Navigation Panel

Protel Autotrax
What is Autotrax?
What is the Purpose of this Site?
Installation - Tasks 1 and 2
Installation - Tasks 3 and 4
Installation - Task 5
Installation - Task 6
How it Works
The Resizing Problem

Let's Design a Circuit
Now Draw It
Place Components
Adding the Tracks

Aston Home

Place the Components

Fire up Autotrax and set a few defaults.  I hate the yellow background to the menus so I always do:

Setup->Menu Colors->Background.  Left-click or press enter to cycle through the available colours.  This doesn't take long as there are only 16 of them.  I like white.

Set the grid dots to 100mil pitch:

Grid->Visible Grid  and type in 100 (if it isn't already) and hit return.

We're going to do a single layer board so we can switch off the unwanted layers.  Do:

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.

The first six layers are the six available layers for multilayer boards.  If you want more layers, tough.

The Top Overlay and Bottom Overlay are the silk-screen legends for the top and bottom sides of the board.

The Ground Plane 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.

Set 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.  

Update: 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).

I 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.

If 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.

Set the track width the 10 mil by Current->Track and typing in 10 followed by return.

Draw the Outline

We first draw the outline.  Press + or - to toggle through the layers until you get to the Board Layer.

Select Place->Track and move to 1000, 1000.  Click to start.  Move to 3000, 1000 and click again, move to 3000, 2500 and click again,  1000, 2500, click then 1000, 1000 click, right-click, right-click.  

You can experiment with Move-Track, Drag->Track, Delete->Track and Undelete.

Picture of the circuit bounding box so far.

Now to place the components.  Start with the resistors.  Select Place->Component and choose AXIAL0.4 to get a wire-ended resistors with a 400mil pad pitch.  Fill in the Reference and Value fields and place it somewhere handy.  Continue with the resistors until all eight are placed.

Board with resistors placed.

I don't like the available capacitors so let's draw one and make a library component from it.

Creating a new component

Use 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.

Before 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\

New Library

Having 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.

You 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.

Block define

Then use Library->Add to add it.  Give it a sensible name.

Now you have your new component, you can use it.  If you have finished with the drafting, use Block->Inside Delete->All Layers->Yes 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 capacitors.

Place 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 screen.

And what's wrong with this???

The 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 positive.

You 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, garbage out.

You will need to re-load the netlist to get the displayed net correct.

I 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.