|
| |
|
|
|
|
|
|
32/64 Bit
|
over 80,000 users worldwide
|
|
|
 |
| |
|
|
|
| |
|
Do you want to easily create your own schematics and PCBs at an
affordable price, and have fun doing it.?
|
|
AutoTRAX EDA and its successor AutoTRAX Design Express (DEX) are powerful integrated
Electronic Design Suites for Electronic Engineers. They have all the features you
expect and need to rapidly and easily take your design from conception through to
production. Its in-built hierarchical project manager lets you perform both top-down
and bottom-up design and reuse design components and sub-systems. Schematic capture
and pcb layout has never been easier.
|
|
Now Playing
View Over 60 Tutorial Videos...
|
Starting with its easy to use schematic capture, you
can drag pre-created parts onto your design sheets and rapidly and reliably connect
the terminals together using wires, buses and off-page connectors.
AutoTRAX ensures that your design remains correct throughout with no ‘dangling wires’
or pcb design rule violations.
You can also create your own parts either in-place on your design sheets or using
the integrated Part Creator. Again, design integrity
is maintained throughout using AutoTRAX’s design rule checker.
Once you have created your schematic capture design you can rapidly simulate its
analog performance using the built-in virtual instruments such as oscilloscopes
and signal generators. Multiple analyses can be produced using the industry standard
SPICE 3f5 simulator that comes free with AutoTRAX.
When you are satisfied with your design and simulation results, you can then quickly
proceed to produce your finished and populated PCB board without leaving the AutoTRAX
program. The AutoTRAX PCB Designer will take your hierarchical
design and place the components, with or without your assistance. Next AutoTRAX
can either autoroute your board or you can use a combination
of automatic and manual routing to quickly and reliably complete all electrical
wiring. The design of AutoTRAX’s internal data ensures you maintain full electrical
integrity with your schematic design.
No surprises with lost or missing PCB tracks or wires, or those ‘extra’ wires.
Now that you have your design finished and routed you can then produce all Computer Aided Manufacturing files you will need to
produce the board, drill the holes, cut its profile, order parts using the Bill
Of Materials, and place your parts using the pick and place files. These files can
be placed together and forwarded to your favorite board manufacturers, electronically
via email.
In only a short time you will see the fruits of your labor and will be pleased at
the time and money you have saved.
The best way for you
to fully appreciate the power and simplicity of AutoTRAX is to see it at first hand.
I am so confident that you will be impressed by what you see. So, why wait? download
the full version of AutoTRAX schematic and pcb software and take it for a test drive.
The AutoTRAX Lite version is free (freeware) and is available to do pcb layout and
create printed circuit boards with its built-in autorouter, 3D visualization.
'Thanks so much for your steadfast support. DEX has a beautiful GUI, by the way!'
Roger Blair - Fremont, California
'I like the product and for the price, that is why I have supported it over the
years.' Craig Caraway - Henderson, Nevada
'Thanks for your help …. now that’s what I call Outstanding Support!!! Major corporations
could learn a lot from you!' Mike Lozano - Lockhart, Texas
|
|
|
| |
|
|
|
I want to express my apprciation to you for allowing us to use
your fine product to teach printed circuit board design. Many of my students learned
to use it well and will specify it when they begin working. I know of one who already
has. The product keeps getting beter and better.
Professor Robert A. Summers, PhD, Computer and Electronics Engineering
Technology, Weber State University Ogden, Utah.
|
|
|
|
| |
|
AutoTRAX EDA Download
Version 9.83
32 and 64 bit.
30th. August, 2010
Please fill in the form below to download a copy of the AutoTRAX EDA program.
This is the full version and is limited to 100 pins and non-profit use if you do
not have a valid license.
|
Please enter your email address
|
|
|
|
You will receive a password by email. The install program is password protected
(Only Windows XP, Vista and Windows
7 are supported).
Please keep up the work on AutoTrax. Each time I download
an upgrade I notice something is easier, faster, more intuitive etc.
Steve Armitstead, Poulton-le-Fylde
|
|
|
|
| |
|
|
|
|
|
|
AutoTRAX EDA/DEX ecad/cad schematic capture software, spice simulation and PCB design
software is copyright © 2010 Ilija Kovačević
|
|
|
Introduction
You've designed your circuit, perhaps even bread boarded a working prototype,
and now it's time to turn it into a nice Printed Circuit Board (PCB) design.
For some designers, the PCB design will be a natural and easy extension of the design
process. But for many others the process of designing and laying out a PCB can be
a very daunting task. There are even very experienced circuit designers who know
very little about PCB design, and as such leave it up to the "expert"
specialist PCB designers. Many companies even have their own dedicated PCB design
departments. This is not surprising, considering that it often takes a great deal
of knowledge and talent to position 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 PCB design is very often an integral part of
a design. In many designs (high speed digital, low level analog and RF to name a
few) the PCB layout may make or break the operation and electrical performance of
the design. It must be remembered that PCB traces have resistance, inductance, and
capacitance, just like your circuit does.
This article is presented to hopefully take some of the mystery out of PCB design.
It gives some advice and “rules of thumb” on how to design and lay out your PCBs
in a professional manner. It is, however, quite difficult to try and “teach” PCB
design. There are many basic rules and good practices to follow, but apart from
that PCB design is a highly creative and individual process. It is like trying to
teach someone how to paint a picture. Everyone will have their own unique style,
while some people may have no creative flair at all!
Indeed, many PCB designers like to think of PCB 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.
Lets have a go shall we...
The Old Days
Back in the pre-computer CAD days, PCBs were designed and laid out by hand using
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
not so fond memories. Those days are well and truly gone, with computer based PCB
design having replaced this method completely in both hobbyist and professional
electronics. Computer based CAD programs allow the utmost in flexibility in board
design and editing over the traditional techniques. What used to take hours can
now be done in seconds.
PCB Packages
There are many PCB 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 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 also 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 PCB
package available. There is however, one distinct exception. Using a PCB only package,
which does not have schematic capability, greatly limits what you can do with the
package in the professional sense. Many of the more advanced techniques to be described
later require access to a compatible schematic editor program. This will be explained
when required.
Standards
There are industry standards for almost every aspect of PCB 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 PCB design, manufacture, testing, and anything else that you
could ever need. The major document that covers PCB 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 PCB 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 PCB for this article.
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 messier. 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, so the 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.
Pads
Pad sizes, shapes and dimensions will depend not only upon the component you are
using, but also the manufacturing process used to assemble the board, among other
things. There are a whole slew of standards and theories behind pad sizes and layouts,
and this will be explained later. Suffice it to say at this stage that your PCB
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 various requirements. There is an important parameter known as the
pad/hole ratio. This is the ratio of the pad size to the hole size. Each manufacturer
will have their own 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 top and
bottom layers. This ratio gets more important the smaller the pad and hole become,
and is particularly relevant to vias. 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 IC’s are better suited with oval shaped pads (60 thou high
by 90-100 thou wide is common). Pin 1 of the chip sould always be a different pad
shape, usually rectangular, and with the same dimensions as the other pins. Most
surface mount components use rectangular pads, although surface mount SO package
ICs should use oval pads. Again, with pin 1 being rectangular. 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 rectangular.
Vias
Vias connect the tracks from one side of your board to another, by way of a hole
in your board. On all but cheap home made 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, they are both just electrically plated holes. But there are differences
when it comes to PCB 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, and vice-versa. Holes
in vias are usually a fair bit smaller than component pads, with 0.5-0.7mm being
typical. 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 PCB professional!
Polygons
“Polygons” are available on many PCB 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. Polygon can either be “solid”
fills of copper, or “hatched” copper tracks in a crisscross fashion. Solid fills
are preferred, hatched fills are basically a thing of the past.
Clearances
Electrical clearances are an important requirement for all boards. Too tight a clearance
between tracks and pads may lead to “hairline” shorts and other etching problems
during the manufacturing process. These can be very hard to fault 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 with your PCB manufacturer first.
For 240V mains on PCB’s 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 an 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 also improves
these figures for a given clearance, and this is often used on military spec PCBs.
Component Placement & Design
An old saying is that PCB design is 90% placement and 10% routing. Whilst 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. It may even make your board unmanufacturable. So there is
a lot to think about when placing components!
Every designer will have their own method of placing components, and if you gave
the same circuit (no matter how simple) to 100 different experienced designers you’d
get a 100 different PCB layouts every time. So there is no absolute right way to
place your components. 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.
|
|
|
|