Fullscreen HTML5Med Res (??MB)HTML4

“Hands On” review and tutorial by Tim Blythman Aimed at “makers” and electronics hobbyists, CircuitMaker is free circuit and PCB design software, from the creators of professional PCB software Altium. In fact, if you have used Altium, you will find CircuitMaker familiar. If you haven’t designed a PCB before, but want to, it’s a great way to get started. This article goes through the all steps from installing the software to producing the files needed to manufacture your PCB. W e use Altium Designer for PCB design here at SILICON CHIP. You may recall our review of Altium Designer 18 in the August 2018 issue (siliconchip. com.au/Article/11189). But Altium also produces another piece of software named CircuitMaker, which is also EDA (electronic design automation) software but is targeted at hobbyists and “makers”. And while Altium Designer costs quite a lot to buy, CircuitMaker is free! While this sounds like a great deal, there are, of course, some restrictions. All projects are stored in Altium’s “cloud” server, and are also available to be viewed by anyone who has a CircuitMaker account. Anyone can make a copy of someone else’s project and add it to their own collection. Such projects may also be subject to open-source licensing restrictions; these vary, but you may be required to make your design files available if they have been derived from another open-source project. As you might expect, CircuitMaker does not have all the features that Altium Designer boasts. For example, it doesn’t have support to simulate the circuit that you draw. But it still has pretty much all the features you need, including an advanced auto-router. This is an introduction to using CircuitMaker, suitable for those who are new to EDA software. We’re going to assume that you’re fairly comfortable with computer software in general, and we will point out some of the things we noticed along the way. As with many Altium products, CircuitMaker is re78 Silicon Chip stricted to the Windows operating system (version 7 or later), although you can browse and view projects from the Circuit Maker website in a browser on many other platforms. You might like to have a look at some of the projects that have been created by others now. These can be found on CircuitMaker’s project page, at: https://circuitmaker. com/Projects A brief introduction to EDA With a modern EDA tool, the design starts with a process called “schematic capture”, ie, drawing the circuit diagram in CircuitMaker. It mainly involves placing components on the schematic and then drawing wires to connect them in the desired fashion. While you are doing this, the software is generating a “netlist”. Each connected group of wires is called a net and is given a unique designation (name). Circuit simulation programs also use netlist files; while CircuitMaker does not have this feature, Altium Designer 18 does. Each component on the circuit is also assigned a “footprint”. This is a representation of the physical component and is used in the later PCB layout stage. A given component can have many different footprints associated with it (such as SOIC and DIP for an IC). While these may look the same in the schematic, they require different handling on the PCB. Once the schematic is complete, it is transferred to the PCB layout editor, populating the blank PCB with all the required component footprints. These can then be dragged into place Australia’s electronics magazine siliconchip.com.au Fig.1: the Layer Stack Manager tells CircuitMaker how the PCB is going to be assembled. This default view shows how a typical doublesided PCB is made. The Gerber files produced at the end of the process consist of one file for each of these layers, plus an eighth which dictates where holes are to be drilled. on the PCB and connected by tracks and vias. A design rules engine ensures that manufacturing tolerances are maintained (such as minimum track separation) and confirms that all nets have been properly routed. The traces on the PCB can be routed manually or an autorouter can run the tracks automatically. While auto-routers keep getting better, they don’t always produce ideal results. The final stage is to export the project in a format which can be used to manufacture your design. These are typically in the “Gerber” format, which virtually all PCB manufacturers accept. In the near future, we hope to do a review of the various ways that you can PCBs made, both at home and from fabricators who will do this for you. Gerber files can be used for all these methods. A two-layer board, such as those we typically create at SILICON CHIP , will consist of eight files (usually bundled inside a zip file), each of which corresponds to a layer within the PCB layout editor. When we speak of a two-layer board, we are referring to it having two conductive copper layers, one on each side of the dielectric (insulating) core, which is typically made from FR4 fibreglass (or Kapton film in a flexible PCB). But there are also separate solder mask, drilling and outline (silkscreen) layer files. These additional files are used at different stages in the manufacturing process. In fact, the various component footprints consist of not much more than a specific arrangement of shapes, such as circles and polygons, on the various layers. A simple pad or via consists of a hole on the drill layer, a copper disc on the top and bottom copper layers, and a similarly sized hole in the solder mask, and may have, for example, a hollow circle defining its footprint on the overlay layer – see Fig.1. Installing CircuitMaker Before downloading and installing CircuitMaker to your Windows PC you need an Altium account, which in turn Fig.2: the CircuitMaker main page appears immediately after launching the software. You can browse other users’ projects, and even make copies for your own use. Not surprisingly, the “My Projects” tab is where you will find your own projects. siliconchip.com.au Australia’s electronics magazine January 2019  79 some local copies are kept in addition to the files kept on Altium’s cloud server. Once the installation is complete, open CircuitMaker and log in. The start page (Fig.2) lists your projects which are stored on Altium’s servers. Starting off with CircuitMaker Fig.3: the Octopart library has a vast number of parts; we couldn’t even count how many 1k resistors there are. When choosing a component for use in CircuitMaker, make sure that it has a PCB footprint. The small black box with a green tick tells us this is the case for this part. Take care that the footprint matches the part you will actually use. requires an email address. You can sign up for one at: https://workspace.circuitmaker.com/Account/SignUp This will send an activation link to your email, which validates your account. You can then use your credentials to sign in at https:// workspace.circuitmaker.com/Account/Login and click “Download” to download and then run the installer. The installer has a long EULA (end-user license agreement) that you will need to agree to before proceeding and you will then be prompted to enter your Altium/CircuitMaker credentials before it installs. The version we installed downloaded another 660MB of files. We normally keep our documents on a network drive, which the installer refused to accept, so we had to set our documents storage location on a local hard drive. It appears 80 Silicon Chip A CircuitMaker project consists of a main project file, which usually contains at least one schematic (.SchDoc file) and one or more PCB files (.CMPcbDoc). It may include other types of files too. To begin, click “My Projects” on the Start tab, then click “Add New Project”. Enter a name and description and choose whether it will be stored in the public folder or a private sandbox. You’re allowed to have two files in the private sandbox, and these cannot be seen by other users. Anything in the public folder can be seen by other users. If you like, you can find our “Simple Uno Clone” project and make a copy of it in your account by using the “fork” option. If you are not sure, you may wish to start with the sandbox. You need to save and then open the project to start working on it. The project will appear in the “Projects” tab at left. From here, you can right-click on the project name, select “Add new to project” and click “Schematic”. Change the name if you wish, then press Enter. You are presented with a blank sheet onto which you can add components. We found this stage was one of the more challenging, but also demonstrates the power of the cloud-based setup. There are literally millions of components to choose from, with many of them added by other users and available to everyone. As with many open source projects, the quality of the user-added content varies. For example, when we were looking for header pins, we found a number that had been customised by other users for a specific role, rather than having a simple set of numbered pins. Another example is that the capacitors we were using for one project contained elements on the board outline layer; if we had used these footprints as-is, the manufacturer would have cut a rectangle out of the board, leaving nothing but a hole for the component to mount on! While many users, particularly those who sell their finished designs, may use specific parts from specific manufacturers in their design; however we often use generic parts in our design. For example, we may want to place a ¼W resistor which you can buy from any retailer. But we couldn’t easily find a generic “¼ W resistor” component that we could use. To add a component, you need to choose one from the many that are available. Pressing the component button on the ribbon opens up a dialog box, from which you can click the “Choose” button to open a search window. The search window is limited to 25 entries, which can be quite limiting. It’s more helpful to click the “View” ribbon button and select “Libraries”. At the top of the panel that appears, you can select between “Favorites”, “Octopart” and “Project”. As you won’t have any favourites yet, choose “Octopart”. Octopart is a company owned by Altium, mainly known for their website octopart.com which collects data from various suppliers (such as element14, Digikey and Mouser) which can then be searched in one place. Australia’s electronics magazine siliconchip.com.au Fig.4: our completed schematic for a simple Arduino Uno clone. We have used ports (the yellow lozenges) for our power connections to simplify the appearance of the wiring. We found it helpful to search on the Octopart website alongside the library view (Fig.3), as the specific manufacturer part numbers gave definitive search results. The Library view gives a lot more information than the basic component window, and in particular, you can tell straight away whether a part has a PCB footprint available. This is important, as we cannot complete the PCB design without a component footprint. We finally found what we needed by searching for “1k resistor axial” and selecting the first item in the list. Once you have found a match for your component, you can rightclick it to add it to your favourites. When you’ve established a good set of favourites, you will not need to spend as much time searching for commonly-used parts. Once you have found the part you need, click “Place” to add it to your schematic. The part appears under the mouse pointer and can be placed multiple times by clicking repeatedly. Stop placing components by pressing the “Escape” key. Once you have opened the library, you will notice it minimises to a small icon to the side of the window, and can be opened again by clicking on the icon. Having placed a part, you will see that it has text above and below it. The upper text (initially “R?” for a resistor, for example) is the designator while the lower text is a comment, which is useful for extra information such as component values or IC part numbers. Either can be edited by double-clicking and changing the “Value” parameter. In our case, we changed “R?” to “R1”. A component can be moved by clicking and dragging it, and if you press the space-bar while the mouse button is down, the component will rotate by 90°. Similarly, pressing “X” or “Y” will flip the part around the horizontal and vertical axes respectively. Once the components have been added and roughly placed, wires can be added by selecting “Wire” from the home ribbon, or simply pressing “W” on the keyboard. This follows an intuitive click and drag process, with the pointer lighting up with a red cross when a connection is ready to be made. As with the place command, pressing “Escape” will cease wiring. Many of the shortcut keys are worth remembering, as they are also used similarly in the PCB editor. You can move components after they have been wired and the wires will generally remain attached to the components. A wire (or component) can be removed by clicking on it and pressing “Delete”. If you have wires that have many connections (power connections would be a typical example), you can add a “Port”, found among the circuit elements. Any ports with the same name are considered connected, meaning wires don’t have to snake all over the schematic. Navigating around the circuit You can hold down the right mouse button and move the mouse to move around the document, as though by dragging. Pressing <Ctrl> while scrolling the mouse wheel zooms in and out. You can also zoom in and out using the “View” menu. Fig.5: the so-called “rat’s nest” that is visible at the start of PCB layout is always messy (hence the name), but clever component placement is the key to turning this into a working PCB. siliconchip.com.au Australia’s electronics magazine January 2019  81 These shortcuts can be changed by clicking on “My Account” from the Start page, and choosing “Preferences”, and then select the System => General Settings option. Creating a PCB layout Once you have finished drawing the circuit (ours is shown in Fig.4), you can proceed to PCB layout. The first step is to create a PCB layout file (.CMPcbDoc) within your project. Right-click on the project name, select “Add New to Project” and click “PCB”. The next step is to transfer the components and netlist from the schematic to the PCB layout. This is done by selecting Project from the Home ribbon, and selecting “Update PCB document...”, or by pressing Ctrl-F5. This brings up a dialog box listing the changes that will be made to the PCB document. It’s a good chance to review what changes are occurring, and you can untick any of the changes if you don’t want them to affect PCB. Usually, though, you leave all options checked, and click “Execute changes”. If, for example, you notice during the PCB layout stage that you have made an error in the circuit, you can go back to the schematic, make the changes, and then use the “Update PCB document” option again to push the changes through to the PCB layout. This is important, as later when we come to check that the PCB is fit for manufacture, everything needs to be consistent. You will now find your PCB document contains a jumble of part footprints that need to be rearranged and connected (see Fig.5). It is said that most of the work in PCB layout is placing the components correctly, so it pays to take your time and organise the components well. The components are connected by fine lines which show where a connection needs to be made. This is often referred to as the “rat’s nest”. Ideally, you should place the components to minimise the length of these links, and also how many times they cross (as it’s not always easy to cross traces on a PCB). As in the Schematic editor, you can use the space bar, X and Y key to rotate and flip the components as you move them. CircuitMaker, like Altium, has a good set of keyboard shortcuts, and we often find that we have our left hand of the keyboard and right hand on the mouse as we work with these programs (you would do the opposite if you are left-handed). Routing tracks To manually lay track, click on the “Route” button on the Home ribbon, then click on the PCB to start the track. Typically, a track will run between two or more components, so it makes sense to start on a component. Clicking again will ‘lock’ the track so that if you need to route it around another component, it won’t collapse on itself. Keep going until you have clicked on an endpoint, then click one more time and press “Escape” to finish routing the track. You will notice that the program automatically avoids conflicting paths and pads, and it will follow a neat 45° path along the way. Much of the cleverness of routing comes from it automatically trying to enforce design rules (such as track spacing in this case) as the routing occurs. Altium refers to this as interactive routing. The layer tabs are useful during the track layout stage, as 82 Silicon Chip Fig 6: the simple Uno Clone, after it has been routed. The top copper layer is shown in red and the bottom copper layer is blue. The colour codes can be seen at the bottom of the PCB editor window and you can change them if you want to. you can switch between layers easily. Pressing “*” on the numeric keypad will toggle between top and bottom copper layers, and if pressed while laying a track, will place a via to allow the trace to continue on the other side of the board. Another useful design rule which you may wish to change, especially for high current designs, is the track width. The track width design rule consists of a minimum, preferred and maximum value. During track routing, pressing “3” will cause the currently laid track to cycle between these widths, allowing you to quickly lay a combination of power and signal tracks. If you wish to try the Auto-router, switch to the Tools ribbon and click “Autoroute”. The default setup is fine, so you can select “All”. We’d recommend selecting “Lock all pre-routes” so that any tracks you have already laid will not be changed. Finally, click “Route All”. To stop the Auto-router, press the “Stop” button on the ribbon. Ctrl-Z (undo) can be used to revert, if you find the layout isn’t to your liking. We usually don’t use Auto-route much, except to check if a component layout is routable. We find that if the computer can complete the routing, a human will do a neater job (see Fig.6). PCB size and shape The board size and shape can be changed at any time, and can be done in several different ways from the “Board Shape” option on the Home ribbon. “Redefine Board Shape” allows you to draw the outline of your board using the mouse pointer, while “Edit Board Shape” allows the existing shape to be tweaked by dragging the existing edges and corners. If you need to create a complex shape, you can compose it from lines and arcs. At the bottom of the PCB editor, there are small tabs representing all the layers. Select the “Outline” layer, then use the line and arc tools under “Place” to draw the outline. Under “Clipboard”, click Select, then “all on layer”. Finally, select Board Shape and Australia’s electronics magazine siliconchip.com.au Fig.7: the 3D rendering is a great tool for visualising that the PCB looks ‘right’, but there are some limitations. If a component does not have a 3D body associated with it (like crystal X1), then the component won’t appear. On the other hand, the footprints of the headers we are using are suitable for male or female parts to be fitted. Note also that the rendered diode body lacks a cathode stripe. Define from Selected Objects. A 3D view of the PCB The PCB 3D view (see Fig.7) can be a handy tool as you are working on the board. You can’t do any editing in 3D mode, but it helps you to visualise how the PCB is coming together. You can get an idea of whether there would be issues with assembly due to the components being too close and so on. You can enter 3D mode by pressing “3” on the keyboard, and return to 2D mode with “2”. Panning is the same as 2D mode, and is done by right-clicking and dragging, while rotation is achieved by shift+right-clicking the mouse. Much of the 3D content (such as component shapes) is from the community, so you may find that not all your components appear as you would expect. If you feel that some of this content could be improved, CircuitMaker provides the means for users to add things like footprints and 3D shapes to components. Design rules Another important item to consider at this stage is the Design Rules (see Fig.8). The “Design Rules” button on the Home ribbon is used to set the rules while the “Design Rule Check” option is used to verify that your PCB meets the rules. The Design Rules are the criteria used to confirm that a board can be successfully manufactured. For example, a board manufacturer might specify that they can produce tracks down to 8 mils in width (0.008”), with a spacing of 10 mils. If you run a track that’s smaller than this, or closer than that, the board you get back may be faulty. So you want the software to alert you if that is the case. The default design rules are quite conservative, so that even a layout that falls afoul of some of these rules can probably be manufactured. Most board fabrication firms publish their design rules, so you can set them correctly in your software. siliconchip.com.au While ideally you should set the design rules up correctly from the start, you certainly can lay out a board and then adjust the rules later. A Design Rule Check will then indicate which areas of the board need attention. You can apply complex rules to certain parts of the board instead of the whole. These can apply to certain nets, for example, to require thicker tracks for those that carry higher currents, or to require more spacing to provide isolation from high-voltage traces. To take advantage of the Design Rules, click on “Design Rule Check”, and then click “Run Design Rule Check” in the window that appears. You will have a list of ‘violations’ appear. If this list is empty, all is well. If you have not finished routing, you should see a number of “Un-Routed Net Constraint” violations. This just indicates that there are no tracks joining points which should be joined, and the layout cannot be considered complete. One constraint which we had to reduce on our design was the “SilkToSolderMaskClearance” constraint, which is the separation between objects on the silkscreen overlay from holes in the solder mask. The problem is that many footprints contain violations of this rule, so you cannot fix them by changing the layout. You would have to edit all the components to eliminate the errors. Manufacturers generally fix this for you anyway, removing any silkscreen lines which intersect with holes in the solder mask. It’s a good idea to ensure that the design rules are fully satisfied before exporting the board. This may require rerouting or rearranging the board, or even modifying the design rules to suit the actual design rule limitations of the board fabrication process. Otherwise, you might get complaints from the manufacturer, or in the worst case, boards which don’t work. Exporting to Gerber files As well as saving the individual files, you also have the option to ‘commit’ the project. This is part of the in-built version control that CircuitMaker provides; there is also an option to revert a project to an earlier stage. Before producing Gerber files, you may be required to commit your project. Once the board is laid out and all the design rules are satisfied, the board can be exported. We prefer to use a two-step process. The first step exports all files except for the drill holes, and the second part exports a file with the drill holes. The reason for this is that the standard drill file format is slightly different than the others (it’s known as “Excellon”). The following export settings work with a number of the board fabrication firms we have tried, but yours may differ. Since the Gerber exporter for CircuitMaker is nearly identical to Altium Designer, any published settings for Altium Designer should work fine. From the PCB layout document, click the “Output” ribbon, and then “Gerber”. On the dialog box that opens up, work through the tabs from left to right. On the General tab, select Inches and 2:5 format. On the Layers tab, select Top Overlay, Top Solder, Top Layer, Bottom Layer, Bottom Solder, Bottom Overlay and Outline. These should be seven of the first nine items, skipping the two Paste layers. The Paste layers are needed for solder paste masks, which you generally don’t need unless Australia’s electronics magazine January 2019  83 Fig.8: rules, rules, rules! The design rules are essential in ensuring that your design can be manufactured. Helpfully, the small diagram indicates where the constraint applies. The rules for your board fabricator may not match CircuitMaker’s defaults but it doesn’t take long to change them to suit. you are having your board fully assembled. Skip the Drill Drawing tab; we will export a separate drill file next. On the Apertures tab, ensure Embedded Apertures is ticked, and on the Advanced tab, the “Generate DRC Rules export file” should be unticked. Click OK, and a save dialog box will appear. Save the file in a known location. The Gerbers are saved as a zip file containing the individual layer files, and we will have to add the drill file later. Windows 10 natively supports working with zip files, although we have long used the 7zip program for working with zip files too. To generate the drill file, click on “NC Drill Files” on the Output ribbon. As for the other files, ensure that Inches and 2:5 format are selected, then click OK, and save the file in the same location. You should have two zip files with similar names. The final step is to add the drill file into the zip which already contains the other Gerber files (see Fig.9). Checking the Gerbers Before sending the files to a manufacturer, it’s a good idea to check them by viewing them with software like gerbv (http://gerbv.geda-project.org/). This was how we spotted the errant board outline strokes from our dodgy capacitor footprints. Simply extract all the files and then open them one at a time in gerbv. You can assign preferred colours and switch layers on and off. Ordering the boards You can then send the Gerber files to be manufactured. Many fabricators provide an online Gerber viewer service. We recommend using this to check that the file appears as you think it should. It’s a good sanity check that the files you have created are compatible with the fabricator’s systems. There are many PCB manufacturers, both here in Australia and overseas, who offer low-cost options for low quantities. Several of these advertise regularly in SILICON CHIP, either in display ads or in “Market Centre”. We haven’t had the opportunity to try all of them but we would be very surprised if they couldn’t all handle your Gerber files. We suggest emailing the manufacturer(s) to check out their pricing for one-off PCBs of the size you are considering. If you have placed the project in your public CircuitMaker 84 Silicon Chip Fig 9: if your Gerber zip file has been assembled correctly, it should look something like this. There should be eight files with the file extensions shown (or similar). For some reason, Excellon NC Drill files usually have a .TXT extension (all Gerber files are essentially text files anyway). Your system may show different file types if these files are associated with a different program. folder, you may wish to publish photos of the completed board or circuit to encourage others to use and improve it. You may even find other users can suggest improvements; this is one of the great advantages of the collaborative nature of open source software in general. Conclusion So you can see from the above that you get many of the useful features from Altium Designer but don’t have to pay a lot of money to do so. The old adage “you get what you pay for” is definitely not true with CircuitMaker! While the package is fairly intuitive after you have had some time to familiarise yourself with its interface, there is extensive documentation available. To answer any questions you may have, check out the docs, including a sample project walk-through, at: https://documentation. circuitmaker.com/ SC Can you export a CircuitMaker file for use elsewhere? The short answer is yes . . . but in some cases there may be a little work required. In general, you simply open the project in CircuitMaker and on the Project ribbon, click ‘Release Project’. Select at least one output from the list presented and click Release. Now, when you view the project on either the CircuitMaker website, the ‘Release’ can be found under ‘Components and Releases’ for that project. Click the download button to download a zip file of the project. The zip file contains the design files inside a ‘Design’ subfolder, and the exported files in the ‘Released’ folder. To open in Altium Designer: If you wish to open the files in Altium Designer, make a copy of them. The .SchDoc schematic file can be opened directly, while the .CMPcbDoc will need to be imported. To i m p o r t i n A l t i u m D e s i g n e r, c l i c k File=>Import=>Altium PCB, and browse to the .CMPcbDoc file and open it. Australia’s electronics magazine siliconchip.com.au