Languguage OS 2/Languguage OS II Version 10-94 (Knowledge Media)(1994).ISO/language/embedded/specinse/easyfree.exe/READ.ME

Text File | 1992-05-21 | 60KB | 1,647 lines

Protel Easytrax (DOS)
Freeware version 2.06
Reference Manual Text File - Read.me


Note: This text file is derived from the original Protel Easytrax
reference manual. The file is approximately 35 A4 pages long.
We suggest that you make a hardcopy for reference when
using the Easytrax demo.


Copyright Notice
This ôfreewareö demonstration software (including this textfile) may be
copied and passed on to others for non-commercial use,
provided the notice of copyright shown below is placed on
the label of the copied disk and that no alterations or changes are made to
the software, this textfile or Copyright notice, below.

All other rights are reserved.


Software Copyright (c)1988 Protel Technology Pty. Ltd.
Original Reference Manual Copyright (c)1988 Protel Technology Pty. Ltd.
READ.ME Copyright (c) 1992,  Protel Technology Inc.

Please read the following disclaimer of liability before using the software.
If you do not accept fully the terms and conditions of use described below,
do not use the software.

THIS FREEWARE VERSION OF PROTEL EASYTRAX IS SUPPLIED
WITHOUT WARRANTY OF ANY KIND INCLUDING , BUT NOT
LIMITED TO ANY IMPLIED WARRANTIES OF
MERCHANTABILITY OR FITNESS FOR ANY PURPOSE.

UNDER NO CIRCUMSTANCES SHALL PROTEL TECHNOLOGY
NOR ITS AGENTS, HEIRS OR SUCCESSORS BE LIABLE FOR
ANY DAMAGES, INCLUDING CONSEQUENTIAL, INCIDENTAL
OR SPECIAL DAMAGES ARISING DIRECTLY OR INDIRECTLY
FROM ITS USE.

Protel and the Protel logo are registered trademarks of
Protel Technology Pty. Ltd. Easytrax is a trademark
of Protel Technology Pty. Ltd.

Epson FX-80 is a registered trademark of Epson America, Inc.
Hercules is a trademark of Hercules Computer Technology.
IBM is a registered trademark of International Business
Machines Corporation.
Microsoft is a registered trademark of Microsoft
Corporation.
MS-DOS is a registered trademark of Microsoft Corporation.


Contents

Introduction

Installation instructions

Tutorial section
1  Tutorial: Getting started
   Loading the demonstration board
   Using the menus
   Identifying items on the board
   Getting information about the board
   Jumping to components and pins
   Some special keys
   Speeding up menu selections
   Quitting from the program

2  Tutorial: Laying out a PCB
   Getting started
   Placing components
   Laying tracks
   Connecting to power and ground planes

3 Tutorial: Plotting a board
   Starting the program
   Loading the DEMO file
   Overview of plotting a board
   Setting the serial port parameters
   Choosing the plot type
   Loading the plotter driver
   Setting the pen parameters
   Plotting the board

4  Tutorial: Gerber plots
   Setting up a Gerber plot
   Creating the Gerber file
   Plotting the pad master


Options Summary



INTRODUCTION

This demo software is not copy protected and we encourage you to
pass it onto other interested people. Please feel free to make
copies of the disk. All we ask is that our copyright notice is
diplayed on the disk label.

Protel Easytrax is a low-cost, yet powerful, software
package for producing printed circuit board (PCB) artwork.
It is a fully-featured system which runs on the IBM-PC/XT/AT
and PS/2 series and close compatibles.

The package has many advanced features including
component library support and comprehensive plotting facilities.


This text file describes how you can quickly and easily explore
the powerful features of the accompanying Protel Easytrax
demonstration software. Easy to learn and easy to use, Easytrax
puts professional-quality PCB layout tools in the hands of
students, hobbyists and part-time designers. Easytrax is the
introductory-level member of the Protel family of Electronics
Design Automation packages.

If you decide to purchase Easytrax, you can do so in confidence
that your workfiles will be fully transferable to Protel
Autotrax, our full-featured design package that features powerful
automatic component loading and autorouting capabilities.
Autotrax accepts a schematic netlist from Protel Schematic and
similar packages, and is available as an upgrade to registered
Easytrax users.

Protel Easytrax provides everything you'll need to design
through-hole, multi-layer PCBs.

In less than an hour you could be designing your own printed
circuit board following the steps outlined in the first
two tutorials. You can also explore the powerful plotting
routines by plotting the DEMO board supplied with the
package on either a standard pen and ink plotter, a laser
printer or a Gerber(rtm) format photoplotter.

You have access to all the features of the full package with
the exception of saving PCB files to the disk. You can,
however, save plotting files generated from the demo board file. The
full Easytrax package also supports Excellon(tm) format numeric
controlled drill files.

When you receive your full version of Protel Easytrax, you
also receive a comprehensive reference manual. It contains many
more tutorials than this demonstration text file, a detailed
explanation of every menu option, as well as a comprehensive
index.

A note about performance:
Protel Easytrax works on the complete range of IBM PC/XT/AT
and PS/2 microcomputers and compatibles. The Easytrax demo can
only be installed on a hard disk. The full program can be run
from floppies but will run twice as fast from a hard disk.

This demo is delivered with a number of graphics drivers that
support CGA, Hercules, EGA, Vega Deluxe, and VGA standard cards
with resolutions of up to 1024x768 and 16 colors. If no graphics
driver is installed the demo will operate using CGA graphics. See
the next section for installation instructions.


Installation instructions

The Easytrax demo software is archived so that it will fit on
one 1.2Mb floppy disk (or two 360K floppies). To install the
software on your hard disk please follow these steps:

     1. Insert the demo disk in drive A: and type A:INSTALL at
        the C:\> prompt and press ENTER.

     2. The installation is in three parts. The first screen
        prompts you to install the Easyedit (PCB editor) files.
        Press ENTER twice to accept the source and target drives.
        You will then be prompted to specify a directory on your
        hard disk. The default is \EASYEDIT. We suggest that you
        install all the demo files into a single directory called
        \PROTEL. Type \PROTEL for the directory option.

    3. You are then prompted to accept or change the previous
        selections. Unless you have made a mistake press Y to
        accept the previous selections.

    4. The second stage of the installation is the copying of
        the Easyplot (PCB plot program) files. Repeat steps 2 & 3
        above.Make sure that you specify \PROTEL as the target
        directory.

    5. Finally the graphics (video card) drivers are installed.
        Again repeat steps 2 & 3 above making sure that you
        specify \PROTEL as the target directory on drive C:.
        Once all the graphics drivers are copied onto the hard
        disk a selection screen appears from which you should
        select the driver that suits your graphics card. If your
        card is not listed, or you are not sure what type it is,
        select the EGA option.

    6. Installation is now complete and you are ready to run the
        Easytrax program.



1 Tutorial: Getting started

This tutorial has been designed to give you a quick overview
of the features of Protel Easytrax. Within minutes you will
be gaining an insight into the way the program can be used
to design printed circuit boards.

If you need some help in setting up your computer to run the
program, or if you are a newcomer to computing you may need
to read Appendix A and Appendix B (near the end of this file)
carefully before proceeding.

If, however, you are ready to begin, simply insert the
demonstration disk into drive A: and start exploring the
power of Protel Easytrax.

In this tutorial you will learn the following skills:

  Starting the Protel Easytrax program;
  Loading the DEMO file;
  Using the pop-up menus;
  Expanding and contracting the display;
  Identifying items on the board;
  Using the cursor keys and the mouse;
  Using the cursor keys with the SHIFT key;
  Getting information about the board;
  Locating components, tracks, vias and pads;
  Changing setup options;
  Quitting from Protel Easytrax.


Starting the Protel Easytrax program

Change to the \PROTEL directory on the hard drive C: and

  Type: EASYEDIT and then press ENTER.

The banner screen appears. Press any key to move to the next
screen. A window opens in the top left-hand corner of the
screen. This is a standard input window which you see many
times while using Protel Easytrax.

Type DEMO and then either press the ENTER key or click the
LEFT MOUSE button. (Note: If, at this stage you do not
want to load a file, you can press ESC or click the RIGHT
MOUSE button to bypass the loading option.) The message:

  LOADING FILE. PLEASE WAIT.

appears, then a PCB file, showing a simple Z80 microcomputer
layout is displayed.

Notice the status line at the bottom of the screen which
gives important information about the board and the position
of the cursor. If you press the cursor keys a few times the
numbers which indicate the position of the cursor change.

The X and Y values are given relative to the position of the
`origin' which always has an X value of 0 and a Y value of
0. It is written as X: 0 Y: 0. If you have not changed the
position of the origin, it is in the bottom left hand corner
of the board.

To reach a position given by X: 500 Y:1000 when the cursor
is at the origin, you move the cursor 500 mils to the right
then 1000 mils upwards.

Notice that all measurements are given in either mils or
inches. A mil is one thousandth of an inch.

Next to the cursor position on the status line is the
currently selected layer. In Protel Easytrax, tracks can be
placed on a number of layers. These include the Top Layer,
the Bottom Layer and four Mid Layers. Components are placed
on the Top Layer and silk screening is usually reserved for the
Overlay. You can switch between these layers using the keys
described at the end of this tutorial. Component pads, free pads
and vias (through-holes) occupy ALL layers except for the Top
Overlay.

The line below the status line is used to display important
messages. This line will display a prompt when some user action is
required. This line is referred to as the prompt line in these notes.


Using the menus

Press the ENTER key or the click the LEFT MOUSE button
and the MAIN MENU window (shown below) appears.

One of the options in the menu is highlighted. This
highlight is called the Selection Bar. The bar can be moved
with the mouse or the UP and DOWN cursor keys. You can
`activate' or `select' a highlighted option by clicking the
LEFT MOUSE button or by pressing the ENTER key.

The demo circuit is too small to work with easily, so it
needs to be expanded. Choose Zoom from the MAIN MENU.
Remember to make sure that it is highlighted, then click the
LEFT MOUSE button or press the ENTER key to select the
option.

Select the Expand option. The screen is redrawn and the
diagram shown in more detail. Select Zoom/Expand once again.


Identifying items on the board

Now move the mouse until the cursor is at X:1075 Y:3525. If
you are not using a mouse, use the cursor keys. If you hold
the SHIFT key down while pressing a cursor key on the
numeric keypad, the cursor will move faster.

As the cursor moves towards the position specified, notice
that the screen may be redrawn once or twice. Remember that
the cursor position is displayed on the status line.

At X:1075 Y:3525 the cursor is at the junction of two
tracks. These are the conductive lines which are usually
placed on the top and bottom board layers. Thin tracks (e.g.
12 mils) are used for normal signals and thick tracks (e.g.
30 mils) can be used for the power supply.

The horizontal track to the left has been laid on the bottom
layer. The vertical track below the cursor is on the top
layer. They are connected by a `via' which is a plated hole
passing through the board which connects the tracks.

Just to the left of the cursor is the outline of a
component. It is a 14 pin chip. Notice at the top right of
the chip there is a component designator U11 and a
description showing that it is a 1488 chip.

The component designator or reference designator usually
consists of a letter indicating the type of component (e.g.
U for an integrated circuit chip, C for a capacitor, R for a
resistor and so on), followed by a number. If you are placing a
number of identical components, once you have provided a reference
designator for the first component eg. U1, subsequent components
will be automatically designated U2, U3 etc, unless you manually
enter a new designator.

Notice that the component has 13 circular `pads' and one
square `pad' The square pad is used to signify pin 1 on the
chip. The pads are the place where the connection is made
between the pins of the component and the tracks.


Getting information about the board

As the cursor moves towards the bottom left hand corner,
notice that the screen may be redrawn once or twice.
Remember that the cursor position is displayed on the status
line.

Select the MAIN MENU, then select Information. Choose the
Status option from the Information window. Notice that
information is provided about the number of components,
pads, holes, arcs, fills, strings, tracks and vias. You will
also notice that information is provided about the name of
the current work file, the current path to the directory
where the work files are stored and the name of the
currently selected library. You can also check the amount of
disk space and system memory that is available.

  Click RIGHT MOUSE or press ESC to exit from the Status
  window.

Now choose Information/Board Dimensions. This window
displays the dimensions of the board. Exit from this window
and then choose Information/Components to see a list of the
library components which have been placed on the board.
Remember, click either mouse button or press the ENTER or
ESC key to exit from each of these options.
You can find more information about a particular component
by using the Edit menu. Choose Edit and then choose
Component. The message on the prompt line (just below the
status line) prompts you to select a component. Move the
cursor until it is positioned on the Z80 chip marked U5
(approximately X:1200 Y:1200).

Now click LEFT MOUSE or press ENTER and a window opens
showing the component designator, the library name
(pattern), a comment and information about the layer and
placement type.

Click RIGHT MOUSE or press ESC to remove the window.
Notice that the:

  SELECT COMPONENT

prompt still appears on the prompt line. Click the RIGHT
MOUSE button or press ESC again to exit from the Edit
option.


Jumping to components and pins

Now choose the Jump option from the MAIN MENU. You can
choose to jump to a place on the board by specifying a
component, a location, a net, the origin, a pad or a string.

This option will be extremely useful in the future when you
are working with a large board.

The Jump option is also useful if you want to identify the
pin numbers for a component. Choose Jump/Component and you
are asked to select a component. Notice that there is a
question mark (?) on the left hand side of the window. This
indicates that there is an information window available
which will provide a list of components held in the memory
of the computer.

Click LEFT MOUSE and the window with a range of choices
appears. Move the selection bar to highlight J2 (a DB9
connector), then press ENTER or click LEFT MOUSE.

The cursor moves to that component on the board and is
situated at pin 1. Now choose Jump/Pad. You will be asked to
select a component. Since the cursor is already over the
required component, press ENTER or click LEFT MOUSE. A
window opens at the top of the screen prompting you to enter
a pin number.

Enter a pin number such as 5 then press ENTER or click
LEFT MOUSE. Notice that the cursor moves to that pin. The
window stays open allowing you to try other pin numbers.
Press RIGHT MOUSE or ESC to exit from this window.

Now choose the Setup option from the MAIN MENU. This menu
allows you to change layer colors, menu colors, the default
pad type and many other factors which affect the layout. Try
changing the menu background color by choosing Menu Color
then clicking LEFT MOUSE or pressing ENTER and observing
the changes in color. Press ESC or click RIGHT MOUSE
when you have finished selecting colors.

By now you should be familiar with the menu structure of
Protel Easytrax and some of the features of board layout. No
attempt has been made to place components or tracks or to
change layers. This will be done in subsequent tutorials.


Some special keys

There are some other keys which have a special function in
the Protel Easytrax program. These are explained below:

  END   Redraws or `refreshes' the screen.
  HOME  Centers the screen about the current cursor
        position.
  PGUP  This key has the same effect as choosing Zoom
        Expand.
  PGDN  This key has the same effect as choosing Zoom
        Contract.
  *     This key is on the right of the keypad. Sometimes
        it also has PRTSC on the same key. It is used to swap
        between the currently selected signal layers.
        The effect can be observed on the status line.
  -     This key is also on the keypad. It is used to
        cycle through all the currently selected layers.
  +     This key is also on the keypad. It is used to
        cycle through the currently selected layers in the
        opposite direction to the - key.


Speeding up menu selections

Before finishing this tutorial you should be aware of a
feature of Protel Easytrax which helps speed up menu
selections once you become familiar with the menu structure.

Each menu option can be chosen by simply pressing the first
key of the option to be selected. Thus to choose Jump Pad
you only need to type J then P.

Quitting from the program
It is important to know how to get out of the program at
this stage. Select the File option and then select Quit or
just type F then Q. A window opens which asks you to
confirm that you want to quit to DOS.
Choose the Yes option and you are returned to the DOS
prompt.


2 Tutorial: Laying out a PCB

In this tutorial the most important aspects of placing
components, using the library, laying tracks and using the
powerful router will be covered.

The tutorial will lead you through the set of steps
necessary to begin designing an RS-232 splitter board. As
there is insufficient space in the text file to describe laying
out the whole board, you will simply place a DB25 connector
and the first of the 16 pin chips as well as some by-pass
capacitors and a resistor.

In this tutorial you will learn the following skills:

  clearing the work space;
  choosing a component from the library;
  placing a component;
  rotating a component;
  assigning component designators and comments;
  identifying pins on components;
  placing tracks manually;
  switching layers;
  using the pad to pad router.


Getting started

The aim of this tutorial is to lay out the section of an RS-
232 splitter board.

There is one DB25RA/F connector, one DIP16 chip, three
capacitors and one resistor on the board. Your first task is
to place these.
You must first make sure that the board is clear. Either
restart the Protel Easytrax program or choose File Clear
Yes. If you start the program again, press ESC or click
the RIGHT MOUSE button in response to the prompt `LOAD PCB
FILE NAME'.


Placing components

Now press PGUP three times then choose Place Component. An
input window with the heading `NAME IN LIBRARY' opens asking
for the name of a pre-defined component. Notice that there
is a question mark on the input line. Press ENTER or click
the LEFT MOUSE button and a list of the components in the
library is displayed.

If you know the name of the component then you could have
simply typed it when the input window opened. In this case
you would have entered the name DB25RA/F and pressed
ENTER
or clicked LEFT MOUSE.

For the purposes of this tutorial, however, select the
component from the library list.

Move the selection bar to the component named DB25RA/F.
Press ENTER or click the LEFT MOUSE button. A window
opens and you are prompted to supply a component designator.

A component designator is usually a letter such as U, J, C,
or R followed by a one or two digit number. Connectors are
often given designators starting with J, so enter J1 in this
case, then press ENTER or click LEFT MOUSE.

You are now prompted to enter a short comment which appears
on the component overlay. Type in DB25RA/F and an outline of
the component appears.

You now see the message:

  MOVING COMPONENT

on the prompt line at the bottom of the screen.

This means that you can now adjust the position of the
component. Press SPACE to rotate the component through 90
degrees, then move the white outline (with the cursor keys
or the mouse) close to the edge of the board - but not so
close that you cannot see the whole component. Try X:500
Y:2500 for example. When the outline is in the correct
position, press ENTER or click LEFT MOUSE and the
component is placed.

The next step is to place a 16-pin chip near the J1
connector. At this stage you are still in Place Component
and the input window has the component name DB25RA/F in it,
since that was the last component chosen. Enter a question
mark and the string DB25RA/F disappears. Press ENTER or
click the LEFT MOUSE button and the information window
opens. Choose the component labelled DIP16 then press
ENTER or click LEFT MOUSE. Enter the designator U1 and
the comment DIP16. Press ENTER or click LEFT MOUSE after
each entry. The outline of the component now appears. Use
the cursor keys or the mouse to move it to X:1900 Y:2200.
Once again, press ENTER or click LEFT MOUSE to fix the
component in place.

Now you need to place three capacitors. The component you
require this time is called RAD0.2. Enter a ? in the input
window. It is not listed in the information window so press
the PGDN key to see the next screen full of names. Choose
RAD0.2 and supply the designator C1 and the comment 22uF.
Press ENTER or click LEFT MOUSE to enter each of these
items. Press SPACE to rotate the outline through 90
degrees, then move it to X:1350 Y:2250. Press ENTER or
click LEFT MOUSE to place it.

The input window is still showing the name RAD0.2 so simply
press ENTER or click LEFT MOUSE to choose that name for
the second capacitor. The designator automatically becomes
C2 and the comment is still 22uF. Rotate the second
capacitor and place it on the other side of the DIP16 chip
at X:2800 Y:2250. Now choose RAD0.2 a third time. Rotate it
and move it to X:1350 Y:1150. Click LEFT MOUSE or press
ENTER to fix it in position.
Click RIGHT MOUSE or press ESCAPE to exit from the Place
Component option.
Now move to a point just above C3 (say, X:1250 Y:1550) and
select Place/Component from the menu. Choose the component
labelled AXIAL0.3. Assign the designator R1 and the
comment 3.3K. Press ENTER to fix the component in position.
Press ESC or click RIGHT MOUSE to exit from the
Place/Component option.

The display might be a bit messy by now so press the END
key to redraw the screen.


Laying tracks

Now you are almost ready to start laying tracks. Before you
can, you need to know the pin numbers of the components. In
the previous tutorial you learned how to identify pin
numbers using Jump Pad. Use this option to find pin 1 on J1,
U1, R1 and C1. From this information you can work out most
of the others. It might also be necessary to locate pin 25
on J1 and pin 16 on U1.

The following table provides a list of the pins which must
be connected.

   U1-1  to C1-2    U1-3  to C1-1
   U1-16 to C3-1    U1-12 to J1-2
   U1-11 to J1-3    U1-10 to J1-5
   U1-9  to J1-4    U1-5  to C2-1
   U1-4  to C2-2    U1-2  to C3-2 to R1-2
   J1-20 to R1-1

The first entry in the table indicates that you must connect
pin 1 on the component U1 to pin 2 on the component C1. The
entry under it shows that you must connect pin 16 on the
component U1 to pin 1 on the component C3.

This information becomes important later as it is the basis
of the concept of a Netlist. A netlist is a list of all
connections on the board. Easytrax allows you to generate a netlist
once all connections have been established. When printed out, this
netlist can be compared with a schematic to verify that all
connections have been completed per the drawing. Each group of
connections in a netlist (e.g. U1-1 to C1-2) is called a
Net.

Try connecting some pads. Press the * key on the
keypad to change from the component side (top layer) to the
solder side (bottom layer). On the status line the layer
indicator message changes from `L: Top Layer' to `L: Bottom
Layer'. Choose Place/Track and the message:

  SELECT TRACK START POINT

appears on the prompt line at the bottom of the screen. Move
the cursor to pin 1 on U1 (it is a square pad) - you are
going to connect it to pin 2 on C1. Click LEFT MOUSE or
press ENTER. The message:

  PLACE TRACK

appears on the prompt line.

Now move the cursor towards C1 keeping the line horizontal.
When the line is half way towards C1 (about X:1650 Y:2200)
click LEFT MOUSE or press ENTER. Press * to change
layers. Now move the line vertically until it is in line
with pin 2 on C1 (about X:1650 Y:2450). Click again or press
ENTER then press * to change to the bottom layer. Move
the cursor to pin 2 and click again or press ENTER.

A connection now extends from U1-1 to C1-2. Notice that this
last section has been placed on the bottom layer and that a
via has been used to change layers. Press ESC or click
RIGHT MOUSE twice to exit from the track laying routine.

You can continue to make the other connections in the same way
for practice. We will now make one of the connections using
the powerful pad-to-pad router option.

Invoking the Pad-to-Pad router

The router option is invoked by the Place/Route command. Select
Place/Route now from the menu or simply type PR on the keyboard.
Notice the message on the prompt line - ROUTE: SELECT FIRST PAD
Move the cursor to U1-11. (It's third up from the bottom on the
RHS of U11). Press ENTER. Notice that you are now prompted to
select the second pad.
Move the cursor to J1-3 and press ENTER. (It's the second round
pad above the square pad on J1).
The router will make the connection for you, automatically
swapping layers and placing vias during the process.


Connecting to power and ground planes

The final connections you have to make are to the power
plane and ground plane. Pin 7 on the DB25RA/F connector and
pin 15 on the DIP16 chip have to be connected to the ground
plane. Pin 16 on the DIP16 has to be connected to the power
plane. (This is assuming, of course, that you are going to
construct a board with power and ground planes.)
Choose Edit Pad. You are prompted to select a pad. Select
pin 7 on the DB25RA/F and a window opens displaying
information about the pad.

Notice that there is an option which shows the power and
ground status. Choose this option and another window opens
listing the possible connections. Choose Relief to Ground
Plane.

Press ESC or click RIGHT MOUSE and you are prompted to
select another pad. Now choose pin 15 on the DIP16 and make
the same connection. Finally, choose pin 16 on the DIP16
chip and connect it to the power plane by choosing the
Relief to Power Plane option.




3 Tutorial: plotting a board

This tutorial shows you how to do a simple check plot of the
DEMO.PCB file. Protel Easytrax has a flexible set of output
routines which allow output to be sent to dot matrix printers,
HP LaserJet & compatible printers, Postscript printers (eg Apple
Laserwriter), pen and ink plotters, photoplotters and disk files.

In this tutorial you will learn the following skills:

  loading the Easyplot program;
  interpreting the menu levels;
  interpreting the status screen;
  loading a .PCB file;
  setting the serial interface parameters;
  selecting the plot type;
  loading a plotter driver;
  setting the pen speed;
  setting the pen size;
  producing a draft plot.

In this tutorial the plotting is done on a simple, single-
pen DMPL plotter. If you do not have a similar plotter you
will need to adjust the tutorial to suit your situation.


Starting the program

To start the Easyplot program simply type: EASYPLOT then
press ENTER
at the DOS prompt. You might need to move into a different
directory before you start the program. Check Appendix A for
details.
The MAIN PLOT MENU is displayed.

  MAIN PLOT MENU
   File
   Information
   Options
   Setup
   Plot
   Print
   Gerber Plot
   NC Drill


Loading the DEMO file

Choose File/Load and enter the file name DEMO in the input
window. An information window opens showing the number of
pads, tracks, components, etc. that are being loaded. A
second pass shows the percentage of the board which has been
analysed.

When the file has been loaded, the status screen is updated
to show the name of the .PCB file, the dimensions of the
board and the amount of free memory remaining. The path name
of the directory is also displayed.

  Path:     C: \FILES
  Layout file: \FILES\DEMO
  Layout size: 5900x5000
  Free memory: 114654

You should check the layout size to make sure that the board
fits on the paper at the scale you choose. Thus, if a board
has a layout size of 6000 x 5000, it will cover an area 6
inches by 5 inches. If you plot it at a scale of 2, it
requires a sheet of paper which is at least 12 inches by 10
inches.

The File menu is still displayed. Press ESC or click
RIGHT MOUSE to return to the MAIN PLOT MENU.


Overview of plotting a board

Now you can use a plotter to produce a check plot. First,
make sure that you have set up the plotter in accordance
with the manufacturer's specifications. For the purposes of
this tutorial we use a DMPL single-pen plotter with a serial
interface running at 2400 baud.

The steps you need to take to set up the correct conditions
for a successful check plot are:

  Set the serial port to the correct baud rate.
  Make sure the other setup parameters are correct.
  Select Check Plot as the plot type.
  Set up the check plot parameters.
  Load the plotter driver.
  Set the pen speed.
  Set the pen sizes.


Setting the serial port parameters

Let's assume that you have a DMPL plotter connected to a
serial port of your computer. (If you haven't, then choose
from the list of plotters provided in Setup Plotter Type -
there must be a plotter driver for your plotter before you
can use it with Easyplot).

Choose Setup Serial Ports and choose either `Serial Port 1'
or `Serial Port 2' depending on which port you have
connected the plotter to. A window opens showing each of the
serial port parameters you can change.

  SERIAL PORT 1 SETUP
   Baud      :  2400
   Data      :  8
   Handshake :  Hardwire
   Parity    :  None
   Stop Bits :  1

If the baud rate is not set to the correct value (in this
case 2400) select Baud and select the value 2400 by
highlighting it and then pressing ENTER or clicking LEFT
MOUSE. You are returned to the Setup Serial Ports menu.

Check that each of the other parameters is set correctly for
your plotter. If you are using a DMPL plotter then the
parameters shown in the previous menu should be correct.
Press ESC or click the RIGHT MOUSE button three times to
exit from this option.


Choosing the plot type

In this tutorial you are going to produce a check plot,
rather than a plot of a particular layer or a specialised
plot such as a solder mask.
Return to the MAIN PLOT MENU and choose Options/Type of
Plot. A window opens showing each of the plot types you can
choose. Use the arrow keys to highlight Check Plot then
press ENTER or click LEFT MOUSE.
Return to the MAIN PLOT MENU and choose Setup Check Plot.
Make sure that the Top Layer, Bottom Layer, Top Overlay and Multi
Layer Pads options are set to `on'.
This ensures that all the information on each of those
layers is plotted. If you set any of these to `off', the
items on that layer are not plotted. Press ESC or click
the RIGHT MOUSE button to exit from this option.


Loading the plotter driver

Choose Setup Plotter. The entry next to Type shows the
currently selected plotter driver. If it is not set to
`DMPL', choose the option and the program scans the
directory and lists all the currently available plotter
drivers. Select the DMPL plotter driver from the list and
then press ENTER or click LEFT MOUSE. You are returned
to the Setup Plotter menu.

Choose Device and another window opens listing the options
you can choose for the port to connect the printer to.
Choose `Serial Port 1' by moving the selection bar to that
option then pressing ENTER or clicking LEFT MOUSE. Check
the other options to make sure they are the same as those
shown below. Press ESC or click RIGHT MOUSE twice to
return to the MAIN PLOT MENU.

A possible set of options is shown below:

  PLOTTER SETUP
   Type         :  DMPL
   Device       :  Serial Port 1
   Scale        :  1.000
   X Offset     :  0.000
   Y Offset     :  0.000
   X Correction :  1.000
   Y Correction :  1.000
   Orientation  :  Auto Centered
   Quality        :Draft
   Software Arc :  On
   Arc Quality  :  5
   Options      :
   Pens         :


Setting the pen parameters

You now need to set the speed at which the pens are to be
driven and the size of pen that you have in the plotter.
Choose Setup Pens Check Plot Pens. You now need to set the
pen speed to a value of 2 inches per second. This figure
seems to work the best with a DMPL plotter.

Hint: You can set the pen speed to a higher value, but the
ink in the pen may not flow quickly enough to form a clear line
on the paper. If you set the value too low then you may get
ink `blotches' on the paper - it also takes a long time to
plot. Experiment with different speeds until you find an optimum
setting for your plotter.

To input the pen speed, highlight the Pen Speed option and
press ENTER or click LEFT MOUSE. Enter the value in the
input window, then press ENTER or click LEFT MOUSE. You
are returned to the Check Plot/Pens menu.

You now need to set the size of the pen you are using. This
is vital so that the printer driver can draw the tracks,
arcs, vias and pads accurately. It is obvious that if you
have a 26 mil diameter pen then it is impossible to draw a
12 mil track at normal scale

If you do not set the pen size, it defaults to 26 mils. To
change the size, choose Pen Sizes from the Check Plot/Pens
menu. Enter the value of the diameter of the pen in mils and
the press ENTER or click LEFT MOUSE. You are returned to
the Check Plot Pens menu. Press ESC or click the RIGHT
MOUSE button four times to return to the MAIN PLOT MENU.


Plotting the board

You are now ready to proceed with the plot. From the MAIN
PLOT MENU choose Plot. You are asked to confirm that you
want to proceed with the plot. Before you choose Yes, check
the large information window on the right-hand side of the
screen which displays all the plot parameters. If any of
these are not correct you need to return to the MAIN PLOT
MENU and change them.

When you are happy that everything is correct choose Yes.
You are then asked to insert pen 1 in the plotter. Make sure
it is securely in place then press ENTER or click LEFT
MOUSE.

The plot should now begin to appear on the paper in the
plotter. When the plot is finished you are returned to the
MAIN PLOT MENU.


4  Tutorial: Gerber plots

In this tutorial you learn how to use the Easyplot program
to create a file which can be used with the standard Gerber
format photoplotter to produce high-quality final artwork.
You probably will not want to go to the trouble and expense
of producing a Gerber plot of the demo board, however, the
tutorial will give you a good overview of the process.

The skills you learn in this tutorial are:

  Selecting a particular plot layer;
  Selecting Setup parameters;
  Selecting apertures;
  Selecting the photoplotting method;
  Generating a match file;
  Generating a Gerber plot file.

Photoplotters produce highly accurate artwork - in fact they
are as accurate as the resolution of the Protel Easytrax
program. The biggest problem is that the equipment can be
very expensive so most board designers need to send their
files to a photoplotting bureau. For this reason, the
Easyplot program produces output files rather than driving a
photoplotter directly.


Setting up a Gerber plot

You need to set up all the same options for a Gerber plot as
you do for a normal plot but there are some extra things to
do as well.

First, you should choose File Load and load the Demo PCB
file. This process is exactly the same as for a normal plot
or print.

In this tutorial you are going to produce a plot of the top
layer and the pad master. For the first plot choose
Options/Type of Plot and select `Top Layer'.

Note that the `Check Plot' option does not work with a
Gerber plot because 1:1 Gerber check plots would be of no
practical value. You should use a printer or pen plotter to
do your check plot and only produce the (expensive) Gerber
plot when you are sure that it is absolutely correct.

Now choose Setup/Gerber and define each of the setup options
you require. The options from which you can choose are shown
in the menu displayed below.

  GERBER SETUP
   Output File    :  \Files\Demo
   X Offset       :  0.000
   Y Offset       :  0.000
   Aperture Tabl  :  PROTEL1.APT
   Match Tolerance:  5%
   G54            :  Off
   Arc Quality    :  5
   Options

The X and Y Offsets can be used in exactly the same way as
they are for a normal plot. By changing these offsets you
can choose to start plotting at a different spot on the
film. This allows more than one plot to be performed on one
film, thus saving on the cost of film.

Next you should choose the Aperture Table which matches that
required by the photoplotter that you are going to use.
While most photoplotters use the Gerber standard for
selecting apertures and for moving to a particular spot on
the film, they vary considerably in the apertures which are
available. To overcome this problem there are a number of
standard Aperture Tables supplied with Protel Easytrax.
Select the aperture table you require by choosing Setup
Gerber Aperture Table. A list of the available aperture
tables is displayed. Highlight the one you require then
press ENTER or click LEFT MOUSE. The name is now
displayed in the Gerber Setup menu.

Next you should set the Match Tolerance percentage you require. An
example might help here. If you have a large number of
circular 62 mil pads on your board, these can be plotted
quickly by selecting a 62 mil aperture and then `flashing' a
light onto the film.

But what happens if the photoplotter does not have a 62 mil
aperture? Some have a 60 mil round aperture and for most
plotting tasks you are likely to require this is close
enough. The Match Tolerance is the figure you set to say
what variation in area you can tolerate. If the program is
able to match an aperture with a pad which is within the
tolerance you set, then it does so automatically.

The area of a 62 mil pad is 3.1415 x 62 x 62 = 12076 square
mils. The area `flashed' by a 60 mil aperture is 3.1415 x 60
x 60 = 11309 square mils. The percentage variation is
calculated as (12076-11309) x 100 / 12076 = 6.35. Therefore
if you set the Match Tolerance to 8% or greater, the 60 mil
aperture is selected automatically.

Don't set the tolerance too high (e.g. 30%) otherwise there
may be problems fitting tracks between pads in some cases.

Some older Gerber plotters need to be sent the code G54
before an aperure change. Thus, if the aperture D10 is to be
selected the software must send a G54 code then a D10 code.
If the plotter requires this code to be sent, set the G54
option to `On'. If it does not need this code, set it to
`Off'.

Some plotters have the ability to draw an arc if the
parameters are supplied. This is not the case with some
Gerber photoplotters. In order to draw an arc, the plot
program must ask the photplotter to draw a number of short
line segments. The greater the number of line segments used
to draw the arc, the longer it takes. The Arc Quality option
allows you to set the length of the line segment (in mils) which is
used to draw the arc. A value of 5 mils is a reasonable
compromise for most jobs.

The steps you have carried out to set up the Gerber plot
are:

  Choose File Load and load the Demo file
  Choose Options Type of Plot, then select Top Layer
  Press ESC or click RIGHT MOUSE
  Choose Setup/Gerber
  Choose Aperture Table and select the required table
  Set the Match Tolerance to 8%
  Set G54 to `Off'
  Set Arc Quality to 5
  Press ESC twice to return to the MAIN PLOT MENU


Creating the Gerber file

Now return to the MAIN PLOT MENU and select Gerber Plot. The
plotting screen appears with the information window on the
right hand side of the screen.

You are asked to confirm that you want to proceed with the
Gerber plot. this gives you the opportunity to inspect the
parameters you have chosen for the plot. If any of them are
incorrect, select No and change them. If you are ready to
proceed select Yes.

The program now attempts to match every item on the board
with an aperture on the photoplotter that you are going to
use. For each item, it looks for an aperture in the Aperture
Table you selected. If it cannot produce a match within the
tolerance you specified it asks you to select from a table
of the closest apertures or enables you to step through the
apertures to manually select one.

You see a display similar to the one below.

  MATCHING DRAFT CODES

  ASSIGNING    :   Circular (28 x 28)

  Match Method     Code   Shape       Size

  Flash Match  :   D19    Circular    (40 x 40)
  Stroke Match :   D15    Circular    (25 x 25)
  Fill Match:  :   D13      Circular    (20 x 20)

A window then opens allowing you to select which method you
want the photoplotter to use to make the shape.

  Select Plot Method
  Flash Method
  Stroke Method
  Fill Method
  Manual Assignment

Make sure that you do not choose the stroke method to create
a pad. If you attempt to, the message:

  CANNOT USE LINE APERTURE FOR MATCH

is displayed.

It is a good idea to minimize the number of Fill Matches, as these
usually take longer to photoplot.

When all apertures have been matched, the message:

  MATCH FILE GENERATED

appears indicating that a file has been created which
matches each shape to be generated with an aperture which is
available on the chosen photoplotter.

The match file shows the shapes which the program has tried
to assign apertures to and the aperture and exposure method
which has been chosen - either by the program or by you. A
sample from a match file is shown below.

ASSIGNING    :         Circular       (28 x 28)
STROKE       : D15     Circular       (25 x 25)

ASSIGNING    :         Circular       (40 x 40)
FLASH        : D19     Circular       (40 x 40)

ASSIGNING    :         Circular       (60 x 60)
FLASH        : D28     Circular       (62 x 62)


Press any key and the final Gerber output file is then
generated. The Gerber file in this case is assigned the name
DEMO.GTL. The extension indicates that it is a Gerber output
file and that it is a plot of the Top Layer.


Plotting the Pad Master

When the first plot is complete you are returned to the MAIN
PLOT MENU.
Now, as an example of a different plot, choose Options Type
of Plot and select Pad Master. Press ESC to return to the
MAIN PLOT MENU.
When you now choose to do the Gerber plot, you are asked
whether you want to reassign the draft codes. If you are
happy with the matches which are stored in the .MAT file
then choose No and the plot proceeds.
This time the Gerber output file is given the extension .GPM
to indicate that it is the Pad Master layer.


5  Options Summary

In this section, each of the major menu options you can
choose are listed along with a brief summary of their
function.

Block
 Define        Defines a block by selecting the opposite
               corners of the rectangle, then selecting any
               reference point.

 Hide          Used to remove the highlight from the
               currently defined block.

 Move          Once a block is defined it can be moved to
               another part of the board. You can move items on
               the current layer or all layers. The block can be
               flipped or rotated during a move with the X, Y and
               SPACE keys.

 Copy          Similar to Block Move except that items are
               copied.

 Inside Delete Deletes items within the currently defined block.

 Outside Del   Deletes items outside the currently defined block.

 Read          Reads a PCB file as a block which can then be
               placed within the current board.

 Write         Saves the currently defined block as a file.
(Not implemented in the demonstration program).

Current
 Cursor Mode   Allows the cursor position to be measured from the
               bottom left hand corner of the board (Absolute) or
               from the position of the floating origin
               (Relative).
 Floating Orig Allows you to set the origin at a point other than
               the bottom left hand corner of the board.

 Layer         Selects the layer which is to be the current
               layer. The currently selected layer can also be
               changed with the *, - or + keys.

 Pad Type      Allows you to select the pad type which you want
               to be the currently selected pad type. When you
               choose Place Pad, it is this pad shape which is
               placed.

 Pad Orient    Pads can either be placed normally or rotated
               through 90 degrees. Choose either `Normal' or
               `Rotated' with this option.

 Track Width   Set a track width from 1 to 255 mils with
               this option.

 String Size   The string size is the size of any text
               characters which you place on the board. It is
               measured in mils.

 String Lines  This variable controls the thickness of the lines
               which make up the strings.

 Via Size      Use this option to change the currently selected
               via size.

 Via Hole Size Use this option to change the currently selected
               via hole size. The hole size must be less than
               the via size.

Delete
 Arc           To delete an arc, choose this option then
               select the arc to be deleted.

 Component     Allows you to delete a component such as a
               chip or connector or capacitor.

 Fill          Use this option to delete a fill from the board.

 Highlight     Allows you to delete the set of tracks which are
               currently highlighted.

 Pad           Deletes a selected pad. Since a pad belongs to
               every layer (except for SMDs and edge connectors)
               it usually does not matter what layer is currently
               selected.

 String        To delete a string, choose this option then select
               the string to be deleted. Make sure that the
               currently selected layer is the layer on which the
               string is placed.

 Track         Deletes a track. You may have to delete a number
               of tracks to remove a complete connection.

 Via           To delete a via, choose this option. A via can be
               deleted from any layer.

Edit
 Component     Allows you to change the designator, pattern
               or comment associated with a component. It also
               allows you to change the layer on which the
               component isplaced and to indicate whether the
               component can be moved during an auto place
               procedure.

 Pad           Allows you to change the shape of a pad and
               also to indicate whether the pad should be
               connected to the power or ground planes.

 Track         Allows you to change the layer the track is
               on or the width of the track.

 String        You can use this option to change the size,
               line width or message in a particular string.

 Via           Allows you to change the via size or the via
               hole size.

File
 Clear         Clears the current board from the memory of
               the computer.

 Dos           Allows you to suspend to DOS to carry out
               routine DOS operations. Type EXIT to return to the
               program.

 Files         Allows you to inspect a listing of files in the
               currently selected directory.

 Load          Loads a .PCB file.

 Path          Allows you to change the currently selected
               directory.

 Quit          Use this option to quit from the program.

 Save          Saves the board you are currently working on.
               It is saved in the directory you have specified
               using the Path option unless you specify
               otherwise.
 (Not implemented in the demonstration program).

Grid
 Snap Grid     The invisible snap grid controls the movement
               of the cursor. Allows precision in placing items.

 Visible Grid  A series of dots on the screen, an aid to
               alignment.

Highlight
 Connection    Allows you to highlight the connection between two
               pads. Point to a track, not a pad, to start the
               highlighting.

 Duplicate     Duplicates a hilighted connection. Select the
               point on the connection you want to act as a
               reference point,then point to the new position.

 Net           Allows you to highlight a complete net.

 Make Netlist  Allows you to create a netlist based on the
               connections you have made on the board. The
               netlist is stored in a file with the extension
               .NET, in the currently selected directory unless
               you specify otherwise.
 (Not implemented in the demonstration program).

 Reset         Removes the highlight from a highlighted net.

Information
 Board Dimen   Displays the current size (inches) of the board.

 Components    Lists the designators of the components which
               have been placed.

 Highl'd Pins  Lists the pins connected to the currently
               highlighted net. This is useful for checking that
               you have connected all the pins that you intended
               to connect.

 Lib Comps     Displays the components in the current library.

 Pwr/Gnd Pins  Lists either the ground nets and/or the power
               nets.

 Status        Displays information about items on the board
               as well as information about memory usage and file
               names.

Jump
 Component     Moves the cursor to pin 1 of a selected component.

 Location      Moves the cursor at a particular coordinate.

 Origin        Moves the cursor to the origin (0/0 coordinate).

 Pad           Moves the cursor to a named pin on a selected
               component.

 String        Moves the cursor to a selected string.

Library
 Add           Adds a highlighted block to a selected library as
               a component.
 (Not implemented in the demo program).

 Browse        Allows you to inspect each of the components in
               the currently selected library.

 Compact       Compresses data in an edited library file.
(Not implemented in the demonstration program).

 Delete        Deletes a component from the currently selected
               library.
 (Not implemented in the demonstration program).

 Explode       Reduces a selected component into editable tracks,
               arcs and pads. Used to create a new component by
               altering an existing one.

 File          Changes the currently selected library.

 List          Lists the components in the currently selected
               library.

 Merge         Moves a component from another library into the
               current library.
 (Not implemented in the demonstration program).

 New Library   Creates an entirely new library.
 (Not implemented in the demonstration program).

 Rename        Renames a component in a library (does not
               rename the library).
 (Not implemented in the demo program).
Move
 Arc           Moves an arc from one part of the board to
               another.
               Cursor must be exactly over the arc when
               selecting it.

 Break         Breaks a track into two sections at a particular
               point.

 Component     Moves a component to another place on the board
               with the option of dragging the connected tracks.

 Drag End      Allows you to drag one end of a track to a new
               position.

 Fill          Moves an area fill.

 Pad           Moves a pad to a new position on the board.

 Re-Route      Allows you to manually re-route a connection
               by breaking a track at a number of points.

 String        Moves a string.

 Track         Moves a track while maintaining connectivity
               with related tracks and vias.

 Via           Moves a via while maintaining connectivity with
               tracks.

Place
 Arc           Places an arc. Use the LEFT and RIGHT cursor keys
               to increase and decrease the radius, and
               the 8, 6, 2 and 4 keys on the keypad to remove arc
               segments.

 Component     Places a selected component from the current
               library.

 Fill          Places a rectangular area of solid fill.

 Pad           Places a pad of the type selected in the Current
                options.

 String        Places a string on the board. The size and
                 thickness of the string is determined by the
               parameters in the Current menu.

 Track         Places a track segment on the currently
               selected layer. The placed track is the size
               selected from the current options.

 Via           Places a via of the size selected in the Current
               options.

Repeat         This option allows you to repeat the
               placement of the last component, track, pad or via
               a specified number of times in a specified
               direction.

Setup
 Comp Text     Toggles display of component text on/off.

 Layer Colors  Selects colors for items on each layer.

 Menu Colors   Selects colors used in the menus,background,etc.

 Keys          Main Menu for macro editor.

 Options       Allows you to change parameters including cursor
               shape, back-up interval, etc.

 Pads          Allows you to define custom pad types.

 Redraw        Selects draft or final quality screen redraw.

 Strings       Sets default size for strings from 36 to 560 mils.

 Toggle Layers Sets each board layer to `on' or `off'.

Un-delete      Whenever you delete an item from the board,
               Protel-Easytrax remembers the deletion. This
               option allows you to restore one or more deleted
               items.

Zoom
 Redraw        Redraws the current screen at the current
               magnification.

 Pan           Redraws the screen at center of cursor position.

 Expand        Selects the next highest magnification from one of
               six zoom levels (also PGUP key).

 Contract      Selects the next lowest magnification (also PGDN
               key).

 All           Redraws the display to include the entire board.

 Keyboard      Selects a zoom level by number.

 Select        Selects a zoom level  from 7 pre-set
               magnifications.

 Window        Selects a section of the board for magnification.



















Additional information this version:

New graphics drivers
This release includes the following new
drivers for the ATI VGA Wonder card and the
Paradise EGA480 card. The drivers are labelled
WOND800.DRV (800x600), WOND1024 (1024x768, Revision
5 cards only) and PEGA480 (640x480). There are a
number of cards that use the PEGA480 chipset.


Memory management
If memory is a problem, make sure that your
operating system is as 'bare' as possible - disable
network software and any TSRs (other than EMS/Mouse
drivers), etc. If memory is still a problem you may
need to consider additional EMS.


Repeat Placement with metric grids
If you are using the Repeat Placement
feature with some fractional metric
grids, the Offsets applied to repeats
can result in some unexpected
placements. This is because the metric
value must be rounded off to two decimal
places. For example the default 25 mil
imperial grid is equal to approx .625
mm, rounded-off to .63 mm by Autotrax.
If you attempt a repeat placement of a
row of pads, this rounding-off will
result in a cumulative error in spacing
as successive pads are placed. The
solution is to use even multiples of the
current snap grid as offsets OR to work
on a 'natural' grid pitch, i.e. .5 mm or
.6 mm OR to stay on the imperial grid,
rather than switching to metric prior to
repeat placement.


Easyplot - version 2.06

Additional Features


Roland 1000 Series plotters
A new plot driver has been added for these popular
plotter models (DXY 1100, 1200, 1300, etc).

    It is called ROLAND RD-GL I.

This supersedes the information in the manual.
However, you should make sure that all
communications parameters are matched between the
program and the plotter.


Improved Path Handling in Easyplot
When you select the Setup/(Plotter, Printer or
PostScript)/Type, to choose a driver, a window
opens allowing you to specify the directory. The
default directory is now always the Easyplot home
directory.

Naming of output files:
The name of the current .PCB file is automatically
applied to output files, as when plotting to a
filename (rather than directly to a port).


PostScript printing
The following PostScript options are supported
by the current version of the Easyplot
program:

PS300A4      A4 sheet  300 dpi resolution
PS300A3      A3 sheet  300 dpi resolution
PS400A4      A4 sheet  400 dpi resolution
PS600A4      A4 sheet  600 dpi resolution
PS1200A4     A4 sheet 1200 dpi resolution
PS1200A3     A3 sheet 1200 dpi resolution
PSLINOA4     A4 sheet 1270 dpi Linotronic
PSLINOA3     A3 sheet 1270 dpi Linotronic
PS300B5      B5 sheet  300 dpi resolution
PS300LT      US letter 300 dpi resolution
PS300LE      US legal  300 dpi resolution


(end)