Basic PCB Layout Tutorial

The Schematic

Before you even begin to lay out your PCB, you MUST have a complete and accurate schematic diagram. Many people jump straight into the PCB design with nothing more than the circuit in their head, or the schematic drawn on loose post-it notes with no pin numbers and no order. This just isn’t good enough, if you don’t have an accurate schematic then your PCB 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, and it can apply equally well to PCB design. A PCB design is a manufactured version of your schematic, so it is natural for the PCB design to be influenced by the original schematic. If your schematic is neat, logical and clearly laid out, then it really does make your PCB design job a lot easier. Good practice will have signals flowing from inputs at the left to outputs on the right. With electrically important sections drawn correctly, the way the designer would like them to be laid out on the PCB. Like putting bypass capacitors 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 yourself when it comes to laying out the board, but they are useful for people reviewing the design.

Your schematic really should be drawn with the PCB design in mind.

It is outside the scope of this article to go into details on good schematic design, as it would require a complete article in its own right.



Imperial and Metric


The first thing to know about PCB design is what measurement units are used and their common terminologies, as they can be awfully confusing!

As any long time PCB designer will tell you, you should always use imperial units (i.e. inches) when designing PCBs. This isn’t just for the sake of nostalgia, although that is a major reason! 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 laying out of your board a lot harder and a lot easier. If you are young enough to have been raised in the metric age then you had better start learning what inches are all about and how to convert them.

An old saying for PCB design is “thou shall use thous”. A tad confusing until you know what a “thou” is.A “thou” is 1/1000th of an inch, and is universally used and recognised by PCB designers and manufacturers everywhere. So start practicing 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, and is NOT to be confused with the millimeter (mm), which is often spoken the same as “mil”. The term “mil” comes from 1 thou being equal to 1 mili inch. As a general rule avoid the use of “mil” and stick to “thou”, it’s less confusing when trying to explain PCB dimensions to those metricated non-PCB people.

Some PCB designers will tell you not to use metric millimeters for ANYTHING to do with a PCB 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” type requirements like hole sizes and board dimensions.

You will find that many PCB manufacturers will follow these basic guidelines also, for 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 counterproductive 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 will also have metric dimensions even though the spacing are designed to 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, PCB design can be confusing!

So whatever it is you have to do in PCB design you’ll need to become an expert at imperial to metric conversion, and vice-versa. To make your life easier though, all the major PCB 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 200thou. 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 inches units being assumed. This is often used for pin spacing on components.

100 thou is a basic “reference point” for all aspects of PCB design, and a vast array of common component lead spacing 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 PCB industry though. Old habits die hard, and imperial still reigns supreme in many areas of practical usage.

Working to Grids

The second major rule of PCB 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 throughhole 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 may. 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 PCB design is instantly recognisable, as many of the tracks will not line up exactly in the center 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 PCB 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 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, you’ll regret it.

A good PCB 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 PCB 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 is often very 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 center 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 PCB designs will be one step closer to being neat and professional.

Working from the top

PCB design is always done looking from the top of your board, looking through the various layers as if they were transparent. This is how all the PCB packages work. The only time you will look at your board from the bottom is for manufacturing or checking purposes. This “through the board” method means that you will have to get used to reading text on the bottom layers as a mirror image, get used to it!

Tracks

There is no recommended standard for track sizes. What size track you use will depend upon (in order of importance) the electrical requirements of the design, the routing space and clearance you have available, and your own personal preference. Every design will have a different set of electrical requirements which can vary between tracks on the board. All but basic non-critical designs will require a mixture of track sizes. As a general rule though, the bigger the track width, the better. Bigger tracks have lower DC resistance, 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 upon the “track/space” resolution that your PCB manufacturer is capable of. 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 thou’s, with track width first and then spacing.

Real world typical figures are 10/10 and 8/8 for basic boards. The IPC standard recommends 4thou as being a lower limit. Once you get to 6thou tracks and below though, you are getting into the serious 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 onto you, so make sure that you don’t go any lower than you need to. As a guide, with “home made” PCB 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 say 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 of the track you are willing to tolerate. Remember that every track will have a certain amount of resistance, sothe track will dissipate heat just like a resistor. The wider the track the lower the resistance. The thickness of the copper on your PCB will also play a part, as will any solder coating finish.

The thickness of the copper on the PCB 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 10degC 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 10degC rise. The DC resistance in milli ohms per inch is also shown. Of course, the bigger the track the better, so don’t just blindly stick to the table.


next part...