You've designed your circuit and perhaps even built a working prototype. Now it's time to turn it into a nice Printed Circuit Board design.
For some designers, producing the PC board will be a natural
and easy extension of the design process. But for others it can be a very daunting task.
There are even very experienced circuit designers who know very
little about PC board design, and they leave it up to the "expert" specialist PC board designers.
Many companies even have their own dedicated PC board design
departments. This is not surprising, considering that it often takes a great deal of knowledge and talent to position maybe hundreds of components and thousands of tracks into an intricate (some say artistic) design that meets a whole host of physical and electrical requirements.
Proper PC board design is a crucial part of an electronic
product. In many designs (such as high-speed digital, low level analog and RF), the PC board layout can make or break the operation and electrical performance of the design. It must be remembered that PC board tracks have resistance, inductance and capacitance, just like your circuit does.
This article is presented to take some of the mystery out of PC
board design. It gives some advice and "rules of thumb" on how to design and lay out your PC boards in a professional manner.
It is, however, quite difficult to "teach" PC board design.
There are many basic rules and good practices to follow but apart from that, PC board design is a highly creative and individual process. Many PC board designers like to think of PC board layouts as works of art, to be admired for their beauty and elegance. "If it looks good, it'll work good" is an old catch phrase.
Let's have a go, shall we...
How it used to be done
Back in the pre-computer CAD days, most PC boards were designed
and laid out by hand using black (or coloured) adhesive tapes and pads on clear drafting film. Many hours were spent slouched over a fluorescent light box, cutting, placing, ripping up and routing tracks by hand. Bishop Graphics, Letraset and even Dalo pens will be names that evoke fond or perhaps not-so-fond memories.
Even before that, literally at the dawn of the PC board age
(which believe it or not was only around WWII), patterns were laboriously drawn using pen and ink. You can imagine how popular were the draftsmen (or probably draughtsmen in those days!) who made a mistake - and even more so, the designer who made a mistake in the first place and tried to blame it on the hapless draftsman!
Those days are well and truly gone, with computer-based PC
board design having replaced hand layout completely in professional electronics and largely in hobby electronics.
Computer-based CAD programs allow the utmost flexibility in
board design and editing over the traditional techniques. What used to take hours can now be done in seconds.
PC board design packages
This is a screen grab from the DOS-based Autotrax PC board layout program. It doesn't have all the bells and whistles of modern packages such as Protel (which in fact evolved from Autotrax) but we wouldn't mind betting that there are still probably more PC boards designed using this (now) freeware package than any other, at least here in Australia.
There are many PC board design packages available on the
market, a few of which are freeware, shareware or limited component full versions. Protel is the defacto industry standard package in Australia. Professionals use the expensive high-end Windows-based packages such as Protel 99SE and DXP. Hobbyists use the excellent freeware DOS-based Protel AutoTrax program, which was, once upon a time, the high-end package of choice in Australia. Confusingly, there is now another Windows-based package called AutoTrax EDA. This is in no way related to the Protel software.
This article does not focus on the use of any one package, so
the information can be applied to almost any PC board package available. There is, however, one distinct exception. Using a PC board-only package which does not have schematic capability greatly limits what you can do. Many of the more advanced techniques to be described later require access to a compatible schematic editor program. This will be explained when required.
While you can download many software packages from the 'net, be
aware that many are not widely used (if used at all) in Australia. It's no good choosing a package and producing a brilliant PC board if the manufacturer you choose cannot handle the file that the package generates.
Similarly, you should never use a "paint" or drawing package to
knock-up a PC board pattern. Invariably, you will find it cannot be produced. (Readers have been known to submit projects for publication in SILICON CHIP with a PC board produced in, for example, Corel Draw. While it's a great drawing package, most PC board manufacturers cannot use any of the myriad of file types it
There are industry standards for almost every aspect of PC
board design. These standards are controlled by the former Institute for Interconnecting and Packaging Electronic Circuits, who are now known simply as the IPC (www.ipc.org). There is an IPC
standard for every aspect of PC board design, manufacture, testing and anything else that you could ever need. The major document that covers PC board design is IPC-2221, "Generic Standard on Printed Board Design". This standard superseded the old IPC-D-275 standard (also Military Std 275) which has been used for the last half century.
Local countries also have their own various standards for many
aspects of PC board design and manufacture but by and large, the IPC standards are the accepted industry standard around the world.
Printed Circuit Boards are also known (some would say, more
correctly known) as Printed Wiring Boards, or simply Printed Boards. But we will settle on the more common term PC board for this article.
Before you even begin to lay out your PC board, you MUST have a
complete and accurate schematic (circuit) diagram.
Some advanced software packages even have the ability to render a 3D image of the board design - also very handy for instruction manuals or marketing.
Many people jump straight into the PC board design with nothing
more than the circuit in their head or roughly drawn with no pin numbers and without any logical order. If you don't have an accurate schematic then your PC board will most likely end up a mess and take you twice as long as it should.
"Garbage-in, garbage-out" is an often-used quote that applies
equally well to PC board design. A PC board design is a manufactured version of your schematic, so it is natural for the PC board design to be influenced by the original schematic. If your schematic is neat, logical and clearly laid out, then it really does make your PC board design job a lot easier.
Good practice will have signals flowing from inputs at the left
to outputs on the right. Electrically important sections should be drawn correctly, the way the designer would like them to be laid out on the PC board. Bypass capacitors should be put next to the component they are meant for.
Little notes on the schematic that aid in the layout are very
useful. For instance, "this pin requires a guard track to signal ground" makes it clear to the person laying out the board what precautions must be taken.
Even if it is you who designed the circuit and drew the
schematic, notes not only remind you when it comes to laying out the board but they are also useful for people reviewing the design. Your schematic really should be drawn with the PC board design in mind.
Imperial and metric
The first thing to know about PC board design is what
measurement units are used, as they can be awfully confusing!
As any long-time PC board designer will tell you, you should
always use imperial units (ie, inches) when designing PC boards. This isn't just for the sake of nostalgia. The majority of electronic components were (and still are) manufactured with imperial pin spacing. So this is no time to get stubborn and refuse to use anything but metric units. Metric will make the laying out of
your board a lot harder, messier and may even make it more expensive to produce. So if you only learnt metric units, then you had better start learning about inches and how to convert them.
An old saying for PC board design is "thou shall use thous". A
"thou" is 1/1000th of an inch, and is universally used and recognised by PC board designers and manufacturers everywhere. So start practising speaking in terms of "10 thou spacing" and "25 thou grid"; you'll sound like a professional in no time!
Now that you understand what a thou is, we'll throw another
spanner in the works with the term "mil" (or "mils"). 1 "mil" is the same as 1 thou, NOT to be confused with the millimetre (mm) which is often spoken the same as "mil". The term "mil" comes from 1 thou being equal to 1 milli-inch.
As a general rule, avoid the use of "mil" and stick to "thou";
it's less confusing when trying to explain PC board dimensions to those metricated non-PC board people.
Some PC board designers will tell you not to use metric (ie,
millimetres) for ANYTHING to do with a PC board design. In the practical world though, you'll have to use both imperial inches (thous) and the metric millimeter (mm). So which units do you use for what? As a general rule, use thous for tracks, pads, spacings and grids, which are most of your basic "design and layout" requirements. Only use mm for "mechanical and manufacturing"
requirements like hole sizes and board dimensions.
You will find that most PC board manufacturers will follow
these basic guidelines, when they ask you to provide details for a quote to manufacture your board. Most manufacturers use metric size drills, so specifying imperial size holes really is counter-productive and can be prone to errors.
Just to confuse the issue even further, there are many
components (new surface mount parts are an example) which have metric pin spacing and dimensions. So you'll often have to design some component footprints using metric grids and pads. Many component datasheets also have metric dimensions even though the lead spacing is on an imperial grid. If you see a "weird" metric dimension like 1.27mm in a component, you can be pretty sure it
actually has a nice round imperial equivalent. In this case, 1.27mm is 50 thou.
Yes, PC board design can be confusing!
So whatever it is you have to do in PC board design you'll need
to become an expert at imperial to metric conversion and vice-versa. To make your life easier, all the major PC board drafting packages have a single "hot key" to convert between imperial and metric units instantly ("Q" on Protel for instance). It will help you greatly if you memorise a few key conversions, like 100 thou (0.1 inch) = 2.54mm and 200 thou (0.2 inch) = 5.08mm etc
Values of 100 thou and above are very often expressed in inches
instead of thous. So 0.2 inch is more commonly used than 200 thou.
1 inch is also commonly known as 1 "pitch". So it is common to
hear the phrase "0.1 inch pitch", or more simply "0.1 pitch" with the inch units being assumed. This is often used for pin spacing on components such as ICs or MKT capacitors.
100 thou is a basic "reference point" for all aspects of PC
board design and a vast array of common component lead spacings are multiples or fractions of this basic unit. 50 and 200 thou are the most common.
Along with the rest of the world, the IPC standards have all
been metricated and only occasionally refer to imperial units. This hasn't really converted the PC board industry though. Old habits die hard and imperial still reigns supreme in many areas of practical usage.
Snap to grid!
You can easily check your current setup - this one (from Autotrax) shows (among other things) that we are are using imperial measurement, we are working on the bottom layer (a single-sided board), our pads are 50 thou round and our track width is 25 thou. Any of these defaults can be changed at will or edited for specifics.
The second major rule of PC board design, and the one most
often missed by beginners, is to lay out your board on a fixed grid.
This is called a "snap grid", as your cursor, components and
tracks will "snap" into fixed grid positions - not just any size grid mind you, but a fairly coarse one. 100 thou is a standard placement grid for very basic through-hole work, with 50 thou being a standard for general tracking work, like running tracks between through-hole pads.
For even finer work, you may use a 25-thou snap grid or even
lower. Many designers will argue over the merits of a 20-thou grid vs a 25-thou grid for instance. In practice, 25 thou is often more useful as it allows you to go exactly half way between 50-thou spaced pads.
Why is a coarse snap grid so important? It's important because
it will keep your components neat and symmetrical; aesthetically pleasing, if you like. It's not just for aesthetics though - it makes future editing, dragging, movement and alignment of your tracks, components and blocks of components easier as your layout grows in size and complexity.
A bad and amateurish PC board design is instantly recognisable,
as many of the tracks will not line up exactly in the centre of pads. Little bits of tracks will be "tacked" on to fill in gaps etc. This is the result of not using a snap grid effectively.
Good PC board layout practice would involve you starting out
with a coarse grid like 50 thou and using a progressively finer snap grid if your design becomes "tight" on space. Drop to 25 thou and 10 thou for finer routing and placement when needed. This will do for 99% of boards.
Make sure the finer grid you choose is a nice even division of
your standard 100 thou. This means 50, 25, 20, 10, or 5 thou. Don't use anything else!
A good PC board package will have hotkeys or programmable macro
keys to help you switch between different snap grid sizes instantly, as you will need to do this often.
There are two types of grids in a PC board drafting package - a
snap grid as discussed and a "visible" grid. The visible grid is an optional on-screen grid of solid or dashed lines, or dots. This is displayed as a background behind your design and helps you greatly in lining up components and tracks. You can have the snap grid and visible grid set to different units (metric or imperial) and this can be helpful. Many designers prefer a 100 thou visible grid and rarely vary from that.
Some programs also have what is called an "Electrical" grid.
This grid is not visible but it makes your cursor "snap" onto the centre of electrical objects like tracks and pads, when your cursor gets close enough. This is extremely useful for manual routing, editing and moving objects.
One last type of grid is the "Component" grid. This works the
same as the snap grid but it's for component movement only. This allows you to align components up to a different grid. Make sure you make it a multiple of your Snap grid.
When you start laying out your first board, snap grids can feel
a bit "funny", with your cursor only being able to be moved in steps, unlike normal paint type packages which everyone is familiar with. But it's easy to get used to and your PC board designs will be one step closer to being neat and professional.
Working from the top
PC board design is always done looking from the top of your
board, looking down through the various layers as if they were transparent. This is how all the PC board packages work (and how all PC boards are depicted in SILICON CHIP).
The only time you will look at your board from the bottom is
for assembly or checking purposes. This "through the board" method means that you will have to become skilled at reading text, on the bottom layers, as a mirror image - get used tor it!
Tracks size & spacing
There is no recommend ed standard for track sizes. What
size tracks you use will depend on (in order of importance) the electrical requirements of the design, the routing space and clearance you have available and your own preferences. Every design will have a different set of electrical requirements which can vary between tracks on the board.
This screen grab from Protel 99 clearly shows the visible grid underneath the board pattern and component layout. The grid is set up to 25 thou - again, we are working in imperial measurement.
All but basic non-critical designs will require a mixture of track sizes. As a general rule though, the wider the tracks, the better. Wider tracks have lower DC resistance
and therefore higher current capacity, lower inductance, can be easier and cheaper for the manufacturer to etch, and are easier to inspect and rework.
The lower limit of your track width will depend on the
"track/space" resolution that your PC board manufacturer can produce. For example, a manufacturer may quote a 10/8 track/space figure. This means that tracks can be no less than 10 thou wide and the spacing between tracks (or pads or any part of the copper) can be no less than 8 thou. The figures are almost always quoted in thous, with track width first and then spacing.
Real world typical figures are 10/10 and 8/8 for basic boards.
The IPC standard recommends 4 thou as being a lower limit. Once you get to 6 thou tracks and below though, you are getting into the serious (and expensive) end of the business and you should be consulting your board manufacturer first. The lower the track/space figure, the greater care the manufacturer has to take when aligning and etching the board. They will pass this cost on to you, so make
sure that you don't go any lower than you need to. As a guide, with "home made" PC board manufacturing processes like laser printed transparencies and pre-coated photo resist boards, it is possible to easily get 10/10 and even 8/8 spacing.
Just because a manufacturer can achieve a certain track/spacing, it is no reason to "push the limits" with your design. Use as big
a track/spacing as possible unless your design parameters call for something smaller.
As a start, you may like to use 25 thou for signal tracks, 50
thou for power and ground tracks and 10-15 thou for going between IC and component pads. Some designers though like the "look" of smaller signal tracks like 10 or 15 thou, while others like all of their tracks to be big and "chunky". Good design practice is to keep tracks as big as possible and then to change to a thinner track only when required to meet clearance requirements.
Changing your track from large to small and then back to large
again is known as "necking" or "necking down". This is often required when you have to go between IC or component pads. This allows you to have nice big low impedance tracks, but still have the flexibility to route between tight spots.
In practice, your track width will be dictated by the current
flowing through it and the maximum temperature rise you are willing to tolerate. Remember that every track will have a certain amount of resistance, so the track will dissipate heat just like a resistor; the wider the track, the lower its resistance. The thickness of the copper on your PC board will also play a part, as will any solder coating finish.
The thickness of the copper on the PC board is nominally
specified in ounces per square foot, with 1oz copper being the most common. You can order other thicknesses like 0.5oz, 2oz and 4oz. The thicker copper layers are useful for high current, high reliability designs.
The calculations to figure out a required track width based on
the current and the maximum temperature rise are a little complex. They can also be quite inaccurate, as the standard is based on a set of non-linear graphs based on measured data from around half a century ago. These are still reproduced in the IPC standard.
A handy track width calculator program can be found at
www.ultracad.com/calc.htm, and gives results based on the IPC graphs.
As a rule of thumb, a 10° Celsius temperature rise in your
track is a nice safe limit to design around. A handy reference table has been included in this article to give you a list of track widths vs current for a 10°C rise. The DC resistance in milli-ohms per inch is also shown. Of course, the wider the track the better, so don't just blindly stick to the table.
Just like any conductor, tracks on a PC board have a certain resistance which must be taken into account when designing a board carrying any significant current. 1oz board is by far the most used in Australia.
Pad sizes, shapes and dimensions will depend not only on the
component you are using but also the manufacturing process used to assemble the board, among other things. There are lots of standards and theories behind pad sizes and layouts and these will be explained later. Suffice it to say at this stage that your PC board package should come with a set of basic component libraries that will get you started. For all but the simplest boards though, you'll have to modify these basic components to suit your purpose. Over time you will build up your own library of components suitable for your own requirements.
There is an important parameter known as the pad/hole ratio.
This is the ratio of the pad size to the component lead hole size in that pad. Each manufacturer will have a minimum specification for this. As a simple rule of thumb, the pad should be at least 1.8 times the diameter of the hole or at least 0.5mm larger. This is to allow for alignment tolerances on the drill and the artwork on the top and bottom layers. This ratio gets more important the smaller the pad and hole become, and is particularly relevant to vias (these
will be explained later).
There are some common practices used when it comes to generic
component pads. Pads for leaded components like resistors, capacitors and diodes should be round, with around 70 thou diameter being common. Dual In Line (DIL) components like ICs are better suited with oval shaped pads (60 thou high by 90-100 thou wide is common). Pin 1 of the chip is commonly a different pad shape, usually rectangular, with the same dimensions as the other pins.
Most surface mount components use rectangular pads (with
circular ends) and the pads should not be any wider than the component itself. Surface tension of the molten solder is an issue and if the wrong pads are used, surface tension can pull the component off line or even upright.
Other components that rely on pin numbering, like connectors
and SIP resistor packs, should also follow the "rectangular pin 1" rule.
Octagonal pads are seldom used and should generally be avoided.
As a general rule, use circular or oval pads unless you need to use
Vias connect the tracks from one side of a double-sided board
to another, by way of a hole in the board.
On all but cheap and low-end commercial prototypes, vias are
made with electrically plated holes, called "Plated Through Holes" (PTH). Plated through holes allow electrical connection between different layers on your board.
What is the difference between a via and a pad? Practically
speaking there is no real difference - both are electrically plated in the "electroless" process but vias are subsequently hidden by the solder mask. So there are differences when it comes to PC board design packages. Pads and vias are, and should be, treated differently. You can globally edit them separately and do some more advanced things to be discussed later. So don't use a pad in place of a via or vice-versa.
Holes in vias are usually a fair bit smaller than component
pads, with 0.5-0.7mm being typical (although they should be larger when they need to carry substantial current).
Using a via to connect two layers is commonly called
"stitching", as you are effectively electrically stitching both layers together, like threading a needle back and forth through material. Throw the term "stitching" a few times into a conversation and you'll really sound like a PC board professional!
"Polygons" are available on many PC board packages. A polygon
automatically fills in (or "floods") a desired area with copper, which "flows" around other pads and tracks. They are very useful for laying down ground planes. Make sure you place polygons after you have placed all of your tacks and pads.
Polygons can either be "solid" fills of copper or "hatched"
copper tracks in a criss-cross fashion. Solid fills are much preferred. Hatched fills result in much larger file sizes and are no longer needed to avoid problems with board warpage.
The Australian design rules specify minimum spacing between tracks for mains wiring (see text); for everything else these figures should be considered minimum. "Internal" means tracks inside a multi-layer board, "external" are tracks on a single-sided or double-sided board. The < and >3050m means the height above sea level at which the PC board will be used.
Electrical clearances are an important requirement for all
boards. Too tight a clearance between tracks and pads may lead to "hair-line" shorts and other etching problems during the manufacturing process. These can be very hard to find once your board is assembled. Once again, don't "push the limits" of your manufacturer unless you have to; stay above their recommended
minimum spacing, if at all possible.
At least 15 thou is a good clearance limit for basic
through-hole designs, with 10 thou or 8 thou being used for more dense surface mount layouts. If you go below this, it's a good idea to consult your PC board maker first.
For 240V mains on PC boards there are various legal requirements, and you'll need to consult the relevant standards if you are doing this sort of work. As a rule of thumb, an absolute minimum of 8mm (315 thou) spacing should be allowed between 240V tracks and isolated signal tracks. Good design practice would dictate that you would have much larger clearances than this anyway.
For non-mains voltages, the IPC standard has a set of tables
that define the clearance required for various voltages. A simplified table is shown here. The clearance will vary depending on whether the tracks are on internal layers or the external surface. They also vary with the operational height of the board above sea level, due to the thinning of the atmosphere at high altitudes. Conformal coating (a non-conductive spray often applied over the
tracks to resist moisture, corrosion, etc) also improves these figures for a given clearance. This is often used on military spec PC boards.
Phew! That's probably enough to take in for one month. Next, we
will look at component placement and design criteria, along with basic routing (or tracking), applying those "finishing touches" which make the difference between an average board and a great board - and we'll also look at the differences between single-sided boards and double sided (or multi-layer) boards. Stay tuned!