates tab of the License Management page. As you would guess, it lets you simulate the circuit represented by your schematic, so you can get an idea of whether it will work before you build it. Screen 9: the Simulation Dashboard is a panel accessible from the Panels button and is actually a ‘wizard’ as it works through the steps necessary to complete a simulation. As well as defining a circuit, you might need to add voltage source(s) to provide simulated power or signals to that circuit. Mixed simulations The simulation extension, accessed directly from the Schematic Editor, is not new. But it was a point of interest during the Altium Roadshow event as this feature has had some upgrades. If you have not seen the simulation feature before, that might be because it is not installed by default. It can be installed from the Extensions and Updates tab of the License Management page, as seen in Screen 8. Altium Designer might need to be restarted after installation. The Mixed Simulations extension is based on the well-known SPICE program (“Simulation Program with Integrated Circuit Emphasis”). We mentioned in our previous review that Altium Designer 21 added a Simulation Dashboard, while Altium Designer 22 adds measurements and plots of many intrinsic and inferred circuit properties. You can open the Simulation dashboard from the Panels button. Apart from your schematic, you may need to add some voltage or current sources; these can be found under the “Simulate → Place sources” menu item. As you can see from the dashboard shown in Screen 9, Altium Designer leads you through the steps needed to complete the simulation. You might siliconchip.com.au expect that the simulation models will be missing unless you have them in your libraries, but Altium Designer includes many inbuilt models that can be used. Of course, the usefulness of these models will depend on how closely they match the parts you’re using in your design. But, at the very least, the included models for resistors, capacitors and inductors will be usable. Summary We have some complicated multiboard projects coming up, so the schematic cross-referencing feature has Australia's electronics magazine come in very handy while checking these designs. It appears that counterholes are not yet widely available amongst PCB manufacturers. But we can see that being a handy feature as it becomes more accessible. For example, designs that use a PCB as a lid on a Jiffy box can be streamlined and improved by using a counterhole to recess the screws that secure the lid. A good number of new and handy features have appeared in Altium Designer 22, making it well worth the time to install the latest version and remain up to date. SC June 2022  87