Fullscreen HTML5Med Res (??MB)HTML4

HOW TO DESIGN Printed Circuit Boards Part 2 by Tim Blythman Professionally made PCBs have become easy to source and quite cheap over the last decade. That means just about anyone who wants to design a custom circuit can make one. So how do you go about turning an idea into a printed circuit board? I n the first part of this series last month, we looked at some of the background surrounding PCB design and manufacture. There was a panel describing the manufacturing process and how the various parts of a Gerber file set are turned into the finished product. We also described the importance of library files and some of the other aspects of Altium Designer (or similar ECAD software) that can streamline the process. For example, Manufacturer Part Search can be used to download the libraries for many parts, so that you don’t have to worry about the process of creating component symbols and footprints. In this article, we will discuss the importance of PCB design rules and show you some of the tips and tricks that we have gathered that will help you during schematic capture and PCB layout. We’ll also explain how you can export your completed design from 66 Silicon Chip Altium Designer and then have it made into actual PCBs. Starting a project We won’t delve into too much detail about actually using Altium Designer, since there are numerous guides online, and we realise that other software packages are available. The Altium Academy YouTube channel has videos on many topics, including a series dedicated to getting started. We’ll focus more on some of the processes and habits that we think will be helpful. At the same time, we don’t want you to get bogged down in minute details. The default settings will be more than adequate for most cases, and you’ll learn more by simply practising the art of schematic capture and PCB design. We mostly use local projects and manage our own version control, so we generally start a project by creating a new project file (File → New → Project) Australia's electronics magazine using our PCB code as a name, possibly appended with a brief description. This will create a new folder with that name; the folder will contain a PrjPcb (project) file with the same name. We typically keep a set of SchDoc and PcbDoc files to use as templates, which helps us to maintain the same style and saves us from having to set up PCB design rules from scratch every time. You might need to start with blank files (File → New → Schematic or File → New → PCB) and develop these as you go. These should be in the same folder as the PrjPcb file. Open the Projects panel and add the files to the project by right-­clicking on the PrjPcb file in the panel and selecting “Add Existing to Project”. This ensures that the files are all associated with each other. Also ensure that your library files are available. Open the Libraries Preferences window from the Components panel. The Install button can be used to add your library files to the list of libraries that are referenced. Make sure that your schematic library is selected in the drop-down menu of the Components panel. If you’re starting from scratch, the most important things to check in your PCB file are that the settings for minimum track-to-track clearance and minimum track width are sensible. For example, around 8 thou (8 mils or 0.2mm) is a sensible initial setting for both. You may also need to adjust the minimum hole size (check your manufacturer’s capability). The minimum via diameter should be roughly twice the minimum hole size. Schematic capture Fig.9 shows a snippet of one of our schematics; note the modular nature. It’s also possible to add notes and frames to label the various parts of the circuit. All these things, as well as components and wires, can be found in the Place menu. Component data sheets will often dictate components like bypass capacitors that need to be included nearby. They might even suggest a PCB layout, which will be helpful in the later stages. Keeping these components as a group will remind you of their purpose. Keeping everything in small groups like this can make it easier to manage the different parts of the circuit. It siliconchip.com.au makes it easier to move things around if that is needed, since there isn’t a mess of connecting wires that need to be adjusted. Instead, the various wires are connected through ‘ports’, which have the names shown. Ports with the same name connect to each other. The names are also carried over to the nets in the netlist (the computer’s internal representation of the wiring connections) and thus the PCB design. Nets that only travel short distances within a group do not need to be named, but it can help to do so. This approach makes it easier to manually copy these small snippets around between projects. Altium Designer also makes it possible to save the corresponding PCB layouts with its Reuse Blocks feature. This is one area where there are two (or more) schools of thought. The approach I will describe here is probably the easiest for the designer, but it can make it more difficult for others to understand your circuit. At the extreme other end are people who insist on connecting everything in the circuit diagram with wires and barely use ports. The result can look messy, but at least you can follow the wires to see what connects where. Perhaps you can find a happy middle ground! the PPS module, so it is easy enough to change the pin allocations by shuffling the ports around if you find that helpful during PCB layout. Sometimes it’s necessary to assign functions to micro pins randomly, then rearrange them as you work on the layout. If you see a red squiggly line near a component pin, that indicates a possible conflict, such as having two outputs connected together. This usually indicates a problem, since the outputs could conflict if set to different logic levels. Sometimes this is a valid arrangement, such as when two slave devices are connected to an SPI bus. In this case, MISO pins are necessarily connected together. While there are settings to disable this warning, we find it is better to know and understand the problem and appreciate that it will, in the SPI case, need to be handled in software. Another common place you will see the red error marker is when two components have the same designator (eg, R1 & C5). Altium Designer’s default is to create each with a “?” suffix (eg, R?), which is simply an indication that these need to be updated before proceeding. Common circuit blocks Many of our designs use microcontrollers, and the in-circuit serial programming (ICSP) header and MCLR pull-up resistors are usually required. Thus, you can copy them from a previous project to save time. It’s easy enough to change the resistor between a through-hole and SMD footprint as required, and rename the 3V3 rail to suit a different supply voltage. Most of our designs use the same standard 0.1in (2.54mm) pitch header for the ICSP connector as this allows a programmer to plug straight in. The 3V3 and GND named ports can be copied and pasted and then wired to the microcontroller chip as needed. Similarly, the VSENSE line will be wired to an ADC pin on the microcontroller, so its port can be copied over, too. Copying the port ensures that you don’t make a mistake while typing its name. Newer 8-bit PICs like the PIC­ 16F18146 allow digital peripherals to be mapped to just about any pin using siliconchip.com.au The process of setting the designators is called annotation; there are several automated options under the Tools → Annotation menu. We often use “Annotate Schematics Quietly”, since that is the quickest. The designators can also be changed manually in the Properties panel of each object. It is a good idea to annotate each section of the circuit as it is laid out, so that related components are numbered consecutively. If there are many components, they are annotated from left-to-right and top-to-bottom. Thus, you can annotate multiple sections in order by temporarily laying them out in the desired order, annotating and then moving them into their final position. As you lay out the schematic file, be sure to pick the correct footprint for each component, so that you don’t miss that step. We often copy and paste resistors and capacitors after the first of these has been picked. Since most of these passives will use the same package, they will probably use the same footprint, and that is an easy way to ensure it. Don’t be tempted to pick a random package and ‘fix it later’ as you may forget and end up with a board that doesn’t fit your components! While you’re at it, add test points as needed. Since they are part of the PCB, they won’t cost anything (they can also act as vias). We’ll move on to PCB layout next, but this is hardly ever a strictly linear process. You might find you need to come back and change the circuit (maybe multiple times!) because something has been missed or needs to be changed. PCB layout Fig.9: using named ports will allow your circuit to be laid out in neat modular groups, and will also give the nets useful names when it comes to the PCB layout stage. Australia's electronics magazine To commence PCB layout, the netlist needs to be translated into footprints and their associated connections. The Tools → Update PCB Document menu item initiates this process. This commences a process that is given the impressive name of an Engineering Change Order (ECO). The ECO summarises the changes that will occur to the associated PcbDoc file and mostly reflects the connections between components more than the physical layout. Sometimes, you might see something in the ECO that doesn’t make sense, telling you that there is a problem with the schematic file. January 2026  67 Errors at the ECO change will also flag inconsistencies between the pins in a schematic library and the pads in a footprint library, or perhaps that a specific footprint can’t be found. These sorts of errors need to be corrected within the libraries or in the schematic before proceeding. Don’t be surprised if you need to go back and forth between the schematic and PCB layout at least a few times before you’re ready to start placing the components and routing the board. Fig.10 shows an ECO that might be seen before PCB layout commences. You might go back later and make a minor change to the circuit that only results in a handful of items listed in the ECO. The red text refers to errors detected in the schematic document. Fig.11 is the PCB document immediately after the first ECO has been executed and all the components and nets have been added. The lines connecting the components are the so-called ‘rat’s nest’ – each line is a net indicating that a pair of pads need to somehow be joined with copper. Design rules Before commencing PCB layout, it’s a good idea to check that your design rules are appropriate. In Altium Designer, they can be accessed (when in the PCB Editor) from the Design → Rules menu. Fig.12 shows the Design Rules window. We mentioned in our recent Altium Designer 25 Review (siliconchip.au/ Article/18307) that the new Constraint Manager can be used to perform much the same task. Since PCB manufacturer capabilities have not changed much, we haven’t felt the need to transition to the Constraint Manager; our existing Design Rules are working well. Many PCB manufacturers also supply a downloadable set of design rules that can be imported directly into various EDA tools. PCBWay has its downloads at siliconchip.au/link/ac8o Altium Designer’s Design Rules also include various preferred values, so you might like to check these, too. Keep in mind that there are some scenarios that might satisfy the design rules but still not be possible to manufacture; the converse may also be true in some cases. For example, routed slots with perfectly square corners cannot be manufactured with a traditional CNC routing or milling process, since the round bit cannot achieve this shape. They may be possible with a laser CNC process at extra cost. A contrasting example is a so-called net antenna, which is typically a copper trace that does not connect two pads and simply ends. In most cases, this is unwanted, since the free end may pick up or radiate RF noise. Of course, if you actually want to create an antenna, you can ignore the ‘error’ flagging the net as an antenna. Another case is the maximum drill diameter being exceeded. In most cases, such holes can be manufactured by CNC routing instead of being drilled. With all that said, most designs for manual assembly are unlikely to fall foul of these traps. The manufacturers that we have dealt with are keen to help out and will often double-check a design if there is any ambiguity. For example, we have designed panel PCBs that lack drilled holes (intentionally) and the manufacturer has asked us to confirm that we have not accidentally omitted the drill file. Component placement There are two critical steps in PCB layout: component placement and trace routing. You will probably go back and forth between the two. Since the components need to be placed before they are connected, a good initial component placement makes the routing stage much easier. To say that PCB design is an art definitely has some truth; it is also true that there is no one correct way to place components or route traces. There will be designs that are poor and some that are good or even excellent, but even those judgements can be subjective. For example, some people like to use ground pours extensively, while others find they can cause noise problems and prefer to route ground connections manually (perhaps with pours in some areas but not others). With that said, it’s always good practice to keep bypass capacitors as close as possible to their corresponding IC pins (one trick is to put an SMD component directly under the IC!). Similarly, power traces should be laid out Fig.10: the engineering change order (ECO) lists all the internal changes that are happening to a PCB design when modifications are made to the circuit schematic (or vice versa). It is a convenient point to check for errors that might have occurred during schematic capture. Fig.11: the chaotic appearance of a freshly generated PCB can be intimidating, but if you group the components as you did during schematic capture, it can be tackled in small steps. 68 Silicon Chip Australia's electronics magazine siliconchip.com.au Fig.12: design rules can also be quite intimidating, but most PCBs intended for manual assembly will have fairly relaxed requirements. Items like the track width, track spacing and hole size are worth checking. to minimise their enclosed loop area; this is often as simple as routing them alongside each other. There have been a handful of times when we have had a design mostly laid out and have needed to restart from scratch, although that is rare. It may be that the design has required one extra component that just cannot be accommodated in the existing layout. ‘Ripping up’ and re-laying a set of tracks is not all that uncommon, though. Other times we have reached the realisation that routing all the required connections is just not possible with the existing component placement; perhaps swapping a handful of microcontroller pins will solve the mess, but at the expense of having to redo a lot of the routing. This can come down to trial and error, although practice will help speed up the process. You’ll note that during the schematic capture phase, we suggested grouping the components into functional groups. A good first step is to move the footprints around so that they are similarly grouped in the PCB document. The process is to route the siliconchip.com.au connections within each group, then connect the groups together. For example, if you have an op amp IC in the circuit, you can place the IC with its bypass capacitor(s), feedback components (mainly resistors & capacitors) and so on. Then you can move that ‘block’ around to see the best place to locate it on the PCB, with the aid of the rat’s nest. At times, it is surprising how much space traces can take up on a PCB, so leave space between components if possible. Extra space will also make assembly easier. The small groups can be arranged quite tightly, but remember to leave room for designators and component values if you want to include them. That room often ends up being a good amount of space to add traces. We usually don’t start routing with the smallest possible track widths or smallest possible vias because larger tracks and vias have better properties (lower resistance, lower inductance, less likely to lift during soldering etc). This means that if we get desperate, we can reduce the widths and sizes Australia's electronics magazine in some areas to give ourselves some extra breathing room. Of course, if you start with everything at minimum size, your routing job will be easier, but then you will likely have to go back later and redo areas to thicken traces where you can (at least if you want to get an optimal result). There might be a couple of components that you decide need to be fixed at a certain location. External connections, such as plugs, sockets and DC jacks need to be near the edge of the PCB. A display should be front and centre, with controls located below it, so that the display is not covered while the controls are being operated. In fact, it’s often a good idea for the first steps of PCB layout to define the size and shape of the PCB based on the case it’s going in, then place all the mounting holes, then all the connectors, LEDs, switches and such that have to go at certain locations around the edge. It then becomes much clearer where certain other components have to go. If you have components that need to stay in place, their location can January 2026  69 Fig.13: laying out your components into groups and then aligning pads with matching nets is a simple strategy but works quite well. Remember that part data sheets will sometimes offer PCB layout suggestions (especially switch-mode regulators). be locked from the Properties panel, which stops them from being accidentally moved. Fig.13 gives an example of a simple strategy that we commonly use. These components are the same as the VSENSE divider seen in Fig.9, dropped in the PCB document as they might be after an ECO. On the left, we have simply grouped them; note that the net names are visible, which helps us to recall their purpose in relation to the rest of the circuit. The right side of Fig.13 shows how these might be wired together. Within the group of components, we find matching nets and align these side by side, rotating the part as needed. The logical flow used is from left-to-right, to match the schematic and the PCB’s external connections. Fig.14 shows a section of the Versatile Battery Checker from the May 2025 issue (siliconchip.au/Article/18121) that has been given a similar treatment. The three components on the right have a similar arrangement to that shown in Fig.13. This gives a very neat result when there are multiple components with the same package size (M3216/1206 in this case) lined up in a row. The SOT23 transistor also fits in quite well. This system also works for arrangements like biasing and coupling networks, such as in audio and other analog circuits. Here, we can use the Properties panel to quickly align multiple components. All components in the group are selected and can be aligned horizontally by setting their Y coordinates to the same value. Each then has its X value set at equal intervals. A 3mm spacing is used for most of the parts in Fig.14. You can also take advantage of the document grid and snap-to-grid 70 Silicon Chip to align components like this. If the circuit uses mostly throughhole parts, a grid spacing of 100mil (0.1in or 2.54mm), or a fraction of this, like 25mil, will allow the parts to naturally snap into the locations dictated by their pin spacings. We generally use a metric grid (1mm or perhaps 0.5mm) for laying out surface-mounting parts. Remember that the snap settings may overrule the grid spacings. Note how in Fig.13, we haven’t laid out a trace for the GND pads. Instead, we plan to connect this to a copper area that will probably cover most of the PCB. This is known as a polygon pour, and you can see these connections in Fig.14. As the name suggests, they can be just about any shape or size. A polygon pour is a copper layer region that can be defined and allocated to a net. When it is ‘poured’, it is shaped so that it avoids anything else within its limits, but will connect to that specific net, kind of like pouring concrete around obstacles on the ground. It effectively fills the area with copper. On many layouts, a polygon pour can remove the need to connect the pads for at least one net (usually GND) and typically more. We often use a polygon pour for ground nets because it is effectively ‘free’ and has the most pads to connect. Multiple polygons can be used in different parts of the board and on both sides of the PCB. Many four-layer boards will have entire layers made of polygon pours allocated to just a single net or a few nets, such as ground or power rails. Thus, polygon pours can help route multiple nets, either partially or fully. Depending on your settings, you may need to manually repour the polygons after making edits near them Australia's electronics magazine or components that are within their extents. Tools → Polygon Pours → Shelve can be used to hide polygons if they are making the screen difficult to navigate. One of the tricks we use is to route ground normally (to ensure that the polygon will actually be able to connect everything), then use the “Select connected copper” command to ‘rip out’ all the copper tracks and replace them with a polygon pour. We can then tweak it by adding via stitching etc. You can see that the connections between the pads and the polygon pour are through narrow copper necks. This is called thermal relief; if the pads were directly connected to the copper area, soldering would be difficult, since the large copper area would draw too much heat away from the pad. Thermal relief settings are adjustable, but we have never had any problems using the defaults. Since the ground net is likely to have the most pads connected, a ground polygon pour can do a lot of work. It is also a very large copper area, so it will have a low resistance; a ground or power circuit is also a good place to have this property. Layers If you use through-hole components on a two-layer PCB, all component pins already have a connection to both sides of the PCB due to the plated through-holes. A handy trick is to run the traces on one layer horizontally and vertically on the other. This works especially well if you have buses with multiple traces running in parallel. Essentially, every throughhole pad is a free via. If you need to join traces on both sides of a PCB, remember that vias are also available (and also free). A via is much like a plated through-hole pad that doesn’t connect to anything else, although they can be much smaller. Since they don’t need to have an external connection, they are often covered in solder mask; this is called a ‘tented via’. We recommend that you set your design rules to enable tented vias. These days, manufacturers even provide the option to plug vias (fill them with glue) and cap them (cover with glue) so they can’t corrode. You can use vias to switch between layers if you need to change between running traces horizontally and vertically. While vias do have a small siliconchip.com.au resistance and impedance (capacitance and inductance), it can be largely disregarded for most things apart from high-speed and RF design. You can also use vias to connect polygon pours on opposite layers. Indeed, most low-voltage (24V) and low-current (1A) designs that are not related to high-speed or RF will work with just about any routing that completes the necessary connections and has traces at least 0.5mm wide. If you’re placing through-hole components on both sides of a PCB, be sure to check that you can solder parts on one side after parts are fitted on the other! While it can be tempting to put components on both sides, because tracks and vias take up board area, it’s often easier to stick to putting components on one side and using the other for track routing. This makes assembly easier. If you have to sprinkle the odd component on the back, like a few bypass capacitors or a shunt resistor, that won’t make assembly much more difficult. It is possible to run a via directly into a surface-mounting pad from a polygon pour or track on the other side of the PCB. This usually works fine for hand-assembled boards, but be aware that the hole will pull solder away from the part and for these reasons, they are not recommended for boards to be soldered by a reflow process. For boards designed to be reflowed, there are ways to safely put vias in pads; they usually involve the plugging/capping option mentioned earlier (which may incur extra cost), or at least tenting the via on the opposite side of the board. Still, that’s an advanced topic we won’t get into any further here. The simplest strategy is to run a short trace and move the via so that it is just outside the pad and will remain covered by solder mask. Checking As you go along, it can help to occasionally run a DRC (design rule check; Tools → Design Rule Check; then Run Design Rule Check). At the start of your layout, this will probably be dominated by “unrouted net” errors. As the name suggests, these are connections that have not yet been made. Any errors apart from unrouted nets are probably worth investigating at this stage. Some errors you get can be safely disabled or ignored (eg, silkscreento-­silkscreen clearances). Others, like short circuits or clearance violations, should be fixed. We often start routing the circuit subsections and then run a DRC to see if any other errors occur; these might mean that the current component layout needs to be changed. You can also see which nets have the most unrouted net errors and might benefit from being connected by a polygon pour. As you work your way through the design, the number of errors reported by DRC should shrink, and how many are left gives you a good idea of how much work is left to be completed. If you’re starting to run into routing difficulties and you’re still seeing 50 unrouted nets, it may be time to rethink your strategy! Double-clicking on an error in the DRC report should zoom in on the location where the error has occurred. If you find that the screen gets too busy with error markers, they can be removed by selecting Tools → Reset Error Markers. Fig.15 shows an example of a DRC report and one of the detected errors. Autorouting Altium Designer has an autorouter (Route → Autoroute) that can do most of the work of routing. It can work quite well for simple designs, but we don’t often use it because we feel that manual routing gives a more neat, elegant and optimal result. We find it can be handy on layouts that are simple but tedious, especially if there are a lot of short traces to be run. Another way we have used it is to find inspiration in finding ways to route traces where we can’t see an obvious solution (routing a complex PCB can sometimes feel a bit like trying to solve a Rubix Cube blindfolded...) There are also tools to help with making your layout neater, particularly regarding traces. Glossing is a tool that works to help lay the traces. It has many settings and is automatically applied during routing, but you can also manually gloss a selected track with the Route → Gloss Selected menu option. Tidying up Once you can run the DRC and get no reported errors, your PCB design is almost complete; what’s left is mostly ‘tweaking’. Component layout and routing the traces in a PCB Fig.14: you can also use the Properties panel to exactly align the X- and Y-coordinates of components. Note the numerous vias connecting the polygon pours to their counterparts on the other side of the PCB. Fig.15: a design rule check will provide a detailed report of what still needs to be done to lay out the PCB. The line shown here is the obvious connection, but more complex cases might require a different solution if many pads are to be connected. siliconchip.com.au Australia's electronics magazine January 2026  71 are necessary facets, but they aren’t the only ones in a well-designed PCB. You’ll note that our PCBs have detailed information on the silkscreen layer, which often requires some attention, too. Even if you are happy to use the component designators, they will probably need to be rotated and aligned to look neat. Having space between rows of components can help here. Fig.16 shows the appearance of the silkscreen markings before (left) and after (right) we reworked the designators and added component values to passives. You can see that even before beginning, the designators are scattered around, having been rotated with their components. We need to rotate them, align them, add values and then organise them in such a way that it is clear which value belongs to which component. This only shows one side of the PCB. For this project; the other side has more components, as well as our logo, the PCB code (including a version letter code) and project name. It helps to use whatever space is available to add useful information. If there is room, you can even add notes, instructions, polarity markings and I/O pin maps as appropriate. Check that the board outline and any cutouts correspond to the lines marked out in GM15 (or whichever layer you have chosen). If you aren’t sure, the Tools menu has various options for turning entities in Altium Designer (board outlines and cutouts) into lines and arcs. Look under the Convert submenu. Remember that for all of Altium Designer’s abilities, the final Gerber export step simply takes the shapes on the various PCB layers and renders them into a very simple output. Many high-level entities, especially board outlines and cutouts, will have no effect unless they are part of an exported layer. It’s also a good idea to view your design in 3D and confirm that everything looks as it should. You can toggle the 3D bodies using Shift-Z to check that the silkscreen markings look correct under the components. You can even export a 3D model (File → Export → STEP 3D) and 3D-print it to see that it aligns with your chosen enclosure. Another handy check is to export as a PDF (File → Smart PDF). Since the PDF format preserves dimensions, you should be able to print the PDF on paper and check that the footprints and layout match your components. We recommend doing this if you have not previously completed a PCB design. Even after this stage, there will be some chances to view the Gerber file output and see that it corresponds to what you intended in your design. There will always be room to make changes until you check out at the PCB manufacturer’s online store. The engineers will check the designs and may ask you to review and re-upload the files if they find a problem. Gerber file export If you are happy with all the checks provided so far, you can export the PCB file to a set of Gerber files. There are a few steps required. The seven layer files are exported, followed by the drill file. These eight files are then bundled together into a ZIP file for upload to the PCB manufacturer’s portal. All the file export options are found under File → Fabrication Outputs. “Gerber Files” is of course the choice for the seven layer files. Fig.17 shows this window in the most recent versions of Altium Designer. The options shown are those that we used for our projects. Note that most PCB manufacturers still seem to use imperial units (inches). You should have two copper layers, two silkscreen layers and two solder mask layers. There will also a file for the board outline; we use GM15 but you could use GM1 or something else depending on what’s convenient. The board outline and any cut-outs inside it are simply defined by line and arc segments that join end-to-end to make a set of closed shapes. You’ll see that there is also the option of exporting a paste mask layer; these files would be used to create a solder paste stencil to apply solder paste to the PCB as part of a reflow soldering process. They are not needed in a manually soldered design. Next, the drill file can be exported using the “NC Drill Files” option. Fig.16: adding component values and cleaning up the silkscreen layer is another skill that requires an artful touch. We like to use the BoM as a checklist to make sure we do not miss any of the components. 72 Silicon Chip Australia's electronics magazine siliconchip.com.au Fig.17: recent versions of Altium Designer use this simplified Gerber export window. We suggest you select inches as the units, since that is the unit that most PCB manufacturers still use. Fig.18: naturally, the drill file settings also need to operate in units of inches to match the other files in the Gerber set. We also like to tick “Use drilled slot commands (G85)” so that pads with slotted holes are exported correctly in the drill file. Fig.18 shows the settings we use. Both these commands will open a view in the Camtastic viewer, but we typically ignore this and it can be closed without saving. The exported files should be in the Project Outputs sub-folder of your project. These files are then collated into a ZIP file, which bundles everything together. We like to add the board dimensions and other non-default manufacturing options to the file name, since these are not recorded anywhere. Otherwise, it’s easy to forget to specify things like the desired solder mask colour or board thickness when ordering PCBs, unless they are the defaults of green & 1.6mm. Fig.19 shows the eight selected files and the ZIP file with its annotations. There are a few other files exported to the outputs folder that are not needed for PCB manufacturing. The CSV file is the BoM (bill of materials) that we mentioned in the previous article. It can be exported from the schematic editor with the Reports → Bill of Materials option. Ordering boards There are many options for ordering PCBs these days, as you have probably siliconchip.com.au seen in advertisements in this magazine. Fig.20 shows the ordering page for PCBWay. Here, we have uploaded a ZIP file Gerber set, and it has been rendered in this view. There is also a separate Gerber viewer that can be accessed at www.pcbway.com/project/ OnlineGerberViewer.html It’s worth having a quick glance at the renders to see if they show any obvious problems. For example, if the drill files are exported with different units to the layer files, the holes may not line up correctly. You can also check that all layers are present and correct, and the PCB appears as you expect. The upload page has automatically detected the dimensions of this twolayer board. You can check that the dimensions are as expected. Factors like hole size and track spacing might also be detected, so you should check these are what you have intended. Generally, boards up to 100 × 100mm are quite cheap, as seen here. The defaults (as shown) are likely to be quickest and cheapest, so are the best choices for prototypes. Options like different solder mask colours are still fairly cheap and fast, as are PCB thicknesses down to around 0.8mm. Australia's electronics magazine Fig.19: the eight selected files here have been collated into the ZIP file near the bottom of this list. We have also added the dimensions and thickness of the PCB to the filename so we don’t forget to specify them when ordering the board. January 2026  73 On the other hand, changing to a different substrate or surface finish can dramatically increase the cost of the boards and may also add to the lead time. It’s easy enough to click through the different board options to see what is possible. Note that some options can require other choices. You might have seen features like edge connectors or castellated pads along the edge of a PCB; these look simple, but can also end up being expensive additions to a design, since they may require extra processing steps to achieve. There are also slower, cheaper shipping options available. We generally like to order several designs at the same time and spread the cost of faster delivery amongst them, since the total shipping cost does not increase much for extra boards. Each board is finalised by pressing Save to Cart, after which you can upload a different design and configure it as needed. After this, the process is much like any other online store. You’ll need to supply a shipping address and make payment before manufacturing begins. Then, you just need to wait until your creation arrives. Summary The ability to have PCBs manufactured has become much more accessible over the last decade, as well as becoming faster and cheaper. PCB design software such as Altium Designer continues to improve and add new features. There really isn’t a better time to start designing PCBs. There are many tools, features and tips in Altium Designer. While Altium provides many learning guides, there are also online communities that can be helpful in finding out how to achieve a specific end. Of course, this series has only just skimmed over the very simplified basics of the topic; there are many other aspects we haven’t mentioned or only briefly touched on. As we stated, designs involving RF, high voltage, high current or high speeds will need settings, design rules and knowledge that we have not covered. Next month’s issue will include an article on advanced PCB design techniques. We’ll also describe the process for ordering PCB assemblies, like the RGB LED Star from the December issue SC (siliconchip.au/Article/19372). 74 Silicon Chip Fig.20: there are many options available for PCB ordering and manufacture, but the defaults are often the cheapest and fastest. The PCBWay website offers these renders of the Gerber files, providing another simple way to check that the design is as you intended before they start making boards. Note also the link to a separate Online Gerber Viewer feature, which will give you a better view. Australia's electronics magazine siliconchip.com.au