Fullscreen HTML5Med Res (??MB)HTML4

HOW TO DESIGN Printed Circuit Boards Part 1 by Tim Blythman The cost of professionally made printed circuit boards (PCBs) has dropped dramatically over the last decade, while the available options have expanded. While we offer PCBs we design for our projects, anyone can make their own custom boards. So, how do you go about turning an idea into a printed circuit board? W e have published several articles about PCB design and manufacturing before. However, we haven’t really explained the entire process of designing and ordering circuit boards from scratch. We wanted to create a series of articles that would be helpful for beginners as well as those who already have some PCB design experience. PCB design is a discipline that is both a science and a bit of an art. This series will offer some techniques and strategies, but PCB design is something that benefits from practice. This article will also talk about processes and terminology. It’s much easier to find information when you know the terms to use. Our Making PCBs article from the July 2019 issue (see siliconchip.au/ Article/11700) mentioned the data and processes that are needed to create a PCB. If you’re not familiar with how PCBs are manufactured, it could 52 Silicon Chip be helpful to have a look at this article to know about the underlying technology and processes. Our review of Altium’s CircuitMaker software from January 2019 (see siliconchip.au/Article/11378) touched on the steps involved in using a software package to turn a circuit into a printed circuit board. But it is not just circuits that can become PCBs. Their price and versatility means that custom PCBs also make excellent panels and enclosure lids; we are sure that they have other uses, too. Electronics design automation (EDA) programs generally include tutorials and guides for getting started. EDA software is more than just PCB design, but that is a large part of it. This series is more about the details that such guides might not cover, including ideas and processes that are involved in good PCB design. Our frequent reviews of the Altium Designer software, most recently in Australia's electronics magazine June (siliconchip.au/Article/18307) reveal that EDA software is continually evolving. Altium Designer We are going to work through the process of PCB design using Altium Designer. It’s the software that we use, but most EDA packages work similarly. So even if you plan to use something else (for example, KiCad), the concepts we discuss will be useful. To keep things simple, we’ll stick to basic two-layer (double-sided) designs. Simple boards like this make up the vast majority of our designs. Two-sided boards are so commonplace now that it isn’t worth the trouble of making a single-sided design. The PCB manufacturers are set up for two-sided processes, and there are unlikely to be savings unless you order thousands of boards. It’s possible to design for boards to be etched by hand, but we have not done that for many years because commercial boards are so inexpensive. There is a free trial option for Altium Designer (www.altium.com/ altium-designer/free-trial/roadmap). The related CircuitMaker package is also free to use, but projects are stored in Altium servers (in “the cloud”) and are visible to other CircuitMaker users. Helpfully, its interface is similar to Altium Designer. See www.altium. com/circuitmaker Both Altium software packages work through two distinct phases. First, there is the process known as ‘schematic capture’. This amounts to drawing the circuit diagram within the software. Internally, the software records the components that are used and how they should be connected. The second stage is PCB layout. This mainly involves placing the components and traces to connect them together. This can be likened to drawing the final PCB design. The many circuit diagrams and PCB overlays in our project articles are taken from these two phases of the PCB project. While it is possible to design a PCB without schematic capture, it’s a far more error-prone process, and we don’t recommend it. The small amount of time invested in drawing the circuit is repaid in the much increased likelihood of your PCB working first time. Before we get to the nitty gritty of PCB design, let’s first look at what we’re trying to achieve. siliconchip.com.au Fig.1: there are lots of options possible when ordering a PCB, but the defaults are usually the quickest and cheapest (and fine for many uses). We suggest sticking with these defaults if you haven’t designed and ordered a PCB before. Source: PCBWay – www. pcbway.com/orderonline. aspx ▶ Fig.2: Altium Designer offers many layer stack options, but the actual parameters shown here are only critical for simulation in cases like RF or high-speed design. It’s simply to show how a PCB is structured and the information here is not processed into the Gerber files. The apparently overly-precise figures are simply imperial values converted into metric. Typical Gerber files for a two-layer board Layer Extensions Board shape/outline .gm, .gm1 or .gbr Top copper .gtl or .gbr Top solder mask .gts or .gbr Top silkscreen overlay .gto or .gbr Bottom copper .gbl or .gbr Bottom solder mask .gbs or .gbr Bottom silkscreen overlay .gbo or .gbr PCB manufacturing Once the PCB layout phase in Altium Designer is complete, “Gerber” files are exported. These are what the PCB manufacturer uses to create the physical boards. In addition to uploading those files (usually as a ‘ZIP’ archive), there will be various options to choose from, such as the colour of the solder mask on the PCB. Fig.1 shows the ordering page, including options, of PCBWay. It looks like a lot of choices, but most of our designs use the defaults as shown. These settings will typically be the cheapest and fastest PCBs to produce. However, it’s worth noting critical siliconchip.com.au parameters like minimum track width and spacing and minimum hole size. These are part of the so-called manufacturing capabilities. For most designs that will be manually assembled, there should be no problem adopting much more generous guidelines. An example can be found at www.pcbway.com/capabilities.html It’s important to set up ‘design rule checks’ that match (or are at least similar to) the manufacturer’s capabilities. This way, the software will flag anything that will cause a manufacturing problem and allow you to fix it before finalising the design. Most of our designs are laid out with margins at least double what is listed Australia's electronics magazine regarding things like trace width and spacing; even the cheapest boards are comfortably within our requirements. However, there are cases, such as when you’re working with fine-pitch SMD ICs, that you have to push close to the standard manufacturing limits. It’s handy to know what PCB manufacturers are capable of producing. If you’re looking to create panels, lids and the like, there is a good range of colours available too. Some even offer full-colour printing on the PCB surface now! Fig.2 shows a so-called layer stack and its visualisation as seen in Altium Designer. The green layers that are not labelled are the solder mask layers; December 2025  53 these are what actually give PCBs their colour, as well as reducing the chance of short circuits while soldering. At left is a ‘via’ connecting the top and bottom copper layers. These seven layers roughly correspond to seven of the eight files in a set of Gerber files. The dielectric layer marks the fibreglass (FR-4) core, and its file indicates the shape of the PCB. An eighth file defines the holes that need to be drilled in the PCB. Most Gerber files are equivalent to a monochrome image, with the colour indicating whether the material on that layer (copper, solder mask or silkscreen printing) is present or not. Due to the way PCBs were historically made, the actual data consists of shapes, called apertures, which are combined to create the final image. Computer technology has changed the way these steps work. The PCB Manufacture panel gives a bit more detail about the different files and layers, and how they relate to the processing steps involved in PCB manufacture. See also the diagram in the panel overleaf showing how various PCB features are created in the various layers. Design overview Fig.3 shows the steps that are required to create a PCB and the associated file types (in the square blocks) that are used in Altium Designer. There will probably be a set of generic component libraries available from your EDA software, but if you are using any components with more than three leads, there is a good chance that you will have to add your own entries. We will cover that too. Schematic capture and PCB layout are fairly manual processes, while the library files and design rules are a major part of the ‘automation’ in EDA. They help to make sure that you end up with a valid and functional result. Tools such as automated design rule checking, automatic routing of traces and hierarchical design can help to speed up the process. The design rules and libraries you use might change depending on how you intend to assemble your PCB. This is part of the field known as ‘design for manufacture’ (DFM). A PCB intended for manual assembly (such as our project PCBs) could be very different from a design intended for mass production through pick-and-place and reflow or wave soldering. For example, we have created library files with large pads and clear silkscreen labels to make manual assembly easier. A mass-produced PCB might cram all the components on one side to avoid a two-pass process. The pads will be small to require a minimal amount of solder and may completely omit silkscreen labels due to lack of space. Consider that the ideal pad size and shape for any given component will be different depending on how it is soldered, what solder is used and even what other components and tracks are nearby. We expect most readers will produce designs for manual assembly like us, so we will concentrate on that. It’s possible to create multi-sheet or multiboard projects with Altium Designer, but we’ll keep it simple, using just a single SchDoc (schematic/circuit) file and a single PcbDoc (board) file. We find that this is sufficient for most our designs. One of the great things about going to the trouble of drawing the circuit in this way is that if you later have to make changes to either the circuit or Fig.3: these are the steps involved in the design and manufacture of a PCB. This article concentrates on setting up libraries, while next month we will discuss design rules and the schematic capture and PCB layout steps, followed by Gerber file exporting and ordering. 54 Silicon Chip Australia's electronics magazine the board, the software will check that they match up. So, for example, if you remove a bunch of tracks to move components, then forget to add one back, it will tell you. You don’t want to find out about it when your new board revision doesn’t work! That’s a lot of background, but we hope that it will provide some insight into why things are done as they are. It’s also the case that there is no single correct way to lay out a PCB; we shall describe the workflow that we find works best for us, but you may decide to vary it once you have some experience. Libraries Good libraries are the foundation of a solid PCB project, so we should start with how to create and use libraries. The Altium Academy channel has a video titled “How To Create Your Own Libraries in Altium Designer” (https:// youtu.be/bOi45nshqP8). Altium can use integrated libraries, but commonly, you will see separate SchLib (symbol) and PcbLib (footprint) files. The schematic library consists of the circuit diagram symbols for various components. They are usually also be linked with specific footprints in the PcbLib file. A footprint corresponds to a physical component package so, for example, the same TO-220 footprint could be used for many component types, such as bipolar transistors, Mosfets, voltage regulators, diodes and so on. There can also be multiple footprints for a given package. Our libraries have variants of the TO-220 package footprint for vertical mounting, horizontal mounting, and with the tab affixed to the PCB using a screw. There are also variants that make provision for a heatsink to be added (possibly even including pads to solder heatsink retaining pins into). The visual representation is important for helping to understand the circuit diagram, but the pins and external connections (such as exposed pads and mounting points) are probably the most critical part. As we go along, keep the Properties tab open so that you are aware of all the different parameters that relate to the elements that you are working with. Fig.4 shows a 74HC595 shift register IC in our SchLib file. The main image shows how it would appear in the circuit during schematic capture. siliconchip.com.au ▶ Fig.5: you can configure your schematic (circuit) symbols however you like. You might see many components laid out like this to neaten the resulting diagrams. Real ICs often have pins in odd places due to silicon limitations; while you can make the symbols reflect that, it isn’t necessary. Fig.4: setting up your libraries will also give you practice in working with the schematic capture and PCB layout tools, since they use similar environments. At lower left are three linked footprints (in a separate PcbLib file); note how they correspond to three different package types. Pin 15 is selected in the main window, and at right are the pin properties, with the mouse pointer selecting from the pin type menu. By making sure this property is set correctly, you can avoid improper connections during schematic capture. The rules will flag cases when a conflict is created, such as when two outputs are connected together, or if an input is not driven by anything. You can also see that the pins on the part show directional arrows for inputs and outputs. A bidirectional pin (such as a microcontroller’s general purpose I/O pin) will show arrows both in and out. The pin names are shown inside the rectangle, and the pin designators (numbers in this case) outside. The designators are what connects a specific pin to a pad within a footprint. This example shows the pins arranged identically to their physical layout. This is not a requirement; other arrangements can be used. Fig.5 shows a CD4017 decade counter with inputs on the left and outputs on the right. The positive supply is at the top and the negative supply at the bottom. siliconchip.com.au This arrangement will almost certainly make the circuit diagram in the SchDoc file neater, but it means that the circuit is less like the PCB layout. However, remember that the point of a schematic diagram is to most clearly represent the function of a circuit, and often that’s quite distinct from the best physical layout on the circuit board. The various components are referenced by their names (design item IDs), so it is important to give unique names to each component. We have adopted the convention of prefixing each name with an underscore to ensure that they are distinct from Altium’s included libraries – see Fig.6. The numerical pin designators that you see are typical for ICs and indeed most components, but this field is a character string, so could be “A” or “K” for the anode or cathode of a diode. “A1” or “A2” could be used for the two anodes of a common-cathode diode. You can also see another very handy feature in Fig.6: components can also be broken into various parts (Part A, Part B etc). In the case of this hex inverter, it makes it easier to swap between using different inverter elements (using a dropdown menu) if this is needed to simplify PCB routing. Parts can also be used to separate logically distinct parts of a component, such as a relay’s contacts and its coil. Altium Designer can handle Fig.6: multi-part components allow flexibility in swapping equivalent sub-parts. Being able to separate the sub-parts can also help in creating a tidy schematic. Australia's electronics magazine December 2025  55 Fig.7: reading and interpreting engineering drawings such as these is a handy skill if you need to create your own footprint libraries. Source: Infineon Technologies – www. infineon.com/assets/row/public/ documents/10/49/infineonbtn8962ta-ds-en.pdf automated pin swapping if you do not wish to do it manually. The schematic editor always works on a 50mil (50/1000in or 1.27mm) grid, so you should make sure that all pins fall on this grid spacing by setting the grid snap. This will make it easier to drag-and-drop wires while editing the schematic. It’s easy to switch between metric and imperial units with the ‘Q’ hotkey. Even components that aren’t connected electrically can be created as components, since the schematic editor can be used to generate a bill of materials (BoM); for example, screws & spacers for mounting. Having a component that can be dropped into the SchDoc file means that it is automatically included in the bill of materials. It’s also a good idea to make sure the names and descriptions are apt, so that the BoM is clear. Something with no electrical connections, like an enclosure, could have a footprint with a 3D body associated, and it would be visible in the 3D view of the PCB and generate an item in the BoM. The enclosure’s footprint could also include a template of the PCB outline so that the PCB’s features can be aligned to the enclosure. 56 Silicon Chip Similarly, components can be marked as ‘no BoM’, meaning they do not generate an entry in the bill of materials. An example of this would be a PCB trace antenna or inductor; there is no separate item that needs to be purchased as the component is effectively part of the PCB. You don’t need to worry about all these ideas right away, but it’s handy to be aware of them when you are creating and editing your library files. This will help make PCB layout go smoothly. Footprints Critical parts of the footprints in the PCB library are the copper layer pads that correspond to the pins in the schematic library. You can also include objects on any layer of the final PCB, and even 3D bodies, which can be used to create quite realistic 3D views of the PCB. By default, the pad designators are matched to the pin designators, but this can be changed if necessary. For simplicity, we try to keep our libraries so that the pin and pad designators match. Creating a footprint from scratch generally requires the component data Australia's electronics magazine sheet to provide the recommended pad geometry. Fig.7 shows the relevant page from the data sheet for the BTN8962 half-bridge driver, with the manufacturer’s suggested pad layout diagram at lower right. Manufacturer-recommended footprints are usually quite compact; we would consider lengthening some of the pads to ease soldering. We’ve found that these sort of diagrams need to be studied quite carefully. The pad sizes are clear enough, but because Altium Designer’s coordinate system is based on the centre of the pads, the pad coordinates will need to be deduced. Note that the pad pitch (which will match the distances between pad centres) is not shown at lower right, but it is marked elsewhere. The Properties tab comes in handy here, since you can directly enter the coordinates that you have calculated. Multiple pads in a row can be selected together and lined up by entering a coordinate that is used for all of them. Although many programs use Ctrl+click to add items to a selection, Altium Designer uses Shift+click for this purpose. For example, we can easily lay out the lower row of pads by putting the centre pad at a zero X-coordinate. The other pads can be placed at multiples of the 1.27mm (50 thou/mil or 0.05in) pin pitch. Knowing metric and imperial equivalents can come in handy. Setting the grid snap to match the pin pitch (or a fraction of it) can also be helpful. You might find an existing footprint in another library that will work, especially if it is a reasonably common type. Altium Designer also has two different footprint creation wizard tools, found under the Tools menu. These work quite well for packages that have a regular pin arrangement. Otherwise, the process of creating a footprint is similar to that for a symbol. The pads are placed as needed, with their shape, size and hole diameter defined. There is no need to manually lay out the solder mask layer, since the pads include both copper and solder mask elements. Silkscreen designators will be added by Altium Designer automatically during the PCB layout stage. Adding just the eight pad elements here will be sufficient to create a functional part. Our libraries include additional component outlines on the silkscreen siliconchip.com.au The PCB Manufacturing Process This is a brief overview of the files in a Gerber set and how they are used to physically create a board. This is for a two-layer PCB; boards with more layers simply have extra files. Often, the PCBs will be laid out in a large panel, possibly with other different designs, with the final step being to separate the PCBs from the panel before shipping them to customers. Our explanation below will necessarily be simplified. The steps shown adjacent are from PCBWay’s website. They also have videos showing the details of each of these steps. Note that steps 3-6 only apply to multi-layer (more than two-layer) boards. You can see the videos at www.pcbway.com/ pcb-service.html The process starts with a large panel of copper-clad FR-4 fibreglass laminate. The most common PCBs use a copper thickness of 0.025mm, which is equivalent to 1oz (28g) of copper per square foot bonded to 1.5mm thick fibreglass (resulting in a nominally 1.6mm finished PCB). Thicker copper layers can be created by electroplating. The first step is to drill and plate the plated holes. These are holes that connect the two sides of a PCB, and might be part of a via or through-hole pad. Thus, they will connect copper areas on both sides of the PCB. The drill locations are stored in an ‘NC drill file’; NC stands for numerical control and the format is quite similar to the GCODE commands that are used to drive CNC machines, including 3D printers. Altium exports these with a TXT file extension, and they are readable with a text editor (like the Gerber files). The drill file itself makes no distinction between plated and nonplated holes. Instead, it is assumed that holes that end inside a copper area at both ends are plated, while those that end in areas without copper are Ground Pour: polygon on top of copper layer This shows the numerous steps involved in manufacturing a PCB. Source: PCBWay – www. pcbway.com/pcb-service. html non-plated. Holes that are ambiguous will probably be flagged as errors by the PCB engineers. (Sometimes people put plated and non-plated holes in separate files.) The design rules typically specify a minimum annular ring (around a hole) that ensures the distinction is clear. Some holes, especially those that aren’t round, such as slotted or irregular shapes, might be defined in the outline layer (GMx file). These are also made at this stage, using a milling machine. The holes are then plated. A chemical process adds a thin layer of copper, which is then thickened by electroplating. Electroplating is much easier to do while there are solid conducting areas of copper on both sides of a PCB. The next step is to etch the copper layers. First, resist layers are applied to the top and bottom of the board using a dry film process similar to DIY PCB etching. Transparency masks are computer-­ generated from the GTL (top layer) and GBL (bottom layer) Gerber files and printed. The resist is cured using the transparencies, and the uncured resist is removed to allow the etchant to act on the copper. Then, the solder mask layers are applied. The apertures in the solder mask Gerber files (GTS and GBS) are used to mark where there are holes in the solder SMD Pad: usually square on top copper and solder mask layers TH Pad: shapes (circles, rectangles or stadium) on copper and solder mask layers possibly with a throughhole VIA: like a TH pad, PCB ID: Non-Plated Hole: drill hole Designators: text on but with no solder text on top not surrounded by copper silkscreen layer mask opening copper layer The anatomy of a printed circuit board. Various items on the PCB are created from elements in different layers here. Fortunately, most EDA programs will manage all the elements when a pad is placed on the PCB. siliconchip.com.au Australia's electronics magazine mask, so it works in the opposite (negative) fashion to the other layers, which normally mark where the material should remain. The etched PCBs are coated with a film of liquid solder mask ink. The ink is selectively cured by exposing it to ultraviolet (UV) light from a projector. This technology is similar to that used in resin 3D printing. The uncured resin is cleaned off, and the remaining ink may be cured further. It’s at this stage that a surface finish may be applied to the bare copper to prevent it oxidising and to improve solderability. We use the HASL (hot air solder level) treatment on the majority of our boards. This involves dipping the entire board into liquid solder, where it adheres to the exposed copper. The excess solder is then blown off using hot air. A different process called ENIG (electroless nickel immersion gold) uses a chemical process to plate a thin layer of nickel onto the copper. Another chemical step then plates gold over the nickel. The nickel layer is needed so that the reaction that deposits the gold can proceed. The silkscreen overlays are added next (GTO and GBO layers). These also use a UV-reactive ink that works like the solder mask layer, except that it is exposed and printed in a positive fashion. The liquid silkscreen is applied and selectively cured. Excess ink is washed away, and the remaining ink is fully cured. The remaining unplated holes and slots are then cut, drilled or routed as needed, using the TXT and GMx layers. This will include the board outline, and will thus result in the board being removed from its panel. There may be a number of different test and inspection steps that occur during the process. AOI (automatic optical inspection) can be used to compare the board appearance to that expected from the Gerber files, while various electrical tests can be used to ensure that the traces have no breaks or short circuits. Once the board has passed testing, it is complete, and it will be packaged and shipped. December 2025  57 layer to ease assembly of the PCB. They also make it easier to see conflicts, such as where components would overlap, for example. You can add unconnected mounting or clearance holes. Like the symbol pins, these are usually marked as such by using the ‘0’ designator. Manufacturer Part Search Many manufacturers now supply library files, so it is easier to use their parts. Thus, it’s worth mentioning the Manufacturer Part Search feature of Altium Designer. It can be opened from the Panels button. Some, but not all, components can be added to your libraries by simply downloading them from the internet. Fig.8 shows this panel, along with a search for BTN8962 half-bridge driver IC. You can see that the listed part name has its full suffix shown, since we need to be specific about which particular package we wish to import. The dropdown labelled “12 SPNs” refers to supplier part numbers; you can click through here to see the listed part at a supplier like Mouser or DigiKey. The search has two results, and the top result includes the models we need for our libraries. The second result with the red struck-out icon does not contain models, and will not help us. Models are visible below that, with the schematic symbol followed by the footprints. You can download the models by right-clicking on the listed item and selecting the option to ‘Download as File Library’. The download is a ZIP file containing several library items. We find it easy to simply open each library file and to copy and paste the items into our own libraries, where they can then be edited as needed. For example, we would change the symbol name to fit our naming scheme. You can also see that the footprint library contains three different footprints. If in doubt, choose the “L” low-density variant, since this will be the easiest to manually solder. The “N” variant is what would likely be used for a mass-produced PCB. You should also check the footprints on downloaded models to be sure that the layers correspond to your conventions. We typically use mechanical layer 15 (GM15) for the board outline, but some models use this for the component courtyard (outline). If this were not changed, we might end up with holes all over the PCB, since we 58 Silicon Chip also use that layer for unplated slots (routed out of the PCB). Making footprints Items like connectors will probably need to be made from scratch unless a downloadable model is available, since they can vary so much. Many SMD connectors also include throughhole mounting pads, so they will need a mix of pads. Most surface-mounting pads simply exist on the top layer (and can be flipped onto the bottom layer with the component). They are automatically allocated a matching solder mask outline, which is expanded slightly to ensure that the pad is fully uncovered, even if there is a slight misalignment. Thus, you don’t need to worry about creating separate items in the copper and solder mask layers. Through-holes are created as a ‘Multi-layer’ item, which includes a drill hole (with settable diameter) and top and bottom layer pads, which can be various shapes including square, round or lozenge-shaped. The two layers are matched in size by default, but each can be set separately. You can also offset the hole centre from the pad centre if needed. We prefer to work with through-hole parts in imperial dimensions, since many components are on a 100mil (0.1in or 2.54mm) pitch. A non-plated hole can be created by setting the pad (copper) layers to have an X-Size and Y-Size of zero. Such a hole could be used for a mounting screw or LED to pass through. It’s a good idea to centre your footprints on the origin (0,0) and arrange them symmetrically if possible. By all means, copy and paste existing footprints (and symbols), then modify them. It will make things easier and will ensure that the style of your components remains consistent. Altium Designer also supports many layers beyond the ones that are needed for PCB manufacturing. Layer Mechanical-1 is often used for so-called 3D bodies, which are the entities used to create 3D views of the components. The simplest of these are extruded shapes, such as a rectangle extruded vertically to form a cuboid, or a circle extruded into a cylinder. Adding even a single 3D body to each component will allow you to better visualise a completed board. In Fig.8, our downloaded model of the BTN8962 includes a simple cuboid 3D body. We often use Mechanical-14 for reference marks and ‘fiducials’. For designs that are mounted in an enclosure, we can mark its walls so that things like jacks and sockets can be aligned correctly. They can also be used to help create the cutting and drilling diagrams, since dimensions and coordinates can be directly read from the Properties. Summary Fig.8: the Manufacturer Part Search can remove the need to do a lot of the work in creating components and footprints within your libraries. However, not all components are supported, and we recommend thoroughly checking the imported files for correctness and consistency. Next month, we will look at some of the strategies we use for designing PCBs, both during schematic capture and PCB layout. This will also include aspects such as PCB design rules. We will follow with the steps involved in finalising your Gerber files and sending them away to be manufactured. In the meantime, you can start SC building your libraries. Australia's electronics magazine siliconchip.com.au