home
***
CD-ROM
|
disk
|
FTP
|
other
***
search
/
Precision Software Appli…tions Silver Collection 1
/
Precision Software Applications Silver Collection Volume One (PSM) (1993).iso
/
demos
/
prodemo.exe
/
MANUAL3.DOC
< prev
next >
Wrap
Text File
|
1987-12-06
|
35KB
|
1,009 lines
PCPRO - Printed Circuit Board Layout
3 Tutorial
3.1 Introduction
This chapter walks the user, step by step, through the usage of
the PCPRO editor. It is intended to provide training in the use
of PCPRO and to give the user a feel for the system. The
tutorial does not go through every possible usage of every
command. Complete descriptions of each command is given in the
command reference chapter following this tutorial.
3.2 Manual Notation
The following notation is used throughout this manual.
The notation "..." indicates to type the characters shown between
the quotes. For example, "XYZ" indicates to type the characters
X, Y, and Z. Do not type the quotes.
The notation --- indicates to press this single key. For
example RETURN means press the return key while G indicates
to press the G key. Unless otherwise noted, either the upper or
lower case value for a key may be used.
An underlined word indicates an item on a menu, or is used to
emphasize particular words.
The notation (xxx,yyy) indicates a coordinate on a PCB. For
example, (1000,2000) indicated the x (horizontal) position is
1000 and the y (vertical) position is 2000. Values of
measurement are expressed in mils. One mil is 0.001 inches. The
value 1000 is one inch.
PCPRO Version 2.50
3-1
PCPRO - Printed Circuit Board Layout
3.3 Running PCPRO
Before using PCPRO the first time, you must run the PCCONFIG
program (supplied on your disk). This program is used to set the
configuration per your system. To run this program enter
PCCONFIG followed by RETURN . Answer the questions as they
are presented on the screen.
To run PCPRO from a floppy disk, put a configured PCPRO disk in
the A drive and enter:
A: (make A disk the default)
PCPRO
If PCPRO has been installed on a hard disk system:
C: (make C disk the default)
CD \PCPRO
PCPRO
The program will begin by displaying a title screen. Press any
key to continue.
3.4 Loading a PCB
To get a feel for the system, we will first load a sample PCB
file on the release disk. We will then learn how to move about
the PCB on the display.
Use the up and down arrow keys on the numeric key pad to
move the menu pointer up and down. The NumLck key must be off.
Move the select indicator to the Load entry, and RETURN . This
is referred to as selecting a menu entry.
We are now prompted for the name of a PCB file. At this point
we could enter the file name of a PCB if we knew it, but since
we do not, press RETURN . Now, we are prompted for the name of
a directory to be searched for PCB files. Press RETURN to use
the local directory.
PCPRO Version 2.50
3-2
PCPRO - Printed Circuit Board Layout
A menu of the PCB files on the current directory is now
displayed. Select the SAMPLE1.PCB entry from the menu. This
demonstration PCB will be loaded and displayed on the screen,
along with the edit menu.
3.5 Moving Around a PCB
We will now learn how to move about a PCB on the display screen.
First, select the Line entry from the main menu. At this point
press the F1 key to demonstrate the help feature. A new
screen of information about the current command (line edit) is
displayed. The help screen always gives general information at
the top and specific information in the bottom section of the
screen. Press the ESCAPE key to exit help and return to the
previous screen.
Now, zoom-in by holding the Ctrl key down and pressing the
PgUp key (numeric key 9). The display will be redrawn at a
larger scale. Zoom in again. It should be noted that you do not
need to wait for the redraw to complete before entering another
pan/zoom command. In this case, the current redraw will be
stopped, and the next redraw will begin directly.
The current coordinate of the cursor is displayed in the
upper-right corner of the screen. Use the cursor keys to move
the cursor to coordinate (1900,900). Follow the track of the
cursor on the screen, and watch the value in the upper-right
corner change.
Function key F5 is the pan-center command. This command is
used to center a given point of a PCB on the display screen.
Press F5 . The point on the PCB were the cursor was located is
now centered on the screen.
Function key F8 is the pan-text command. This command is
used to locate a text string on a PCB. Press F8 and enter
"U005" RETURN (at the top of the screen). The program will pan
the display so that the located string is displayed. The
position of the cursor is the coordinate of the text.
PCPRO Version 2.50
3-3
PCPRO - Printed Circuit Board Layout
The display may be directly panned in a given direction by
holding down the ALT key and pressing one of the cursor arrow
keys. The pan will take place when the Alt key is released.
Let's pan down. Hold down the AlT key, press the down arrow
(numeric key 2), and release the Alt key. The portion of
the PCB that was below the bottom of the screen is now
displayed. Now, pan to the right three times and pan down once.
The connector portion of the PCB should now be displayed.
Now, zoom-out with Ctrl-PgDn . Display the whole PCB with
Ctrl-Home .
Holding the Shift key down and using the cursor keys will move
the cursor ten units at a time. Hold the Shift key down and
use the left and up arrows to move quickly to coordinate
(0,0). Now, zoom in once with Ctrl-PgUp .
3.6 Selecting Layers for Display
We will now explore how to select the layers of information that
are displayed on the screen. This is controlled by the F4 or
D (for display) key. These two keys perform the same command.
Press D to pop-up the display layer control menu. You will
notice that each layer of the board is listed along with its
type and current display color. If the color is off, then that
layer will not be displayed. The actual colors and number of
colors available will depend on your particular hardware. The
display state of each layer is changed by pressing RETURN or
using the right and left arrow keys. Move the menu pointer
to the silk-screen layer and press the RETURN key until it
indicates off. Now, proceed to turn all the layers except the
Component and All layers to off. Exit from the menu by pressing
the ESCAPE key. The display will be redrawn per the new
settings. Notice that only the component layer is displayed.
Now, let's display just the solder-side layer by entering D ,
toggle the component layer to off, toggle the solder-side layer
to the color of you choice, and ESCAPE . Now only the
solder-side is displayed.
PCPRO Version 2.50
3-4
PCPRO - Printed Circuit Board Layout
3.7 Cursor Grid
The cursor grid is set to 50 by default. You have probably
noticed that the cursor steps 50 units each time the arrow keys
are pressed. Pop-up the cursor grid menu by pressing the G
key. Move the pointer to the X grid selection and RETURN .
Enter "25" and RETURN . This sets the X cursor grid value to
25. Do the same for the Y grid. Now, press ESCAPE to exit the
grid menu. Move the cursor about the screen with the arrow
keys. Notice that the cursor now moves in steps of 25.
This completes a summary of how to start the PCPRO editor, load
an existing board, view the board, control the display of
selected layers, and set the cursor grid. Now ESCAPE to
return to the edit menu. ESCAPE again to return to the main
menu.
3.8 Creating a New Board
Our assignment is to create a small board entirely from scratch.
This board is intentionally small; however, it demonstrates the
steps by which any board, regardless of size is created. The
schematic, parts list, and net list for the board is given in
Figures 3-1 and 3-2. The specification for the board is as
follows.
1. Board size is 4.00" x 4.00".
2. Board has 2 signal layers, 12 mil lines.
3. Power and ground provided by power
planes.
4. Solder mask required.
5. Silk screen required.
6. Drill drawing required.
PCPRO Version 2.50
3-5
PCPRO - Printed Circuit Board Layout
Figure 3-1 Schematic Drawing
PCPRO Version 2.50
3-6
PCPRO - Printed Circuit Board Layout
Figure 3-2 Part and Net List
Part List
---#--Part---Count--Instances-----------------
1 ... 1 CONN
2 320 2 R001 R002
3 LED 2 D001 D002
4 LS20 1 U001
5 LS74 1 U002
Net List
---#-Net name---Nodes-------------------------
1 #001 U002:3 U001:6
2 #002 U002:6 R001:1
3 #003 R001:2 D001:1
4 #004 U002:11 U001:8
5 #005 U002:8 R002:1
6 #006 R002:2 D002:1
7 +5V CONN:9 U002:2 D001:2 U002:12
D002:2 U001:14 U002:14
8 GND CONN:11 U001:7 U002:7
9 I1 CONN:1 U001:1
10 I2 CONN:2 U001:2
11 I3 CONN:3 U001:4
12 I4 CONN:4 U001:5
13 I5 CONN:5 U001:9
14 I6 CONN:6 U001:10
15 I7 CONN:7 U001:12
16 I8 CONN:8 U001:13
17 NC U002:5 U002:9
18 RESET CONN:10 U002:1 U002:13
PCPRO Version 2.50
3-7
PCPRO - Printed Circuit Board Layout
We will begin the new board by selecting the New entry on the
main menu. Since we already have a board loaded, we will be
questioned whether or not we wish to lose the changes made to
the current board. Answer yes by pressing the Y key.
Figure 3-3 Board Setup Menu
We are now presented with the new board setup menu as shown in
Figure 3-3. As mentioned before, the board size is 4" x 4", so
we want to set X Low and Y Low to zero (default), and X High and
Y High to 4000. Move the pointer to X High and RETURN . Enter
"4000" at the top of the screen and RETURN . Repeat the same
procedure for Y High.
The board has two signal layers, a power layer, a ground layer,
a solder mask, a silk screen mask, and a drill drawing. Set the
# of Layers to seven.
Now, we will set the type of layer for each of the seven layers.
Select Layer types from the menu. We are now presented with a
menu showing each layer and the default setting for the layer
type. Select layer 1 from the menu. Set the type to Comp-side
(from the new menu). Set layer 2 to Sldr-side. Set the
remaining layers as follows: 3=Silk Screen, 4=Solder Mask,
5=Drill Dwg., 6=Power/gnd, and 7=Power/gnd. ESCAPE to exit
PCPRO Version 2.50
3-8
PCPRO - Printed Circuit Board Layout
this menu.
The board size, number of layers, and the type of each layer is
now defined. More layers may be added later (if necessary).
ESCAPE to complete the board definition.
3.9 Adding the Crop Marks
We will now add lines which designate the four corners of the
board.
Select the Lines entry from the edit menu. Set the line width to
5 by pressing the W key and entering the value. Notice that
the first letter of the values displayed in the bottom status
line is the key used to set that value. Use the L key to
pop-up the layer selection menu. Select the All layer. The All
layer indicates that the lines which are to be drawn will be on
all layers of the board.
Move the cursor to (100,0) and RETURN to begin a line. Move
to (0,0) and return to draw a line segment. Move to (0,100) and
RETURN to complete the upper-left corner mark. ESCAPE to
terminate this line.
PCPRO Version 2.50
3-9
PCPRO - Printed Circuit Board Layout
Figure 3-4 Crop Marks
Now, move to (0,3900) and RETURN to begin the lower-left
corner mark. Complete the marks for this corner. The two
remaining corners can be completed at (3900,0) and (3900,3900)
as described above. The screen should now look like Figure 3-4.
ESCAPE to return to the edit menu.
3.10 Adding the Connector
We will begin by adding the pads for the connector. Select the
Pads function from the edit menu. Now, press the P key. The
menu on the left indicates which one of the 25 available pad
shapes/types is the "current pad". The window shows only 20 pads
per screen. The user can view the rest of the pads by moving
the pointer down. The PgUp and PgDn keys may also be used.
The window on the right side of the screen displays all the
parameter values for the current pad.
PCPRO Version 2.50
3-10
PCPRO - Printed Circuit Board Layout
In this tutorial we will use only the pre-defined pads; however,
you can change this pad parameters per your application. If the
exact pad shape required is not in the pad table, we could select
one of the pad numbers by pressing RETURN . This places us in
the parameter window for that pad, and we could design a custom
pad to meet our special requirements.
Move the selector to pad number 10. Observe the size and type
of this pad. This is the pad we will use for the connector. Now,
ESCAPE to return to the edit menu.
The connector has 11 fingers. We will place the connector on
the top side of the board, so enter L and select the Comp-side
layer. We will place the connector along the left edge of the
board. Move the cursor to (150,1000). Enter RETURN to place
a pad here. Move down 100 mils to (150,1100). Enter RETURN
to add the second pad. Add the remaining 9 pad down the left
side, spaced 100 mils apart.
For now, if a pad is added incorrectly, place the cursor on the
pad and DEL to remove it. Use N to set the current pin
number to the correct value and add the pad in the correct
location.
ESCAPE to return to the edit menu. Select the Text function.
Move to (100,900) and RETURN . Enter "CONN" and RETURN . This
identifies the connector. We will learn more about the text
command later. ESCAPE to return to the edit menu.
Now, we will combine all the connector pads into one component.
Select the Components function. Move to (150,1000) and
RETURN . Answer yes, Y to the prompt. Move to (150,800) and
RETURN to begin marking the area of the component. Move to
(250,2100) and RETURN to complete the component area. All the
pads of the connector and the text label are now one component.
ESCAPE to return to the edit menu.
This is the method of adding pads for special shapes, such as
connectors or new symbols. In this case pads are added one at a
time, and then combined into a single component.
PCPRO Version 2.50
3-11
PCPRO - Printed Circuit Board Layout
Figure 3-5 Connector
3.11 Adding Symbols
Adding pads for standard components is much easier than the way
we made the connector. For standard components, we will add a
symbol which will add all the pads for a component to the board
at once.
Now, we will add the symbol for the two IC's, U001 and U002.
Select the Load Symbol/Area function. Enter "DIP-14" and
RETURN .
Move the cursor to location (650,600). You can see the outline
of the symbol on the cursor. Press the MARK key. Notice that
the symbol outline rotates on the cursor by 90 degrees. Press
MARK three more times to return to the original orientation.
Press RETURN to add the symbol for U001. Move to (650,2100)
and RETURN to add the symbol for U002.
PCPRO Version 2.50
3-12
PCPRO - Printed Circuit Board Layout
The remaining four components are all two pin discrete parts.
ESCAPE to exit the current symbol. Select the Load
Symbol/Area function again and enter "DISC-2" RETURN . Place
this symbol at the following locations: R001 at (1500,1000),
D001 at (2500,1000), R002 at (1500,1400), and D002 at
(2500,1400). ESCAPE to return to the edit menu.
We now have all the component footprints placed on the board.
Now, let's update the component number (text) on the symbols to
the proper values. Select the Text function. First, move the
cursor to (0,0) and Ctrl-PgUp to zoom in on the display. Move
the cursor to the location of the component name for U001
(750,550). Enter U to update the text value. The current
value, U000, will appear on the input line. Change the value to
U001 and RETURN . Notice that the component value on the board
is now U001.
Update the numbers for all the other components using the same
procedure that we just used for U001. The text coordinates are:
U002 (700,2050), R001 (1650,1050), D001 (2650,1050), R002
(1650,1450), and D002 (2650,1450). When finished, ESCAPE to
return to the edit menu.
3.12 Add Net Names
Each pin on the board may be assigned the name of the net
(signal) that the pin connects to. Assignment of net names is
always optional, and is not required to complete the layout a
PCB. However, the adding of net names will greatly assist in
routing the board, and will make checking the board from the
net-list report much easier. Use the same net names used on the
schematic for the circuit.
Select the Assign Net/Part function from the edit menu. Now
select Net-Pad from the next menu. We are now ready to assign
net names to pads.
PCPRO Version 2.50
3-13
PCPRO - Printed Circuit Board Layout
We will work directly from the net list given in Figure 3-2.
Move the cursor to the location of U002 pin 3 and RETURN . Now
enter the net name, #001 and RETURN . Now, move to U001 pin 6
and assign net name #001. All the pads that belong to net #001
have now been assigned. Continue working from the net list until
all the pads on the list have the proper net name assigned. The
net NC is the no connect net. You do not need to name the pads
of this net. If a wrong name is assigned, just move to that pad
and RETURN to display the current value of the name. Correct
the name and RETURN to enter the new value. Another aid is to
place the cursor on a pad and press the I key for identify.
This will list information about the pad on the screen. This
may be used to identify the pin number of a particular pad.
ESCAPE to exit the identify function.
When all the net names have been assigned, ESCAPE to return to
the edit menu.
This may seem like a lot of work; however, most new boards are
created directly from the schematic data, such as with the EDIF
processor. In this case, names are generated automatically.
PCPRO Version 2.50
3-14
PCPRO - Printed Circuit Board Layout
Figure 3-6 Components Placed
3.13 Add Part Numbers
For completeness, we will also assign a part number to each of
the parts on the board. Select the Assign Net-Part function
from the edit menu followed by selecting the Part-Component
function from the assign names menu. Move the cursor to the
area of the connector and RETURN . Enter connector and
RETURN . Likewise, assign the following parts: R001 and R002
is 320 ohm, D001 and D002 is LED, U001 is LS20, and U002 is LS74.
When all the part names have been assigned, ESCAPE to return
to the edit menu.
PCPRO Version 2.50
3-15
PCPRO - Printed Circuit Board Layout
3.14 Name Power/Ground Layers
Since this board has power and ground layers, we will assign the
net name for power and ground to the appropriate power layers.
Select the Assign Net/Part function. Next, select the
Layer-Pwr/Gnd function. Now, select power layer number 6.
Enter "+5V" for the net name and RETURN .
Repeat this procedure to assign net name "GND" to power layer
number 7.
3.15 Routing the Board
We are now ready to add the routes that connect the pads
together to make the desired circuit. Once again we will work
directly from the net list given in Figure 3-2. Select the
Lines entry from the menu.
First, we will choose the desired width of the route lines.
From our specification, this is 12 mils. Enter W (for set
width), "12", and RETURN . For this board, we will use the
component-side for the mostly horizontal routes, and the
solder-side for the mostly vertical routes.
From our list, we will route the #001 net first. This net
connects from 002 pin 3 to 001 pin 6. Move the cursor to U002
pin 3 (650,2300). Enter L and set the layer to the
solder-side. Press the N key. This will display a prompt-line
to the nearest pad that this pad connects to. This is for
reference only, the line is not part of the board; however, it
is extremely helpful in routing boards by indicating what pads
need to be connected together. The line may be turned off by
pressing the N key again. Press the N key several times to
flash the path. Leave the line turned on for the next step.
We are now positioned on one end of the route to be made, and we
have an indicator showing where we are going. Press ENTER to
begin the route. Now move to (750,2300). Notice that the line
we are about to draw is displayed. RETURN to add this segment
to the PCB. Now move to (750,1100) and RETURN . Move to
PCPRO Version 2.50
3-16
PCPRO - Printed Circuit Board Layout
(650,1100) and RETURN . This completes this route and this
net. ESCAPE to terminate this line. Press N to remove the
net-prompt line.
Now, we will route the next net, #002 which connects U002 pin 6
to R001 pin 1. Move the cursor to the location of U002 pin 6
(650,2600) and press N . Route this net as follows: Use the
T key to toggle to the component-side. RETURN to start the
net. Move to (800,2600) and RETURN . At this point we will
add a via and switch to the other side of the board by pressing
RETURN again. Move to (800,1150) and RETURN . RETURN
again to add a via here. Move to (1500,1150) and RETURN to
complete this route. Enter ESCAPE to terminate the route and
N to remove the net-prompt. Net #002 is now complete. Now,
let's guide you through one more net, #003. Move to U002 pin 6
at (2000,1150). N to display the path prompt. This is an
easy one! RETURN to start the line, move to (2500,1150),
RETURN to add the line, and ESCAPE to complete this net.
This is how nets are routed. See how the adding of net names
pays off! If you do not add net names, you will not be able to
display the net prompt-lines, and you will have to locate the
end points of each net path all on your own.
Now, use the net list and proceed to complete the rest of the
nets on this board, just like we routed the first three nets.
Warning! When you make a route to one of the connector pads,
remember that these pads are only on the component-side of the
board. Make sure your connection to the pad is also on the
component-side. Also, the connector pads for nets +5V and GND
may be connected to the power layers by routing a short line and
ending it with a via. The via will connect to the power plane.
PCPRO Version 2.50
3-17
PCPRO - Printed Circuit Board Layout
Figure 3-7 Component & Solder Sides
PCPRO Version 2.50
3-18
PCPRO - Printed Circuit Board Layout
3.16 Adding Text
We have already worked some with the text command. Now, we will
learn how to add addition text strings to the board. Text is
often added to identify the layer of the mask, the company name,
copyright notice, etc.
Select the Text function from the edit menu. Enter L and
select the component side layer. Enter S ,"62", RETURN to set
the text height to 62 mils (1/16"). Move to (1000,300) and
RETURN to add a text string. Enter "Copyright (c) 1987 by Me"
RETURN . The text will appear on the board at the location of
the cursor and have attributes which match the current settings
displayed at the bottom of the screen.
Enter A and select Up for the angle. Move to (3500,2000).
RETURN and add the string "Component Side". Change to the
layer, L , to Solder side. RETURN and add the string "Solder
Side". Likewise, add the names for the Power, Ground, Assembly,
and Drill Drawing layers.
You may add any additional text as desired. Set the angle,
size, and mirror factors as desired. To changed the factors for
an existing text string, set the parameters to the new desired
values, place the cursor on the string and U for update.
Change the string if required and RETURN to update the text.
To delete a text string, place the cursor on the text, set the
layer to the layer for the text and DEL .
When complete, ESCAPE to return to the edit menu. ESCAPE
again to return to the main menu.
PCPRO Version 2.50
3-19
PCPRO - Printed Circuit Board Layout
3.17 Reports
Select the Reports function from the main menu. Generate a
parts list and a net list (pads only option). If you have a
printer, enter "PRN" to send the reports to the printer. Compare
these reports with the input net and parts list. They should
agree.
3.18 Saving the PCB
Now we will save our masterpiece to a disk file. Select Store
from the menu. Enter "MYBOARD" and RETURN . This will save
the board into the file MYBOARD.PCB.
3.19 Exit the Editor
We are finished with the PCB for now. Select Exit from the menu
to exit the program. If you wish, you may run the PCPLOT
program to make plots of the board you have just created.
3.20 Additional Training
The tutorial your have just completed is designed to familiarize
you with the basic steps in using the editor to create a PCB.
To become a more advanced user of PCPRO, and to use its features
to your best advantage, the following self-training procedure is
suggested.
Start the PCPRO program and create a new board (any size). Go
through each command on the menus, one at a time. For each
function, display the help information with key F1 . Study the
options for each function and practice each of these operations
on the board. Do not try to construct a real or complete PCB.
Just use the board as a scratch area to practice the commands.
For example, practice the Edit text command by placing text of
various sizes, angles, mirroring, layers, etc. on the board.
Move a text string. Move an area of text strings. Update a
text string. Delete a text string. Do this for each function
PCPRO Version 2.50
3-20
PCPRO - Printed Circuit Board Layout
and you will be a "power user" of PCPRO. Also, refer to Chapter
4 for a complete reference to each of the PCPRO commands.
PCPRO Version 2.50
3-21
