This is only a preview of the November 2003 issue of Silicon Chip.
You can view 27 of the 104 pages in the full issue, including the advertisments.
Items relevant to "A 12AX7 Valve Audio Preamplifier":
Items relevant to "Our Best LED Torch EVER!":
Items relevant to "Smart Radio Modem For Microcontrollers":
Items relevant to "The PICAXE, Pt.8: The 18X Series":
Items relevant to "A Programmable PIC-Powered Timer":
Purchase a printed copy of this issue for $10.00.
Here’s the second part of our short series on designing your own PC bards. This month, we take up from where we left off with component placement and design. Part 2 – by David L. Jones I t’s often said that PC board design is 90% placement and 10% routing. While the actual figures are of no importance, the concept that component placement is by far the most important aspect of laying out a board, certainly holds true. Good component placement will make your layout job easier and give the best electrical performance. Bad component placement can turn your routing job into a nightmare and give poor electrical performance – perhaps not even work at all. It may even make your board unmanufacturable. So there is a lot to think about when placing components! Every designer has their own method of placing components. If you gave the same circuit (no matter how simple) to 100 different experienced designers, you’re likely to get 100 different PC board layouts. So there is no absolute right way to place your components. It’s largely a matter of experience. But there are quite a few basic rules which will help ease your routing, give you the best electrical performance and simplify large and complex designs. Getting down to basics Here are some basic steps required for laying out a complete board: www.siliconchip.com.au Set your snap grid, visible grid, and default track/pad sizes. Throw down all the components onto the board. Divide and place your components into functional “building blocks” where possible. Identify critical tracks on your circuit and route them first. Place and route each building block separately, off the board. Move completed building blocks into position on your main board. Route the remaining signal and power connections between blocks. Do a general “tidy up” of the board. Do a Design Rule Check. Check your board thoroughly. Then get someone else to check it! This is by no means a be-all and end-all check list – it’s highly variable depending on many factors. But it is a good general guide to producing a first-class layout. A bit more detail Let’s look in more detail at the procedure described above. We have already looked at the grids and track/pad sizes. These should be the first things that you set up before you start doing anything. No exceptions! Many people like to jump straight into placing all the components into what they think is the most optimum position on the board, all in one hit. While this can work for small circuits, you don’t have much of a The very first step in designing a PC board using any PC board software is to set the snap grid, visible grid and default track/pad sizes. This screen (from the popular “Autotrax” freeware) shows how it is done. Other software packages will have similar settings. November 2003 85 hope when you have more complex circuits with hundreds of components spread across many functional circuit blocks. Why? Because it’s very easy to run out of “routing space” which is the room to lay down all your tracks. If you fix all your component positions and then try to route everything, you can easily paint yourself into a corner, so to speak. Alternatively, if you space the components out too much, you can end up with a large board that does not make efficient use of space. The hallmark of an inexperienced designer is a board that has every component evenly spaced out and then has thousands of tracks and links or vias criss-crossing the board. It might work but it can be ugly and inefficient, not to mention bigger and more expensive to manufacture. The best way to start your layout is to get ALL of your components onto the screen first. If you have a companion schematic package, then the simplest way to do this is to get your PC board program to import your schematic design and select all the components automatically. This will also be discussed later. If all you have is a PC board program, then you’ll have to select each compo86 Silicon Chip nent from the library and place them manually. With all the components on screen, you should get a good indication of whether or not your parts will easily fit onto the size (and shape) of board that you require. If it looks like it’s going to be a tight fit, then you know that you will have to work hard to try and keep the component spacing “tight” and the tracking as efficient as possible. If it looks like you have plenty of room, then you can be a bit more liberal in your layout. Of course, if it looks like you have Buckley’s chance of getting your components on the board, you’ll have to go back to the drawing board. Now analyse your schematic and determine which parts of the design can be broken up into “building blocks”. Often this is fairly obvious. For example, say you have a complex-looking active filter in your circuit. This would typically have a single input line and a single output line but will have lots of components and connections as part of the filter. This is a classic “building block” circuit and one that lends itself well to combining all of these parts together in the same location. So you would grab all of these parts and start to arrange them into their own little layout off to one side of your board. Don’t worry too much about where the actual block goes on your board yet. You will also need to partition off electrically sensitive parts of your design into bigger blocks. One major example is with mixed digital and analog circuits. Digital and analog just do not mix and will need to be physically and electrically separated. Another example is with high frequency and high current circuits; they do not mix with low frequency and low current sensitive circuits. We’ll have more about this later. As a general rule, your components should be neatly lined up: ICs in the same direction, resistors in neat columns, polarised capacitors all around the same way and connectors on the edge of the board. Don’t do this at the expense of having an electrically poor layout or an overly big board though. Electrical parameters should always take precedence over nicely lined up components. Symmetry is really nice in PC board design. If you have something like two identical building block circuits side by side and one is laid out slightly differently, it sticks out like a sore thumb. If you have placed your components www.siliconchip.com.au wisely, 90% of your work will be done. The last 10% is just joining the dots, so to speak. Well, not quite –but good placement is a good majority of your work done. Once you are happy with the component placements, you can start to route all the different building blocks separately. When finished, it is then often a simple matter to move and arrange the building blocks into the rest of your design. The Design Rule Check (DRC) will be covered later but it is an essential step to ensuring that your board is correct before manufacture. A DRC basically checks for correct connectivity of your tracks and for correct widths and clearances. Getting someone to check your board may sound like an overly bureaucratic process but it really is a vital step. No matter how experienced you are at PC board design, there will always be something you overlooked. A fresh pair of eyes and a different mindset will pick up problems you would never see. If you don’t have anyone to check your board over, then you’ll have to do it yourself. Get a printout of your schematic and a highlighter pen. Now, compare every single electrical “net” connection (connection between two points) on your board with the schematic, net by net. Highlight each net on the schematic as you complete it. When you are finished, there should be no electrical connections left that aren’t highlighted. You can now be fairly confident that your board is electrically correct. Basic routing Now it’s time for some basic routing rules. Routing is also known as “tracking”. Routing is the process of laying down tracks to connect components on your board. An electrical connection between two or more pads is known as a “net”. Keep nets as short as possible. The longer your total track length, the greater its resistance, capacitance and inductance – all of which can be undesirable factors. Tracks should only have angles of 45°. Avoid the use of right angles and in no circumstances use an angle greater than 90°. This is important to give a professional and neat appearance to your board. PC board packages will have a mode to enforce 45° movements – make use of it. There should never be a need to turn it off. Contrary to popular belief, sharp right angle corners on tracks don’t produce measurable EMI or other problems. The reasons to avoid right angles are much simpler – it just doesn’t look good and it may have some manufacturing implications. Forget nice rounded track corners, they are harder and slower to place and have no real advantage. Stick to 45° increments. Rounded track bends belong to the pre-CAD taped artwork era. “Snake” your tracks around the board – don’t just go “point to point”. Point to point tracking may look more efficient to a beginner at first but there are a few reasons you shouldn’t use it. The first is that it’s ugly, always an important factor in PC board design! The second is that it is not very space-efficient when you want to run more tracks on other layers. Enable your electrical grid, which is sometimes referred to as a “snap to centre” or “snap to nearest” option. Let the software find the centres of pads and ends of tracks automatically for you. This is great for when you have pads and tracks which aren’t lined up to Both of these PC boards are electrically identical; both would of course work the same. But you can see instantly just how much better the board on the right looks with the tracks following the 45° design rule. www.siliconchip.com.au In this case, the bypass capacitors on the power rails are too far removed from the supply pins on the ICs. Notice the difference? It not only looks neater and also takes up a lot less real estate – it will work better! your current snap grid. If you don’t have these options enabled then you may have to keep reducing your snap grid until you find one that fits – far more trouble than it’s worth. There is almost never a reason to have these options disabled. Always take your track to the centre of the pad; don’t make your track and pad “just touch”. There are a few reasons for this. The first is that it’s sloppy and unprofessional. The second is that your program may not think that the track is making electrical connection to the pad. Third, with surface mount components, an off-centre track-pad connection can again cause solder surface tension to pull the component out of alignment. Proper use of a snap grid and electrical grid will avoid problems here. Use a single track, not multiple tracks tacked together end to end. It may make no difference to the look of your final board but it can be a pain for future editing. Often you’ll have to extend a track a bit. In this case, it’s best to delete the old one and place a new one. It may take a few extra seconds but it’s worth it. People looking at your finished board may not know but you will know! It’s the little touches like this that set good PC board designers apart. Make sure your tracks go right through the exact centre of pads and components, and not off to one November 2003 87 side. Use of the correct snap grid will ensure that you get this right every time. If your track doesn’t go through the exact centre then you are using the wrong snap grid. Why do you need to do this? It makes your board neater and more symmetrical and it gives you the most clearance. Only take one track between 100 thou pads unless absolutely necessary. Only on large and very dense designs should you consider two tracks between pads. Three tracks between pads is not unheard of but we are talking seriously fine tolerances here. For high currents, use multiple vias when going between layers. This will reduce your track impedance and improve the reliability. This is a general rule whenever you need to decrease the impedance of your track or power plane. Don’t “drag” tracks to angles other than 45° “Neck down” between pads where possible. Eg, a 10 thou track through two 60 thou pads gives a generous 15 thou clearance between track and pad. If your power and ground tracks are deemed to be critical, then lay them down first. Also, make your power tracks as BIG as possible. Keep power and ground tracks running in close proximity to each other if possible, don’t send them in opposite directions around the board. This lowers the loop inductance of your power system, and allows for effective bypassing. Keep things symmetrical. Symmetry in tracking and component placement is really nice from a professional aesthetics point of view. Don’t leave any unconnected copper fills (also called “dead copper”), ground them or take them out. If you are laying out a non-platedthrough double-sided board, then there are some additional things to watch out for. Non-plated-through holes require you to solder a link through the board on both the top and bottom layer. Do not place vias under components. Once the component is soldered in place you won’t be able to access the joint to solder a feed through. The solder joint for 88 Silicon Chip Adding a chamfer to a “T” junction doesn’t just look neater, it helps prevent undercutting. Likewise, “teardrops” added to the joins between tracks and pads looks neater and also helps prevent etching problems. the feed through can also interfere with the component. Try to use through-hole component legs to connect top tracks to bottom tracks. This minimises the number of vias. Remember that each via adds two solder joints to your board. The more solder joints you have, the less reliable your board becomes, not to mention that that it takes a lot longer to assemble. Finishing Touches: Even though you have finished all your routing, your board isn’t yet complete. There are a few last minute checks and finishing touches you should do. If you have thin tracks (<25 thou) then it’s nice to add a “chamfer” to any “T” junctions, thus eliminating any 90° angles. This makes the track more physically robust, and prevents any potential manufacturing etching problems. But most importantly, it looks nice. Check that you have any required mounting holes on the board. Keep mounting holes well clear of any components or tracks. Allow room for any washers and screws (especially when it comes to mains voltage clearances). Minimise the number of hole sizes. Extra hole sizes cost you money, as the manufacturer will charge you based on not only the number of holes in your boards but the number of different hole sizes you have. It takes time for the very high-speed drill to spin down, change drill bits and then spin up again. Check with your manufacturer for these costs, but you can’t go wrong by minimising the number of hole sizes. Double check for correct hole sizes on all your components. Nothing is more annoying than getting your perfectly laid out board back from the manufacturer, only to find that a component won’t fit in the holes! This is a very common problem; don’t get caught out. Ensure that all your vias are identical, with the same pad and hole sizes. Remember your pad-to-hole ratio. Errors here can cause “breakouts” in your via pad, where the hole, if shifted slightly can be outside of your pad. With plated through holes this is not always fatal, but without a complete annular ring around your hole, your via will be mechanically unreliable. Check that there is adequate physical distance between all your components. Watch out for components with exposed metal that can make electrical contact with other components, or exposed tracks and pads. Change your display to “draft” mode, which will display all your tracks and pads as outlines. This will allow you to see your board “warts and all”, and will show up any tracks that are tacked on or not ending on pad centres. If you wish, add “teardrops” to all your pads and vias. A teardrop is a nice “smoothing out” of the junction between the track and the pad and is, not surprisingly, shaped like a teardrop. This gives a more robust and reliable track to pad interface, better than the almost right angle between a standard track and pad. Don’t add teardrops manually though, it’s a waste of time. But if your program supports automatic teardrop placement, feel free to use it. Single-sided PC board design Single-sided design can greatly reduce the cost of your board. If you can fit your design on a single sided board then it is preferable to do so. Look inside many of today’s consumer items like TVs and DVD players, and you will almost certainly find some single-sided boards. www.siliconchip.com.au Just about all of SILICON CHIP’s boards are single-sided. They are still used because they are so cheap to manufacture. And in the case of SILICON CHIP boards, single sided are much easier for those who wish to make their own from the printed patterns or downloaded web files. Single-sided design requires some unique techniques which aren’t required once you go to doubled-sided and multi-layer design. It is certainly more challenging than a double-sided layout. Probably the biggest differences is that some links (jumpers) may be required when it is impossible to avoid tracks crossing over one another. However, links should be avoided if at all possible. In fact, a single-sided board design will be regarded inversely proportional to the number of jumper links used. “No links” earns the admiration of many peers! Component placement can be even more critical on a single-sided board, so it won’t always be possible to have all your components nice and neatly aligned. Arrange your components so that they give the shortest and most efficient tracking possible. www.siliconchip.com.au It is like playing a game of Chess; if you don’t think many moves ahead then you will get yourself in a corner pretty quickly. Having just one track running from one side of your board to the other can ruin your whole layout, as it makes routing any other perpendicular tracks impossible. Many designers will route their board as though it is a double-sided board but only with straight tracks on the top layer. Then when the board is to be manufactured, the top layer tracks are replaced with jumper links. This can be a rather inefficient way to approach single sided design and is not recommended. You must be frugal in your placement, and don’t be afraid to rip everything up and try again if you see a better way to route something. Double-sided PC board design Double-sided PC board design gives an extra degree of freedom for designing your board. Things that are next to impossible on a single-sided board become relatively easy when you add an additional layer. Many (inexperienced) designers tend to become lazy when laying out double-sided boards. They think that component placement doesn’t matter and that hundreds of vias can be used to get them out of trouble. They will often lay out components like ICs in neat rows and then proceed to route everything using right angle rules. This means that they will route all the tracks on the bottom layer in one direction and then all the tracks on the top layer perpendicular to the bottom layer. The theory is that if you chop and change between layers enough times you can route almost anything using a “step” type pattern. This technique can be ugly and inefficient and is a throwback to the old manual tape days. Many basic PC “auto routers” work in this way. Stick to using good component placement techniques and efficient building block routing. Double-sided design can also give you the chance to make use of good ground plane techniques, required for high frequency designs. This will be discussed later. That’s all for this month. Next we will look at more advanced topics like multi-layer boards, ground planes, high frequency design, auto routing and SC design for manufacturing. November 2003 89