Fullscreen HTML5Med Res (??MB)HTML4

Hands-On PC BOARD DESIGN For Beginners; Pt.2 This month, we describe how to use the basic features of Autotrax to create a simple PC board design. Along the way, you’ll learn about layout defaults, placing components and routing tracks. You’ll also learn how to edit and create your own component libraries. B By PETER SMITH OTH THE MOUSE and keyboard can be used to navigate the menu structure and edit board layouts within Autotrax. In practice, you’ll use a combination of both. Let’s see how it works. The main menu is displayed by pressing <Enter> or clicking <Left Mouse>. Selections within the menu are then made either with mouse movement or with the arrow keys. To exit the menu at any point, hit <Esc> or click <Right Mouse>. It is also possible to navigate the menus by simply keying in the first character of the desired entry. For example, pressing <F> <Q> <Y> in sequence is equivalent to selecting File -> Quit -> Yes from the menu. A number of often-used menu items can also be accessed using control keys. For example, holding down <Ctrl> and pressing <P> jumps to Current -> Pad Type. A list of the commonly used short66  Silicon Chip cut keys appears in Table 1. Note that once selected, editing functions (such as pad/track placement) remain active until after you’ve hit the <Esc> key or clicked <Right Mouse>. However, you can switch active layers with the <+> and <-> keys on the numeric keypad or change the zoom level with <Z> even while in edit mode. Setting options Shortcut keys, layer and menu colours and a whole host of other editing functions can be customised from within Autotrax’s Setup menu (Fig.1). To get to the Setup menu, start Autotrax and press <Esc> when prompted to load a PCB file. Next, press <Enter> to display the main menu and choose Setup from the list, or simply press <S>. To get up and running with your first design, you need only review the settings within two out of the 10 menu entries (see Figs.2 & 3). The remaining options can remain at their defaults for now. Now back at the main menu, press <C> to display the Current menu. Settings here determine the defaults used when laying down your design. Many of these will be changed “on the fly”, as the design progresses. However, the grid must always remain set to “Imperial” and the floating origin to “0,0”. Fig.4 shows typical defaults. Many of the Current settings are displayed along the status line at the bottom of the screen. These are interpreted as follows: L - layer, P - pad type, T - track width, S - string size, G - snap grid. The X & Y values show the current cursor position in thousandths of an inch. Grid size Next, press <G> to set the grids. We recommend 25 thou for the snap grid and 100 thou for the visible grid. Generally, you should leave the snap grid set to 25 thou throughout the design. This is a very important requirement. If a board is routed on different grids, it will be difficult to get tracks and pads to “snap together” nicely. It will also make it much more difficult to maintain minimum manufacturing clearances between tracks/ pads. On occasion, a finer grid will be needed for working in tight areas, or when connecting metric-leaded components, for example. In this case, step www.siliconchip.com.au down to a 5-thou snap grid just for the particular area of interest. Defining the board outline Elsewhere in this article, you’ll find details of a simple PC board design (for a power supply) that we’ve created to help demonstrate the essentials. Rather than “pulling apart” the completed design, let’s start at the beginning – and recreate the design from scratch. The first task is to define the board outline. For any project, board shape and size will depend on the number and size of components, as well as the dimensions of the enclosure (if any) that you wish to fit the final product into. Our power supply will be a freestanding module, without an enclosure. Therefore, the initial board size is just an educated guess and can be adjusted at a later stage if necessary. The board outline is drawn on the top overlay, using a 10-thou track width. To do this, first check the current layer and track size, which you’ll remember is always visible on the status line. Use the <+> key on the numeric keypad to switch from the bottom layer to top overlay if necessary. To change track width, simply hit <Ctrl + T>. Press the <P> then <T> keys to enter track placement mode and position the cursor at the bottom left of the work space (X:0, Y:0). Click <Left Mouse> to start laying the track. Move in a vertical direction for 2.7” (X:0, Y:2700), then click <Left Mouse> again. You’ll probably need to zoom in to get a closer look; hit <F6> to move closer, <F5> to move away or <F10> to fill the screen with your work thus far. Now move in a horizontal direction for 1.45” (X:1450, Y:2700) and click <Left Mouse> again. This completes the left side and one end of the board outline. Continue the track down the right side and opposite end to form a complete rectangle. If you make a mistake, first press <Esc> or click <Right Mouse> to exit track placement mode. Next, press <D> <T> and click on the track to delete it. When done, press <Esc> again to exit track deletion mode. Deleting and replacing tracks is just one way of editing a design. In most cases, it is quicker to edit the track position (or its end point or route). This can be achieved with the Track, Drag End and Re-route commands, acceswww.siliconchip.com.au Fig.1: design defaults and user preferences are accessible via the Setup menu. Fig.2: the Toggle Layers menu allows you to switch on only the layers that you need. As shown here, single-sided designs require only the Bottom Layer, Top Overlay and MultiLayer enabled. with a library of commonly used components (TRAXSTD.LIB). Unfortunately, this library is unsuitable for use without major editing. Many pads are too small for non-plated-through (single-sided) designs and the hole sizes don’t equate to the metric drill sizes commonly used in Australia. We’ll describe how to edit and create your own libraries a little further on. For the moment, use the SIMPLE.LIB library that we’ve built especially for this design. It can be obtained from the SILICON CHIP web site (see panel entitled “Power Supply Demo Design”). To load a new library file, press <L> to bring up the Library menu, then <F> to get the file name prompt. The file shown will be the currently loaded library, in this case C:\AUTOTRAX\ TRAXSTD.LIB. Change this to read C:\ AUTOTRAX\SIMPLE.LIB and press <Enter> to load it. Initial component placement For a typical design, we would now need to check that a matching “footprint” exists in the library for each unique component in the parts list. As SIMPLE.LIB already contains all of the relevant footprints, we can skip this step and go straight to placement. Table 2 lists all the components in this design together with the matching footprints in SIMPLE.LIB. Let’s begin by placing the three resistors (R1, R2 & R3). Fig.3: the Options menu draws together Press the <P> then several important but mostly unrelated <C> keys and you will be controls. For example, the Drag option prompted for the name determines how Autotrax handles tracks of the component to be connected to a component when you placed. By default, the move it. Track Mode, on the other hand, determines whether Autotrax enforces name of the last compoorthogonal track placement. Use the settings nent used is displayed. shown here as a starting point. You can simply press <Enter> to place the same component again, or type sible via the Move menu. In addition, in the desired component name ditrack widths can be changed using the rectly. You can also change the name Edit -> Track command. to a question mark (?) and press <EnNote that as with all operations in ter> to see a list of all footprints in the Autotrax, you can use the keyboard library (Fig.5). as well as the mouse to place and edit If using the latter method, highlight components and primitives (tracks, “RES0.4” in the list (determined pads, etc). The arrow keys move the from Table 3) and press <Enter>. For cursor around, and the <Enter> key is “Component Designator”, enter “R1”, equivalent to a left mouse click. and for “Comment”, enter the component’s value, which in this case is Loading the library “120R” (we’ve used “R” instead of the Autotrax is supplied complete “Ω“ symbol). You can now move the March 2004  67 Fig.4: the Current menu primarily defines the current primitive sizes. For example, if you were to hit <P> <P> to place a pad, you’d get 100 thou round pads using these settings. Leave the “Floating Origin” and “Grid” options set as shown here. resistor around the board and drop it by pressing <Enter> or clicking <Left Mouse>. For the moment, place all components just outside the board outline. Note that as soon as you drop the resistor, you’ll be prompted to place another. Simply follow the same procedure to place R2 and R3, entering the appropriate resistance values (from Fig.8) in the “Comment” field. That done, load all the remaining components using the circuit diagram (Fig.8) and footprint list (Table 2) as your guides. The final result should look something like that shown in Fig.6. Mounting holes If mounting holes are required, place them next; trying to fit them in later can be a real pain! For a typical 3mm screw & stand-off combination, use a 220-thou round pad with 120-thou hole. This large pad size ensures that they’ll be enough clearance around the spacer (or nut) and screw head during assembly. In the demo design, we initially placed a hole at each corner but were later able to move the bottom pair up into unused space. This reduced the board length by about 10mm. Doing the shuffle Now the real work begins! Obviously, the aim is to arrange the components within the board outline so that it will be possible to connect them as shown on the circuit diagram. Press the <M> and then <C> keys and click on a component to pick it up. To rotate the component left by 45°, hit the space bar. As before, press <Enter> or click <Left Mouse> to drop it. 68  Silicon Chip Fig.5: using the Library -> List command lists all of the components in the currently loaded library – in this case SIMPLE.LIB. So how do you know where to place each part? Well, in all but the simplest of designs, you’ll need to move components around after the initial placement to “get the right fit”. In some cases, you may even need to “rip up” your design (tracks and all) and redo it a number of times! Experience has a lot to do with it too. The more layouts you do, the quicker you’ll be able to find a layout that works. Our recent PC Board Design Tutorial series (Oct. – Dec. 2003) will really help from here on. Much of the information presented in the series is not duplicated here, so it should be considered mandatory reading. Don’t cram all the components close together; adjacent components must not physically interfere with one another. Some layouts will progress faster if you initially leave at least Table 1: Handy Shortcuts Key Sequence Command <Ctrl + G> Current -> Grid <Ctrl + P> Current -> Pad Type <Ctrl + Q> File -> Quit <Ctrl + S> Current -> String Size <Ctrl + T> Current ->Track Width <F1> Place -> Pad <F2> Delete -> Pad <F3> Place -> Track <F4> End track <F5> Zoom -> Contract <F6> Zoom -> Expand <F7> Move -> Re-Route <F8> Delete -> Track <F10> Zoom -> All <+>, <-> and <*> keys on the numeric keypad can be used to cycle between defined layers. enough space to fit a 30-thou track between adjacent component pads. Laying the tracks To begin the layout, hit <Ctrl + T> and select a 70-thou track width. Check that you’re on the bottom layer, and then press <P> followed by <T> to enter track place mode. To reposition tracks after initial placement, use the Break, Drag End, Re-route and Track commands, accessible via the Move menu. Place a couple of tracks and experiment with these commands now – you must be completely familiar with how they work. Remember that you can zoom in and out with the <Z> command, even in edit mode! We used 70-thou tracks for most of the design, increasing to 100 thou for the main current-carrying conductors. Notice how we had to “neck down” from 100 to 70 thou to connect to REG1. Two overlapping 100-thou tracks form part of the ground connection. Where space permits, it’s a good idea to use as much copper as possible for high-current rails. Although not particularly evident on this simple design, it’s important to constrain track placement to 0, 45, 90, 135, 180, 225, 270 or 315-degree orientation. This is called “orthogonal” placement and it makes maintaining consistent track-to-track and trackto-pad clearances easier. The “Track Mode” setting in the Options menu can be set to “Orthogonal” to automatically enforce this mode. However, some users prefer to set this option to “Non-ortho” and align tracks by eye, as the auto mode makes track placement less predictable. Another method is to initially route www.siliconchip.com.au all the tracks with 90° corners. This works well on simple, uncluttered designs. Once the layout is almost complete, go back and put in 45° corners (“chamfers”) using the Re-route command. The result is more pleasing to the eye and it helps to prevent undercutting during etching. Track to pad joints Generally, tracks should be routed all the way to the centre of pads. Also, when laying multiple tracks together to make a wider copper area, make sure that there is a sizeable overlap. Autotrax draws pads on top of tracks, so obscuring where tracks actually end. Once you’ve completed your layout, check for inconsistencies by changing the track and pad redraw mode to “Draft”. You’ll find this option in the Setup - > Redraw menu. Strings Strings (free text) can be placed on most layers. To enter a string, press the <P> and then <S> keys and type in the text. When complete, press <Enter> or click <Left Mouse> and you’re ready to place it. At this point, you can rotate the string by pressing the space bar, flip it with the <Y> key or reverse it (for the bottom layer) with the <X> key. On copper layers, allow at least 10 thou clearance between strings and other objects (tracks, pads, etc) to avoid potential shorting/etching problems. A 5-thou snap grid allows accurate placement. The default string size can be changed via the Setup -> Strings menu, although 60 thou is recommended for most work. Strings can be edited (moved, sized, etc) via the Move -> String, Edit -> String and Delete -> String menu commands. All components include two “special’ strings; the “designator” and “comment”. These can be moved about just like free strings but cannot be edited or deleted with the string commands mentioned above. Instead, you must edit them via the Edit -> Component menu. Note that whenever you edit a component and change the display mode for either of these strings from “Show” to “Hide” (or vice versa), you have the option of applying the change globally. To reduce clutter, some users prefer to hide all of the component comments (or designators, depending on design complexity) until after most www.siliconchip.com.au Fig.6: once the board outline has been drawn, load all the components and temporarily position them outside the outline. Notice that we’ve initially hidden all of the component “comment” strings. Fig.7: our completed layout. Notice how the strings on the bottom layer have been “flipped”. of the work is done. It’s also possible to determine whether the “designator” and “comment” strings are hidden or displayed during initial component placement – see the Setup –> Component Text menu. Block operations The Block menu commands al- low you to move, copy or delete an entire section of your design at once. Anything that can be selected within a rectangular border can be acted upon en masse by these commands. In addition, block commands are used when creating new library footprints (see Libraries further on). Before using any of the block commands (except Hide and Read), you must first define the block. Press the <B> and then <D> keys and move the cursor to the first corner of the desired area. Click <Left Mouse> or press <Enter> and move the cursor to the opposite corner. A rectangular outline expands behind the cursor as it is moved, indicating the selection area. Click <Left Mouse> again to lock in the selection. Finally, choose a reference point. This will be used as the axis for the move and copy commands. In addition to move, copy and delete, you can also write the defined area to disk as a .PCB file. This can be retrieved later using the complementary Read command. Block operations should be used with caution; always, always save your work first! Saving your work Whenever editing a design, save your work regularly via the File -> Save menu. It’s also a good idea to save a backup copy of your work before starting a new editing session. March 2004  69 Power Supply Demo Design Fig.8: a complete and accurate circuit diagram is required before you attempt even the simplest of layouts. Here’s the circuit for a simple DC power supply that we’ve used as our demo design. It uses a conventional 3-terminal regulator, with the output voltage programmable via resistors R2 & R3. A lthough Autotrax includes a demonstration design (DEMO. PCB), it is far too complex to be of use to the first-timer. We decided instead to create our own simple design, the layout for which appears in various stages throughout this article. The complete circuit and overlay diagrams appear in Figs.8 & 9. You can download the design (PSU.ZIP) from the Silicon Chip web site at www.siliconchip.com. au – look in the software download area. This file also includes the SIMPLE.LIB library referred to in the text. Unzip PSU.ZIP into your C:\AUTOTRAX directory. How it works The Simple DC Power Supply is based around the well-known LM317T 3-terminal adjustable voltage regulator. These devices are Autotrax automatically saves a back-up copy of your work for disaster recovery purposes. You can change the backup interval (in minutes) and the filename used via the Setup -> Options menu. An interval of between 10 and 20 minutes is typical. Loading the demo design With the information presented 70  Silicon Chip extremely robust, having in-built over-temperature and over-current protection. The supply can accept an input of up to 28VAC or 40VDC and provide a well-regulated DC output in the range of 1.2V to 37V. Output current is 1A maximum and depends on the input to output voltage differential. Using the specified heatsink and at room temperature (25°C), The LM317 can safety dissipate 2.5W of power. You can use this power level to calculate the maximum output current for a given input to output differential. For example, with 16V at the input to the regulator and 5V at the output, the maximum current is: IOUT(MAX) = PDMAX/(VIN - VOUT) = 2.5W/16V - 5V = 0.227A The output voltage can be programmed by selecting appropriate thus far, you should be well on your way to completing the demo design. Alternatively, if you’d rather load the “one we prepared earlier” and experiment with that instead, then follow the instructions in the “Power Supply Demo Design” panel to download and install the relevant files. So you’ve finished the board layout – what now? Well, the following R2 & R3 Values For Common Output Voltages Output Voltage R2 R3 3V 5V 6V 7.5V 9V 12V 15V 1.2kΩ 3kΩ 11kΩ 1.2kΩ 3.3kΩ 3.3kΩ 3.9kΩ 470Ω 2.7kΩ 5.6kΩ 8.2kΩ values of R2 & R2, according to the formula: VOUT = 1.25 x (1 + (R2||R3)/R1) A list of commonly used voltages and the corresponding values for R2 and R3 appear in the above Table. Alternatively, you can install a miniature 5kΩ multi-turn potentiometer in place of R2 & R3 for a 1.2V to 27V half of this article describes several concepts and features of Autotrax that will help you to get started with your own creation! Multiple layers or wire links? A good single-sided PC board design is one that requires no wire links – or so we’ve heard. The reality is that no matter how proficient you become, www.siliconchip.com.au Parts List 1 PC board, code 04103041, 36.8mm x 68.6mm 1 LM317T adjustable positive voltage regulator (REG1) 6 1N4004 1A diodes (D1-D6) 1 5mm red LED (LED1) 2 2-way 5.08mm-pitch terminal blocks (CON1, CON2) Capacitors 1 2200µF 50V PC electrolytic 1 100µF 63V PC electrolytic 1 10µF 50V PC electrolytic 1 100nF 63V MKT polyester Resistors (0.25W 1%) 1 1.5kΩ R2 (see table) 1 240Ω (R1) R3 (see table) not straddle or otherwise interfere with them!). If you wish, you can disguise you links by using zero ohm resistors instead of plain old tinned copper wire. These are available in standard “1/4W” package styles from the usual electronics outlets. Fills and arcs Large copper areas are easily created with the Place -> Fill command and edited in a similar manner to the previously described “primitives” (pads, tracks, strings, etc). Fills should be used in place of multiple overlapping tracks wherever possible, as editing is far more efficient. Autotrax supports arcs of any diameter and width with one to four quadrants. Avoid these on the copper layers unless you know what you’re doing. Libraries Fig.9: companion overlay diagram for the completed design. You can purchase a ready-made PC board from RCS Radio at www.rcsradio.com.au if you would like to build one, or wait until next month to find out how to make the board yourself! adjustment range. Note that the voltage at the input terminal of the 3-terminal regulator some of your designs will require links to make those last few connections. Of course, depending on complexity, a two-layer (or more) design might also be the answer, especially if you have limited space to work with. Multiple-layer designs are for experienced designers only, so we won’t cover them here! Typically, a link is just a straight www.siliconchip.com.au (REG1) must be at least 2V higher than the programmed output voltage. piece of wire with a pad at either end. We recommend a minimum pad size of 70 thou (85 thou preferred) with a 28 or 32-thou hole. Draw a track between the two pads on the component overlay to indicate the link position. To give the assembled board a professional appearance, wire links should be oriented and aligned with surrounding components (they should As mentioned previously, the standard Autotrax library (TRAXSTD.LIB) is unsuitable for use without major editing. One option is to obtain a complete set of libraries on CD-ROM from RCS Radio. These are supplied “ready to go” and are optimised for use on non-plated through board layouts. Contact Bob Barnes on (02) 9738 0330 or check out www.rcsradio.com.au for more information. An excellent component library is also available from Airborn Electronics at www.airborn.com.au/layout/ autolib1.html. Note that this library is optimised for plated-through (double -sided) board design. This means that the pad sizes (for through-hole components) are too small for use on single-sided boards. However, you can readily use it as your reference library, editing footprints as required and adding them to your own library. Building your own library Library components are made up of all the familiar primitives. However, their individual elements are not free to move; they’re bound together in a fixed relationship to one another. We can break that relationship, edit the individual primitives and then regroup them again at will. Let’s experiment with an existing component from SIMPLE.LIB. First, find some free space (anywhere outside the border) of the power supply demo design if you have it March 2004  71 Table 2: Component Designators & Matching Footprints In SIMPLE.LIB Component Library Footprint C1 C2 C3 C4 CON1-CON2 D1–D6 LED1 REG1 R1-R4 HEATSINK CE0.3/0.71 CE0.1/0.2 CE0.2/0.4 CM0.1/0.2 TB2W DIODE0.5 LED5MM TO220V RES0.4 HS6021 Table 3: Use These Hole Sizes In Your Designs Design Size (thou) Drill Size (mm) 120 80 60 50 40 36 32 28 24 3.00 2.00 1.50 1.20 1.00 0.9 0.8 0.7 0.6 open, or start a new design. Make sure that the snap grid is set to 25 thou and place a “RES0.4” component from the library. Next, “explode” the component by selecting the Library -> Explode menu command and clicking on it. “Exploding” the component simply means converting all of its primitives to free (unbound) elements. You can now edit the pads and tracks that form the outline (on the overlay) just like any other free primitives. To prove the point, change the pad sizes to 120 thou now using the Edit -> Pad command. That done, let’s save the modified footprint back to the library as a new component. First, use the Block -> Define command to select just the desired primitives. For a reference point, you can either click exactly in the centre of the component or in the centre of one of the pads. This will be the axis point when placing the component from the library later. Next, select Library -> Add from the menu. You’ll then be prompted for a name for the new component. Type in “RTEST” and press <Enter> and you’ve successfully created your first component! Once you’ve created the new component, the original “exploded” component remains. As it’s still highlighted (defined inside a block), you can quickly remove it with the Block -> Inside Delete command. Of course, you could also use Block -> Hide and delete the primitives individually! The Library menu provides a host of other functions. You can rename and delete components, merge libraries and create new libraries. The Compact function should be used after editing to tidy up the internal file structure. Important: a library must never have more than 200 components. If you attempt to add more than 200 components, your library will be corrupted! Always save a backup copy of a library before editing it! Pads, tracks & hole sizes For single-sided board design, the minimum pad size to use with through -hole components is 70 thou, with 80 or 85-thou recommended. Other typical sizes are 100, 120 (or 125) and 150 thou. Stick with round or square pad shapes. The library components must closely match the physical size, footprint and lead diameter of the real components. You can get the necessary information from the manufacturer’s data sheets or measure the components yourself using Vernier callipers. Callipers with an LCD display make this job even easier. 72  Silicon Chip Single-in-line (SIL) and dual-in-line (DIL) packages with 0.1-inch pitch pins (ICs, for example) are an exception. The recommended minimum size for these is 60 x 120 (rounded rectangles). Never use round pads for this job – they may well lift off the board as soon as they’re heated! It is important that the holes sizes used in your designs closely translate to the commonly used metric drill sizes used here in Australia – see Table 3 for a list of typical hole sizes. An exception to this rule would be if your boards were being made in the US. In this case, refer to the manufacturer for their requirements. This is something that you should always do before submitting your designs anyway – it might save you a lot of money! For a handy one-page summary of recommended track, pad and hole sizes, get a copy of RCSTRAXY.PCB, available free from RCS Radio at www. rcsradio.com.au Advanced topics Autotrax includes the ability to automatically place components and route all or part of your designs. Experienced users would probably agree that this feature is of limited use. Manual placement and routing always gives a better result! If you want to experiment with these features, you’ll need a netlist of your design. Netlists are usually generated by schematic capture software. They describe all of the components in a design as well as how they are connected. Our simple power supply design includes a netlist file (PSU.NET) that can be loaded using the Netlist -> Get Nets command. Once loaded, you can turn on the “rats nest” display using Netlist -> Show -> All Nets. Note that before using any of the auto place or route functions (see the Netlist menu), you must define the board outline on the “Board” layer. To do this, first turn on the Board layer via Setup -> Toggle Layers. Next, switch to the Board layer and duplicate the outline drawn on the Top Overlay. Next month Next month, we’ll show you how to make a hardcopy of your design. This will enable you to check that all the components will fit on your completed board. It can also be used to make your SC own PC boards at home! www.siliconchip.com.au