Fullscreen HTML5Med Res (??MB)HTML4

Give your circuit that PROFESSION When it comes to contributed projects or circuits, there are few things more frustrating than finding the circuit has been drawn (apparently) by “a thumbnail dipped in tar” – or near equivalent. Here’s an easy way to make them look good! N ot only do poorly presented circuit diagrams increase the likelihood of errors, they also make it more difficult to understand the basic circuit operation. And if those at SILICON CHIP cannot understand it, how are readers going to? The Editor will be much more impressed by a neatly laid out diagram with standardised symbols, all components at right-angles and all the components in scale. How do you do it? Many years ago Protel had a circuit drawing package called Schematic. Unfortunately it was less than acceptable – the frustration and poor results with this program prompted me to think about an alternative. The one I use might sound a little unusual at first glance. It’s the Protel Autotrax PCB (Printed Circuit Board) layout package which of course is intended to lay out PC boards. But I find gives excellent results when drawing circuits – and as a bonus is quite easy to use. An even bigger bonus is that it won’t cost you anything. Now well and truly superseded, Protel Autotrax can be downloaded free from www.altium. com/altium/altiumsite/community/ downloads/altium-freeware-enduser-license-agreement/en/autotrax.cfm If you find entering all that a bit daunting, simply go to www.altium. com and go to the “community” tab, thence “downloads”! This program was covered quite thoroughly (mainly in its normal PC board layout mode) in the February, March & April 2004 editions of SILICON CHIP. So I won’t go into all that detail again but will cover aspects of using it as a circuit drawing program. Briefly, though, you need to know that Protel Autotrax has two parts – the first, the part you actually “draw” with, is called TRAXEDIT.EXE. When you want to print out your masterpiece, you’ll need the second part, called TRAXPLOT.EXE. However, be warned: as Autotrax is getting pretty long in the tooth (it’s Which one looks better? This one or the one on the right? Unfortunately, the example at left is a positive masterpiece compared to some which we see! 72  Silicon Chip siliconchip.com.au diagrams NAL look! been around since the 1980s) video and printer drivers can be problematic. In fact, we seldom use Traxplot – at SILICON CHIP we work mostly with EPS (encapsulated Postscript) files and use a little utility called “GRABEPS” which converts Autotrax (*.PCB) files directly into *.EPS files. Grabeps can be downloaded from www.electronicsaustralia.com.au Will Autotrax work on XP and VISTA? Being a DOS-based program, Protel Autotrax performs best on a computer operating under DOS. However, that is not to say it won’t operate under a Windows command prompt because, in most cases, it certainly will. We have had no major problems using Protel Autotrax on PCs running Windows 98, 2000, ME and XP. As Rick Walters has mentioned in this article, drivers for particular printers and video cards might be something of a problem; however (so far!) not for us. You might have noticed that the list above doesn’t mention Windows Vista. This is a whole new ballgame because it works quite differently to the earlier operating systems. Unfortunately we haven’t had the opportunity to test Autotrax on Vista before going to press (like many organisations, our computers primarily operate under Windows XP). There is a fair amount of discussion on the net about operating old DOS programs under Vista – the majority suggest that using a program called DOSBox (or several similar programs) will allow you to use most DOS-based software on a Vista machine. by Rick Walters find the folder labelled SCHEMATI in the May 2009 section and click or double-click on it. It will open, showing a single zipped file. Download and save it to c:\schemati. You will need to unzip them before use – in the majority of cases, doubleclicking on a *.ZIP file will bring up the appropriate unzip utility – but if it doesn’t, there are numerous zip/unzip utilities which you can download from the web. Before you start Firstly we need a dedicated directory which I have (for obvious reasons) called SCHEMATI (DOS-based programs cannot use directory or file names with more than eight characters). If you don’t know how to create a directory (now also called folders), check the side panel. Create your directory and call it SCHEMATI or whatever 8-letter name you desire. It should now appear listed alphabetically under the C: drive. We have placed all the files you will need in a directory called SCHEMATI. Log onto www.siliconchip.com.au/downloads Drawing a circuit Drawing a circuit, especially a large and/or detailed one, is not a simple task. Some of the larger ones you see in SILICON CHIP may take many hours, or even days, to draw. As well as showing the interconnections between the various devices the drawing tries to group relevant components in reasonably close proximity, as well as tending to flow from left to right with inputs on the left and outputs on the right. The area where this often does not hold true is that we tend to bring power +5V/+18V 100nMc 100nMc 1 2 3 4 5 6 7 Q12 Q13 16 Vcc 16 Q10 IC1 4060 Q14 2 13 Q6 R Q5 CKin CKO1 Q4 1 14 Q8 Q9 Q7 15 CKO2 16 IC2A C 4518 CE 12 8 Q0 Q1 Q2 R 11 100u 100nMc Q3 3 4 9 5 10 IC2B C Q1 CE Q2 6 R 15 7 Q0 Q3 11 12 1 13 2 IC3A C 4518 CE Q1 Q2 14 8 Q0 R 7 Q3 3 Q0 4 9 5 10 C IC3B CE Q1 Q2 6 R 15 Q3 11 12 13 14 10 9 E 22k 8 200Hz 1k 100Hz 10Hz RESET 1Hz 0.1Hz 10M 3.2768MHz TITLE 22p 270p X1 siliconchip.com.au 10p SIMPLE FREQUENCY DIVIDER A4H NUMBER SIZE DATE 040212 FILE FDIV1 REV 0 DRAWN R.W. May 2009  73 Protel Autotrax key commands As an (old!) DOS program, Autotrax relies extensively on keyboard commands instead of mouse clicks. Actually, this works rather well, especially as you get more skilled in using the program. Most of the letter codes are prettymuch self explanatory. The commands in red are the ones you’ll use the most for circuits (you can virtually ignore the rest unless, of course, you’re drawing PC boards!) How they work Typing the first character (as shown in bold below) brings up the options list (which follows). For example, when you type b (block) you will see a number of options. When you type the second letter, particular option is invoked. So bd would be block define (ie, tell Autotrax where the block is), bm would be block move and so on. br (block read) and bw (block write) allow you to save a block as a file and read it back as a component. This is useful where, for example, you may have six seven segment decoders driving six LED displays. You draw it once, write it out to a file, then read it back five times and place it. The Autotrax commands b block – allows you to “block off” areas of your diagram and do something with them: d define, h hide, m move, c copy, i inside delete, o outside delete, r read, w write. c current – gives a list of the current setup d delete – a arc, c component, f fill, h highlight, p pad, s string, t track, v via e edit – a arc, c component, p pad, s string, t track, v via f file – l load, s save, q quit, plus many more g grid – s snap: 25, v visible: 100 h highlight – c connection, d duplicate, r reset i information – c dimensions, c components, plus others j jump (to) – c component, c location, c net, o origin, p pad, s string l library – a add, b browse, c compact, d delete, e explode, f file, l list, m merge, n new, r rename m move – a arc, b break, c component, d drag end, f fill, p pad, s string, t track, v via p place – a arc, c component, f fill, p pad, s string, t track, v via s setup – all the options for drawing, already setup for you u undelete – allows undeletes from 1 up z zoom – see S PgUp and T PgDn below Four arrow keys move the cursor in 25-thou steps S (Page Up) – Zoom around mouse position T (Page Down) – Shrink around mouse position + (Plus on keypad) – steps through Track Colours – Red - Yellow - Brown - (Minus on Keypad) – steps in reverse direction to + 74  Silicon Chip in on the right hand side. An additional benefit of Autotrax is that the IC pins are numbered with the pin function near the number. This prevents transcription errors when going from an IC data book to draft circuit to final circuit. We will explain how to draw the Simple Frequency Divider Circuit on page 72. Start the program by clicking (or double-clicking) on the “Traxedit” shortcut in the Schemati folder. The shortcut tells Windows to run the program in a window but it actually boots to full screen. Once TRAXEDIT is loaded it appears on the opening screen as AUTOTRAX with “Press a key to continue”. Having pressed, you are presented with a light grey screen with a grid of white dots. Across the bottom of the screen (similar to the Windows Taskbar) is a yellow bar with letters and numbers similar to the following: X:2000 – Y:1200 mils – L:Top Layer – a block of colour – P:Round 50 – T:20 – S:60 – G:25. In order these mean: X and Y show the mouse co-ordinates at startup, L is the layer you are working on, The block of colour (Red, Brown or Yellow) indicates the colour of the track you will draw on the screen, P indicates the pad type and size, T is the track width, S is the string size and G is the grid step. If you are using the bottom layer, the yellow block of colour melts into the yellow background, so you won’t be able to see it. You will note that after the Y position is the word mils, which means 1/1000 of an inch, usually abbreviated to “thou.” (however, for clarity, we generally leave the full stop out – ie, “thou”). Even with metrication, most components are based on an imperial measurement – all through-hole ICs, for example, have pins 100-mils (0.1”) apart. Below the X: as you select functions a prompt will appear to assist you. Drawing a circuit is much the same as “drawing” a PC board pattern. Instead of pads and physical components, you select circuit symbols. You join them using very fine “tracks”, as you would the PC board pads etc. The first step in drawing a circuit is to define the area in which we can operate. While Autotrax allows the use of a mouse it is far quicker to use a combination of the mouse and keyboard keys. In the following description (selecting a library) using a mouse we would click the mouse, move to Library, click the mouse, move to File and click. Using the keyboard we would type  (Library File). In both cases the loaded library file will show but it is obvious which is more efficient and usually much quicker. Selecting a library Type lf (or click the mouse as above). Normally we will use SCHEMATI.LIB. If you can’t remember the library name, press the keyboard question mark  then K and the libraries will be displayed. At this stage you only have two, IC.LIB and SCHEMATI. LIB. Select SCHEMATI.LIB. Type  (Place Component) then type  (a horizontal A4 page). siliconchip.com.au This screen grab shows what you will see running Autotrax. The type of information you get on screen (bottom strip) is explained in the text. The nearlycompleted circuit diagram is that which is shown in its printed-out form on P73. Every time you place a component you are asked for a COMPONENT DESIGNATOR then a COMMENT. For this component we want neither, so just press K, which gives you a blank. Locate the A4H outline at 0,0 then press K, then right click or press P (escape). Now type  (Library Explode). The prompt on the bottom line will read SELECT COMPONENT. Move the mouse into the rectangle then click or press K. This will leave a brown outline of the A4 page area in which our circuit will need to be contained. You will be asked to confirm. We explode the library item to turn it into primitives which means that Autotrax sees the brown outline as just that and not a component, otherwise we would end up with a lot of components inside a component and a myriad of problems. Right click or press P to exit LE. ESC ESC Placing the title block Next we place the title block but before we do so you need to zoom the active display, so press the S key on the keypad twice. This should just about fill the screen with the brown surround. Press pc (Place Component) then overtype A4H with TITLE. Again no designator or comment! Move it where you prefer it. It’s normal practice to place it at the bottom right (as you can see). We will come back and enter some details later but let's keep placing components. Placing components Overtype TITLE with CAP. Again, if you don’t know the name of the component type a question mark, then press K. A list of components will be displayed. My approach is to keep the component name as short as possible, as long as it is recognisable and identifiable. Why waste time and effort typing CAPACITOR when CAP will do? (But don’t be caught using names like “trans” – it could be a transistor, a transformer, a transducer, a transmogrifier, a transcombobulator . . .) siliconchip.com.au As this is the first capacitor we type c1 for the component designator, then press K. For comment we type the value of the capacitor, 100nmc for a 100nF monolithic ceramic & press K. The capacitor symbol will appear and can be moved about with the mouse. A left click will place it. Repeat Creating a directory (folder) in XP Click or double-click (depending on how your computer is set up) on the My Computer shortcut on your desktop. Click or double-click again on the C: drive (mine is called WINDOWS_XP) but yours will possibly be named differently. Click on FOLDERS to divide the screen. Move the mouse to a blank area on the right hand panel and Right-click. Move down to NEW, pause a moment, then across and up to FOLDER. Left-click and a folder called “New Folder” will be created. While New Folder is hilighted blue, type SCHEMATI. This name should now appear alphabetically listed in the left hand panel under C: Close My Computer. Creating a shortcut to schematic Click or double-click (depending on how your computer is set up) on the My Computer shortcut on your desktop. Click or double-click again on the C: drive (mine is called WINDOWS_XP) but yours will probably be named differently. Find the SCHEMATI directory you have created. Click on it to open it and the files will be listed in the right hand panel. Hover over those named TRAXEDIT and find the one that is TRAXEDIT with no suffix (blue bar at top with XP). The size should be 170kB. Right click and move to SEND TO then move to DESKTOP and click. It will be named SHORTCUT TO TRAXEDIT. You can rename it if you wish by right clicking and moving to Rename. May 2009  75 the sequence twice. The capacitors will be sequentially numbered and the description repeated. Next we will place the electrolytic, so instead of CAP overtype electro. It will need to be designated C4, as we have changed the component type, and the comment will be 100u. Now place the other three capacitors (CAP) 22p, 270p and 10p. The crystal identity is XTAL, the designator X1, the comment 3.2768MHz. Rotating a component You will notice that both the crystal and the 270pF capacitor are rotated by 90° – but we don’t use special components. If placing the component, pressing the spacebar will rotate it 90°; if it is already placed press mc (Move Component), click on it, then press the spacebar. Each press rotates the component by 90° so four presses brings it back to where you started! Next place the three resistors. Their identity is RES, the first designator R1 and the comment 1k, then 10M & 22k respectively. As previously explained, there are two libraries: IC.LIB and SCHEMATI.LIB. We have been using the SCHEMATI library but to place ICs we have to use the IC library as there is a limit to the number of components that a library can hold. Right click to release PC then type lf (Library File), press K & C:\ SCHEMATI\SCHEMATI.LIB will show. Type ic, then press K. There is no need for the .LIB suffix but you may include it if you wish. If you type ll (Library List) you will get a list of all the ICs in the library. Press K to exit LL. Placing integrated circuits We wish to pc (Place Component) 4060, designator IC1, comment 4060. Position it towards the LHS (you can always move it later). Now PC 4518A, IC2A, 4518 to the right of IC1. PC 4518B IC2B, (blank) to the right of IC2A. Where an IC consists of two or more elements within the one package (as in the 4518 above which is a dual decade counter) I make it a practice to only identify the A element with the type number. If you label them all, then at a quick glance you might count four 4518s in the circuit instead of two. Repeat the layout for IC3A & IC3B. Your ICs will not be numbered or identified. Press P, then ec (Edit Component). ESC Identifying integrated circuits Click on IC1 the 4060, click on DESIGNATOR in the panel, K, move down to HIDE, click, move to SHOW and click. Follow with three right clicks or three Ps. IC1 will now be displayed above 4060. Do the same for IC2A & B and IC3A & B.P from EC and type ms (move String). Ensure the task bar displays yellow then click on IC1 and position it to between Q12 & Q13. Position 4060 between Q13 & Q14. Then move and position the titles for IC2 & IC3. You can identify any component but I usually don’t identify resistors, capacitors and other miscellaneous bits. Now all the ICs are placed we need to go back to our SCHEMATI.LIB so press P (or right click) to get out of Move String then lf, SCHEMATI.LIB then K. We now have to place 13 ground symbols (GND) and nine ESC ESC ESC 76  Silicon Chip jumpers (JMP) but these are best left until later. For the best appearance, ensure all the tops of the ICs are on the same Y grid (ours is 4100). If not type mc (move component) then move the mouse to the inside of the component and click. Move it to the required location and click to lock it in place. You are again prompted by the taskbar. NOTE! You can only move components when the red or yellow colour bar is displayed on the taskbar. They will not move if the brown bar is showing. Drawing the connections Connections between components (remember, we are using “tracks”) are always drawn in red. Draw the trace from IC1/3 to IC2/2. If you are still in move component mode, press P (or right click), ensure that you have the red bar in the taskbar then type pt (Place Track). The track width has been set to 20 thou in the initial setup you downloaded and the visible grid to 100 thou The actual step increment using the mouse or the four arrow keys on the keyboard is 25 thou. Move your mouse to the line from pin 3 and click. Move the mouse to the left until you reach the grid then click again, move the mouse vertically until you hit the grid again, click, across, click, down, click then across to pin 2 of IC2A, click. Now press P (or right click). This disconnects the track from the mouse. You may need to zoom to the area you are working in (plus key on keyboard). Next move the mouse to IC1 pin 12, click and draw the track to IC2 pin 7, clicking each time you want to change direction. Right click to decouple the track from the mouse. If you have previously laid out PC boards using Autotrax these instructions will be instinctive. Now join IC2b pin 15 to the junction of IC1/12 and IC2/7 and then to IC3/7 and IC3/15. Connect IC2A/3 to IC2B/10, IC2A/14 to IC3/2 and IC3/6 to IC3/10. Now draw the supply rail at the top of the ICs. Start at the left and click to go towards IC1/16. Stop 50 thou past the grid dot, then right click to break the track, move the mouse down 100 thou and draw the track to the IC. Go back up and join the pin 16s on IC2 and IC3, then continue the track towards the right hand side. Right click twice (once to release the track, the second to exit from PT) then type pc (place component). Placing miscellaneous components Type join (K) accept its ID (K) and ensure the comment is blank (K) them move your mouse to the sup- ply line above IC1/16. Click and a dot will appear. Move the mouse above IC2A/16 and click three times, then place it. Another three clicks in the same vertical plane as 100Hz and place, then three clicks and so on, for each join. Next the four on the reset line, then the four on the CE (clock enable) inputs. Knowing you need three for the crystal area place three at random there. The jumpers are placed in a similar manner. Type pc , when you see JOIN displayed type jmp (jumper). Place the nine jumpers in like manner making sure the tracks run right up to the start of the arc. The reason for this will be explained shortly. Finally place the six ARROWS. They will initially point to the right, so the RESET one will need one press of the SPACEBAR to rotate it 90°, the others will need three presses (270°). The COMMENT for each arrow is 200Hz, 100Hz etc. siliconchip.com.au Using mc (move component) place the resistors, capacitors and crystal (click on each component, move it, then click again to place it) in their correct locations. Now draw the connections to pins 10 and 11 in IC1. The ground symbol is GND so these (13) can now be placed and the tracks drawn. Checking the layout To check your circuit for continuity and connections place the mouse on the +5V/18V arrow and type hn (highlight Net). All the Pin 16s should be connected. The connections are obvious on this simple circuit but in a complex one it is much harder to check. Place the mouse on IC1 pin 3 and type hn. The track should be continuous to 200Hz following the jumper. This is why you need to take the track right up to the jumper arc to ensure continuity. Filling in the title block Type ps (Place String), type simple freq uency divider, click and move it to the title space, then click to release it. The text will be too small (60 thou) so et (Edit Text) and try 80. Still a bit too small? 90 should just fit. Type a4h and move it to the SIZE window, then fill in REV(ISION), DATE and DRAWN. File is the name you will use to save the circuit. If you use Autotrax to lay out your PC boards ensure that the circuits are saved in the SCHEMATI directory and the PC boards in a different directory, as both have the suffix PCB and if you give them the same name (which is logical) and put them in the same directory, one will overwrite the other. Creating a component While you have a wide range of components available you will probably need additional items in due course. As an example, in the January 2009 issue of SILICON CHIP, John Clarke used a 12F6754/P microprocessor. We don’t have one in the library, but looking at the device it is an 8-pin integrated circuit similar to a PIC08. So we would “create” a new IC using that. Move the mouse to blank area of the screen, (making sure you have IC LIB selected) type pc (Place Component) PIC08 then press P or (right click). Then le (Library Explode), confirm yes. Press the plus key until you see Top Overlay and the red or brown bar change to yellow (bottom centre of screen). Type ds (Delete String), selecting each description in turn. Next type ms (Move String) then select and place the pin numbers in the correct position. Finally type ps (Place String). The top left corner displays what you are typing. Pressing K places the text under the control of the mouse. Locate it and click to lock ESC 1 Vcc 2 7 P00/SO P-08 3 6 P04 P01 4 SI P03 Gnd 8 P02 5 1 4 Vdd ---MCLR 5 6 GP2 GP1 12F6754/P 3 AN3 7 GPO GP5 2 Vss 8 Creating a component is usually much easier if you modify an existing one. Don’t forget to rename it! siliconchip.com.au Printing your circuit In the drive for bigger, better and bloated programs, support for old DOS-based software and printers is rapidly (and probably not unreasonably) disappearing. Protel was written to interface to brands of serial and parallel printers which were popular at that time but now obsolete. Most desktop computers and some laptops still have a parallel output port but not for much longer, as new motherboards are phasing it out. In a recent magazine issue only four of the ten units reviewed had a parallel port. If you have a parallel port on your computer and you own an HP deskjet printer with parallel input, you are ready to roll. Protel’s output program is called Traxplot.You can create a shortcut to it as we described for Traxedit. It appears that all HP deskjets support laser 300 DPI (HP640c, HP649c & HP948c all do) and the plot setup is for these printers. My old HP649c packed up recently and on the advice of my cartridge supplier, I went to the local Salvation Army depot and purchased both an HP640c and an HP948c. They were quite expensive though: $5.00 each with both black & colour cartridges fairly full! The print parameters are set up, so pressing fl (File Load) will give you C:\SCHEMATI\*.PCB. Press ENTER and select FDIV1.PCB. The file will load. Press P (escape) o get back to the FILE menu then move down to print. Press P or click. You will be asked to confirm PRINT, so click or press y. A few seconds later you should have a printout of your masterpiece. If you don’t have an HP printer various other methods of printing were discussed in the April 2004 issue. An updated version of Ghostscript has recently been released. it in place. If you want to move any strings then ms and click will let you place them. Once you are satisfied type bd (Block Define). Click and move the mouse diagonally to encompass the device and click. You are now asked for a reference point. For this device I would use the left tip of the wire from GP2 and a similar place for all ICs. When placing the device in a circuit the mouse is located at the reference point and you should always put this point on a grid dot. Having defined the block it has to be saved to the library. Type la (Library Add). You will be asked for a name, then Autotrax checks to ensure this is not a duplicate name then asks you to confirm the new name. Before deleting the block place the new component and make sure you are happy with it. Then type dc (Delete Component) and click on the one just placed (unless you plan to use it), then type bi (Block Inside Delete) and confirm Yes, then when asked “all layers”, type a (ie, biya). Backup File Protel periodically backs up the file you are working on. With a modern computer it happens so quickly you are unaware of the save. The file is named TRAXEDIT. ABK. (which stands for AutoBacKup). Should you have a computer crash, lockup or a power failure, once you are running again, delete the file you were working on (FDIV1. PCB) or rename it (FDIV1.BAK) then rename TRAXEDIT. May 2009  77 So what do WE use? We are often asked which software we use to draw SILICON CHIP circuit diagrams. We use Corel Draw but don’t use Corel’s symbols. We have an extensive component library which we have drawn up over many years (in fact, we created the Corel Draw library from the pen-and-ink component library which we drew when we started the magazine). As we imply above, Corel Draw does contain its own electronic component symbol library (among many other libraries). There is nothing wrong with using this library if you want to – we just believe ours looks much better! The latest version of Corel Draw (X4) is a fairly expensive package (~$500-$800 or more, depending where you get it) but we’ve seen earlier versions (eg V11) legitimately downloadable from the net for very cheap prices (eg, $US60!) – and you’d be able to do almost as much with an earlier version. ABK as FDIV1.PCB. When loaded, you will see that you have only lost a few minutes’ work. If you wish you can load each of the files and compare them. Bill of Materials (BOM.EXE) Once you have finished drawing your circuit you can generate a bill of materials – or what we would call a parts list. The Simple Frequency Divider circuit produced the following BOM. It has been compressed to take less space. 78  Silicon Chip _______________________________________________ FDIV1.PCB 9:21 9-1-2009 Bill of Material Summary Page : 1 DESCRIPTION QUAN. COMPONENT DESIGNATOR(S) 43 A1 A2 A3 A4 A5 A7 A8 A9 A10 A11 A12 A13 A14 A15 A16 A17 A18 A19 A20 A21 A22 A23 A28 A29 A31 A32 A33 A34 A35 A36 A37 A38 A39 A40 A41 A42 A43 A45 A46 A48 A49 IC2B IC3B +5V/+18V 1 A30 0.1HZ 1 A27 1HZ 1 A26 1K 1 R1 3.2768MHZ 1 X1 10HZ 1 A25 10M 1 R2 10P 1 C7 22K 1 R3 22P 1 C5 100HZ 1 A24 100NMC 3 C1 C2 C3 100U 1 C4 200HZ 1 A47 270P 1 C6 4060 1 IC1 4518 2 IC2A IC3A RESET 1 A44 Obviously we can extract the components (R, C, X & IC) SC from the list. siliconchip.com.au