Fullscreen HTML5Med Res (??MB)HTML4

Hands-On PC BOARD DESIGN For Beginners; Pt.3 In this final instalment, we describe how to print Autotrax PC board designs from within Windows. We also present a low-cost method for making your own PC boards at home. By PETER SMITH O NCE A BOARD layout is complete, a full-size printout of the design allows you to quickly verify that everything will actually fit. You can position the components in their intended positions on a paper mock-up of the assembly and check for interference between adjacent components, as well as verify component footprints. If the PC board is to be installed in an enclosure, you can use a paper cut-out of the board to check that it will fit as intended. In addition, if the design includes components that must protrude through panel-work (LEDs, switches, etc), then you can often use the printout as a drilling template. Autotrax includes a separate program called “Traxplot” for printing tasks. Unfortunately, the list of printers it supports is now rather dated, meaning that it probably won’t work with your particular model. As Traxplot is a DOS-based program, it can’t “see” Windows printers – it uses its own printer driver. The problem is worse in Windows NT, 2000 & XP, where the printer is jealously guarded by the operating system, locking out DOS-based drivers altogether. Luckily, with the addition of some free software and an extra step in the process, you can still print your designs from within Windows. Let’s have a look at what’s involved. Printing basics Fig.1: load your .PCB file via the File menu as the very first step. Fig.2: Traxedit’s Options menu. Set the “Type of Plot” to the layer that you wish to print. A “Check Plot” prints all selected layers (see Fig.3) superimposed on one another. 12  Silicon Chip As well as being able to print to a variety of old (by today’s standards) printers and plotters, Traxplot can generate Postscript output. Postscript is a very powerful, universal printing language supported by many high-end printers and photo typesetters. Traxplot can also be configured to send its Postscript output to a file rather than a printer port. So all we need is Windows-based software that can read Postscript files and print them out and there are quite a number that can do this. For example, CorelDraw and Photoshop can both handle Postscript files. For those who don’t already have a program that can read Postscript, www.siliconchip.com.au we’ve included details of a free viewer that can be downloaded from the Internet. Getting started As well as being able to print each layer individually (which we’ll see later on), Traxplot can print layers superimposed on one another – in a similar format to what you see on-screen. The top overlay is shown in grey (not colour, unfortunately) to differentiate it from the tracks and pads on the bottom layer. The result is quite legible and works well for simple single-sided layouts. This is called a “check plot” and it’s ideal for verifying component fit. Let’s see how it’s done. Launch Traxplot and you’ll be presented with the main menu (Fig.1). The first job is to load the .PCB file, so press <F> to get to the “File” menu. Next, press <P> to change the “Path” and edit the displayed value to point to wherever you’ve saved your .PCB files. The default location is C:\AUTOTRAX. That done, press <L> to choose the Load entry and you will be prompted for the file to be loaded. Simply hit <Enter> here to see a list of all the .PCB files in the chosen directory. Now use the arrow keys (or mouse) to highlight the PSU.PCB file (created last month) and press <Enter> again to load it. By now, you will have noticed that the menu system is similar to that in Traxedit. To select an entry, highlight it using the mouse or arrow keys and then press <Enter> or click <Left Mouse>. Usually (if it’s unique), the first letter of an entry acts as a shortcut. To back up one level, hit <Esc> or click Right Mouse. Once you’ve loaded the demo design, hit <Esc> to return to the main menu. Next, press <O> to select Options and bring up the “Setup Options” menu (Fig.2). Change the “Type of Plot” to “Check Plot” and the “Pad Hole Guide Size” to 20 thou or thereabouts. Other settings can remain at their default values. Again from the main menu, press <S> and then <C> to get to the “Check Plot Setup” menu. This is where you choose which layers should be printed. As shown in Fig.3, you need only turn on the “Bottom Layer”, “Top Overlay” and “Multi Layer Pads” for a single-sided layout. The last task is to define and configure the output device. Press <S> to www.siliconchip.com.au Fig.4: you’ll find all the Postscript options under the Setup -> Postscript menu. Fig.3: for a check plot, enable the layers that you want printed via the Setup -> Check Plot menu. get to the “Setup” menu (Fig.4), then highlight “Postscript” in the available list and press <Enter>. The “Postscript Setup” menu appears (Fig.5). Next, highlight “Type” and press <Enter>. Press <Enter> again to accept the default driver path of C:\ TRAXPLOT and you’ll be presented with a list of all the available Postscript drivers. Simply highlight “Postscript 1200dpi A4” in the list and press <Enter>. Finally, highlight “Device” in the “Postscript Setup” menu and press <Enter>. This entry determines where Traxplot sends the Postscript output. Choose “File” and press <Enter>, and you’ll be prompted for the filename. Hit <Enter> again to accept the default, which in this case is C:\TRAXPLOT\ PSU. There’s no need to add an extension to the filename, as Traxplot will assign this automatically, according to the type of printout. For example, the file for a check plot will be named PSU.SCK, whereas for a bottom layer print, it will be PSU.SBL. Note the options for scaling and correction. Generally, these should remain as shown. However, if you find that your printer has a small, consistent scaling error (eg, slight stretching of the length), you may be able to compensate for it by adjusting these parameters. OK, we’re all set. Returning to the main menu, highlight “Postscript” and press <Enter> to create your check Fig.5: use these settings for Postscript output. Of course, the “Device” file name can be changed to whatever you desire. Don’t change the “offset” and “correction” parameters unless you know exactly what you’re doing! April 2004  13 Fig.7: GSview allows you to convert images to a variety of graphics formats. Individual layers can then be edited in your favourite graphics program. In the example shown here, we’ve colour-coded each layer and superimposed them for an eye-catching effect. Fig.6: after generating a Postscript file of the design in Traxplot, it can be viewed and printed from within Windows using a variety of different programs. Here we’re using GSview for the job (it’s free!). plot. If all goes well, you will get a report of “Postscript File Generated” and a new file named PSU.SCK will have been created in the C:\TRAXPLOT folder. Postscript viewer As mentioned previously, many popular Windows-based graphics packages are capable of displaying and printing Postscript files. If you don’t already have one of these, then we suggest Ghostscript and GSview, a free interpreter and viewer that you can download from www.cs.wisc. edu/~ghost. Make sure that you download the Windows (Win32) versions! Ghostscript must be installed first, followed by GSview. Installation is simply a matter of double-clicking on the downloaded files and following the prompts. Once installation is complete, launch GSview and load the PSU. SCK file created earlier. Note that in the GSview “Open” dialog, you must change the “Files of Type” to “All Files (*.*)” in order to see files with extensions other than the defaults. A “DSC Warning” message will appear when the file is opened; click on the “OK” button to continue. Fig.6 shows the loaded image. You may find that some images Silicon Chip Binders  Each binder holds up to 12 issues  SILICON CHIP logo printed on spine & cover Price: $A12.95 plus $A5.50 p&p each. Available in Australia only. Buy five and get them postage free. Just fill in & mail the handy order form in this issue; or fax (02) 9979 6503; or ring (02) 9979 5644 & quote your credit card number. 14  Silicon Chip REAL VALUE AT $12.95 PLUS P & P appear to be “cut off”. This can be corrected by enabling the “EPS clip” setting on the “Options” menu. GSview includes a host of other settings, allowing you to change things like media size and orientation. There’s no need to change any of these for now. To print the image, select File -> Print from the main menu. You can also save the image in a variety of graphics formats via the File -> Convert menu. This gives a great deal of flexibility in how a design is displayed. For example, you might want to print a multi-layer design with each layer displayed in a different colour. To do this, print each layer separately from Traxplot, then export it in the desired format and manipulate it using your favourite graphics package. We produced a colour version of the demo design to show the effect (see Fig.7). Alternative printing methods Apart from the methods described above, there are a number of other ways of obtaining high-quality prints of your PC board designs. For example, “LaserPC” looks ideal for those producing sophisticated designs requiring film output. Check out http:// traxlaserplot.sourceforge.net for more information. Another method involves the installation of a special Traxplot printer driver that produces .PCX file output. The resultant .PCX files can be displayed, printed and converted to any graphics format using free Windows software. Note that during in-house tests, we found that the PCX driver failed to scale the output correctly when using high resolutions (1200dpi) and large board sizes. Apparently, this is caused by a limitation within Traxplot, not a bug in the driver itself. Nevertheless, this driver would be an excellent way of producing prints of smaller designs (and board graphics for the Internet) with little effort. You can obtain a copy from www.airborn.com.au/layout/ printdrv.html Thanks go to Matthias Hartl, the author of the PCX driver, and Airborn Electronics for making the driver (and a lot of other useful Autotrax information) available for free! Board manufacture If careful examination of the check plot doesn’t reveal any problems, then www.siliconchip.com.au Making Your Own PC Boards: Step-By-Step 1 Laser print or photocopy the bottom layer onto the dull (emulsion) side of the Press-n-Peel film as described in the text. Cut out the result with scissors, leaving about a 5mm border around the image. 4 The idea is to heat the entire board evenly, until it reaches the temperature of the iron. The time required will vary according to your iron and the size of the board. Generally, somewhere between 1.5 and 4 minutes should do it. Of course, you shouldn’t use steam! 3 2 Prepare a section of blank PC board that is at least 5mm larger than the image size. Using a fine file, remove any burrs from around the edges that may have resulted from cutting or shearing. Thoroughly clean the copper with a new scouring pad or steel wool (not sandpaper). Use plenty of water and a drop or two of liquid soap. The surface should be evenly bright and perfectly clean. Flush under running water to remove any traces of soap and dry thoroughly with a clean, lintfree cloth. You must NOT touch the copper surface of the board with your fingers. Position the Press-n-Peel film image side down on the copper and centre it within the available space. Now “iron on” the film using only light downward pressure. A piece of plain paper between the iron and the film helps to prevent burning and sticking. The film manufacturer suggests a temperature of between 135°C and 162°C. Apparently, this should be somewhere between the “acrylic” and “polyester” settings on a typical iron. 7 Clean off the Press-n-Peel image just before you’re ready to drill and populate the board. Again, use a scouring pad with liquid soap and running water. 6 5 Quench the board and film under cold running water, and then gently peel off the film. The board will be hot, so take care! Our result wasn’t too bad for a first attempt. It appears that we applied the iron for a little longer than necessary, as the image was slightly “smeared”. www.siliconchip.com.au Etch the board using ferric chloride or Ammonium Persulphate per the directions included with the chemical. Here we’re using a commercial etching tank complete with a fish tank heater and an aerator. If you’ve never done this before, we suggest that you refer to the “Making Photo Resist PC Boards At Home” feature in the March 2001 issue of SILICON CHIP. Note that these chemicals (especially Ferric Chloride) are highly corrosive! 8 After drilling and cutting to the correct size, we’re ready to assemble the boards. Note how the slight image smearing (see step 5) resulted in “rough” copper edges – but the result is still quite useable! A coating of circuit board lacquer can be applied to prevent corrosion. April 2004  15 Fig.8: multiple designs can be laid out for printing with the aid of Traxedit’s Block operations. Leave enough space between the board outlines so that you’ll be able to separate them without difficulties after the etching and drilling processes. your design is almost ready to go. If you’ll be sending it to a board manufacturer, then it is imperative to first make sure that it meets all of the manufacturer’s requirements. This will include things like the inclusion of corner cut marks/routing outlines, layer identification, minimum clearances and valid hole sizes. These requirements vary between manufacturers, so we’ve not listed them here. All manufacturers that we know of will accept your designs in Protel .PCB format. This is a big advantage for the casual designer, as it means that there’s no need to learn how to create Gerber and NC drill output files. By way of explanation, Gerber files are used to photoplot your design onto film, whereas NC drill files are used to control the drilling machine. The manufacturer will produce these files from your Autotrax .PCB file. Making your own PC boards If you have a little spare time and want to save some money, you can make your own PC boards at home. Traditionally, this has involved the use of light-sensitised PC boards, UV exposure and chemical etching. This is still a favoured method, particularly with the availability of reliable, low-cost pre-sensitised PC board material. You can refer to our article entitled “Making Photo-Resist PC Boards At Home”, published in the March 2001 issue of SILICON CHIP, for details of this method. Another method gaining popularity eliminates the need for light-sensitised PC board material (and therefore UV exposure) altogether. It allows you to transfer your designs directly onto untreated PC board copper – ready for etching! This is achieved with the relatively new “Press-n-Peel” system. Just Press-n-Peel! The basic materials needed for this system are blank PC board, Press-nPeel transfer film, a standard clothes iron and a full-size printout of your artwork. The PC board pattern is first laser printed or photocopied onto the Pressn-Peel film, which is then “ironed on” to the bare copper. Following this, the sheet of film is peeled away, leaving behind a black resistive coating defining the layout image. Then all that’s required is the usual etching process to expose your masterpiece! The procedure for preparing a design for etching is depicted in an accompanying panel. The first step requires you to print the design onto the Press-n-Peel film, so let’s look how this is achieved in some detail. Printing the pattern Fig.9: two copies of two images laid up and ready for printing onto the Pressn-Peel film. Because the film is ironed-on emulsion side down, board images must be printed in reverse (text shown in mirror image). This is the default (“normal”) orientation in Traxplot. However, if you’re using a photographic method that requires the opposite (“flipped”, or “right reading”) orientation, it can be changed via Options -> Flip Layer Setup. 16  Silicon Chip A print of the bottom layer of a design is easily obtained using the methods already described above. Note, however, that you need to change the “Type of Plot” setting in the Traxplot Options menu from “Check Plot” to “Bottom Layer” (Fig.2). In addition, it’s important that the “Pad Hole Guide Size” is set to 20 thou or thereabouts. This generates a smaller-than-life size “hole” in the middle of each pad, to be used as a target when drilling the holes. If you have a laser printer, you can print directly onto the Press-n-Peel file. Be sure to do a test print on plain paper first! If you have an inkjet printer, you must first print the design onto paper and then photocopy the result onto the Press-n-Peel film. www.siliconchip.com.au Note that you should set you printer (either laser of inkjet) to its maximum print density. The print density is usually configurable from the printer “Properties” menu. To produce multiple copies of the same design or a number of different designs on the same section of PC board, simply arrange all of the designs in a single .PCB file before printing. For example, we used the Block operations in Traxedit to make three additional copies of the demo design, arranged so that they fit across the bottom of a sheet (Fig.8). The Block -> Read command can be used to import other designs. Doing it on the cheap A similar method to that described above uses “toner transfer” from a sheet of plain paper, rather than specialised sheets of blue film. All you need in this case is an ordinary laser or photocopied print of your artwork. Of course, the results won’t necessarily be as “sharp” or as repeatable as those that can be achieved with Press-n-Peel film – but if you’re on a tight budget, it’s worth a try. Check out the February 2001 issue of SILICON CHIP for all the details. Did you know . . . ? Finally, Postscript (.EPS) format images of most of the PC boards published in SILICON CHIP can be downloaded from our web site at siliSC conchip.com.au. Converting From Positive To Negative Undoubtedly, some readers will prefer to use a photographic process for making their boards. In many cases, a negative, rather than positive image of the PC board pattern is required for the exposure. This can easily be produced by converting the Postscript image to graphics format and “reversing” it before printing. Let’s look at an example. With the board image open in GSview, select File -> Convert and choose the “bmpmono” format at 600dpi. When entering the filename, be sure to append a “.BMP” extension. The newly created bitmap file can then be opened in almost any graphics package and converted to a negative. We used “Irfanview”, which is available for free download from www.irfanview.com. To get the image to print properly (and to reduce file size), crop it down so as to include just the board with a small border around the edge. To convert to a negative, select Image -> Negative from the main menu. If your graphics program lacks this option, then simply use the palette editor to change black to white and vice-versa. Fig.10 shows a negative image of the demo design ready for printing. Important: never “resample” or Fig.10: if you’re using a photographic process instead of the “Press-n-Peel” method described here, then you may need a negative rather than positive image. Here we’ve used Irfanview to reverse the blacks and whites. “resize” the image – it must remain untouched (at 600dpi) to ensure sharp edges and accurate scaling. Always do a test printout and check board dimensions before going any further. Limited Stock Electronics TestBench Electronics TestBench is a valuable 128-page collection of 20 top test equipment projects from the pages of SILICON CHIP. Includes: Power Supplies, Semiconductor Testers, Inductance Meter, Cable & Wiring Tester, Pink Noise Source, Zener Diode Tester, Crystal Checker, Sound Level Meter, Insulation Tester, Logic Probes, Low Ohms Tester, Remote Control Tester, Telephone Exchange Simulator, High-Voltage Insulation Tester. SPECIAL PRICE: $9 (INC P&P & GST). Note: may be shop-soiled. Order by phoning (02) 9979 5644 & quoting your credit card number; or fax the details to (02) 9979 6503; or mail your order with cheque or credit card details to Silicon Chip Publications, PO Box 139, Collaroy, NSW 2097. www.siliconchip.com.au April 2004  17