ProfitPress Mega CDROM2 …eeware (MSDOS)(1992)(Eng)/ProfitPress-MegaCDROM2.B6I/APPS/CAD/PADSPCB.ZIP/MANUAL.PCB

Text File | 1992-01-16 | 70.6 KB | 2,169 lines

INTRODUCING PADS-PCB


Welcome to the PADS-PCB Evaluation Package. It
has been prepared to introduce you to the most
powerful low-cost PCB design system you can
buy for your personal computer--PADS-PCB.
PADS-PCB is the best price/ performance
solution to the cost of designing circuit
boards.  PADS-PCB is easy to learn and use--so
whether you only occasionally design PCB's or
you spend full time at it, PADS-PCB can help
you. Many people have a difficult time
believing that a CAD system that sells for so
little can really be so powerful.  We know  it
can, and want to convince you also.   That's
why we created the PADS-PCB Evaluation
Package.

If you've ever evaluated CAD before, you are
probably tired of demo disks.  Don't worry,
this is not another demo!  Instead, it is real
working software, with all the capabilities and
outputs of the actual software. The only limit
is that the  PADS-PCB Evaluation Package is
limited to designs of about 30 IC's. The
Evaluation Package includes some sample
designs to teach you the basic operation of
PADS-PCB.  Once you are familiar with the
operation, you are free to use PADS-PCB to
design your own boards, using the 6000 parts
included in the library.

You  can use this Evaluation Package together
with the PADS-Logic Evaluation Package. You
can start with the net list database from
PADS-Logic, and can see how changes in the
schematic  can be automatically transferred
to PADS-PCB.

The installation instructions for loading the
software  are given in the Installation manual
located at the front of this manual. If you do
not have a printed copy of this manual, the
instructions are located in the file
INSTALL.DOC, located on this disk.



USING PADS-PCB


The Evaluation package can be run as either an
automatic self-running demonstration, or as an
interactive design tool.

Running  the Self-Running Demonstration

To start the automatic self-running
demonstration:
1)    Make the \PADSDEMO directory your current
directory by typing:
    CD \PADSDEMO<CR>
2)    Then type:
    PCBDEMO<CR>

The PADS-PCB self-running evaluation will
start. This is an automatic program that tells
you about PADS-PCB while running the actual
software. The self-running evaluation shows
the primary features of PADS-PCB with a series
of pop-up windows and demonstrations.  It is
designed to give you a quick overview of the
PADS-PCB features, as you view the graphics.
Several comments:
o To pause the self-running demonstration,
press the space bar.
o When you are ready to continue again, press
the space bar again.
o Message windows will be displayed for a
fixed amount of time and are then removed to
continue. If you wish to proceed faster,
select any key other than the space bar.
o To exit from the self-running
demonstration, press CTRL-X.  (While
depressing the CTRL key, select X).This will
return the program to the interactive software
discussed below. You can exit from PADS-PCB by
pressing ALT-X.  (While depressing the ALT
key, select X.)


Running the Interactive PADS-PCB Program

Most users will want to work with the software
to evaluate the features of PADS-PCB. To start
the interactive portion of the PADS-PCB
evaluation
1)    First make the \PADSDEMO directory your
current directory by typing:
    CD \PADSDEMO<CR>
2)    Then you type:
    PCBS<CR>
    to enter the program directly, or you can
type:
    PADSGO<CR>
    to enter the PADS Command Shell, used to
select one of several PADS design programs.
To enter the PADS-PCB program from the PADS
Shell, place the mouse cursor over the box
labeled PADS-PCB and select it with the
left mouse button.

The PADS-PCB copyright notice and the message:
Press any Key to Continue
will appear.  Press a key and PADS-PCB will
load into memory and you can start designing.

Should you encounter any problems, call your
local dealer or, in the U.S.A., call our
Technical Support Hot Line at [phone].




USING PADS-PCB


You should  begin your use of PADS-PCB by
becoming acquainted with the graphical user
interface of the software, and the basic
operation of the system.

The Graphical User Interface

The initial screen presentation is divided
into 4 main sections: the Working Area, the
System Information Window, the Command Menu
Window, and the Prompt Line.

The Working Area is the large black area that
fills the major portion of the graphic screen,
not occupied by menus and the prompt line.

On the left side of the screen is the System
Information Window and the Command Menu
Window.

The System Information Window displays the
following information (from the top):
o Cursor Position    The  X  and  Y position
of the cursor with respect to
the system origin (0,0).
o Grid XX    The user grid in thousands of
an inch.
o Level N    The current layer of the
design
o Width    The current width for all
traces and lines
o Job Name    The design job name
o "Postage Stamp"     Locates the position of
the window relative to the
circuit board.
o  Menu Path    This  multi-line title window
lists the path for the
current menu.

Below the System Information Window  is the
Command Menu. This displays  the command
options available in the current menu. These
commands are mapped to the function keys F1
through F10.

At the bottom of the Working Area is the
Prompt Line. This is the primary means of
communication between you and PADS-PCB.
Potential error messages are also displayed
here.

Changing the Grid and Layer

PADS-PCB has a system grid of .001". You have
the freedom to place components, route traces,
or define the board outline to the nearest
.001".  However, working on a .001" grid is
often not important and, in fact, can be
annoying.  What is needed is the same
reference used in manual PCB design - a grid.
The Grid parameter provides you this, only our
grid is better than your manual grid because
the computer's accuracy insures  you stay
exactly on the grid you select.  You can
change PADS-PCB's  grid from .025" to .100" or
to .200", or .093"--simply by typing a new
grid value.

The grid is currently set to 100 mils. Move
the mouse, and you will see the cursor move
and the X Y coordinate values update in 100
unit (.100") increments.  Type:
G10 <CR>
You will see the Grid parameter in the System
Information Window change to 10. When you move
the mouse, movements will be in 10 mil
increments instead of 100 mils, as indicated
by the Cursor display.  You can also set the
grid to a metric value, so that you can work
in millimeters, rather than inches. This is
done by selecting the Parameters command in
the SetUp menu.

Another important item in the System
Information Window is the Level or Layer
parameter.  PADS-PCB supports boards with up
to 30 levels.  You select the level you want
to place an item on by simply typing a new
value for the Level Parameter.  Like Grid, it
can be changed by typing its first letter,
"L",  followed by a value from 1 to 30 (or 0
to put an item on all layers) and <CR>,
indicating the new level or layer you want.
The display changes to the new current layer,
so you will immediately know if you have
entered the correct value.

Selecting Commands from the Menu

PADS-PCB  uses  a  hierarchical  command  menu
structure, which starts with a main menu and
has a series of sub-menus organized for
efficient operation. In the first,  or main
menu, there are nine sub-menus: IN/OUT, SETUP,
CREATE, PLACE, ROUTE, CHECK, ECO, REPORTS and
CAM.  When a sub-menu is selected from the
main menu, the  name  of  that  menu  is
displayed in the System Information Area.  The
command options associated with the sub-menu
will  appear  in  the Command Window,
replacing the commands of the main menu.
Sometimes there is more than one level of sub-
menus, so you must make an additional
selection.  We suggest you look at each of the
menu selections to understand what options are
available.  Menus have been organized to
correspond with the way you work. All
placement functions are in the Place menu, for
example.

Commands are selected  in two ways, by using
function keys F1 through F10 located on your
keyboard, or with your mouse.  The numbers to
the left of the commands correspond to the
function key numbers, and  F10 always is the
EXIT command. To select commands with the
function key, simply select the corresponding
number key.

To select with the mouse, move the cursor over
the command option and select it with the left
mouse button. When a 3-button mouse is
available, menu items can be selected with the
middle button by holding down this button and
moving the mouse. As the mouse is moved, the
highlight bar will scroll through the menu
options. When the left button is pressed, the
highlighted menu command is selected and the
cursor returns to its position in the working
area. The right mouse button always is used to
select the EXIT command.

Loading A Design File

All  circuit board files, or "jobs",  are
stored on your hard disk as individual DOS
files with the extension .JOB.  To work on a
design, you first load the file from your hard
disk into memory.  This is done as follows:
1)     Select In/Out command (F1) from the main
menu.  A new menu will appear, with the
commands of the  In/Out menu.
2)     Select the Job In command (F1).  The prompt
line at the bottom of the screen will
request you to input a file name.  Type:
* <CR>
3)     A pop-up directory lists the names of the
job files supplied with the evaluation.
Place the cursor over DEMO and press the
left mouse button to bring the design file
named DEMO into memory.   We will use this
design to explore the powers of PADS-PCB.

Storing Your Job to the Disk
Designing a complex board will take time.  You
should periodically save the design onto the
disk as a file. To store the design on disk,
follow these steps:
1)    Select the In/Out menu (F1).
2)    Select Job Out (F2). You are requested to
give a file name with the message:
Job output file name (CR=PCB.job):
3)    You should use a unique file name. Type
this name, followed by <CR>. If this file
already exists, you will be asked to
overwrite it.  Your design job is stored in
a few seconds on the disk, while the
Working indicator is displayed.

Windowing Commands

PADS-PCB provides a complete set of window
control commands, based on the numeric keyboard
located to the right of the main keyboard.
(Note: Your keyboard must have NUM LOCK turned
off in order  to access the Windowing Keys.) The
function of each key is as follows:

    Num 1 (End): Redraw the screen
    Num 2 (down arrow): Move the window down
    Num 3 (Pg Dn): Zoom out
    Num 4 (left arrow): Move the window left
    Num 6 (right arrow): Move the window
right
    Num 7 (Home): Show the entire board
    Num 8 (up arrow): Move the window up
    Num 9 (Pg Up): Zoom in
    Num 0 (Ins):  Reposition window with
cursor in center
    Num .  (Del): Start creating a window box

Try zooming in several times to see how much
detail can be seen.  Try the other commands
until you are comfortable with them.  If you get
"lost," selecting the Num 7 key (Home) will show
the whole board. Remember that the Postage Stamp
Window indicates the position of the viewing
window relative to the board.

Assigning Colors to Items

PADS-PCB uses a 16 color palette to let you
set any item on any layer in the design to a
color of your choice. To change the color
assignments:
1)    Exit In/Out to the main system menu (using
F10).
2)    Enter the SetUp menu ( F2).
3)    Select the Display function (F1). When you
select Display, the design disappears and
is replaced by a menu for color selection.
The top row is the palette of 16 colors.
4)    To assign an item on a specific layer to a
desired color, move the cursor on top of
the color and select with the left mouse
button or F1.
5)    You can assign a color to any level of any
item in the database. Select one of the
layer numbers that correspond to the item
whose color you wish to change. A highlight
box of the color selected surrounds the
layer number.  To make an item invisible,
set it to black, the background color.
6)    When you select Exit (F10), the design is
redrawn  with the selected colors.

Note: a short-cut way to select the Display
command is with the macro Alt-D

Modeless Commands

You have already seen two modeless commands, G
for grid and L for level. Modeless commands
are time-savers; they let you select commands
without going through the menu hierarchy. The
following lists all of the time-saving
modeless commands that are available to you in
PADS-PCB.
Sxxx    Searches  whatever  the  user
specifies.   xxx     can  be  a part,   a  part
with  a  specific pin, or     an x-y
coordinate.
T xx yy    Changes current text height (xx) and
width (yy).
C    Select either the standard or full
screen cursor.
Gx    Changes the current system grid to x
mils.
N nnn    Highlight a named trace in the
design.
R n    Show all lines wider than n at their
real width.     All traces smaller are shown as
a center line.
Ctrl PgDn    Cursor position relative to last
selection.
Alt-9    Displays the requested file entered
at the     Prompt Line at your CRT.
Alt-0    Displays the error messages from
PADS-PCB.
Arrow Keys    Moves cursor 1 grid in the
requested direction.     These  arrow are the
separate arrow keys, not     the arrow keys
on the numeric keypad.
Three of these commands require further
explanation, as you will use them often.

Examining Specific Nets
It is often useful to look at a specific
signal, or group of signals in the circuit to
check for cross-talk, impedance, etc.  PADS-
PCB allows you to examine one signal or a set
of signals with all other nets invisible with
a few simple commands.  If you want to see
only power and ground, do the following:
1)    Enter the SetUp menu (F2). Select  Net Attr
(F5).
2)    A  pop-up menu appears in the Working Area.
Three Signal Name entries are listed: --
All--, GND, +5V.  Currently, all three are
marked ON.  Move the cursor over the ON in
the Disp column next to All, and select
(F1). The value in the Disp column marker
next to ALL should change to OFF,
indicating all of the nets with the
exception of GND and +5V will be invisible
when you repaint the screen.
3)    Exit from the command with F10 and you will
see that only the GND and +5V nets visible.

What if the signal you want to see is not in
the pop-up menu? You may select a new signal
to be viewed other than +5V and GND.
1)    If you re-enter the Net Attr option, one of
the menu choices is Add Item (F2).  Select
it.
2)    The message:
Net name to add>
is displayed on the Prompt Line.
3)     DATA1 is one of the signals in the design.
You can highlight it by typing:
DATA1<CR>
4)    DATA1 appears in the pop-up menu with the
Disp value set to ON.  Set  DATA1 to ON
and all the other net names to OFF in the
pop-up menu, and exit with F10 to
redisplay the design.  You will now see
only signal net DATA1 displayed.

The other values in the Net Attr command allow
you to define the routing rules for each net
in the circuit.


Highlighting a Net in the Design
It is sometimes useful to see all the nets in
the layout ,and to highlight  one so you can
visualize it in its position relative to the
other traces. To do this, do the following:
1)     Set all of the nets currently marked OFF to
ON with the Net Attr option.  Exit from the
command.
2)    Type:
N DATA1<CR>
3)    You will see the net named DATA1 change
color and stand out against the other nets
in the layout.
4)    Type:
N <CR>
    to unhighlight the net.

Defining the Dot Grid
The Dot Grid is a convenient way to help you
measure distance.  Note that the dot grid is
independent of the system or snap grid, and
changing it will not affect the system grid.
You may change it as follows:
1)    Enter SetUp (F2)
2)    Select  Params (F4)
3)    The cursor will flash over the Dot Grid
value. Type in:
 250 <CR>
    to set the Dot Grid to .250".  The dot grid
is redrawn and spaced at .250",  rather
than 1.0"  intervals.

Reviewing the Job Limits

The Shareware version of PADS-PCB is fully
functioning, but the maximum design size has
been limited. The maximum number of parts,
connections, gates, and so forth is limited, to
allow you to do a design with a complexity of
approximately 30 IC's. This limit will vary,
depending on the type of circuit, number of
connections, and other parameters of your
design. If you are doing a design that
approaches this limit, you should check  the
system limits to see how close you are. This is
done as follows:
1)    From the Main menu, select Reports (F8),
then select Job Limits (F5).
2)    Input a file name to the prompt:
Job Limits Status output file name (CR=Printer):
3)    The job limits will be displayed in the
Working Area. For each data type in the
circuit, you will see the current number
used and the maximum number available. If
you reach the maximum number, the software
will prevent you from adding any more
items.



PLACING COMPONENTS


Now that you are familiar with the general
operation of PADS-PCB, it is time to learn the
functions for designing a circuit board.  The
first step in designing a circuit board with a
CAD system is placing the components. This is
a little different from manual design, where
you would normally start by placing some
components, route them, place more components,
continue routing, etc. If you think about it,
the reason you work this way is so that you
leave enough room for the routes, and it's
very difficult to visualize if enough room is
there unless you route the traces. PADS-PCB
lets you visualize the interconnection pattern
of the circuit during placement before you
route because you can display the logical
connections between components.  Of course,
you can work the old way; you're just not
forced to anymore.

In this chapter, you will be working with a
small mixed analog/digital board, to
understand the principles of component
placement with PADS-PCB. You will learn the
interactive as well as the automatic placement
commands.

Bring in job PLACE using the Job In command.
The components are scattered around the edge
of the board.  You will be placing these on
the board. Currently all of the components
except the integrated circuits (IC's) are
"glued" in place. This means that they cannot
move until you "unglue" them with the Unglue
command.

Matrices and Group Rotations

You are going to place the IC's on a pre-
defined matrix. From the main menu, select
Place (F4), then Autoplace (F8), followed by
Mat Place (F3).  All of the IC's will
automatically be placed at regular intervals
on the pre-defined matrix.  You also can
create your own matrix.
As you can see, the matrix we created is
better suited to IC's oriented vertically than
horizontally, so you need to rotate them.
Exit back to the Place menu, and select
Rotate (F3).  You can either point at an
individual components, and select it, or
rotate all of them together. Type:
U*  <CR>
and all of the IC's will rotate at the same
time.



One way of determining component placement
quality is by counting the total length of all
connections in the design- the shorter the
total length, the better the placement.  As
the placement proceeds, you can recheck this,
in order to tell if you are improving the
placement.
1)    Select Exit (F10), then  Auto Place (F8)
again, then Net Length (F7).  The prompt
line gives you the current X, Y and X+Y
connection length.
2)    Next, you will reorder the nets to reduce
or minimize the connection length.  Select
Length Min (F6).  This automatically
reorders the nodes in a net to result in
the minimum connection length for that net.
The connection total length is reduced, and
the prompt area message indicates the
"before" and "after" X, Y and total
connection length.
3)    Select Exit (F10) to return to the Place
menu.

Moving Components

Now try moving individual IC's.
1)     Select the Move (F1) command.
2)     Select a component by placing the cursor
over it, and pressing the left mouse
button. The component,  along with its
connections, will be highlighted. The
"Postage Stamp" in the System Information
Window displays the component name, part
type, logic family, and decal name.
3)    As you move the cursor, the component will
follow. You will also see that the
connections follow the component as it
moves. We call this "dynamic rubber
banding."
4)    You can rotate the component with Rotate
(F2).
5)    The component is set into position with
Complete (F1).
6)    Exit (F10) takes you back to the Place
menu.

Placing Components on the Solder Side

PADS-PCB lets you place components on the back
side of the board. Try this.
1)    Select Opposite (F4).
2)    Move the cursor over one of the IC's, and
press Select (F1). The component will
appear to mirror, and will move to the
opposite side, as indicated by the
component outline changing color.

Placing Discrete Components

Next we will place some of the Discrete
components.
1)    Glue down the  IC's.  Select Glue (F5) in
the Place Menu, and type:
U*<CR>
You will see each component highlighted, in
turn.
2)    Make the resistors and the crystal movable
by selecting Unglue (F6) and typing:
Y*<CR>
R*<CR>
This will unglue the crystal and all
resistors.   Move each of these components
onto the board. You use the connection rubber
band to show the IC's to which they are
connected, so you can position as close to
these components as possible.

Using Alternate Decals

PADS has a feature called Alternate Decal
which permits you to instantly change the
physical shape or "Decal" of a part.  For
example, let's suppose you wished to stand
resistor R1 on end, rather than horizontal.
1)    Use  Pg Up to zoom in on the resistor.
2)    Select Move (F1) from the Place menu, then
select R1 with the cursor.  When R1 is
attached to the cursor, select  Alternate
(F5).  The resistor changes to a decal that
represents a "stand-up" resistor.
3)    Select Complete (F1) to set the resistor R1
in place.

Placing a Group of Components

Group placement operations speed up the
placement process. You can define  components,
traces, connections, as a single group
element,  and then move, rotate, delete,
mirror, or copy the group with a single
command.
1)    Using the Job In command , load the job
called GROUP. You will notice there is a
small analog circuit in the lower left-hand
side of the board.
2)    Select Group Oper (F9) from the Place menu.
3)    To define the group, place the cursor in
the lower left-hand corner of the group,
select Define Group (F1), and pull the
cursor until the Analog circuit is enclosed
within the rectangle formed. Then select
Complete (F1), to finish defining the
group.
4)    You are asked if you wish to move track
segments in group not tied to grouped
components. Respond with Y.
5)    Use Move (F1) to move the group around.
While you are moving, only the outline is
displayed.  When you set the group down
with Complete (F1), the components and
traces are redrawn.

Copying a Group
1)    You  can copy the group, by using Copy
(F2).
2)    The copy is attached to your cursor. Move
it to a vacant area on the board.
3)    Set it with Complete (F1). Note that the
system renames the components on the copied
circuit, so that duplicate part names do
not exist on the board.

A group can be saved to disk and used in
another design with the Cut and Paste
commands, allowing you to define a sub-circuit
and repeat it on other boards.

Autoplacement with PADS-PCB

Load the file APLACE with the Job In command.
This is a 20 IC board ,with components not yet
placed.  The two mounting holes, connector P1,
capacitors C1 and C2, and IC U21, have already
been placed in their final location.  We will
use this file for demonstrating some
Autoplacement features.
1)    A placement matrix for the IC's has been
set up.  If you wish to see the matrix,
select Place (F4) from the main menu, then
Auto Place(F8), then Set Matrix (F4), and
you will see the first matrix.  This is
then to be used for IC's.
2)    You control which components are to be
acted upon by the autoplacement commands by
the use of the Glue (F5) and Unglue (F6)
commands.  Any component that is glued will
not be effected by automatic placement. Any
component that is unglued, will be effected
by automatic placement.  To place the IC's,
you must first Unglue only the IC's.
Select Unglue (F6), and then in response to
Select (F1), type:
U*<CR>
3)    All IC's now are unglued, including the
memory chip U21 that is already on the
board.  We want to keep U21 in its fixed
location during autoplace.  To do this,
select Glue (F5)and use the mouse cursor to
select U21.  Insure the part is fixed in
place with Move (F1). You should not be
able to move U21.
4)    From the Auto Place (F8) menu, Select Auto
II (F2).
5)    Select  Initial (F1) to start the Initial
Placement. This command will move all the
unplaced components (IC's) up on the matrix
in an intelligent  fashion.  The placement
command places parts that are closely
connected to the connector or to U21 in a
position as close as possible to these
parts, so that this total connection length
is at a minimum.
     Observe the messages that appear at the
Prompt Line.  In less than a minute's time,
the unplaced IC's are moved onto the board
and placed on the matrix.  Notice that the
discrete components were not placed,
because they are glued down.
6)    All the memory IC's except one have been
placed in the two upper matrix rows.   At
this point, you will use the Swap command
to improve the placement.  The Swap command
will try swapping pairs of adjacent parts
to improve the placement. Select Swap Pairs
(F3), and observe the messages.

Gate and Pin Swapping

You can also use Gate and Pin swapping to
reduce the connection length.
1)     From the Place menu, Auto Place(F8), Swap
Items (F1), then Swap Gates (F2).
2)    The message:
Gate/Pin Swap Report File Name (CR=Printer):
    invites you to give a file name for the
"was-is" report that  is  generated  during
the  swapping  process.   Respond to the
message giving the file the name:
SWAP <CR>
3)     Run Auto (F2) to start the automatic gate
swapping function.  Select Exit (F10), then
repeat the sequence for Swap Pins (F3).
You will find that the connection length is
reduced by these operations.

The Gate and Pin Swap Report file will be used
to update the schematic, using the PADS-Logic
Engineering Change Order (ECO) update
capability.  After the schematic is
automatically updated with the gate and pin
swap information, it will match the board
design.

Evaluating Placement Quality

You have already seen that the Connection
Length command will give you a measurement of
the placement quality. In addition, there are
two other placement analysis tools  in PADS-
PCB that you may use to evaluate the placement
results.  The first tool is the Histogram
command, which will display the density of
connections for each channel in the circuit.
The second is the Connection Density Map,
which displays the connection density in each
area of the circuit, using colors to show the
density of connections, with red indicating
areas of congestion where routing may be a
problem.
1)    From the Auto Place menu, select Auto II
(F2), ConDensity (F5). Select Histogram
(F1), and respond to the
Routing Grid Size (5-250)[100]:
    prompt with:
25 <CR>
    A graph will be displayed across the top of
the board, and along the left side.  The
graphs represent the ratio of "Connections-
To-Routing Channel Ratio" for each 25 mil
routing channel in both the X and Y
Direction.  The peaks in the graph
represent potential routing problem areas.
2)    Select Density Map (F2), and respond to the
prompt:
Density map Grid Size (25-500)[100]:
    by typing:
100 <CR>

In this simple design example , you will not
have a problem routing the connections. In a
more dense board, you would examine the red
areas and try to improve the placement around
them.

Other Placement Functions

There are a number of other placement commands
you can use. The first, Net Attr, is used to
define the rules for defining the connection
pattern for nets. A second,  Connection Bias,
lets you select how the connection length is
used during automatic placement. This feature
allows you to place components:
o Using Minimum Connection Length, or
o Minimum Connection Length, yet biased
against Long Connections, or
o Minimum Length, yet biased against Angled
Connections, or
o Minimum Connection Length, yet biased
against Long Angled Connections.

The Auto Rename command enables you to
automatically rename all of the parts, and
create a file used to update the schematic.
You can define the renaming sequence any way
you wish: Horizontal/Vertical, Right to Left,
Top to Bottom, and rename all components in a
specific type, such as IC's, or all components
on the board.



TURNING CONNECTIONS INTO
ROUTES

In CAD terminology, a "connection" is not a
physical piece of copper etch, but instead
represents a logical signal in the schematic.
It is displayed as a straight line rubber band
between two component pins in PADS-PCB.
Connections are displayed for two reasons --
during placement they will help you see which
components should be near each other; during
routing they show you where your destination
target is, and also when you need to make room
for other routes.

"Routing", whether automatic or interactive,
is the process of converting the logical
connections into physical "traces" or "routes"
either interactively or automatically.  In
this section, we will work with one job at two
different stages, before and after routing.
You will try interactive routing, and then
editing routes.

Interactive Routing of Connections

This exercise is an introduction to the
interactive route options, to get you familiar
with them:
1)    Bring in job  ROUTE, using the Job In
command from the In/Out menu.
2)    You will see the upper left corner of a
small 2-layer circuit board.  The component
outlines are yellow, the pads are green,
and the logical connections are white.
There are no routes yet. You are going to
route - that is, convert some of these
logical connections into physical etch-
these connections.
3)    From the Main menu, select the Route (F5)
command menu.
4)    Place the cursor over one of the white
connections -- try the vertical one
connecting to pin 9 of U1, to pin 5 of U3
on the left center of the working area.
Move the cursor over the connection near to
pin 9 of U1 and select Route Conn (F1).
5)    You will see the white connection
disappear, and be replaced by a short red
route (because you are on layer 2) with a
grey connection at its end.  By moving  the
cursor, you move the red route segment up,
down, left, or right,  at a 45 or 90 degree
angle from the pin. Note the information
display on the left side of the screen,
with the message:
DATA4
U1.9
U3.5
Width 12
    indicating that the signal being routed is
signal DATA4.  It connects pin 9 of IC U1,
and pin 5 of IC U3.  It has a width of
.012".  Whenever you are routing, this
display will give you the route information
to tell you what you are doing. The menu
now gives you a new set of options you may
use while routing.
6)    Next, change layers with Level (F4).  The
routed segment turns blue, which is the
color for traces on layer 1.
7)     Put a corner in the route  with Add Corner
(F1).  You may proceed in eight directions
(90 and 45 degree directions) from this
corner.  Try this. To put the next segment
at any angle, select Angle (F3).  Now the
route segment follows the cursor exactly,
and you can put any angle in the trace.
Selecting Angle (F3) again puts you back
into the 45/90o only mode again.
8)    Select Level (F4) again. You will see the
second route segment turn red, indicating
its back on layer 2, and that a via has
been put at the intersection of the two
segments in the route.  PADS-PCB
automatically puts in vias for you.
9)    Route towards the destination pin, putting
in corners as appropriate. Note that the
grey connection always follows the end of
the route and connects it to the
destination, pin 5 of U3. You can complete
this route only at the correct destination
pin.
10) You can stop the route without finishing
it at the destination by selecting End
(F8).  Try this.  Note the connection
remains between the end of the route and
the destination pin. This is a partial
route. You can go on to route another
connection, or move existing traces to
clear up a block.
11) Put the cursor on the purple connection
part of the partial route, and select Route
Conn (F1) to pick up the route again. Route
it to the destination pin.  To complete the
route, select Complete (F9).  This will
finish the route on the destination pin,
inserting a corner to change direction if
necessary to reach the pin.

Converting a Route to a Connection

You can convert traces back to connections:
1)    Put the cursor on any part of the route you
wish to convert to a connection, and select
Unroute (F7).
2)    The route will disappear, and the following
message will be displayed on the Prompt
Line:
Confirm Unrouting Y/(N)?
    Type Y  or F1 to confirm the process. The
trace is removed and the white connection
is redisplayed. If you type N or F10, the
route will reappear.

Whenever you delete any type of data item, you
will be asked to confirm the process.

Changing the Width of a Route

It is possible at any time during routing to
change the width of a trace. To illustrate
this, at some point  in the middle of routing
a trace,  do the following:
1)    Type:
W75<CR>
    This changes the width of the trace segment
you are currently routing to a new width of
.075". You will see the width change, as
soon as you move the cursor.  Also, the
Global Width display changes to 75.
2)    To change the width back to .012", type:
W12 <CR>

You may change the trace width of any segment
of any route at any time. You have complete
control over every route segment on the board
-- you can neck down, or up as you choose.

You may also change the width of a trace
segment, a complete trace, or a net after it
is routed, with the Line Width (F7) command in
the Modify (F5) option of the Route menu.

Routing Tips to Remember

o I f you make a mistake in positioning a
corner, you can use the Delete Corner (F2)
option to back up quickly.
o You use Angle (F3) to corner at any angle,
not just 45 degree or 90o.
o The Complete (F9) command is used to finish
a trace; it is not an autorouter. It follows
very simple rules to finish the route, and
will finish only on the correct pin.
o To "copper share", you must follow the route
all the way to the destination pin, putting in
corners and vias as appropriate.
o Move the mouse with small movements. Let the
route catch up to the cursor position before
continuing.
o Have connections, traces, and pads, visible;
component outlines and names invisible.
o Enlarge the view so that you see only about
4-8 IC's, not the entire board.
oAs you edit routes, you will "erase" portions
of some of routes and pads. They are still in
the database and you should periodically
repaint the screen by selecting Key 1 (End) on
the numeric key pad.

Modifying an  Existing Route

You will quickly learn that some traces you
have routed need to be changed (or "edited" in
CAD terminology) in order to put in the other
routes.  If you are designing manually, this
usually means heavy use of an eraser, and
possible mistakes when rerouting.

Moving an  Existing Route Segment
1)    Select the Modify (F5) option.  You have a
number of options available. These allow
you to move the traces in a number of
different ways.
2)    Move the cursor over a vertical trace
segment, and select Move Seg (F2). Note
that as you do, the trace changes color and
is highlighted. This allows you to see the
entire net better while you are routing it.
3)    As you move the cursor right and left, you
will see the vertical segment move to
follow the cursor. The route segments that
connect to the vertical segment will also
either extend, or retract so that they
remain connected to the ends of the segment
being moved. You cannot lose connectivity
while routing.  Position the segment where
you want and complete it (F1).

Moving a Via or Corner
Try using the other Modify commands.
1)    Put the cursor on a route corner, or via
and select Move Corner (F1).
2)    As you move the route corner, watch what
happens.  The segments joined by the
corner, as well as the route segments
forming these segments will move  as the
corner follows the moving cursor.
3)    Select Angle (F2).  In this mode, only the
segments forming the corner will move.
Angle is a mode command, so selecting it
again will change back.

Cut Segment
Cut Seg (F3) is interesting.  It will cut a
single segment into 3 segments.
1)    Move the cursor onto a route segment,
choose Cut Seg (F3), and watch what
happens.
2)    In Cut Segment mode, Swap Crn (F3) lets you
move the other portion of the segment you
cut originally.

Reroute Traces
Rather than move corners and segments in a
route, you can  reroute a segment. This can be
somewhat faster to do, depending on the trace
you are moving. Often this will seem more
natural to the first time CAD user, too. You
reroute by doing the following.
1)    Place the mouse cursor on a trace segment
and select Reroute (F9).
2)    The segment of the trace you select will
turn back to a connection and you can start
routing it. Start from the end of the
segment closest to the cursor.
3)    Continue routing the trace until you have
established a new path back to the other
end of the original segment and select
Complete(F9) to finish it. It may take a
couple of times to get use to this feature
but once you do it will be very useful.

Some Hints When Modifying Routes
o Plan what you want to do before you do it.
Try to think about route changes in terms of
the commands in Modify Route.  The most
powerful are Move Corner, Move Segment and Cut
Segment, and Reroute.
o When selecting a trace segment or corner,
select it at an unambiguous point, not where
it crosses another trace.




AUTOROUTING WITH PADS-PCB


PADS-PCB has three autorouting options, PADS-
Route, PADS-PowerRouter and PADS-SuperRouter.
o PADS-SuperRouter is an excellent choice for
complex digital through-hole designs. Based on
rip-up techniques, it is capable of achieving
100% results on complex circuits.
o PADS-PowerRouter is the highest performance
autorouter you can buy running on a Personal
Computer. Using shove as well as  rip-up
algorithms, it is capable of achieving 100%
routing results on most of today's circuit
boards.

Both PADS-PowerRouter and PADS-SuperRouter are
too sophisticated to explain in this manual,
so we have chosen to include PADS-Route in the
evaluation. PADS-Route  includes 3 separate
routers: two specialized, fast routers for
memory and power bussing, and a third general
purpose router for all the other connections.

Using the Power and Ground Router

The power and ground bus router is a
heuristic, or pattern router.  This means that
it tries to route with a predetermined
pattern. This router is useful for digital
boards that do not have buried power planes.
1)    Bring in job ROUTE2.  This board is
unrouted.
2)    From the main menu, select  Route (F5),
then the Auto Route option (F2).
3)    Two messages will prompt you to select the
routing and via grids:
Routing Grid (25) >
Via Grid [0]>
    You should respond to both with
25 <CR>
4)    A new message is displayed:
Select Router Passes (F7) then select Connections to be
routed
    You will first define the autorouting
passes. Select Setup (F7) and use the mouse
to select SHORT P/G in the pop-up window,
then Select Exit (F10).
5)    You  will route the entire board, so select
Board (F4).  This will start the
autorouter, and in the System Information
Window, you will see displayed the number
of connections selected for routing, and
later, information on the router status and
success rate.
6)    Traces will be displayed as they route,
with blue traces on Layer 2, and green
traces on Layer l.
7)    After the autorouter is complete, you are
presented with the results.  The autorouter
has completed about 85% of the power and
ground connections.  The connections it has
routed are excellent quality, probably very
similar to manual routing.  Those it did
not complete either did not fit  the
heuristic pattern, or conflicted with
others.  You might interactively complete
these at this time.

Using the Memory Router

The memory router is heuristic, like the power
router. It is used as follows:
1)    You must first display the connections to
be routed.  From the Main menu, select the
SetUp (F2) menu, and then select Net Attr
(F5). Go to Net Attr With the mouse, select
the display setting for ALL connections,
changing it to ON.
2)    Exit from the SetUp menu. Select the
Autoroute option (F2) in the Route menu.
3)     Two messages will prompt you to select the
routing and via grids:
Routing Grid (25) >
Via Grid [0]>
    You should respond to both with
25 <CR>
4)    A new message is displayed:
Select Router Passes (F7) then select Connections to be
routed
    You will first define the autorouting
passes. Select Setup (F7), select SHORT P/G
again to turn it off, then select SHORT
MEMORY, HORIZ/VERT and SHORT ONLY.  Then
select Exit (F10).
5)    You can route a specific net.  Select Net
(F3).  You will be prompted with:
NET NAME TO SELECT>
    Type J <CR> and <CR> again.  The number of
connections selected is displayed and  the
autorouter will start.  You can watch the
routes being made.
6)    Next route the entire boards.  Select Board
(F4).  The memory traces will be routed.

Using the Maze Router

The Maze autorouter routes two layers at a
time, but you can route multi-layer boards
with up to 30 layers by selecting two layers
at a time.  This router has a number of
individual passes, which will use
progressively more powerful methods to route
the connections.  You might  choose to run one
or more passes at a time, stop and
interactively edit the results, then continue
autorouting.  In this exercise, we will run a
number of the routers at one time.
1)    Continue with the design where you have
just routed the Memory Connections.
2)    Select SetUp (F7).  Turn off, or deselect
all of the  passes from being routed.  Then
select the passes named ONE VIA, THREE VIAS
and FIVE VIAS.  They should be highlighted
as they are selected.
3)    When you are done, select Exit (F10), then
Board (F4) to route all connections in the
circuit.  As the autorouter works, the
finished routes are displayed, and the
results are updated in the System
Information Window.
4)    When the router is finished, most of the
unrouted connections are near the
connector.  You would typically spend a few
minutes editing the routes to finish the
remaining connections.



CHECKING THE DESIGN


The Check commands will automatically check
your entire design for violations of your
minimum spacing rules.  (These are defined in
the SetUp menu).  An effective Check function
is absolutely vital in a CAD system. Without
it, you are absolutely guaranteed to make
either short circuits or minimum clearance
violations. PADS-PCB  indicates violations
with colored markers. The colors for errors
can be assigned by layer with the Display (F1)
command in the SetUp menu.

DRC Violations

You will see how check works in PADS-PCB  in
this exercise.
1)    Load the job named CHECK.  This is an
already routed board.  From the main menu,
select Check (F6)  and then select Spacing
(F1) to begin the spacing rules checking.
2)    The System Information Window will display
the status of the check activity and the
number of errors found.  When Check is
complete, you will see colored error
markers  displayed at the point of the
errors in the design. Each colored marker
indicates an error.
3)    At the top of the layout there is a trace-
to-text error. This is because the trace
has been routed through text placed on
layer one.   Zoom into this area, move the
trace with Modify Route, and rerun the
Check function.
4)    Fix the other trace-to-trace and trace-to-
pad errors and rerun the Check program.
The error markers will disappear, if
corrected properly.

In addition to design rule checking, which is
a check of physical correctness, PADS-PCB also
provides additional checking functions:
o There are three netlist checks, to let you
check the finished design database against the
original schematic netlist.  Net lists from
PADS-Logic, Schema, and Futurenet compatible
systems are supported.
o The Tie Plane check command insures that all
component pins which are part of a net that is
a power plane are correctly connected to the
plane.



PRODUCING ARTWORK
DRAWINGS


PADS-PCB supports a wide range of
photoplotters, matrix printers, laser
printers,  and pen plotters.  The pen plotter
software can be used to produce check plot
quality drawings - useful to give to
Engineering or to help you analyze entire
layouts - and artwork quality drawings which,
when produced at 2:1 and photo reduced, are
suitable as reproduction artwork, helping you
save the cost of photoplotting.

Producing a Drawing on a Laser Printer

This exercise will show how to produce laser
printer outputs with PADS-PCB. The procedure
is similar for all outputs.
1)    Bring in job CHECK. We will use this design
to demonstrate the post-processors.
2)    From the main menu, Select the CAM (F9)
menu.  You will be prompted with:
Specify CAM output sub-directory:
3)    Type in the name for a new sub-directory
under the CAM directory  using, for
example, your initials as the name of the
sub-directory. A new sub-directory will be
created under the CAM directory, and all
output drawing files will go into it. We do
this so that your software and job
directories don't get cluttered with
temporary work files.
4)    You have four options:
    o Direct (F1) creates drawings and artwork
directly.
    o Batch (F2) creates drawing from
previously created CAM files.
    o Defaults (F3) lets  you define the
aperture table, the drill tooling, and
other CAM parameters.
    o Verify  (F4) produces a pen or printer
plot from a photoplotting file.  This lets
you check your artwork file before you
spend money producing a bad plot .
5)    Select Direct (F1).  A new command window
is displayed, and you have the option to
produce photoplotting, pen plot, laser
printer, drill or matrix printer output.
Select Laser Printer with your cursor (F1).
Then select Proceed either with the mouse
or with F2.
6)     The menu display changes to let  you select
the type of drawing you want.  Start with
an Assembly Drawing.  Select "Assy Dwg-Top
Side," with the cursor.  Note that 30
levels are displayed, with Level 1 and 27
highlighted.  This is because Level 27 is
reserved, by convention, for top assembly.
    (Note: Levels 23 - 30 are reserved by
convention for a variety of drawings but
can be used for routing, if needed).
    Select Proceed (F2).
7)     The next menu display lets you choose which
items will be plotted, highlighted in grey.
For each type of output, we have already
provided the typical items that appear on
the drawing.
8)     To change the default plot options, put the
cursor on the Level 1 box to the right of
Text, and select this with Select (F1).
The box will change color, indicating that
text is no longer selected. Select Proceed
(F2) to go to the next menu.
9)     The next menu lets you select the size of
the drawing, rotation, and other functions.
For this plot, leave these settings
unchanged and select Proceed.
10) The last menu lets you store the results
into a file for later plotting, or create
your drawing immediately. To produce a
drawing, select  the label Proceed With
Current Selection with the cursor, then
select Proceed (F2).  The system will be
busy for a short period,  and then begin
plotting.
11) After you have produced the first drawing,
try producing other types of drawings.  You
will see how easy it is.  And if there is a
drawing type that is not a standard output,
you can use the general plot option to
produce custom outputs.

PADS-PCB Reports

PADS-PCB can produce a number of useful
reports from your design database, including
net list reports, an unused gate and pin
reports, board status, and a report about the
design limits. The best way to find out about
them is to produce some reports.
1)    If you have not already done so, load a
design file into memory.
2)    Select the Reports (F8) menu from the main
menu. Print out each of the reports, using
the command options in the Reports  menu to
become acquainted with their contents.  Any
report can be printed immediately, or sent
to a disk file for later review or editing.

The reports available from  PADS-PCB in the
Report menu are as follows:
o Net List  (F1) gives the entire net list for
the design.
o Unused (F3) lists all unconnected parts,
gates, and pins.
o Statistics (F4) provides information on the
number of routed and unrouted connections,
pins, via, board density, trace length, etc.
o Job Limits (F5) indicates the maximum limits
of the system and the usage with the current
design.
o Part List 1(F6) and Part List 2 (F7),
display the parts list in two different
formats.

When a report is selected, a prompt invites
you to type the name of the file to be
created. Type a file name, followed by <CR>
The file may be listed to the printer, or can
be displayed by selecting Alt-9, and giving
the name of the file.



MAKING CHANGES TO YOUR
DESIGN


When you are placing or routing a board with
PADS-PCB, you don't have to worry about
accidentally changing your net list
connectivity. PADS-PCB has built in checks to
make sure you don't destroy that netlist. This
raises an important question, though.
Sometimes you will want to change the design-
how is this done with PADS-PCB?  We have
collected all of the functions that can change
the connectivity and put them into a single
menu, called ECO (Engineering Change Order).

In this chapter you will add a large capacitor
to a design, and connect it to power and
ground.  You will also delete pin 7 of U21
from signal 21.  Finally, you will rename
signal net DA00 to SIGA, and rename component
U10 to U50.
1)    Call up the design 1STLOOK. From the main
menu, select ECO (F7).
2)    Because the changes you make in the board
must go to the schematic, select To Sch
(F1) . The following message will be
displayed:
Output schematic ECO report file name (CR=Printer):
    Respond with a file name, for example
ECOTEST, followed by <CR>. As you make
changes in the design, they are
automatically added to this file.

Adding a New Part to the Job

1)    Select Add Part (F5). Select Keyboard I/O
(F2)
2)    To the prompt:
Name of part type for new part>
    Respond
R*<CR>
3)    The library browse command provides an easy
method to scan a list of components
visually.  A pop-up window is presented.
The bottom half shows a list of parts
corresponding to your wild card command, in
this case all parts beginning with R. The
top half shows the symbol for the currently
highlighted part.  You can use the arrow
keys to scroll through the list of
components, or you can place the cursor
over a part type and press Select (F1) to
view the specific graphical symbols.
4)    To add the 1/8 Watt resistor, place the
mouse cursor over STD: R1/8W, choose Select
(F1), and then Accept (F2).
5)    The system prompts:
Reference designator for new part>
    Respond by typing:
R25<CR>
    The pop-up window disappears and the
resistor will be attached to the cursor.
6)    Move the cursor around and notice how the
part follows. Set the resistor in place
with Complete (F1).

You can also add a part without using the
library browse function.  Next you will add a
capacitor, with the part name CAP\MA20.
1)    Select Add Part (F5). Select Keyboard I/O
(F2)
2)    To the prompt:
Name of part type for new part>
    Respond:
CAP\MA20<CR>
3)    The system prompts:
Reference designator for new part>
    Respond by typing:
C100<CR>
    The capacitor will be attached to the
cursor.
4)    The new capacitor appears in white attached
to the cursor. You are now able to position
the component in the design.  Rotate it
(F2), place it in the layout, and set it
with Complete (F1).

Adding  Connections to the Design

Next you will connect the new capacitor to
Power and Ground.
1)     New connections are added with  the trace
width displayed in the System Information
Window. Before adding the connection, set
width to .050" with the W modeless command:
W50 <CR>
2)     Select Add Conn (F1).  You may either type
the connection or point at it with the
mouse cursor. Put the cursor on a pin in
the circuit that is connected to ground ,
and select it with Select (F1).  Note:  The
component name,  the selected pin, and the
signal name are shown in the System
Information Window. Check to see that the
signal is Ground, and the Ground net is
highlighted.
3)     When moving the cursor, you will see a
brown connection following the cursor.
Move the cursor  to the lower  pin of the
new capacitor and select F1 again to
complete the connection.
4)     You could continue to tie more pins to the
signal with additional selections, but
let's stop here.  Select Exit (F10).
5)    Repeat steps 2-4 to add the Power
connection, +5V, to the capacitor.

You have just added a connection by pointing
at the start and end pins. Sometimes it's
easier to add connections by typing the pins,
particularly if the ECO is in the form of a
list of changes.  Let's see how this is done.
1)    Select Keyboard (I/O). To the prompt:
Starting connection pin - reference designation.pin>
2)    Type:
R9.2 <CR>
    This selects pin 2 of R9 to start the
connection.  The cursor moves to this pin.
3)    To connect the other end of the connection,
select Keyboard I/O(F2) again.  To the
prompt, type:
R4.3<CR>
4)    The cursor moves to R4 pin 3, and the
connection is drawn.  Select Exit (F10) to
complete the net.

You may also add traces, with the Add Route
(F3) command. When this is selected, you have
the same capabilities for defining the trace
path as when manually routing traces.

Removing a Pin from a Net

A typical change order that you might get from
the design engineer is to disconnect a
specific pin from a signal.  In some CAD
systems, this is very difficult to do.  See
how easily this is done, as you remove U21 pin
7 from its net.
1)    First, identify this pin visually.
2)    Select DisConn Pin (F4) from the ECO menu.
3)    Select Keyboard I/O (F2).
    To the prompt:
Pin to disconnect -- reference designation.pin>
     Type:
U21.7 <CR>
    The cursor will move to pin 7 of U21, and
the 2 routes connected to U21.7 will be
highlighted.  You will be asked to confirm
the deletion with the prompt:
Confirm pin disconnection from net Y/(N)?
    When you type Y, the highlighted routes
will disappear, a new connection will be
created, connecting U20.7 to U2.3, the two
pins that were at the ends of the two
removed routes.  Select Exit (F10).

Renaming Nets and Components

Before you change the net name DA00 to SIGA,
highlight the DA00 net by typing at the prompt
line:
    NDA00<CR>
Signal DA00 will be highlighted. This is the
net name you will change.
1)    From the ECO menu, select RenameNet (F3).
2)    Select KeyBoard I/O (F2).
3)    To the prompt:
Name of net to rename>
    Type:
DA00<CR>
4)    The system responds
Old net name is DA00 New Name>
    Type:
SIGA<CR>

Now, rename component U10 to U50.
1)    From the ECO menu, select RenamePart (F7).
2)    Select KeyBoard I/O (F2).
3)    To the prompt:
Reference Designator of part>
    Type:
U10<CR>
    U10 will be highlighted and the prompt
responds:
Reference Designator is U10 New Reference Designator
    Type:
U50<CR>

Listing the ECO File

When all changes are done, exit from the ECO
menu back to the Main menu. You can display
the ECO file by typing:
Alt-9

To the prompt asking for the file to be
displayed, type the name of the file that  you
created
ECOTEST<CR>

The file is displayed. To remove it, select
the Esc key.

Forward Annotation of Changes

It is also possible to automatically update
the PCB with changes made to the schematic.
The From Sch command is used to send a set of
changes made in the schematic to the circuit
board. This list of changes is calculated by
comparing your current schematic with an
existing job file.  Differences are listed as
a series of changes that are stored in an ECO
file and can be used to automatically update
the board. The changes can include: Added
Parts, Deleted Parts, Added Connections,
Deleted Connections, Renamed Nets, Re-named
Parts, and Changed Part Type of Parts.
1)    First, load the design file 1STLOOK using
the Job In command.
2)    You can view the ECO file that will be used
to update the 1STLOOK design, by typing:
Alt-9
3)    To the prompt asking for the file to be
displayed, type the name of the file that
was created.
REV1.ECO<CR>
    The file is displayed. To remove it, select
the Esc key.
4)    Select the ECO (F7) command from the Main
menu. Select From Sch (F2).
5)    To the prompt:
Input schematic ECO file name>
    Type:
REV1.ECO
6)    Then, type an error output file name at the
prompt line to direct all error messages
into this file.
7)    The file is read in, and the design is
changed. You will see the parts added at
the system origin, and the connections
added will appear as yellow lines.

Changing the Size of Component Pads

Parts have pre-defined pad sizes in the
library, which are brought into the design
with the part. You are not limited to these
pads however. It is very easy to change the
shape and size of pads during a design, as the
following exercise illustrates:
1)    From the main menu, select the SetUp (F2)
menu, then select Pads (F2).
2)    You will change pin 1 of the 20 pin IC to
be 80 mil square pad, and pin 2 to be a 60
mil pad with a 39 mil annular hole. To the
prompt:
Name of Part Decal
    type:
DIP20
3)    The current pad definition for the DIP20 is
displayed in a pop-up window. Currently all
pins and pin 1 are listed. For each, there
is a definition for the top layer (T), for
the inner layers (I), for the bottom layer
(B), and for layer 25.
4)    Position the cursor over the box for the
size of the pad on level T of pin 1 and
select (F1). Type:
80<CR>
    to change this value.  Repeat this for the
bottom level B.
5)     You need a new pad definition for pin 2.
Since it is not currently listed, select
Add Pin (F4). To the prompt:
Enter new pin number>
    Type:
2<CR>
6)     The current settings for pin 2 are
displayed. For both the top and bottom
layers, change the value in the SHP column
to A (to make the shape annular), and add a
new value in the column INT DIAM of 39.
7)     Select Complete (F9) to confirm the change.
8)     The design is redrawn with the new pad
definitions for pins 1 and 2.



Creating a PCB without a Schematic


You may want to design the circuit board
without first starting with a net list  or a
schematic.  This can be done in PADS-PCB,
using the On-the -Fly command. With this
command, you can create a board, add parts and
connections. As you work, you will be creating
design connectivity.

1)     Load  the job ONTHEFLY. The board outline
and the connector have been created and
placed in this design.
2)     Select On-the-Fly (F8) from the In/Out
menu. Select Add Part (F5),  then Keyboard
I/O (F2).
3)     In response to the prompt:
Name of part type for new part>
    Type:
7404 <CR>
    A 14 pin IC is added to your cursor. This
is U1, and is a 7404. Note you can rotate
the part  and move it around. Place the
part with Complete (F1).  If necessary,
repaint the screen with the (End) key.
4)     Repeat this step, adding a resistor with
part type R1/4W.
5)     Select Add Conn (F1), to add connections
with the cursor, in the same way as in  the
ECO command.  You must  set the trace width
with the W modeless command before  adding
connections.
6)     You may also add traces, with the Add Route
(F9) command. When this is selected, you
have the same capabilities as you do when
manually routing traces.



CREATING PCB PARTS


You have now completed the evaluation of the
main design features of PADS-PCB. What you
have not seen yet is the creation  of parts.
You can edit library data, add parts quickly,
or delete parts. All parts are maintained in a
powerful database that makes access time under
2 seconds for any part. A part in PADS-PCB
consists of 2 items: a decal of the physical
part, and part electrical data. This
electrical data is shared between PADS-PCB and
PADS-Logic.

Creating a New Part Type

You will already have the decal for most of
the new parts that you will create. This is
because all 14 pin IC's use the same physical
decal, DIP14, no matter what their electrical
characteristics. If this is the case for you,
it is very easy to create a new part, as this
exercise shows. We will create a new
integrated circuit, to be called AM27C256.
This is the same part that has been created in
the PADS-Logic Evaluation Package.
1)     Select the Create (F3) menu from the Main
Menu. Then select Part Type (F6)
2)     Select New Part (F1). To the prompt,
respond:
AM27C256<CR>
3)     Select Part Info (F1) to modify the
electrical information. This defines the
PCB symbol, the part attributes that are
extracted for reports, the default power
and ground pins, etc.
4)     The part info text screen will be presented
and you proceed to fill in all the data
necessary.
    o There is no part type prefix, so this
line may be left blank.
    o The Logic Family  defines the  family
with which the part is associated, i.e.,
TTL, CMOS, ANA (for Analog), etc.  Since
this is a CMOS part, enter:
CMO
    o The PCB Decal entry defines the name of
the physical shape that will be used for
the part in the circuit board. Since this
is a 28-pin DIP IC,  enter:
DIP28\400
    o Part Attributes. You may assign any type
of attributes to a part.  Allocate 2
attribute lines and enter in the
information below in the two lines. Note
that all lines start with a description,
followed by a colon (:).
PART DESC: 32K x 8 bit EPROM
MFG #1: AMD
    (Note: You may want to add new attributes
such as  "Vertical Height," which may be
useful for mechanical packaging or thermal
analysis. Discrete parts would also have a
"value" attribute and a "tolerance"
attribute.)
    o The Non-Numeric Pin Number entry lets you
define a  part with pin names rather than
numbers. As this part  uses pin numbers,
leave this entry as N (No).
    o The Number of Gates parameter indicates
the number of gates in the part. Enter a 1.
    o The Number of Signal Pins entry is used
to define  standard power and ground pins
in the part. The Am27C256 has 3 standard
signal pins,  VPP (pin 1), GND (pin 14),
and +5V (pin 28), therefore, enter:
3
    o You must define the pin number, signal
name, and the track width.
    On the first line, enter the pin number as
1, the signal name as VPP, and the track
width as 50.
    On the second line, enter:
14    GND    50
    On the third line, enter:
28    +5V    50
5)     When you finish entering the electrical
information, select Complete (F9).
6)     Select Save (F9).  A <CR> will save the
part to your user library.  Exit (F10) will
return you to the design. You may now add
this part to the design with the add Part
option in the On-the-Fly (F9) command from
the In/Out menu.

Creating a Decal

In this exercise, you will create a 14 pin IC.
As this already exists under the name DIP14,
you will make a new version and call it
MYPART. Remember IC pads are 100 mils apart,
and the two rows are 300 mils apart.
1)    From the main menu, Select Create (F3),
Part Decal (F5), and Create (F1)
2)     To the prompt, give the new decal the name:
 MYPART<CR>
    The design is stored and you are in the
part library editor. With the commands of
the part library editor, you can make the
physical outline of the part, move its
name, put in terminals, relocate the part
origin, put text on the decal, etc.  You
can create a part for either two-layer or
multi-layer design.
3)     It is easier to work on a 100 mil grid. Set
the grid to 100 by typing:
G100 <CR>
4)     Select Terminals (F3), then Add Term (F1).
5)     There is now a terminal attached to the
cursor, named "1".  Place the pin in the
center of the screen and select Complete
(F1).
6)     Select Add Term (F1) again. A second
terminal is added to the cursor , labeled
"2". Place the terminal one cursor
movement, or 100 mils,  to the right of the
first. If necessary, use Zoom In so you can
easily move a single cursor movement.
Continue placing pins 3 through 7 in this
manner, with a separation of one cursor
movement. Then place pin 8 above pin 7,
separated by 300 mils. You can use the
cursor X Y display to check the distance.
7)     Place the remaining pins 9 through 14, then
Exit (F10).
8)     Move the cursor on top of pin 1 and select
Origin (F4). This makes pin 1 the origin of
the part in the design.
9)     You must next create the part outline. Set
the grid to 25 by typing:
G25 <CR>
10) Select Outline (F1) and 2-D Lines (F4).
Place the cursor at -25,50 by using the S
modeless command:
S-25 50<CR>
11) Select New Poly (F1), and  move the cursor
to 625,50. Select Add Corner (F1).  Move
the cursor to 625,250 and select Add Corner
(F1) again.  Move the cursor to -25, 250
and select Complete (F9).  PADS-PCB will
add the last corner and close the outline.
12) Next, define the default position of the
component name. From the main Part Decal
menu, select Move Name (F2), and move the
name and part type to the center of the
outline.
13) Select Save (F9) and respond with a <CR>
to the prompt. You have created a 14 Pin IC
Decal.  You have now added the Decal to
your user library in the actual PADS-PCB
package.



OTHER COMMANDS


You have used most of the important commands
of PADS-PCB in the exercises of this manual.
You are free to experiment with the other
commands described below.  If you have
questions, call your local PADS dealer or our
hot-line support team, or order a copy of the
entire user manual.

ASCII File Commands

PADS-PCB provides a totally open database,
through its ASCII file commands. Users who
wish to do so may convert a PADS-PCB design to
another CAD system by first outputting the
circuit as an ASCII file with the ASCII Out
command. Similarly, the ASCII In command will
convert a text file in PADS format into a
complete board layout . Similar facilities
exist for the libraries as well as the
designs.

2-D Lines and Add Text  Commands

The 2-D Lines and Text commands provide the
ability to create any general drawing item,
solid or dashed lines, polygons, title blocks,
etc.,  and text entries or notes in the PCB
design.  There is also a 2-D Lines library
capability, for storing created items into the
library for use on other boards.



YOUR NEXT STEP


PADS-PCB has been designed by PADS Software
Inc., specifically to solve the problem of PCB
design. It is not a general purpose CAD
drafting system, but is instead a highly
focussed tool developed to meet the needs of
engineers and design draftspersons for a low-
cost, but effective tool based on personal
computers. There is no other PCB design
system, at any price that is as simple to use,
and at the same time offers the power and
flexibility of PADS-PCB and its flexibility
for a wide range of design technologies.

If your designs are small, this Shareware
version of PADS-PCB is more than adequate to
design your circuits. Please use it with our
compliments.

If you need the capability of designing
circuit boards 400 or more IC's, you should
consider the actual version of PADS-PCB.  It
has all of the features of this shareware
version, plus greatly expanded system limits,
and it comes with a 400 page user manual
describing all of the commands of the program
in detail.   More than thirteen thousand
engineers are using PADS-PCB today.

If you would like to put the powers of PADS-
PCB to work on your next project, you can
order  it from your local authorized PADS
Dealer or contact PADS Software, Inc.
(telephone: [phone], fax: 508-486-
8217).

Once again, thank you for your time and
interest.  We welcome any additional questions
you may have about PADS-PCB or any other of
our PADS products.

When you have finished your evaluation of
PADS-PCB, feel free to make copies and pass it
on to a friend or colleague.
PADS-PCB Evaluation Guide

                       PADS-PCB Evaluation Guide


1

        1

PADS-PCB Evaluation Guide

                       PADS-PCB Evaluation Guide


1

        1

PADS-PCB Evaluation Guide

                       PADS-PCB Evaluation Guide


1

        1

PADS-PCB Evaluation Guide

                       PADS-PCB Evaluation Guide


1

        1

PADS-PCB Evaluation Guide

                       PADS-PCB Evaluation Guide


1

        1

PADS-PCB Evaluation Guide

                       PADS-PCB Evaluation Guide


1

        1

PADS-PCB Evaluation Guide

                       PADS-PCB Evaluation Guide


1

        1

PADS-PCB Evaluation Guide

                       PADS-PCB Evaluation Guide


1

        1

PADS-PCB Evaluation Guide

                       PADS-PCB Evaluation Guide


1

        1

PADS-PCB Evaluation Guide

                       PADS-PCB Evaluation Guide


1

        1

PADS-PCB Evaluation Guide

                       PADS-PCB Evaluation Guide


1

        1

PADS-PCB Evaluation Guide

                       PADS-PCB Evaluation Guide


1

        1

PADS-PCB Evaluation Guide

                       PADS-PCB Evaluation Guide


1

        1