Best of Shareware/Best of PC Windows Shareware 1.0 - Wayzata Technology (7111) (1993).iso/mac/ZIPPED/DOS/CAD_CAM/ACADPCB.ZIP/ACADPCB.DOC

Text File | 1992-12-21 | 59KB | 981 lines

                           +-------------------+
                           |    AutoCAD-PCB    |
                           +-------------------+
          Software Accessories For Electronic Design Using AutoCAD(tm).

            ["AutoCAD" is a registered trademark of Autodesk, Inc.]

+==============================================================================+
| SUMMARY:                                                                     |
| This package contains the software "add-ins" to make AutoCAD capable of doing|
| manually routed printed circuit board designs.  It has "script" files that do|
| the initial setup for these kind of drawings, menu files that create screen  |
| menus optimized for the commands most frequently used in electronic design,  |
| and a collection of pre-drawn blocks that can be inserted into drawings to   |
| speed design work.                                                           |
+==============================================================================+

                                Shareware Stuff . . .

These tools were developed by Paul Marxhausen of the University of Neb-
raska-Lincoln Engineering Electronic Shop to provide engineering students
who have access to AutoCAD-equipped PCs a method of doing electronic design.
They may NOT be sold or distributed for any form of compensation.

The user is encouraged to use these tools and modify them however they wish;
however, if you wish to distribute and share modifications of these files,
please do so under a name other than AutoCAD-PCB and in a different archive
file, if you are sending them to a BBS or Internet archive.  We would like to
keep the integrity of the file list above intact.  Our support for these tools
begins and ends with this free distribution, released in December 1992; ad-
ditional enhancements or releases are not planned at this time.

                                INTRODUCTION

Computer Aided Design is a very powerful way to create printed circuit boards,
especially when one has the use of professional-level software packages that
"capture" computer-drawn schematics, or have auto-routing capabilities.
However, use of CAD for PC boards involves the obstacles of  A) the often
substantial amount of time invested in learning the software; B) the intricacies
of getting from a bunch of bytes on a computer to a finished printed circuit
board; and  C) the substantial obstacle of COST.  Good quality PCB CAD programs
can cost upwards of a thousand dollars.  Inexpensive CAD programs can be
inflexible or inadequate.  AutoCAD-PCB was created to afford persons with access
to AutoCAD a way to do PCB CAD work quickly, inexpensively, and effectively.

NOTE TO NEW AUTOCAD USERS:
While these tools make it faster and easier to set up and edit electronic
drawings, it is assumed that the user has a basic working knowledge of AutoCAD
commands and procedures.  For example, this manual doesn't spell out how you
select an object with the pointer or a window.  If you are new to AutoCAD, be
advised that while it has menu features and on-line help (HELP command), it is,
like many fully-featured CAD packages, a very complex, elaborate, and sometimes
confusing piece of software.  However, it is also very powerful: if there's
anything you want to do in a drawing, AutoCAD has a way to do it.  If you are
serious about this work, you'll want to have access to the AutoCAD manuals or to
one of the many books available on the use of AutoCAD in local bookstores.

NOTE TO ALL USERS:
Read ALL of this documentation, start to finish - it's not that long.  It's
important to understand what these tools do with AutoCAD, or you'll end up doing
a lot of uneccessary swearing and hair-pulling, which is all too common when
using AutoCAD in the first place.  Especially pay attention to what the custom
menus do, because some of the menu items are not what they seem (see the PTRACE
menu, for example.)


                                  THE TOOLS

THE SCRIPTS:
An AutoCAD script is a file of commands that AutoCAD can execute in "batch"
mode.  Scripts can be executed either by using the SCRIPT command while running
the AutoCAD drawing editor, or by giving a script name when you run AutoCAD from
the MS-DOS command line.

Example:

C:>ACAD MYFILE PCB  <return>

This will start AutoCAD and create the new drawing MYFILE.DWG. The script file
PCB.SCR will set up AutoCAD for certain predefined parameters.  NOTE, however,
that you actually only have to run the setup script when creating a NEW drawing,
because after you save your new drawing, all the setup information, menus, etc.
will be saved with it and all you will have to do in the future is load your
drawing with the normal ACAD MYFILE command line.

[If you're already in the middle of running AutoCAD and are editing a drawing,
you can do the same setup using the AutoCAD SCRIPT command.  However, use the
PCB2.SCR file if you do so, or it'll mess up trying to create a new drawing.
(ex: SCRIPT PCB2)]

If you want a handy way to create new drawings, use the batch file called
PCB.BAT.  It's just one line:

ACAD %1 PCB

Now, if you type  PCB  MYFILE  it'll do the same thing shown above.

The PCB Script will do several things: set up the screen units, size, grid,
axis, and snap units; define several drawing layers; and load a customized menu.

Screen and Units
The screen units used with AutoCAD-PCB are mils, or thousanths of an inch.  (One
mil = .001 inches).  This is common usage in printed circuit board design work.
It's easier to work with AutoCAD when you can tell the program that you want a
trace that's 13 mils wide instead of .013 inches, or to set the snap units to 25
mils instead of .025 inches, etc. The limits of the drawing are set to 11,000
mils by 8,500 mils, or 11 by 8.5 inches, to correspond to the standard letter
sized sheet of paper that most drawings will be printed or plotted upon.
(Please be sure to read the section on "Printing, Plotting and Production"
before you try to get a hard copy of your drawing, or you may be faced with the
task of trying to print out a drawing that AutoCAD thinks is almost a thousand
feet long, actual size.)  Note that you can change your limits or draw outside
of them if you wish.

The SNAP is like an invisible grid whose size the user can define.  When drawing
lines or selecting points on the drawing, the cursor will "snap" to these points
only if SNAP is on.  This makes it easy to line up objects. The SNAP defaults to
25 mils, and can be toggled between that setting and a 100 mil snap with the
SNAP submenu.  These snap settings are useful in PC board work because most
standard pin spacings are .1 inches, or 100 mils.  Thus, using a 100 mil snap
makes it easier to place parts on the board in proper alignment, while the 25
mil snap gives finer control for routing traces while still making it easy to
line up with objects on the 100 mil grid.

The screen grid defaults to 500 mils, or a half inch, to give the user a rough
idea of where he is on his drawing.  The axes around the edge of the drawing are
spaced at 100 mils to make it easy to line up parts.

The drawing defaults to FILL OFF, which means that thick things like traces and
pads are drawn as outlines, not areas completely filled with color.  This is for
reasons of speed: drawing a lot of complex, filled entities really can make your
computer groan.  If your drawing is small or you have a fast '486 computer
or you just can't live without the filled lines, enter FILL ON.  However, any
non-filled structures you happen to have on screen won't fill unless you also
type REGEN to regenerate the drawing.

+=============================================================================+
| IMPORTANT: AutoCAD-PCB assumes that you are drawing the circuit board from a|
| TOP VIEW, looking down at the component side of the board.  In effect, as   |
| you draw the traces you are doing so as if you had a transparent board.     |
| This is because integrated circuit data books always give their chip pin-   |
| outs as a top view, and it's easier to route your traces in a top-view mode.|
| However, when it comes time to plot or print the traces to make a circuit   |
| board negative or similar, it will be necessary to MIRROR this view, which  |
| is easily done in AutoCAD.  For more details, consult the Printing and      |
| Plotting section below.                                                     |
+=============================================================================+

While these default settings are useful, you may want something different.  Any
of these settings can be changed at any time with the appropriate commands.  If
you want to change the defaults for these or any other settings, you could edit
the PCB.SCR file with any text editor.  However, if you do want to make changes
in the start-up script, we would prefer that you copy PCB.SCR to another file
name and make your changes on that file for your own use, so that there doesn't
end up being a whole lot of different variations all named PCB.SCR associated
with this software package.

THE LAYERS
AutoCAD works with "layers"; it's very similar to having a stack of
transparencies that you can switch between and draw on individually.  This
allows the user to make certain structures a different color, or hide them
from view so that only certain structures are dealt with, or many other
useful things.  Similar to standard electronic CAD practice, AutoCAD-PCB makes
up these distinct layers:

LAYER   COLOR   FUNCTION
---------------------------
PADS    CYAN    The solder pads associated with all component leads.
BOTTOM  BLUE    The traces on the bottom side of the circuit board
TOP     RED     Traces or jumpers on the top side of the circuit board.
PARTS   MAGENTA The physical outline of the electronic components.
LABELS  GREEN   Any labels or text associated with parts or points on board.
OUTLINE WHITE   The physical edges of the PC board, and any mounting holes.

Commercial PCB CAD programs often have a good many more layers than this,
but for most single or double sided boards, these will suffice.  You can always
create more layers if you wish.  The LAYERS command in the custom PCB menu
makes it easy to switch between these layers and turn them off and on.

IMPORTANT: as will be discussed at length below, just because you are using
a certain layer doesn't mean everything you create is going to be on that
layer.  When you insert the predefined shapes, their component parts will
appear on the layers for which they were created.

THE BLOCKS
"Blocks" in AutoCAD are just pieces of drawings that you can insert wherever
you need them.  You can make anything that you draw into a block with the
BLOCK command and put it into your drawing with the INSERT command.  If
AutoCAD doesn't find a block you've asked to insert already defined inside of
your drawing, it will go out to your default disk drive and directory and look
for a .DWG file of the same name, and use it for the block.  If you have all the
AutoCAD-PCB .DWG files in your directory, you'll have access to them as
predefined blocks.  The blocks are the following:

BLOCK           DESCRIPTION
---------------------------------------------------------------------------
OP60            Oval Pad, 60 mil.  Used where traces will be run between pads.
SP60            Rectangle Pad, 60 mil.  Designates pin 1 on the DIP blocks.
RP60            Round Pad, 60 mil.
RP70            Round Pad, 70 mil.
RP80            Round Pad, 80 mil.
RP90            Round Pad, 90 mil.
RP100           Round Pad, 100 mil.
RP120           Round Pad, 120 mil.

8DIP            8 pin Dual Inline Pin integrated circuit socket.
14DIP           14 pin DIP socket.
16DIP           16 pin DIP socket.
20DIP           20 pin DIP socket.
24DIP           24 pin DIP socket.
28DIP           28 pin DIP socket.
40DIP           40 pin DIP socket.

R1_4W           1/4 Watt Resistor.
R1_2W           1/2 Watt Resistor.
R1W             1 Watt Resistor.
R2W             2 Watt Resistor.

DISCAP1         Disc capacitor.
DISCAP2         Disc capacitor.

RADCAP1         Radial lead capacitor.
RADCAP2         Radial lead capacitor.
RADCAP3         Radial lead capacitor.
RADCAP4         Radial lead capacitor.
RADCAP5         Radial lead capacitor.

AXCAP1          Axial lead capacitor.
AXCAP2          Axial lead capacitor.
AXCAP3          Axial lead capacitor.

HEADER8         8 pin Dual In Line (100 mil spacing) header socket.
HEADER10        10 pin header socket.
HEADER14        14 pin header socket.
HEADER16        16 pin header socket.
HEADER20        20 pin header socket.
HEADER26        26 pin header socket.
HEADER34        34 pin header socket.
HEADER40        40 pin header socket.
HEADER50        50 pin header socket.
HEADER60        60 pin header socket.

DB9             DB9 type socket.
DB25            DB25 type socket.
DB37            DB37 type socket.

DIODE1 - DIODE2         Diodes.
XTAL                    Crystal.

When you INSERT these, you'll see that these blocks will have solder pads on
the PADS layers, component outline on the PARTS layer, etc. regardless of
which layer you are currently using.

The discrete parts, like the resistors and capacitors, aren't strictly
necessary: you can simply use a pair of pads anywhere you need such a part.
The handful of discrete parts included are simply for convenience. There is
such a wide range of sizes for devices such as electrolytic capacitors that
you will probably have to do some measuring of your own and use discrete solder
pads for such parts.

Please note that the names for these parts in the INSERT submenus are different
than these file names.  (Example: Menu displays "Res 1/4W" instead of "R1_4W").
This is to make the menu more user-friendly and easy to understand.  However,
you should be aware of these differing names if you are entering the INSERT
command from the command line instead of using the INSERT submenus to pick out
blocks.  Thus, if you type INSERT <Ret> and the program prompts you for a block
name, you would enter "R1_4W" to get your quarter-watt resistor.

Wait a Minute - Where Did My Part Go?
There's only one tricky thing about using these blocks: AutoCAD treats them as a
SINGLE UNIT, not as a collection of pads and lines, etc.  This is great when you
want to move a block around; you do a MOVE and point to the block and the whole
thing moves around together.  This is terrible when you just want to change or
move one little part of that block.  For example, if you wanted to erase a
single solder pad on the block IC40, you'd enter ERASE and point to the pad, and
the ENTIRE BLOCK will select.  Continue, and the whole thing will erase.  How do
you get around this?

Two ways: first, you can enter INSERT from the command line. When you are
prompted for the block name, put an asterisk (*) before the name of the block,
for example, " *DIP40 " instead of " DIP40 ".  When you execute an INSERT this
way, it puts the block into the drawing as a collection of individual lines and
shapes, instead of as a single unbreakable block.  You can then erase, move,
copy, or otherwise edit individual parts of the block.  HOWEVER, you can't go
back after you've done this; if you want to move the entire block now, you'll
have to do a MOVE and then WINDOW, then bracket the whole thing with a window.

The second way to edit parts of a block is to use the EXPLODE command.  This is
a little better, because you can go ahead and use the menu or command line to
INSERT your block in the usual way, but if you find you have to go back to make
a change on a part of it, just type EXPLODE and point to the part.  It'll end up
looking exactly the same, but it's no longer a single unit.


THE MENUS
The custom menu (PCB.MNU/PCB.MNX) loaded by the PCB script simply attempts to
make some of the commands commonly used when drawing PC boards easier to access
by way of the menu on the right hand-side of the screen.  (All references to
menus in this document refer to this menu, NOT to the drop-down menus at the top
of the screen.)  Additionally, some of the predefined blocks are more easily
accessed by this custom menu.  However, it is possible to use AutoCAD and these
software add-ins entirely from the command line.

Notice that some of the menu items don't actually perform the command when
you select them; instead, they produce a SUBMENU of commands.  For example,
selecting ZOOM will get you a list that includes "In_2X", "Extents", "Window",
and a number of other ZOOMing options.  Selecting one of these will actually
execute the desired command, with the option.

Some of the Submenus don't cover up all of the main menu, and you can continue
to access commands on the main menu that are visible; however, you can end up
with yet another submenu laying over the top of the last one, and things can get
confusing.  SO, the best thing to do is to exit a submenu when you're done with
it by selecting the -BACK- command at the bottom of the submenu.  This gets
especially important when a submenu has a sub-submenu, as with the INSERT
command where there are several classifications of blocks that you can insert.


                                  MENU TOUR

Let's just look at all of the custom menu items, in the order they appear on the
menu.  Some are simple; some have multiple layers of submenus.  We'll look at
them all.  READ ALL OF THIS: there are things that are discussed later in this
manual that assume you know everything here.

- CANCEL
The *CANCEL* menu item that is always at the top of the menus is just a way to
execute a Control-C with the menu instead of the keyboard.

- PTRACE
The traces created by the menu item labeled "PTRACE" are NOT drawn with
AutoCADs TRACE command.  Instead, when you choose a trace from the PTRACE
submenu, you'll be drawing it with the PLINE command.  Why is that, when AutoCAD
has a perfectly good TRACE command that lets you draw traces of any width?  Two
reason: first,PLINE is a lot more flexible.  You can do some amazing things
like make the width of the trace vary continuously as you go, or make it go in
curves with the ARC option, or many other things.  The second reason has to do
with the fact that when you draw something with the AutoCAD TRACE command, you
end up with something that is made up of a bunch of independent little sections.
Try to MOVE, ERASE, or COPY a TRACE, and you have to select every little section
of it wherever it changes direction.  In contrast, a trace made as a PLINE is
treated as one undivided unit from start to finish, no matter how many twists
and turns it takes.  The first time you have to erase a long, elaborate trace to
redo it,you'll appreciate being able to just do an ERASE and point to any point
on the whole trace, instead of having to point to each of many little sections.

- - DrawPowr, DrawWide, DrawMed, DrawThin
The PTRACE menu can give you traces of any width you'd like.  (By the way,
don't try to just use the LINE command for signal traces, hoping that your
plotter will make wide enough lines.  Not a reliable method at all.)  The custom
menu gives you a choice of four: Thin (13 mil), Medium (30 mil), Wide (60 mil),
and Power (100 mil).  My general practice is to use traces that are plenty wide
when I can; it means you have less copper to etch off, less chance of a minor
flaw in the drawing or negative making a break in the trace, and you have less
lead resistance.  I use the Medium width where there's room for it.

- - Chamfer
To "chamfer" something means to cut little 45 degree angle edges on places where
lines meet at 90 degrees.  This is pretty common on printed circuit boards.
With the chamfer command at your disposal, you can go ahead and just run all
your traces with right-angle corners, then go back and angle the corners later.
The chamfer distance, which is how far back from the 90 degree corner the angle
starts, defaults to 50 mils.  You can change this by entering the CHAMFER
command from the command line and specifying a different distance.

- - Edit
Choosing Edit on the submenu gets you a LOT of other subcommands.  And choosing
VertEdit [Vertex Edit] on THAT subsubmenu gets you a lot more items, which can
get pretty confusing; but these menus can let you do powerful things like move
or add corners, etc.  Here's where you'd be wise to sit down with the AutoCAD
manual and/or the AutoCAD HELP command; read all you can about the PLINE command
and the PEDIT command, and you'll understand what these menu items are
attempting to do.  Again, you can do a PEDIT from the command line too; the
menus are for speed and convenience, and once you know what the commands are
about, they will speed your work.  This is one case where using the AutoCAD
manuals is HIGHLY RECOMMENDED - the PEDIT commands are very powerful and useful,
but it's easy to enter the wrong thing at the wrong time.  'Nuff said.

- LAYER
This menu lets you switch between the various layers of the drawing and turn
them on and off.  See the section on LAYERS for an explanation of what layers
ACAD-PCB defines and how they are used.

- INSERT
Insert lets you insert the predefined blocks or any other blocks you may have
defined.  The predefined AutoCAD-PCB blocks are found under one of several
submenus: Caps (capacitors), DIPs (IC sockets), Pads (solder pads), Resistor
(guess), Connects (connectors), and Misc (odds and ends).

- LINE
Executes AutoCAD LINE command without any bells or whistles.

- COPY
Executes AutoCAD COPY command.

- ERASE
Executes AutoCAD ERASE command.

- MOVE
Executes AutoCAD MOVE command.

- ZOOM
Executes AutoCAD ZOOM command, but also provides some ZOOM options as a submenu.

- PAN
Executes AutoCAD PAN command.

- TEXT
Executes AutoCAD TEXT command.

- SNAP
Gives you a submenu to set snap to fine (25 mil), coarse (100 mil),
user-specified, or turn it off or on.

- HELP
Executes AutoCAD HELP command.

- SAVE
Executes AutoCAD SAVE command.

- SAVEEXIT
Executes AutoCAD END command.

- QUITEXIT
Executes AutoCAD QUIT command.

More Menu Customizing
Got some ideas for improvements of your own?  Want to add a couple of commands?
The custom menu is created with the file PCB.MNU.  Take a look at this file with
a text editor and if you're at all handy with programming you'll catch on
quickly how AutoCADs menus are built.  Again, the AutoCAD manuals describe the
format of this kind of file in detail.  Once a .MNU file has been created, it is
compiled into the .MNX file that AutoCAD actually uses at run time by using the
MENU command while running the AutoCAD editor.  [The author of these tools used
the SHELL command to change the PCB.MNU file while still running AutoCAD, then
used MENU to load/compile the menu to see instantly how the changes worked.]



                            DRAWING A BOARD
How Many Sides?
So much for tools - how do you draw a board?  First, you'd better decide on how
many sides you're going to be using.  To give you some idea of what's involved
with this decision, and to show you how the "pros" do it, get yourself just
about any commercially manufactured printed circuit board, such as an expansion
card from a personal computer or similar.  Take a look at how the chips are laid
out and the traces are run.  People making boards for a living have a big stake
in giving their boards a tight, efficient layout.

However, people making boards for a living use something you may not want to get
involved with, and that's called "multi-layered boards."  Time was, PC boards
only had traces on the bottom side.  And in fact, not only can you do a lot of
projects with single sided boards, but they are far and away the easiest and
cheapest kind of PC board to produce . . . from the standpoint of exposing,
developing, and etching them.  But even on a simple design, you're going to find
traces that you just can't seem to get from here to there without crossing
something, and you'll start putting jumper wires on the top of the board.  From
there, it's only a short jump to wanting to do a double-sided board.

The tradeoff?  Well, putting traces both top and bottom can cut your design time
considerably, because you spend less time trying to snake leads around some
torturous path from here to there without crossing another lead.  You can always
just run your problem trace on the other side of the board.  You'll see a lot of
this on commercial boards: traces that stop and switch over to the other side
of the board two, three, or four times before they get to where they're going.
Being able to do this makes it easier for the designer, but tougher on whoever
is fabricating your finished board.  In particular, if you're etching your own
board, you probably won't be able to make "plated-through holes", where there is
metal between pads on the bottom and top.  Without such plating, you HAVE to
solder leads on BOTH sides of the board if you need the signal to get to both
sides: this can be very difficult to do with many integrated circuit sockets.
At the UN-L E.E. Shop, we try to stay with single-sided designs unless we have a
large number (30 or more) of jumpers going on the top side.

Commercial boards don't stop at double-sided any more, either: many of them,
especially computer boards, actually have additional layers INSIDE the board.
(The board is made by laminating very thin circuit board layers into a single
piece.)  Usually, these internal layers will be used to make a ground plane that
takes ground to all appropriate pins; similarly, there will often be a layer
dedicated to getting 5 volts to all the chips.  This makes a board designers job
even easier, but it makes production by anything less than a professional
fabricator pretty much impossible.

OK, OK, But How Do I Draw The Board?
No sweat.  Use the menus or command line to get to the OUTLINE layer, draw the
outline of your board; go to the PADS layers and use the predefined blocks to
drop your IC sockets and other component pads where you want them; then go to
the BOTTOM layer and use the PTRACE menu to hook up wires from pad to pad.
Voila, you're done!  Right?

Well, almost.  Actually it's not much more than just that.  It's just that it
can take a lot of time trying to get the darn traces from Point X to Point Y
without crossing each other.  And how do you decide where to put your chips?
And what about running traces between pins?  And on, and on . . .

As far as chip placement goes, you have to have a good idea of how your circuit
is wired.  If you don't have at least a scribbled schematic with the pin numbers
of your chips labeled on it, you're really going to be groping in the dark.
Really, component placement is just a mixture of good common sense, a good eye
for topology, and a computer video game player's passion for solving problems.
(Being good with mazes helps, too!)
Try starting with obvious things: for example, most 28 pin DIP memory devices
have similar pin-outs that facilitate having them sit all in a row.  You're
probably going to want to have them as close as possible to the CPU, if this is
a microprocessor board.  What side of the CPU does the data buss come out of?
You're trying to make the simplest, shortest, and most direct connection between
devices that have to be connected.  You're also going to want to keep your
analog and digital sections of your circuit seperate from each other when you
can, to keep digital noise out of your analog circuits.

Aside from that, you can make your own rules about the layout.  Sometimes you
have to "break the rules" in order to get everything routed.  For example, it's
a common sense practice to have most of your chips oriented the same way, with
the notched ends all pointed the same direction - it's logical and looks good;
but I've had to put the chips in "backwards" before just because that was the
only way to get the traces routed in a straightforward way.

Which Traces First?
It's a good idea to take care of some connections before others.  For example,
on our hypothetical microprocessor board, you're going to have a keen interest
in where the data buss lines have to go, because they have to go a lot of places
and they all should go there together (unless you want to route each one
individually.)  More obviously, how are you going to get power and ground to all
of your chips?

This is a point where the multi-layer people have it good.  They can forget
about worrying about power and ground because they have entirely different
layers to deal with those.  But when you're struggling to route a single-sided
board, you'll find that those darn power leads seem to be in the way every time
you're trying to place a signal trace someplace.  Yet most design guides say to
run power and ground first!  What do you do?

I've taken to running nice fat power and ground traces more or less around the
outer edges of the board, then using jumpers on the top to bring them over to
the chips.  This eliminates some of this difficulty.  And you will find that
after all is said and done and drawn, that you'll be able to make some of the
power and ground buss connections on the bottom with traces.  It's just that I
feel that if I'm going to have to use a few jumpers here and there anyway, I'd
rather use them on power and ground to simplify my life, instead of having to
jumper, for example, all eight data buss leads over a power supply trace.

Many times you have to work in tight spaces, ESPECIALLY if you have to run a
trace between two pads that are 100 mils apart.  At that point, you have to go
to a Fine trace, or you can end up with traces and pads that look like they have
space between them when you're zoomed in close on the screen, but which will end
up touching when you print or plot the thing out, or have a negative made of
your drawing.  When you are trying to run leads between pads, it's almost
certain that you'll have to use the 60 mil width pads (OP60, SP60, RP60) and the
13 mil Fine trace. [I've seen professional CAD packages that claim to be able to
put two or even three traces BETWEEN two pads that are on 100 mil centers; fat
chance.  You'd have to have awfully skinny traces and mighty tiny pads, which
may be possible with professional boards but is an invitation to frustration and
no-functionality with "amateuer" boards.  Even if you manage to produce the
extremely high-resolution output needed, you'll have traces that break easily
and peel up when you solder to them.]

For running power and ground leads, using wider traces is advisable.  I often
use the Wide trace for this, while the Power width is so wide that I generally
reserve it for use in those big fat power and ground busses that I run around
the periphery of the board.  Again, this is all pretty much common sense stuff.
Not enough width choices on the menu?  Enter TRACE from the command line and it
will ask you for the width first, defaulting to the width of the last trace if
you just hit <Return>.  Think you used the wrong size?  The "Edit" item under
the PTRACE menu (which executes a PEDIT command) will let you change the width
of an entire trace after the fact, which is nice.

How About Some Extra Caps?
If you weren't already aware of it, it's a standard practice with circuit boards
using logic chips to place a small (.01 to .1) "despiking" capacitor from power
to ground of every chip, AT THE CHIP.  Even with a nice solid five volt supply
attached to your board, power often has a long way to go to the chips, sometimes
down some very skinny traces.  The resulting added lead resistance means that
"spikes" or fluctuations can occur on the power supply right at the chip as
devices switch or change their current demand.  This can lead to all sorts of
really, really frustrating and untraceable malfunctions.  Do yourself a favor;
despike everything you can.  In addition, I will often add one small (10 to 100
microfarad) electrolytic cap across the power supply to ground on the board,
often at the point that is farthest from where power connects to the board.
This helps to keep the power supply solid and smooth.

Making Changes
Unless you're making a very simple circuit on a very large board the odds are
that at some point in your drawing, you're going to have to make a lot of major
changes.  The chip layout you chose just doesn't get enough leads close enough
to where they have to be; or the circuit is too large to fit on the board you've
chosen; or any other of a number of things can happen.  In any case, this is
where using CAD to draw the board absolutely beats anything else hands down.
Want to move a whole chunk of the circuit to another spot?  Enter MOVE and
select the parts and just drag them where you want them.  Have a part of the
circuit that is duplicated several times?  You can use the COPY command to make
multiple copies of anything and drop them wherever you want them.

The only bad thing is that if you do start moving things around, you're going to
end up having to erase a lot of traces and redraw them.  Unlike real electronic
CAD packages, the traces you draw with AutoCAD won't "rubber band", or stretch
and contract to stay connected to the pads.  You've just got to draw them over.
However, you can do some moving of the trace corners with the PTRACE menus
"Edit" submenu (really the PEDIT command.)

There isn't enough space here to explain all of the many things AutoCAD can do
to modify your drawing, like ROTATE parts, CHAMFER traces, SCALE structures up
and down, etc.  Again, make liberal use of the HELP command and the AutoCAD
manuals and you'll find a wealth of commands that can do just about anything you
have in mind.

OOPS . . .
And above all, check out the OOPS and UNDO commands, which can back you out of
even the most catastrophic mistakes with ease.  This will save you many near
heart attacks and spare the world a lot of harsh and ugly language.

                       PRINTING, PLOTTING, AND PRODUCTION

Producing your finished drawing is where things get crucial.  It's also where
AutoCAD shines, because A) it's a vector-based drawing package and will
reproduce your drawing at the highest resolution of your printer or plotter; B)
it supports a vast variety of output devices; and C) it can be made to output
your drawing to exactly the correct scale.

If you just want to get a rough-and-ready hard copy, you can use just about
anything to print out the drawing.  However, if your intent is to obtain
camera-ready output that can be used to create a photographic negative, such
as would be required to expose a negative-photo-resist copper circuit board,
you're almost certainly going to need either a plotter with very fine output
resolution (150 dots per inch or better) such as a laser printer; or you will
need to use a pen plotter.  We'll discuss both those options in a moment, but
first let's look at some other considerations.

Mirrors, Scales, and more...
As mentioned earlier, it's most common (and AutoCAD-PCB assumes) to draw printed
circuit boards from a top view, as if looking at the bottom traces through a
glass board.  But when it's time to print out the bottom traces and pads to make
a photographic negative, you need a mirror image of the drawing.  This is easy
to do with AutoCAD, although it can take a little time if it's a complex
drawing.  To keep from making any non-recoverable mistakes in this massive
alteration of the drawing, I generally exit to the DOS command line and make a
copy of my drawing file under a different name to do the mirroring with.  (EX:
C> COPY MYFILE.DWG MIRROR.DWG)  Once you have your drawing on the screen, enter
the command MIRROR <Ret>.  When it asks you to select the objects to mirror, you
can select your entire board by entering "W" (for Window) and then bracketing
the whole board with a window.  You can hit <ret> indicate that you're done
selecting objects to mirror.  AutoCAD then asks for the first and second points
of a mirror line; this is the line around which the drawing will be mirrored.
If you want to keep both the original drawing on screen and have the mirror
version next to it, pick a mirror line outside of your drawing of the board.  If
you want to mirror the drawing and have the original view deleted, you can pick
a mirror line that's right down the middle of the board.  AutoCAD then asks if
you want to delete the "old objects", by which it means all the stuff you're
trying to mirror.  Again, if you want to keep both the drawing and it's mirror
image, reply "N", but if you're mirroring the board "in place" by putting a
mirror line down the middle, you'd better answer "Y" or you'll have a very, very
big mess on the screen.  When you hit return, the program will churn away and
after a while (depending on the complexity of your drawing and the power of your
computer) you'll have your mirror image.  You may have succeeded in mirroring
the image right off the edge of the screen; if so, you can see everything you've
got by using the ZOOM EXTENTS command.

Now you have a view of the board from the bottom, perfect for making a negative
for the bottom.  However . . . you've probably still got some things like
component edges, and labels, and top-side traces or jumpers, none of which you
want to see on a drawing you're going to use to make your actual negative.  This
is where the use of layers gets very handy.  You can turn your TOP, LABELS, and
PARTS layers off with the menus or from the command line, and all you'll see are
the PADS and BOTTOM and OUTLINE, which is what you want.  Incidentally, before
you start printing or plotting, you'll also have to make sure you have FILL
turned ON and do a REGEN so that it will output nice solid lines, not just
outlines of your traces.

Obviously, if you're going to make a negative for the TOP of the board, you
don't have to mirror it.  You can just turn off the BOTTOM and PARTS and
LABELS layers and you'll be ready to go.  (Leave PADS on, though.  The TOP and
BOTTOM share the solder pads layer.)

Printers and Plotters
If you are trying to make a hard copy that will become a photographic negative
(or positive, if you're using positive-resist circuit boards), the whole idea is
to get output that is A) as FINE and SHARP a resolution as you can possibly get,
and   B) as UTTERLY, SOLIDLY BLACK as you can manage.  There are ways to enhance
both your resolution and your contrast, if this is a problem, as we'll see.  But
first let's look at some straightforward ways to get our artwork.  Please note
that again, you may want to have access to AutoCAD manuals to help you if you
need to change the configuration of AutoCAD to handle a different output device,
or to change the way it uses that output.  This is done with the "Configure
AutoCAD" command (5) available when you first start AutoCAD.

Laser Printers
Laser printers can give you both sharpness and blackness. With plenty of toner
and at 300 dots per inch, you can get camera ready, 1:1 artwork from a laser
printer.  However, please note that some Laser Printers, especially older HP
LaserJets, don't have enough memory to print an entire 8.5" by 11" page at
300 dots per inch.  In this case, you either have to keep your drawing size
to less than half a page (which is frequently possible), or you have to
run the printer at 150 dots per inch, which you can do by changing AutoCAD's
configuration.

I've been told that you can laser print-plot on vellum, which is translucent
to light, and use it as a positive for positive-resist boards directly,
without transferring it to film.  It's also possible to laser print
with special paper, plastic, and/or toner to make an image that is then
directly transferred to a non-sensitized copper board with a hot clothes
iron.  On someone's suggestion I have even tried this with plain paper and
ordinary toner, with mixed success, mostly on really small items.
I will definitely state that at UN-L's Engineering Electronics Shop, we've found
negative resist boards a whole lot more reliable to work with, as they are
less critical in their exposure and development than positive resist boards.
We HAVE attempted to laser print directly onto the kind of overhead transparency
sheets that are designed for use with photocopy machines.  YOU MUST HAVE THE
KIND OF SHEETS DESIGNED FOR PHOTOCOPIERS OR YOU CAN GET A BLACK, MELTED MASS
OF PLASTIC IN YOUR LASER PRINTER!!!  Anyway, it can work, but generally speaking
the resulting black-on-clear positive image is either not black enough, or may
contain a lot of "pinholes" where it's supposed to be black.  Little irreg-
ularities like that will drive you insane if you go ahead and make a board and
don't realize that pinholes have created traces with breaks in them.  On top of
all that, this does give you a positive image and like I said, we're not really
fond of positive resist etching processes.  BUT . . . it's a tempting way to go.
It might be worth at least a try.

[NOTE: I'll keep referring to "your negative", assuming that you are making a
drawing with black traces on white paper and then having a photo negative made
with clear traces on black.  If you are using a positive-etch board you will
need a POSITIVE film transparency made, with black traces on clear film.  Any
lab that can make one can make the other.  Be sure you get this straight with
whoever's making your "negative."]

Pen Plotters
The best laser printer can meet it's match from even a modest pen plotter.
Pen plotters can give you smooth lines without the slightest hint of the
"jaggies".  However, the user must remember the goals of "sharp and black"
and take some precautions when using pen plotters.  The most important one
is, obviously, to have a plotter pen that's very sharp and has plenty of
ink.  Reasonable results can be obtained with the common disposable felt-tip
plotter pens, if you use a nice new one.  However, for the real McCoy, try
to find a steel-tipped ink plotter pen that you can fill with India ink.
These are like fine-point drafting pens and give superior consistency of
line.  However, they're not always easy to find and they aren't cheap.  But
if you plan to do a lot of this kind of work, you won't regret getting one.

A nasty byproduct of plotters, however, is the possibility of the ink lines
spreading or smearing.  If you use ordinary paper, perhaps a sheet from your
computer's fan-fold printer paper, you're going to see your lines bleed all
over the place.  You need to find paper that's good and "hard".  There is
drafting paper available that has this quality; also, you'll find that a lot
of the inexpensive photocopy paper these days has one "hard" side for use
with copiers and laser printers.  You can actually feel the added smoothness
of the hardened side.

What If My Printer or Plotter Isn't So Great?
As we'll discuss in a moment, the general practice is to plot or printer-plot
your drawing out in the actual size, so a simple contact photo negative can be
made at a 1:1 ratio.  However, if your output resolution isn't so great - a
laser or dot matrix printer that's plenty black but only 150 dpi or so - you can
get around it by making your output exactly twice as large as what you'll need.
You then tell the people making your negative to shrink your image down by
EXACTLY half.  This is a common practice in professional manufacturing.

If you are having trouble getting the image black enough, try taking your
print or plot to a photocopy machine and duplicate it on that.  Maybe even
copy the copy, if need be.  This can sharpen and blacken your image, but it
can also lead to extra spots, holes, and other degenerations, so examine
your copies carefully.  You may need to touch them up by hand with a black
pen.

How about combining the last two suggestions at once - using a copy machine to
reduce your image in half while at the same time making it blacker?  Good idea,
EXCEPT . . . photocopier optics are not designed to give you PRECISE and EVEN
reduction or enlargement.  You'll probably end up with things that don't really
line up, which is disasterous when ICs and other parts require precise .1 inch
spacing.  You can give it a try, but make sure you set some of your parts onto
the output to see if it's actually the right size before you run off to have a
negative made.  This is a good idea regardless of how you print or plot your
drawing.

Here We Go ... Ready to Plot!
OK, having waded through all that, you're now ready to actually plot out your
drawing.  You can either choose Printer Plot a Drawing or Plot a Drawing from
the list of choices that appears when AutoCAD is first run; or you can enter
PRPLOT or PLOT from the command line if you are still editing a drawing.

AutoCAD will ask you just what you want to plot.  "Display" plots everything
that happens to be on the screen at the moment.  "Limits" plots to the limits of
the drawing, which we set to the default of 8.5 by 11 inches.  "Extents" only
plots what's inside of the farthest extent of the actual lines and artwork in
your drawing, i.e., everything.  "Window" lets you bracket a chunk of your
drawing and just plot it, which is useful if you're trying to plot just the
mirror image of the bottom you made, or you're trying to keep the area plotted
to less than half a page because you're using a memory-starved laser printer.
"View" refers to any particular views of the drawing you may have saved with the
VIEW command.

AutoCAD will then put up on the screen all of the print/plot options currently
in force and ask you if you want to change anything.  Generally speaking:

I've had very inconsistent results with plotting large drawings to a file
instead of directly to the printer: sometimes it works perfectly and is an
easy way to transport your output to a different machine that has a better
printer but doesn't have AutoCAD, but sometimes the resulting print has flaws
in it.

The size units should be inches.

The Plot origin can be 0,0.

The Plotting area should match whatever paper you're plotting on, usually
8.5 by 11.

With printer-plotting, you generally DO rotate 2-dimension plots 90 degrees;
with pen plotters, usually not.  It depends on your drawing.  Try it and see.
If you are printer-plotting on a LaserJet with 500k RAM you may want to NOT
rotate your drawing so it can all fit in the top half of a 8.5 x 11 inch paper
and thus be printed at 300 dots per inch.

Hidden lines should NOT be removed.  This is a 2 dimensional drawing that
shouldn't have any hidden lines.  If you answer yes, your computer could go
away for a very, very long time trying to hide some of your layers.

+==============================================================================+
|                            AND THE BIG ONE . . .                             |
| The scale of the drawing.  IF YOU WANT AN ACTUAL SIZE OUTPUT, THE SCALE OF   |
| PLOTTED INCHES = DRAWING UNITS MUST BE 1=1000.  If you want a double-size    |
| output so they can "Shoot it down" photographically by 1:2, you should give  |
| a scale of 2=1000 or 1=500.                                                  |
+==============================================================================+

However, if you're just plotting out a copy to look at, not etch, and you want
it nice and big so you can see all the details, you can answer "F" or "Fit" for
the scale, and AutoCAD will (theoretically) make the drawing fit your piece of
paper.  BUT . . . for some unfathomable reason, it seems that as often as not
when you tell AutoCAD to make the drawing "Fit", it will then come up and say
that the drawing will exceed the limits of the paper.  Real useful command,
right?  To this day I don't understand this.  The way to get around this is to
tell AutoCAD to plot an area larger than what you actually need plotted, for
example, tell it to plot everything inside a window, but then make sure you
include a wide margin around the thing you want to plot.  Then, if AutoCAD tries
to scale it to FIT and says that it'll be losing some of the drawing, it's just
going to lose some of that blank margin.

I've Got My Nice Sharp, Black Drawing - Now What?
Now you've got to mull over your options.  There are PC board labs that will
make your board for you if you just provide them with the artwork you've
created.  (And if you provide them with suitable quantities of cash.)  If you're
just producing a single board, you may find out that this is a pretty expensive
way to go, because there are set-up fees, and negatives to make, and possibly
minimum orders to fill, so the first board or boards end up costing quite a bit.
However, if you're making a whole lot of them, this is well worth looking into.
After the initial costs, most PC board outfits can then crank out large numbers
of your board at a very modest cost.  This is especially nice when they offer
such things as drilling out all of the holes, screening of labels or solder
resist, and plating-through the holes.  If you're going into limited production,
do check this out.  But many times, you just want one or two copies of your
board.  At this point, you should look into other options.  Check the ads in the
back of electronics magazines, check your local papers, ask around at Radio
Shacks, read the Yellow Pages, and see if there isn't a small business or local
hobbiest who will produce single boards or small quantities for a reasonable
cost.

If you're going to make your own PC board using a photo-negative-resist process,
you need to find someone to make you a nice, HIGH CONTRAST negative from your
artwork.  Our Shop uses the University of Nebraska-Lincoln's Photographic
Productions lab.  The kind of photo shop that just cranks hundreds of rolls of
color print film through a machine in an hour is probably not going to know what
you're talking about, but there are many other commercial places that will.  Try
custom photo printing places, professional camera stores, or even your local
professional photographer, who may do his own darkroom work.  One of these
places should be able to either help you or steer you to someone who can.

Once you've found this marvelous individual, tell them you need a HIGH CONTRAST
negative made.  If your drawing is actual size, make sure you specify that it
must be 1:1.  If you've made a double-sized drawing, make sure they know it must
be reduced by EXACTLY 2:1.  Emphasize that the black areas must be as solidly
black as possible.  These people aren't dumb: explain just what it is you're
doing and they'll understand the need for precision and high contrast.

And Then ? . . .
Once we get to exposing, developing, and etching the board, things get a little
less certain because there are different kinds of boards and different kinds of
chemicals.  Most photosensitized boards that you can buy locally will include
instructions regarding how long to expose them, and how to develop them.  Please
remember that sometimes these instructions are enclosed in the light-tight
package the circuit boards are sold in: DON'T OPEN THE PACKAGE IN THE LIGHT!
While PC boards are not as sensitive as photographic film, it doesn't take much
light to "nuke" your board and make it unusable.  Open the package in the dark
or in a safe-lighted room.  Sometimes you can buy the board and enough developer
to finish it all in a single inexpensive kit.  This is handy because you're sure
you've got the right stuff for the job and you don't have to invest in more
chemicals than you're going to use.

The procedure for exposing most boards is pretty much the same: you clamp your
negative or positive on top of the PC board in a dark room, then expose it to
ultraviolet light for a while.  The UV light in common flourescent bulbs will
expose many boards in 20 to 45 minutes.  It's better to get real UV lamps,
because you can cut your exposure time down to about two minutes, and because
fast, high-intensity exposure seems to be more forgiving of the quality of your
negative than slow, low-intensity exposure.
------------------------------------------------------------------------------
BE CAREFUL - SOME TYPES OF UV LIGHT ARE EXTREMELY HAZARDOUS TO THE CORNEAS
                                OF YOUR EYES!!!!!!!
------------------------------------------------------------------------------
Oh, and one major, major caution: MAKE SURE YOU PUT THE NEGATIVE ON THE RIGHT
WAY.  We've seen a lot of boards expose, develop and etch beautifully and then
discovered that the pattern was backwards because the negative was on upside
down.  How do you avoid this?  PUT TEXT ON YOUR TRACE LAYERS, remembering to
make it BACKWARDS on the bottom so it's forwards when you mirror the bottom.
When you expose the board, make sure you can read your text forwards.

The chemicals for developing and etching the boards are available locally
and also include instructions on how to use them.  Follow the instructions
religiously, as many of the chemicals involved in these processes are REALLY
NASTY to breath and/or touch.  Use good ventilation if you value your brain
cells and lungs.  And keep the etchant off of your hands or clothes - you won't
notice it at first but then your skin will start to burn.  Ouch.  Also, not only
will used etchant make indelible stains on your clothes but you'll find the
cloth starts to disintegrate when you wash it.  The most common etchant is some
nasty stuff called ferric chloride; if you can find it, try to get yourself some
sodium persulfate etchant.  Sodium comes as a powder you mix with water, is
transparent so you can see your board etch more clearly, and turns a nice bright
blue as it becomes saturated with copper so you know to throw it away.  (NOT
down your drain unless you want to eat holes in your plumbing.)
------------------------------------------------------------------------------
ONE MORE TIME: PRINTED CIRCUIT BOARD DEVELOPMENT AND ETCHING INVOLVES CHEMICALS
THAT CAN CAUSE SERIOUS INJURY IF INHALED, INGESTED, OR HANDLED IMPROPERLY. USE
* ALL * SAFETY PROCEDURES SPECIFIED BY THE MANUFACTURER AND KEEP ALL EQUIPMENT
AND MATERIALS SECURE FROM ACCESS BY CHILDREN OR OTHER NON-QUALIFIED PERSONS.
------------------------------------------------------------------------------

Our Little Advertisement . . .
Making the board sound a little daunting?  Just want to draw it and print it and
have some other poor fool play in the darkroom with the toxic stuff?  If you
are a UN-L student, staff, or faculty member, you should know that the UN-L
Engineering Electronics Shop has the facilities to etch PC boards if provided
with a negative and the photosensitized board.  The EE Shop tries to keep a few
small boards in stock to sell if you haven't got one you've purchased elsewhere.
We will expose, develop, and etch, and optionally tin-plate your board, for a
modest fee.  We have the necessary chemicals for developing negative-resist
boards; if you want to use a positive-resist board, you'll need to also provide
us with the chemicals for that board.  It's not uncommon for such chemicals to
be packaged in small kits,or bundled with a board, for the production of just
one PC board.

The EE Shop will NOT drill out the holes on your finished board.  It's hard to
overstate the amount of time required to drill boards - go ahead, count the
number of holes on your design!  Even a small board, such as a microcontroller
circuit, can end up with 400 to 1000 holes!  To drill the holes, it's best to
have the use of a drill press.  Even a drill press that just has a hand drill in
a movable clamp will work.  You'll also need a number of small drill bits,
ranging in size from #60 to #70 or so.  YOU NEED MORE THAN ONE, because YOU WILL
end up breaking one at some point.  The EE Shop WILL permit you to use our drill
presses, BUT you have to provide your own bits.  Also, as mentioned earlier, we
don't have the means to "plate-through" the holes on a double sided board.

THIS OFFER TO SERVE AS A BOARD ETCHER DOES NOT EXTENT OUTSIDE THE CONFINES OF
THE UNIVERSITY OF NEBRASKA - LINCOLN.

Closing comments:
In searching for a CAD tool for electronic design that was available to our
undergraduates, we've recently been evaluating the PADS software shareware
edition and found it has considerable advantages over using AutoCAD.  Still,
our tools may fill a niche where people already have AutoCAD installed.
If you are knowledgable about AutoCAD, you'll see that creating these tools
was not enormously difficult, although it WAS very time - consuming. Every time
I use them, it seems I find something I could have done better, or I think of
another predefined block I could have added; but I had to quit at some
point.  As I mentioned, I don't intend to add to these tools, leaving that
for others to do.  If you want to drop me a line, I'm accessible on the Int-
ernet at  [e-mail] or [e-mail].  HOWEVER: I WILL NOT
serve as an on-line substitute for an AutoCAD manual, and I'm not interested
in tutoring anyone in the basic principals of AutoCAD when that information
is quite available elsewhere. If you don't have a manual or access to one,
you're probably not using a legal copy of AutoCAD!

Our shop is also a good source of general advice regarding various methods of
prototyping, circuit design, and other neighborly advice.  Stop by and see us
some time.

Paul Marxhausen
Electronics Tech III
Engineering Electronics Shop
Mail:     209N Walter Scott Engineering Center
Location: 122 Walter Scott Engineering Center
University of Nebraska-Lincoln
Lincoln, NE 68588-0511
Internet Email:   [e-mail], [e-mail]