====================================================================== NOTE: This is an exerpt from the documentation for ... +-------------------+ | AutoCAD-PCB | +-------------------+ Freeware Accessories For Electronic Design Using AutoCAD(tm). ...written by Paul Marxhausen. Since this document has a lot of tips that are applicable to using ANY kind of software in the creation of PC boards and discusses other aspects of board creation/etching/etc., I've edited out the information that applies only to AutoCAD-PCB and left the "generic" information. Just remember there are still things here that are AutoCAD-specific. The entire document can be read by downloading ACADPCB.ZIP from oak.oakland.edu in /pub/msdos/autocad (or any other SIMTEL mirror site.) Extra comments have been added in [square brackets] where needed. ========================================================================= [Note: any drawing program used to make a PCB MUST have a "snap to grid" feature of some type to line up parts . . .] The SNAP is like an invisible grid whose size the user can define. When drawing lines or selecting points on the drawing, the cursor will "snap" to these points only if SNAP is on. This makes it easy to line up objects. The SNAP defaults to 25 mils, and can be toggled between that setting and a 100 mil snap with the SNAP submenu. These snap settings are useful in PC board work because most standard pin spacings are .1 inches, or 100 mils. Thus, using a 100 mil snap makes it easier to place parts on the board in proper alignment, while the 25 mil snap gives finer control for routing traces while still making it easy to line up with objects on the 100 mil grid. --------------------------------------- +=============================================================================+ | IMPORTANT: AutoCAD-PCB assumes that you are drawing the circuit board from a| | TOP VIEW, looking down at the component side of the board. In effect, as | | you draw the traces you are doing so as if you had a transparent board. | | This is because integrated circuit data books always give their chip pin- | | outs as a top view, and it's easier to route your traces in a top-view mode.| | However, when it comes time to plot or print the traces to make a circuit | | board negative or similar, it will be necessary to MIRROR this view, which | | is easily done in AutoCAD. For more details, consult the Printing and | | Plotting section below. | +=============================================================================+ --------------------------------------------- DRAWING A BOARD How Many Sides? So much for tools - how do you draw a board? First, you'd better decide on how many sides you're going to be using. To give you some idea of what's involved with this decision, and to show you how the "pros" do it, get yourself just about any commercially manufactured printed circuit board, such as an expansion card from a personal computer or similar. Take a look at how the chips are laid out and the traces are run. People making boards for a living have a big stake in giving their boards a tight, efficient layout. However, people making boards for a living use something you may not want to get involved with, and that's called "multi-layered boards." Time was, PC boards only had traces on the bottom side. And in fact, not only can you do a lot of projects with single sided boards, but they are far and away the easiest and cheapest kind of PC board to produce . . . from the standpoint of exposing, developing, and etching them. But even on a simple design, you're going to find traces that you just can't seem to get from here to there without crossing something, and you'll start putting jumper wires on the top of the board. From there, it's only a short jump to wanting to do a double-sided board. The tradeoff? Well, putting traces both top and bottom can cut your design time considerably, because you spend less time trying to snake leads around some torturous path from here to there without crossing another lead. You can always just run your problem trace on the other side of the board. You'll see a lot of this on commercial boards: traces that stop and switch over to the other side of the board two, three, or four times before they get to where they're going. Being able to do this makes it easier for the designer, but tougher on whoever is fabricating your finished board. In particular, if you're etching your own board, you probably won't be able to make "plated-through holes", where there is metal between pads on the bottom and top. Without such plating, you HAVE to solder leads on BOTH sides of the board if you need the signal to get to both sides: this can be very difficult to do with many integrated circuit sockets. At the UN-L E.E. Shop, we try to stay with single-sided designs unless we have a large number (30 or more) of jumpers going on the top side. Commercial boards don't stop at double-sided any more, either: many of them, especially computer boards, actually have additional layers INSIDE the board. (The board is made by laminating very thin circuit board layers into a single piece.) Usually, these internal layers will be used to make a ground plane that takes ground to all appropriate pins; similarly, there will often be a layer dedicated to getting 5 volts to all the chips. This makes a board designers job even easier, but it makes production by anything less than a professional fabricator pretty much impossible. OK, OK, But How Do I Draw The Board? No sweat. Use the menus or command line to get to the OUTLINE layer, draw the outline of your board; go to the PADS layers and use the predefined blocks to drop your IC sockets and other component pads where you want them; then go to the BOTTOM layer and use the PTRACE menu to hook up wires from pad to pad. Voila, you're done! Right? Well, almost. Actually it's not much more than just that. It's just that it can take a lot of time trying to get the darn traces from Point X to Point Y without crossing each other. And how do you decide where to put your chips? And what about running traces between pins? And on, and on . . . As far as chip placement goes, you have to have a good idea of how your circuit is wired. If you don't have at least a scribbled schematic with the pin numbers of your chips labeled on it, you're really going to be groping in the dark. Really, component placement is just a mixture of good common sense, a good eye for topology, and a computer video game player's passion for solving problems. (Being good with mazes helps, too!) Try starting with obvious things: for example, most 28 pin DIP memory devices have similar pin-outs that facilitate having them sit all in a row. You're probably going to want to have them as close as possible to the CPU, if this is a microprocessor board. What side of the CPU does the data buss come out of? You're trying to make the simplest, shortest, and most direct connection between devices that have to be connected. You're also going to want to keep your analog and digital sections of your circuit seperate from each other when you can, to keep digital noise out of your analog circuits. Aside from that, you can make your own rules about the layout. Sometimes you have to "break the rules" in order to get everything routed. For example, it's a common sense practice to have most of your chips oriented the same way, with the notched ends all pointed the same direction - it's logical and looks good; but I've had to put the chips in "backwards" before just because that was the only way to get the traces routed in a straightforward way. Which Traces First? It's a good idea to take care of some connections before others. For example, on our hypothetical microprocessor board, you're going to have a keen interest in where the data buss lines have to go, because they have to go a lot of places and they all should go there together (unless you want to route each one individually.) More obviously, how are you going to get power and ground to all of your chips? This is a point where the multi-layer people have it good. They can forget about worrying about power and ground because they have entirely different layers to deal with those. But when you're struggling to route a single-sided board, you'll find that those darn power leads seem to be in the way every time you're trying to place a signal trace someplace. Yet most design guides say to run power and ground first! What do you do? I've taken to running nice fat power and ground traces more or less around the outer edges of the board, then using jumpers on the top to bring them over to the chips. This eliminates some of this difficulty. And you will find that after all is said and done and drawn, that you'll be able to make some of the power and ground buss connections on the bottom with traces. It's just that I feel that if I'm going to have to use a few jumpers here and there anyway, I'd rather use them on power and ground to simplify my life, instead of having to jumper, for example, all eight data buss leads over a power supply trace. Many times you have to work in tight spaces, ESPECIALLY if you have to run a trace between two pads that are 100 mils apart. At that point, you have to go to a Fine trace, or you can end up with traces and pads that look like they have space between them when you're zoomed in close on the screen, but which will end up touching when you print or plot the thing out, or have a negative made of your drawing. When you are trying to run leads between pads, it's almost certain that you'll have to use the 60 mil width pads (OP60, SP60, RP60) and the 13 mil Fine trace. [I've seen professional CAD packages that claim to be able to put two or even three traces BETWEEN two pads that are on 100 mil centers; fat chance. You'd have to have awfully skinny traces and mighty tiny pads, which may be possible with professional boards but is an invitation to frustration and no-functionality with "amateuer" boards. Even if you manage to produce the extremely high-resolution output needed, you'll have traces that break easily and peel up when you solder to them.] For running power and ground leads, using wider traces is advisable. I often use the Wide trace for this, while the Power width is so wide that I generally reserve it for use in those big fat power and ground busses that I run around the periphery of the board. Again, this is all pretty much common sense stuff. Not enough width choices on the menu? Enter TRACE from the command line and it will ask you for the width first, defaulting to the width of the last trace if you just hit . Think you used the wrong size? The "Edit" item under the PTRACE menu (which executes a PEDIT command) will let you change the width of an entire trace after the fact, which is nice. How About Some Extra Caps? If you weren't already aware of it, it's a standard practice with circuit boards using logic chips to place a small (.01 to .1) "despiking" capacitor from power to ground of every chip, AT THE CHIP. Even with a nice solid five volt supply attached to your board, power often has a long way to go to the chips, sometimes down some very skinny traces. The resulting added lead resistance means that "spikes" or fluctuations can occur on the power supply right at the chip as devices switch or change their current demand. This can lead to all sorts of really, really frustrating and untraceable malfunctions. Do yourself a favor; despike everything you can. In addition, I will often add one small (10 to 100 microfarad) electrolytic cap across the power supply to ground on the board, often at the point that is farthest from where power connects to the board. This helps to keep the power supply solid and smooth. Making Changes Unless you're making a very simple circuit on a very large board the odds are that at some point in your drawing, you're going to have to make a lot of major changes. The chip layout you chose just doesn't get enough leads close enough to where they have to be; or the circuit is too large to fit on the board you've chosen; or any other of a number of things can happen. In any case, this is where using CAD to draw the board absolutely beats anything else hands down. Want to move a whole chunk of the circuit to another spot? Enter MOVE and select the parts and just drag them where you want them. Have a part of the circuit that is duplicated several times? You can use the COPY command to make multiple copies of anything and drop them wherever you want them. PRINTING, PLOTTING, AND PRODUCTION Producing your finished drawing is where things get crucial. It's also where AutoCAD shines, because A) it's a vector-based drawing package and will reproduce your drawing at the highest resolution of your printer or plotter; B) it supports a vast variety of output devices; and C) it can be made to output your drawing to exactly the correct scale. If you just want to get a rough-and-ready hard copy, you can use just about anything to print out the drawing. However, if your intent is to obtain camera-ready output that can be used to create a photographic negative, such as would be required to expose a negative-photo-resist copper circuit board, you're almost certainly going to need either a plotter with very fine output resolution (150 dots per inch or better) such as a laser printer; or you will need to use a pen plotter. We'll discuss both those options in a moment, but first let's look at some other considerations. --------------------------------------------------------- Printers and Plotters If you are trying to make a hard copy that will become a photographic negative (or positive, if you're using positive-resist circuit boards), the whole idea is to get output that is A) as FINE and SHARP a resolution as you can possibly get, and B) as UTTERLY, SOLIDLY BLACK as you can manage. There are ways to enhance both your resolution and your contrast, if this is a problem, as we'll see. But first let's look at some straightforward ways to get our artwork. Please note that again, you may want to have access to AutoCAD manuals to help you if you need to change the configuration of AutoCAD to handle a different output device, or to change the way it uses that output. This is done with the "Configure AutoCAD" command (5) available when you first start AutoCAD. Laser Printers Laser printers can give you both sharpness and blackness. With plenty of toner and at 300 dots per inch, you can get camera ready, 1:1 artwork from a laser printer. However, please note that some Laser Printers, especially older HP LaserJets, don't have enough memory to print an entire 8.5" by 11" page at 300 dots per inch. In this case, you either have to keep your drawing size to less than half a page (which is frequently possible), or you have to run the printer at 150 dots per inch, which you can do by changing AutoCAD's configuration. I've been told that you can laser print-plot on vellum, which is translucent to light, and use it as a positive for positive-resist boards directly, without transferring it to film. It's also possible to laser print with special paper, plastic, and/or toner to make an image that is then directly transferred to a non-sensitized copper board with a hot clothes iron. On someone's suggestion I have even tried this with plain paper and ordinary toner, with mixed success, mostly on really small items. I will definitely state that at UN-L's Engineering Electronics Shop, we've found negative resist boards a whole lot more reliable to work with, as they are less critical in their exposure and development than positive resist boards. We HAVE attempted to laser print directly onto the kind of overhead transparency sheets that are designed for use with photocopy machines. YOU MUST HAVE THE KIND OF SHEETS DESIGNED FOR PHOTOCOPIERS OR YOU CAN GET A BLACK, MELTED MASS OF PLASTIC IN YOUR LASER PRINTER!!! Anyway, it can work, but generally speaking the resulting black-on-clear positive image is either not black enough, or may contain a lot of "pinholes" where it's supposed to be black. Little irreg- ularities like that will drive you insane if you go ahead and make a board and don't realize that pinholes have created traces with breaks in them. On top of all that, this does give you a positive image and like I said, we're not really fond of positive resist etching processes. BUT . . . it's a tempting way to go. It might be worth at least a try. (NOTE: I'll keep referring to "your negative", assuming that you are making a drawing with black traces on white paper and then having a photo negative made with clear traces on black. If you are using a positive-etch board you will need a POSITIVE film transparency made, with black traces on clear film. Any lab that can make one can make the other. Be sure you get this straight with whoever's making your "negative.") Pen Plotters The best laser printer can meet it's match from even a modest pen plotter. Pen plotters can give you smooth lines without the slightest hint of the "jaggies". However, the user must remember the goals of "sharp and black" and take some precautions when using pen plotters. The most important one is, obviously, to have a plotter pen that's very sharp and has plenty of ink. Reasonable results can be obtained with the common disposable felt-tip plotter pens, if you use a nice new one. However, for the real McCoy, try to find a steel-tipped ink plotter pen that you can fill with India ink. These are like fine-point drafting pens and give superior consistency of line. However, they're not always easy to find and they aren't cheap. But if you plan to do a lot of this kind of work, you won't regret getting one. A nasty byproduct of plotters, however, is the possibility of the ink lines spreading or smearing. If you use ordinary paper, perhaps a sheet from your computer's fan-fold printer paper, you're going to see your lines bleed all over the place. You need to find paper that's good and "hard". There is drafting paper available that has this quality; also, you'll find that a lot of the inexpensive photocopy paper these days has one "hard" side for use with copiers and laser printers. You can actually feel the added smoothness of the hardened side. What If My Printer or Plotter Isn't So Great? As we'll discuss in a moment, the general practice is to plot or printer-plot your drawing out in the actual size, so a simple contact photo negative can be made at a 1:1 ratio. However, if your output resolution isn't so great - a laser or dot matrix printer that's plenty black but only 150 dpi or so - you can get around it by making your output exactly twice as large as what you'll need. You then tell the people making your negative to shrink your image down by EXACTLY half. This is a common practice in professional manufacturing. If you are having trouble getting the image black enough, try taking your print or plot to a photocopy machine and duplicate it on that. Maybe even copy the copy, if need be. This can sharpen and blacken your image, but it can also lead to extra spots, holes, and other degenerations, so examine your copies carefully. You may need to touch them up by hand with a black pen. How about combining the last two suggestions at once - using a copy machine to reduce your image in half while at the same time making it blacker? Good idea, EXCEPT . . . photocopier optics are not designed to give you PRECISE and EVEN reduction or enlargement. You'll probably end up with things that don't really line up, which is disasterous when ICs and other parts require precise .1 inch spacing. You can give it a try, but make sure you set some of your parts onto the output to see if it's actually the right size before you run off to have a negative made. This is a good idea regardless of how you print or plot your drawing. I've Got My Nice Sharp, Black Drawing - Now What? Now you've got to mull over your options. There are PC board labs that will make your board for you if you just provide them with the artwork you've created. (And if you provide them with suitable quantities of cash.) If you're just producing a single board, you may find out that this is a pretty expensive way to go, because there are set-up fees, and negatives to make, and possibly minimum orders to fill, so the first board or boards end up costing quite a bit. However, if you're making a whole lot of them, this is well worth looking into. After the initial costs, most PC board outfits can then crank out large numbers of your board at a very modest cost. This is especially nice when they offer such things as drilling out all of the holes, screening of labels or solder resist, and plating-through the holes. If you're going into limited production, do check this out. But many times, you just want one or two copies of your board. At this point, you should look into other options. Check the ads in the back of electronics magazines, check your local papers, ask around at Radio Shacks, read the Yellow Pages, and see if there isn't a small business or local hobbiest who will produce single boards or small quantities for a reasonable cost. If you're going to make your own PC board using a photo-negative-resist process, you need to find someone to make you a nice, HIGH CONTRAST negative from your artwork. Our Shop uses the University of Nebraska-Lincoln's Photographic Productions lab. The kind of photo shop that just cranks hundreds of rolls of color print film through a machine in an hour is probably not going to know what you're talking about, but there are many other commercial places that will. Try custom photo printing places, professional camera stores, or even your local professional photographer, who may do his own darkroom work. One of these places should be able to either help you or steer you to someone who can. Once you've found this marvelous individual, tell them you need a HIGH CONTRAST negative made. If your drawing is actual size, make sure you specify that it must be 1:1. If you've made a double-sized drawing, make sure they know it must be reduced by EXACTLY 2:1. Emphasize that the black areas must be as solidly black as possible. These people aren't dumb: explain just what it is you're doing and they'll understand the need for precision and high contrast. And Then ? . . . Once we get to exposing, developing, and etching the board, things get a little less certain because there are different kinds of boards and different kinds of chemicals. Most photosensitized boards that you can buy locally will include instructions regarding how long to expose them, and how to develop them. Please remember that sometimes these instructions are enclosed in the light-tight package the circuit boards are sold in: DON'T OPEN THE PACKAGE IN THE LIGHT! While PC boards are not as sensitive as photographic film, it doesn't take much light to "nuke" your board and make it unusable. Open the package in the dark or in a safe-lighted room. Sometimes you can buy the board and enough developer to finish it all in a single inexpensive kit. This is handy because you're sure you've got the right stuff for the job and you don't have to invest in more chemicals than you're going to use. The procedure for exposing most boards is pretty much the same: you clamp your negative or positive on top of the PC board in a dark room, then expose it to ultraviolet light for a while. The UV light in common flourescent bulbs will expose many boards in 20 to 45 minutes. It's better to get real UV lamps, because you can cut your exposure time down to about two minutes, and because fast, high-intensity exposure seems to be more forgiving of the quality of your negative than slow, low-intensity exposure. ------------------------------------------------------------------------------ BE CAREFUL - SOME TYPES OF UV LIGHT ARE EXTREMELY HAZARDOUS TO THE CORNEAS OF YOUR EYES!!!!!!! ------------------------------------------------------------------------------ Oh, and one major, major caution: MAKE SURE YOU PUT THE NEGATIVE ON THE RIGHT WAY. We've seen a lot of boards expose, develop and etch beautifully and then discovered that the pattern was backwards because the negative was on upside down. How do you avoid this? PUT TEXT ON YOUR TRACE LAYERS, remembering to make it BACKWARDS on the bottom so it's forwards when you mirror the bottom. When you expose the board, make sure you can read your text forwards. The chemicals for developing and etching the boards are available locally and also include instructions on how to use them. Follow the instructions religiously, as many of the chemicals involved in these processes are REALLY NASTY to breath and/or touch. Use good ventilation if you value your brain cells and lungs. And keep the etchant off of your hands or clothes - you won't notice it at first but then your skin will start to burn. Ouch. Also, not only will used etchant make indelible stains on your clothes but you'll find the cloth starts to disintegrate when you wash it. The most common etchant is some nasty stuff called ferric chloride; if you can find it, try to get yourself some sodium persulfate etchant. Sodium comes as a powder you mix with water, is transparent so you can see your board etch more clearly, and turns a nice bright blue as it becomes saturated with copper so you know to throw it away. (NOT down your drain unless you want to eat holes in your plumbing.) ------------------------------------------------------------------------------ ONE MORE TIME: PRINTED CIRCUIT BOARD DEVELOPMENT AND ETCHING INVOLVES CHEMICALS THAT CAN CAUSE SERIOUS INJURY IF INHALED, INGESTED, OR HANDLED IMPROPERLY. USE * ALL * SAFETY PROCEDURES SPECIFIED BY THE MANUFACTURER AND KEEP ALL EQUIPMENT AND MATERIALS SECURE FROM ACCESS BY CHILDREN OR OTHER NON-QUALIFIED PERSONS. ------------------------------------------------------------------------------ Our Little Advertisement . . . Making the board sound a little daunting? Just want to draw it and print it and have some other poor fool play in the darkroom with the toxic stuff? If you are a UN-L student, staff, or faculty member, you should know that the UN-L Engineering Electronics Shop has the facilities to etch PC boards if provided with a negative and the photosensitized board. The EE Shop tries to keep a few small boards in stock to sell if you haven't got one you've purchased elsewhere. We will expose, develop, and etch, and optionally tin-plate your board, for a modest fee. We have the necessary chemicals for developing negative-resist boards; if you want to use a positive-resist board, you'll need to also provide us with the chemicals for that board. It's not uncommon for such chemicals to be packaged in small kits,or bundled with a board, for the production of just one PC board. The EE Shop will NOT drill out the holes on your finished board. It's hard to overstate the amount of time required to drill boards - go ahead, count the number of holes on your design! Even a small board, such as a microcontroller circuit, can end up with 400 to 1000 holes! To drill the holes, it's best to have the use of a drill press. Even a drill press that just has a hand drill in a movable clamp will work. You'll also need a number of small drill bits, ranging in size from #60 to #70 or so. YOU NEED MORE THAN ONE, because YOU WILL end up breaking one at some point. The EE Shop WILL permit you to use our drill presses, BUT you have to provide your own bits. Also, as mentioned earlier, we don't have the means to "plate-through" the holes on a double sided board. THIS OFFER TO SERVE AS A BOARD ETCHER DOES NOT EXTENT OUTSIDE THE CONFINES OF THE UNIVERSITY OF NEBRASKA - LINCOLN. Closing comments: In searching for a CAD tool for electronic design that was available to our undergraduates, we've recently been evaluating the PADS software shareware edition and found it has considerable advantages over using AutoCAD. Still, our tools may fill a niche where people already have AutoCAD installed. If you are knowledgable about AutoCAD, you'll see that creating these tools was not enormously difficult, although it WAS very time - consuming. Every time I use them, it seems I find something I could have done better, or I think of another predefined block I could have added; but I had to quit at some point. As I mentioned, I don't intend to add to these tools, leaving that for others to do. If you want to drop me a line, I'm accessible on the Int- ernet at mpaul@unlinfo.unl.edu or mpaul@engrs.unl.edu. HOWEVER: I WILL NOT serve as an on-line substitute for an AutoCAD manual, and I'm not interested in tutoring anyone in the basic principals of AutoCAD when that information is quite available elsewhere. If you don't have a manual or access to one, you're probably not using a legal copy of AutoCAD! Our shop is also a good source of general advice regarding various methods of prototyping, circuit design, and other neighborly advice. Stop by and see us some time. Paul Marxhausen Electronics Tech III Engineering Electronics Shop Mail: 209N Walter Scott Engineering Center Location: 122 Walter Scott Engineering Center University of Nebraska-Lincoln Lincoln, NE 68588-0511 Internet Email: mpaul@unlinfo.unl.edu, mpaul@engrs.unl.edu