and set a few defaults. I hate the yellow background to the
menus so I always do:
Left-click or press enter to cycle through the available
This doesn't take long as there are only 16 of them.
the grid dots to 100mil pitch:
and type in 100 (if it isn't already) and hit return.
going to do a single layer board so we can switch off the unwanted
Setup->Toggle Layers and
left-click (or return) to turn on and off. We want the Bottom Layer, the Top Overlay, the Board Layer and the Multilayer turned
on. Escape or right-click to exit.
first six layers are the six available layers for multilayer boards.
If you want more layers, tough.
and Bottom Overlay
are the silk-screen legends for the top and bottom sides of the board.
and Power Plane
are for the copper sheet layers. These are negative layers in
that what you draw on the screen is removed from the copper.
You'll see what I mean later on.
Board Layer is for
the drawing of outlines and other useful drafting stuff. Keep Out Layer is
for the autorouter to avoid.
Multilayer is for
pads that are repeated through the whole board on all six copper layers.
up your library file. We can use the default but if you have
moved it, then you will have to type in the directory path to where you
put it for Autotrax
to find it. In my case, I type E:\autotrax\library\
the 'return' and it will list the .LIB
files it finds. Which is one so select it.
This doesn't always seem to work correctly in VirtualBox Windows 2000.
Sometimes, it just gives a NO FILES FOUND IN DIRECTORY message. There
are files and you can access them but you have to specifically type in
the name of the library you want. DOS-style
typing-it-all-out-and-not-making-mistakes-else-we-have-to-type-it-all-over-again. I don't know why it does this.
For example: C:\AUTOTRAX\LIBRARY\MYLIBS\MYLIB1 (with or without the .LIB at the end).
have tinkered with the number of files in the directory and with trying
to delete some of the big ones. It might be one library file it
objects to. I god down to about five library files and it worked
but which didn't really answer the problem.
you type Library-List, it will give a
list of components it finds. Library->Browse, it will
allow you to inspect them. After escaping from Browse, it will
remember the last component you looked at ready to place one.
the track width the 10 mil by Current->Track and typing in
10 followed by return.
first draw the outline. Press + or - to toggle through
the layers until you get to the Board
and move to 1000, 1000. Click to start. Move to
and click again, move to 3000, 2500 and click again, 1000,
click then 1000, 1000 click, right-click, right-click.
can experiment with Move-Track, Drag->Track, Delete->Track and Undelete.
to place the components. Start with the resistors.
Select Place->Component and choose
to get a wire-ended resistors with a 400mil pad pitch. Fill
the Reference and Value fields and place it somewhere handy.
Continue with the resistors until all eight are placed.
don't like the available capacitors so let's draw one and make a
library component from it.
Current->Pad to select a
suitable pad size from the table. 70 mil is reasonable at
this stage. Place two pads 200 mils apart and draw a box
round them as shown in the picture. Use Edit->Pad to change the
designator for both pads. The designators need to match what
has been used in the netlist. I will later change all the pad
sizes to 70 mil and all the holes to 32 mil (0.8mm) because that's what
I do. You don't have to but it is sensible to reduce the
number of tool sizes for the drilling operation.
I start saving components to libraries all over the place, I'm going to
create a new library so I don't foul up my old one. Use Library->New and give it a
snappy name in the chosen location. You will need to type it
in as it doesn't like shorthand relative paths like .\Library\
created your new library, you need to select it by using Library->File.
Backspace until just the path remains with the trailing
backslash (i.e. E:\AUTOTRAX\LIBRARY\) and hitting return will bring up
the two libraries you now have. If there's only one, you've
stored your new one somewhere else.
then need to do Block->Define and draw a
box around all the bits you've drawn that you want to be retained in
your component. Select a reference point. This is
personal preference but the middle is usually handy.
use Library->Add to add it.
Give it a sensible name.
you have your new component, you can use it. If you have
finished with the drafting, use Block->Inside
to get rid of it. Place your new components like you did with
the resistors. I don't like my outline above so I made new
ones for the connector, the transistors and MOSFET and the tantalum
them all on the board and then select Netlist->Get Nets, type in
the location of your netlist and then select Shortest Path etc
etc to get it fully loaded. Then select Netlist->Show Nets->All to get it in the
what's wrong with this???
pads on the capacitors and transistors are connected up wrong.
This is because the pads on the PCB don't agree correctly
with the pins on the schematic. Let's put it right.
Edit your pads until they do. Start with the MOSFET
as it has its pads identified on the schematic. That is, the
drain is pin 2, gate is pin 1 and source is pin 3. Similarly
with the transistors: collector is pin 3, emitter is pin 2 and base is
pin 1. The capacitors have pin 1 is negative and pin 2 is
will notice that this is all a pain in the arse
and really error-prone. It is a good idea to stick with your
own choice of library models that agree between the schematic and the
PCB editor. I have changed this manually but it could easily
go wrong if I were dealing with a complex board where all my capacitors
were in the wrong way round and all the transistors had their legs
crossed. Autotrax will allow you up to four
letters/characters for the designator. If you use +VE, -VE,
COLL, BASE, EMIT, SRC, ANOD etc. etc then your netlist will be easier
to read and if your schematic outlines use the same, there is far less
chance of getting a mistake creep in.
Also, be consistent. If you use E, B and C on one outline, don't use BASE, COLL, EMIT on another.
Computers: garbage in,
will need to re-load the netlist to get the displayed net correct.
have also turned off the display of the component values by using Edit->Component->(select
component)->Comment->Hide->Hide followed by Yes to the global
request. I have also used Move->String to move all
the designators within the component for convenience and to reduce
clutter at this stage. I've done this with the snap grid set to 5 mil.