home
***
CD-ROM
|
disk
|
FTP
|
other
***
search
/
Belgian Amiga Club - ADF Collection
/
BS1 part 41.zip
/
BS1 part 41
/
Pro-net pre-release NTSC.adf
/
pronet.feature
< prev
next >
Wrap
Text File
|
1987-12-21
|
90KB
|
2,332 lines
GENERAL DESCRIPTION OF PRO-NET COMMANDS AND FEATURES
***********************************************************************
* *
* Refer to "read.me" on the AutoDemo disk for other information *
* *
***********************************************************************
TERMS AND CONVENTION:
- click
Click the left mouse button to select a mode (function) or add
a piece of graphic information to the drawing.
Click the right mouse button to delete a piece of graphic (such
as a symbol of an NAND gate) information on the screen
pointed to by the cursor.
- IFK's
The Intelligent Function Keys. They are the ten Function Keys
located at the top of the keyboard. In PRO-NET, these
Function Keys are intelligent because the same Function Key
performs different tasks in different modes. The tasks to be
performed by these Function Keys at any moment are
automatically shown at the bottom of the screen.
- IFK-Name
An IFK called "Name".
- IFK levels
The IFK's guide the user through an operation by providing
the next available set of IFK's for the user to select. These sets
form the IFK levels. An IFK at a certain level is expressed as :
IFK-NameA/IFK-NameB/...../IFK-NameX.
For example, the IFK-Line appeared if you first select IFK-Edit,
then IFK-New, IFK-OK. Therefore, the selection of IFK-Line
can be expressed as:
IFK-Edit/ IFK-New/ IFK-OK/ IFK-Line
or, in its short form:
IFK-Edit/New/OK/Line
This expression can further be expressed as:
IFK-Edit/./Line
if and only if the same set of IFK's (that contains the next IFK,
in this example, the IFK-Line) appear no matter what
intermediate steps (other than <ESC> which means abort)
have taken place.
- Select
Either press the IFK or click at Icon of the IFK.
- Add button
The left button of the mouse.
- Delete button
The right button of the mouse.
- Entry Bar
The color bar above the IFK icons at the bottom of the screen.
It is used for the user to enter additional information and for
the program to display the status of the operation.
- Bold face
All commands are shown in Bold.
These commands are entered by one of the following
methods:
1. Selecting the appropriate IFK.
2. Using the hot key.
Some Commands require additional information from the
user, this information is entered at the Entry Bar.
- Leading Capital
Names that have special meanings in PRO-NET have their first
character capitalized.
- Directory Structure
If PRO-NET is installed using the "install_pn_dh" (see Section
"Quick Start"), the following directory system is automatically
setup for you under a subdirectory "/PRO-NET". For Floppy
systems, the following directory is disbursted among
diskettes, therefore, you MUST follow the procedure in
Section "Defining Library Parts" when you have to modify the
Library.
The file Directory Structure for PRO-NET is as follows :
PNPOST (dir)
PNLIB (dir)
TTL (dir)
MOS (dir)
VLSI (dir)
ECL (dir)
ANALOG (dir)
DISCRETE (dir)
MTTL (dir)
USER (dir)
SYMBOL (dir)
SCHEM (dir)
PNDIR (dir)
TTL
MOS
VLSI
ECL
ANALOG
DISCRETE
MTTL
USER
SYMBOL
SCHEM
- Files
The files that are associated with a schematic called "name"
are as follows :
name.1 Page 1 of the schematic "name"
name.2 Page 2 of the schematic "name"
. .
. .
. .
. .
. .
name.SupNet ASCII file, optional Net list provided by user
for schematic "name".
name.net ASCII file, net list of the schematic
"name".
name.bom ASCII file, Bill of Materials (Part List) of the
schematic "name".
name.err ASCII file, error report of schematic "name".
name.map ASCII file, component map of schematic
"name".
Other system files (you don't normally care about these files,
as long as you are not trying to alter them):
PNDIR A file that contains the PRO-NET directory
system. It contains the directory files of PRO-NET,
when a schematic is deleted or added, or when a
Device is added or deleted, this file will be automatic
updated.
PNLIB all PRO-NET files are kept here.
name.M System internal file containing information
linking different pages together. This file is part of the
schematic "name".
- Hot Keys
Key strokes used to enter command(s) at any screen in any mode.
In PRO-NET, when you hit the "Help" key, the Hot Key definition will
show up as follow:
<Help>
get this help information
<CTL-G>
show Grid ON/OFF
<CTL-S>
grid Snapping ON/OFF
<CTL-U>
grid size goes Up (bigger) by one size
<CTL-D>
grid size goes Down (smaller) by one size
<CTL-B>
Move the PRO-NET screen to the Back of other screens
of the system.
<DEL>
scroll wall ON/OFF
<ENTER>
redraw screen
<ESC>
back up one IFK level. In some cases, abort currrent
operation.
<ARROW KEY>
unconditional scroll
OVERVIEW:
PRO-NET stands for 'PROfessional NET list generator'. Thanks to the powerful
graphic capabilities of the AMIGA computer and to the brilliant Intelligent
Function Keys (IFK) of PRO-NET, users now can create professional
schematics with speed and ease.
Besides creating beautiful schematics, Flow Charts, Organization Charts, etc.,
PRO-NET emphasizes the importance of net list generation which provides
sufficient information for the PRO-BOARD (*) to perform Auto Component
Placement at an expert level (**), and to perform such tasks as Rat Nesting,
Guided Routing, Automatic Coordinate marking , Automatic Surface trace
handling and Net List comparison.
PRO-NET and PRO-BOARD are tailored to work with and for each other, they
therefore could accomplish many tasks that other stand alone schematic
capture programs or pcb layout programs could not do. Most of these tasks
are tedious and repetitive, and should be done on the computer rather than
manually by hand. Some examples of these tasks are:
-- Automatic assignment of label and section numbers for components such
as U17, pin 1,2,3 of an 74F00. The assignment also avoids conflicts in
component placement which will be performed later by PRO-BOARD.
-- Automatically creates page references on a schematic for every signal
name on every page of that schematic. For a schematic of many
pages, this is previously a tedious job that could hardly be right if it is
done by user manually.
-- Rat's nest helps the component placement process which is of vital
importance to a good PCB layout.
-- Automatically assign and mark XY coordinates on the PCB.
-- Automatically rename IC by coordinates, such that U17, now becomes
3D, on the PCB.
-- Automatically rename IC by coordinates on schematic to match that of
the PCB.
-- Creates BOM, Spare List, Component Map, Loading Analysis, Error
List.
-- Automatically compare Net List produced by PRO-NET with results
from PRO-BOARD and report discrepancies.
-- PRO-NET and PROBOARD provide all these powerful features, on top
of the extremely friendly user interface. We are confident that the
users will find that they are truly "PROLIFIC" systems.
The relationship of PRO-NET and PRO-BOARD in the design cycle of
a schematic diagram and its corresponding PCB is depicted in the
brochure attached.
* PROBOARD, the PROfessional pc-BOARD design package, another
professional program designed by PROLIFIC INC.
** Option not available in the release 1.2
COMMAND DESCRIPTION:
Hot Keys :
Key strokes used to enter command(s) regardless of what screen you
are at and what mode you are in.
In PRO-NET, when you hit the "Help" key, the Hot Key definition will
show up as follow:
<HELP>
get this help information
<CTL-G>
show Grid ON/OFF
<CTL-S>
Snap on grid ON/OFF
<CTL-U>
grid size goes Up (bigger) by one size
<CTL-D>
grid size goes Down (smaller) by one size
<CTL-B>
put the PRO-NET screen behind all other system
screens.
<DEL>
scroll wall ON/OFF
<ENTER>
redraw screen
<ESC>
back up one IFK level, or, in some cases, abort current
operation.
<ARROW KEY>
arrow keys on the keyboard performs unconditional
scrolling.
IFK COMMANDS AND OTHERS :
\- - - - :
Add Bus Entries to the left end of a Line. Orientation of the
Entry being from lower right to upper left.
- - - -/ :
Add Bus Entries to the right end of a Line. Orientation of the
Entry being from lower left to upper right.
/- - - - :
Add Bus Entries to the left end of a Line. Orientation of the
Entry being from lower left to upper right.
- - - -\ :
Add Bus Entries to the right end of a Line. Orientation of the
Entry being from upper left to lower right.
(Arrow-Down) :
This IFK moves the Selection Bar (Box) Down the list.
In Note/Text mode, this IFK specifies that text is written from
top to bottom.
(Ar-Right) :
In Note/Text mode, this IFK specifies that text is written from
left to right.
(Arrow-Up) :
This IFK moves the Selection Bar (Box) Up the list.
Pg(Arrow-Down) :
This IFK moves the Selection Bar (Box) one Page Down the
list.
Pg(Arrow-Up) :
This IFK moves the Selection Bar (Box) one Page Up the list.
(Big-Dot) :
In Edit/Dot mode, this IFK select the Biggest Dots to be added
to the intersections of Lines.
(Mid-Dot) :
In Edit/Dot mode, this IFK select the Medium size Dots to be
added to the intersections of Lines.
(Sml-Dot) :
In Edit/Dot mode, this IFK select the Smallest Dots to be
added to the intersections of Lines.
Above :
Conn, Above, and Below are mutually exclusive functions.
When a Signal Label is added, it can be added above the line,
below the line, or at the end of the line with a box around it as
a connector pin designation.
Add :
The left button of the mouse means select or Add.
Adjust :
To move a middle section of line without breaking it.
Example: Move the middle section of the following line from
location a to location b:
_______________________________
|
|
|
______________ |
| |
| |
a b
____________________
|
|
|
_________________________ |
Steps:
1. Under the Line mode, press the IFK-Adjust.
2. Click the select button of the mouse on the vertical
line.
3. Move the cursor to the left or to the right, the vertical
line will follow the cursor while maintaining the
continuity of the line.
4. Position the vertical line of the cursor at point b.
5. Click the Select button of the mouse to put the vertical
line at point b.
6. Hit ESC key to get out of the Adjust mode.
Note that there are limitations in IFK-Adjust: A line can not be
adjusted if one end of the line has a Dot or if one end of the
line vertically intersects a Device Pin (this is normally avoided
in schematic capture to begin with).
AllClr :
Clear all the IC pin definitions.
Arc :
In Edit/Note/Arc or DefLib/Defsym/Arc mode, add or delete
Arcs.
Arcs are drawn counter clockwise. You specify the two end
points on the arc, and then select the radius of the arc on the
bisector given by PRO-NET. If you drag the mouse when the
bisector appears, you can see the radius shown at the bottom
of the screen.
Arcs can be drawn with narrow (IFK-Narrow) or wide (IFK-
Wide) lines.
Arcs can be repeated (IFK-Repeat) at one to four grids below
the current Arc. The number of grids is selected by IFK-Leap-
N where N=1,2,3,4.
Attr :
To define the Attributes of the device. Refer to Section
"DEFINING LIBRARY PARTS".
Below :
The Signal Label will be placed below the line. Refer to IFK-
Above and IFK-Signal.
Bold :
Select Bold face Text. Also see Bold.
BOM :
Ask Post Processing to generate the BOM (Bill Of Material). If
this IFK is active, BOM will be generated in Post Processing.
Bound :
To define the Boundary of the Symbol, this is normally the last
step of the defining a Symbol. If a Device later uses the
Symbol, the Boundary of the Symbol will become the
Boundary of the Device. Note that when Devices are called
out to a schematic, their Boundaries can not overlap each
other.
Box :
In Edit/Note/Box or DefLib/Defsym/Box mode, add or delete
rectangular Boxes.
Boxes are drawn by specifying any two diagonal vertices. You
can drag the mouse and see the box change size
dynamically.
Boxes can be filled (IFK-Fill), or drawn with narrow (IFK-
Narrow), wide (IFK-Wide) or dashed lines (IFK- '- -').
Boxes can be repeated (IFK-Repeat) at one to four grids below
the current box. The number of grids is selected by IFK-Leap-
N where N=1,2,3,4.
Bundle :
Bus-Entries + Bus (thick Line) = Bundle
<A> Bus-Entries : select the Bus Entry orientation using the
first four IFK's.
<B> Click at the end of a Line to place the Entry.
<C> Use IFK-Repeat if desired to draw another Entry at the
next lower end of Line.
<D> Select IFK-Bus, draw thick Lines as needed. Use Next to
start another Bus. IFK-Repeat has no effect here.
Bus :
To add thick lines as part of a Bundle. A Bundle represents
many Signal lines 'bundled' together.
You can add Signal label such as ADDR<0:31> to a Bus. You
can also specify whether the Page Reference be generated
automatically for the Signal label. This is done by IFK-+PgRef;
if +PgRef is on when the Signal label is created, then Page
Reference will be created automatically for this Signal later in
the Post processing.
Please also refer to IFK-Bundle.
CalSym :
In DefSym, you can use this IFK-CalSym to call out existing
Symbols and use them to form a new Symbol (Complex
Symbol). You can not call out Complex Symbols to form
Complex Symbols. Complex Symbols always have extension
".C" in the Symbol Directory. You can also call out an existing
Symbol, modify it to a new Symbol.
In DefDev, you use this IFK-CalSym to call out a Symbol, this
becomes the symbol of the Device being defined. You can
call out Complex Symbol also. Only one Symbol can be called
out for a Device.
ChgLib :
Change Library; to open or close Sub-Libraries or to change
the paper size or template size. You can only change to have
a larger paper and/or to have a smaller template than what you
have been using for the schematic.
Circle :
In the Edit/Note/Circle mode or in the DefLib/DefSym/Circle,
add or delete circles.
Circle is drawn by clicking at the center then at the
circumference of the circle.
Circles can be filled (IFK-Fill), or drawn with narrow (IFK-
Narrow) or wide (IFK-Wide) lines.
Circles can be repeated (IFK-Repeat) at one to four grids
below the current circle. The number of grids is selected by
IFK-Leap-N where N=1,2,3,4.
Clear :
To clear the entry line input area.
Conn :
To create scattered Connector symbols. This may or may not
affect the Net List, see "Advance Technique" section for the
detail discussion about drawing connectors.
To add a Connector symbol in the schematic, select Conn,
type in the Connector pin identifier such as J4-11, then click at
the end of line to add connector symbol at that line.
Also refer to IFK-Above, IFK-Signal.
Connector pin number can be stepped through like other
Signal Label. Refer to IFK-Step @.
Config :
Configure the system, e.g. printer type, plotter type.
Copy :
Under IFK-File (File Management) mode, Copy a schematic to
another name in the same disk or different disk. You can also
copy a schematic to the same name in a different disk using
this IFK.
Note that when you copy one page of a schematic to another
file, all pages of the schematic are copied at the same time.
You can enter the Edit mode to delete pages that you don't
want one page at a time. This is necessary for the following
reason:
You can ask (IFK-Zone-1,2,3) PRO-NET to assign Device
Numbers and Device Sections automatically when Devices
are called out from the Library (to the schematic). These
Device Numbers and Device Sections are being kept track of
across all pages of the schematic. Had you been able to copy
one page of the schematic, the book keeping of the Device
Number and Device Section would have been corrupted.
In Edit/Copy mode, this IFK-Copy is used to Copy devices
from one place of the schematic to another. You can use the
IFK-Zone-1,2,3 or Zone-X to control the Device numbers (refer
to IFK-Zone-1).
DefDev :
Define Device; refer to DefLib and the Section "Defining
Library Parts".
DefSym :
Define Symbol; refer to DefLib and the Section "Defining
Library Parts".
DefLib :
Define Library; DefLib is used to define a Symbol, Complex
Symbol, Title Block, or Device in a sub-library. To use a Device
in a schematic, the sub-library whom the Device belongs to
must be opened first. Libraries are opened according to the
Design Rule established when a new schematic page is
drawn. Libraries can be opened or closed at the Device
/ChgLib (Change Library) also.
To define a Device with a new Symbol (graphic shape), you
must define the Symbol first. A Symbol can be shared (used)
by many different Devices.
For details of DefLib, refer to the Section "DEFINING LIBRARY
PARTS".
Delete :
In Edit mode, erase the file selected.
In DefLib/DefDev , erase the Device selected.
In DefLib/DefSym , erase the Symbol selected.
Device :
A. To get a Device from the opened libraries into the
schematic. Libraries are opened in the Edit/New
(Rule) screen, or the Device/ChgLib screen.
The steps of getting a Device into the schematic are:
1. Select IFK-Device.
2. Optionally select the Zone-1, 2, or 3 which
determines what Label to use;
Zone-1 selects unused 'U' numbers (or
Resistor Modules numbers or any other
Devices that were defined as multiple section
elements in the libraries) from U1 to U399 (or
RM1 to RM399 etc.).
Zone-2 selects unused 'U' numbers from U400
to U699 (or RM400 to RM699 etc.).
Zone-3 selects unused 'U' numbers from U700
to U999 (or RM700 to RM999 etc.).
The default is Zone-1.
3. Type in the Device Name such as '74LS74'
and <CR>.
4. Drag the Device to the desired location and
click the mouse left button to settle the
Device.
B. To Modify an existing Device or to define a new
Device in the Library, refer to the Section "Library
Parts".
DevNam :
IFK-DevNam (Device Name) is used to define the Text and
location of the Device Name Label such as 74LS244.
This Device Name could be different from the Device file
name you assign when you Save the Device. This is very
useful since you sometimes need to define a Device in
several different ways. For example, 74LS244 can be defined
as two independent four bit tri-state buffer or it can be defined
as one eight bit buffer. You may use one definition in one
application and the other in another application.
With Field Programmable Logic such as PAL's so popular
these days. This flexibility is extremely useful.
DevNum :
IFK-DevNum (Device Number) is used to define the location of
the Device Number Label such as 'U', 'R' or 'C', etc.
This Device Number Label will be concatenate with a numeric
assigned by PRO-NET automatically or assigned by user
manually (refer to IFK-Zone-1, 2, 3 and X) when schematic is
being entered. For example, 'U' becomes 'U14'.
Df0: :
Select floppy disk drive 0 to Load from or to Save to.
Df1: :
Select floppy disk drive 1 to Load from or to Save to.
Dh0: :
Select hard disk drive 0 to Load from or to Save to. Normally,
when you install PRO-NET to the hard disk, a directory
system is created under the root, and under Sub-directory
PRO-NET.
Dir :
To get the Directory of the Schematic files. Please refer to
IFK-Copy.
Dot :
Used to add or delete a dot in the drawing. If the dot is placed
on the intersection of two lines, the two lines are joined
together, otherwise, the dot has no effect in the Net List.
A dot can also be used to cancel out a small square box that
appears at the end of a line. For example, if you draw a line on
the screen with both ends open, you should see a small
square box at each end of the line. If you move a device to the
line such that one end of the line coincides with one pin (tip)
of the device, they may seem to be connected, but in fact they
are not. To connect them, you must add a dot to that small
square box. This will cancel out the small square box.
Down :
When IFK-Signal is active, IFK-Down forces the number
embedded in the Signal label to decrement by one (1) every
time IFK-Step@ is pressed.
In Zoom, Zoom Down by 1/2 X (devices are half the current
size on screen). The last Zoom Down may not be as small as
1/2 X of the former size.
Drag :
The word 'Drag' is used throughout this manual, it means
pressing down the mouse left button while sliding the mouse
to put the cursor at the desired location.
Edit :
Edit old or new schematic. When selected, a directory of
schematics is shown. If you want to create a new schematic,
just select the IFK-NEW.
ErrChk :
To ask the Post Processing to perform Error Checking, which
includes Loading Analysis, Output contention checking, Net
without output error checking, also generate the total
worse case current consumption of the whole schematic
(all pages).
File :
File management. Note that since PRONET maintain its own
directories and files. To Copy a schematic Page to another
name, or to Rename, etc., you must use this IFK-File. To
Delete a file, you have to use IFK-Delete under Edit mode.
Copying Library Devices from one disk to the other is done
differently. See Section "Library Parts" for more information.
Fill :
Fill the enclosed area of a Box, Circle, Closed polygon-by
stripes, etc.
Flip :
Reverse sections the Line you have just drawn, such that the
horizontal section becomes the vertical section and the
vertical section becomes the horizontal section.
Hidden :
An attribute of the piece of information being added. If this IFK
is on, the piece of information being added will have an
attribute of "hidden". All information with hidden attributes will
not be printed or plotted.
As an example, you can go to the DefDev (Define Device)
mode, call out the Device 'GND'. You will find that this Symbol
uses Hidden Pin Number, Hidden Device Number label, and
Hidden Device Name label. You can find some more
examples in Section "Surface Power and Surface Ground
traces" under "Advanced Technique".
H-Ref :
When this mode is selected, clicking the Add (left) button or
the Delete (right) button of the mouse will Add or Delete a
Horizontal line on screen. This line is of type Note (see Note
mode); which has no effect to the connections between
Devices (i.e. no effect on the Net-List). It is used for alignment
purpose such as lining up the Signal Name, the position of
Devices, etc.
Reference lines are not printed or plotted.
Icc :
You select this IFK when you need to enter the maximum total
current consumption of the Device. This parameter is used
only for the calculation of the maximum total current
consumption of a voltage (the heaviest loaded one) of the
design as shown in the schematic. This is to help the circuit
designer to calculate the Power Supply requirements. Please
also refer to IFK-Attr and Section "Defining Library Parts".
Label :
Label is an option under Modify mode. You can Modify the
Device Number Label, the Device Type Label and the Device
Pin Label with the following limitation.
Device Number Label: you can change it to any other
Device Number as long as that Number is not already used.
You can change it to a Device Number which is already used
by the same type of IC, in this case, you will be asked if you
want to swap the two Device Numbers. However, it can not
swap Device numbers of devices on different pages. If you
really want to do that, you have to use some tricks:
Step a. Change the Device Number A to an arbitrary
new Device Number X.
Step b. Go to the other page, change Device number
B to A.
Step c. Go back to the original page, change Device
Number X to B.
Device Pin Label: When swapping IC sections, you can
Modify the Pin Label. You only need to modify any one pin in
one section and the rest will be automatically modified for you.
If there is only one IC section for an IC, then Modify pin is not
allowed.
Device Type Label: You can Modify a Device Type Label if
and only if the new Device Type has the same Symbol
(graphic) as the old one.
For example, you can Modify a 74LS138 to a 74F138 but not
74LS139. If you really want to do that, you simply delete the
old device and add the new one.
Labels also appear under DefDev, they are used to define the
location of the Device Name and the Device Number label.
Large :
Select Large Size Text. You can add Text to the Symbol being
defined under the DefSym mode. You can add Text to the
schematic under the Edit/Note/Text mode.
Leap-N :
Each time you press IFK-Leap-N, N is incremented by 1, until
N=4, next press of IFK-Leap-N changes N back to 1.
N represents the number of grids (grid size currently
selected) to be Leaped over when patterns are to be
repeated. In other words,
'N multiply (current grid size)' is the distance between
consecutive repeated patterns.
Line :
To get into the Line screen, where Lines are Added, Deleted,
Adjusted in various ways.
You can use the Add (left) mouse button to start a Line, to
settle and to continue the same Line.
You can Delete a Line by clicking the delete (right) mouse
button.
You can start a new Line by pressing the Next Key.
After you draw a Line at an IC pin, you can duplicate the Line
at the next lower IC pin (same IC) by using Repeat.
You can Flip the orientation of a Line immediately after you
draw it. i.e. change the vertical Line into a horizontal Line and
change the horizontal Line into a vertical Line.
You can rubber move a section of a Line easily by using
Adjust (refer to IFK-Adjust).
You can setup a vertical or horizontal Line for the alignment of
various elements (Device, Text, Signal Name etc.) by using V-
REF or H-REF.
A small square at the end of the Line indicates that the Line is
not connected to any other place -- even if it seems to be
connected.
-Logic :
In Edit/Modify, it is used to Modify a positive logic gate to its
DeMorgan equivalence.
In DefLib/DefDev, this is to specify the DeMorgan equivalence
of a logic gate.
+Logic :
In Edit/Modify, it is used to Modify a negative logic gate to its
DeMorgan equivalence.
Map :
To ask the Post Processing to generate a Component Map for
the schematic. For each Component, the Component Map
shows you all the pages in which the Component appears.
Modify :
In the DefDev/Attr/PinAtt mode, Modify is used to enter or
modify the attributions of the pins of a device. refer to section
"Defining Library Parts" for more information.
In the Schematic Edit mode, Modify is used to change Label
or Logic sense (+Logic symbol or Logic sense (+Logic symbol
or the -Logic symbol).
Move :
In this mode, click the Add button of the mouse on Devices to
select them, then press IFK-OK, drag the mouse to move
devices to new position and press Add button of the mouse to
settle the Device.
You can perform a rubber-band Move (Rubber Move) by
selecting IFK-Rubber. Rubber Move allows you to move a
Device without breaking its connections. You can only Rubber
move one Device at a time. After the Rubber Move, you can
enter the IFK-Line/Adjust mode to Adjust the Lines (refer to
IFK-Adjust).
Narrow :
Select Narrow Lines or Stripes. Lines and Stripes has different
properties. Refer to IFK-Stripes for more information.
Net :
Ask the Post Processing to generate a Net List for the
schematic. Refer to IFK-Post for more information.
New :
In Edit mode, start a new schematic or a new schematic page.
After a file name is given to the new page, a screen will be
displayed for you to specify the Design Rule for the page. The
Design Rule specifies the following :
(a) The Paper Size to be used for the schematic. It is selected
by entering the corresponding number (as shown on screen)
when the selection Box (Bar) is at 'Paper Size' location.
Standard paper size:
A : 8.5 X 11 inches
B : 11 X 17 inches
C : 17 X 22 inches
D : 22 X 34 inches
E : 34 X 44 inches
(b) The Template Size to be used for the schematic. Standard
template sizes are those specified by the MIL-STD-860
standard or ANSI Y32.14 standard :
A. FULL size
B. 1/2 size
C. 3/8 size
E. 1/4 size
(c) The Sub-libraries opened for this schematic. Press 'Y' to
opening the Sub-libraries pointed to by the selection Box (or
Bar).
In DefLib/DefDev mode, this IFK-New is used to define a new
Device.
In DefLib/DefSym mode, this IFK-New is used define a new
Symbol.
Next
To start another Line or Stripe or Bus.
Or, in the DefDev/Attr/PinAtt mode, this IFK-Next is used to
call out (with IFK-Recall active) the attributes of the next pin
(current pin number +1).
Norm :
In Edit/Zoom mode, IFK-Norm always brings you back to the
Normal operation screen. You can not Edit (change) anything
after the schematic is Zoomed to a smaller size.
Note :
Note can be anything you draw or write. They will not affect
the Net list of the schematic. But they will be printed or
plotted.
In Note mode, you can write text from left to right or from top
to bottom in different fonts : small or large, normal or Bold.
You can draw various types of Stripes, Boxes, Circles, Arcs in
narrow or thick line, etc.
NxtSct :
To define the pin number of next section of the IC.
OK :
Tell the system to proceed since You have completed
checking, or have entered the information PRONET needs.
PgRef :
To ask the Post Processing to generate the Page References
for every Signal name of the schematic and insert them to the
schematic automatically.
-PgRef :
After Page References are added to the schematic
automatically by the Post Processing. You could delete a
Page Reference (such as: [2,3,23,25]) using this IFK-PgRef.
When this IFK is active, click the delete (right) button at the
Page Reference to delete it.
+PgRef :
When Signals are being added to Lines or Bus, you use this
IFK-+PgRef to indicate whether these signals should have
page references. IFK-+PgRef active means you want page
references, inactive means you don't. Page references are
generated in Post processing. Please also refer to Bundle,
Bus.
Pick :
Select the item high lighted or boxed on screen.
Pin :
Used to define the pin number and pin location of the Device,
A pin has to be located in one of the four quadrants around
the tip of a stripe (of the Symbol).
If the Device has more than one section (e.g. 7400 has four
sections), you can go to another section by pressing IFK-
NxtSct (Next Section).
Please refer to "Defining Library Parts" for more information.
A pin can be defined as Hidden (not shown in schematic). A
typical example of using a Hidden Pin is the Pseudo Device
defined to represent the Ground Symbol. Normally you do not
want to see a pin number assigned to a Ground Symbol.
Please refer to "Surface-Power-Trace and Surface-Ground" in
Section "Advanced Technique" for more information.
PinAtt :
For every Pin of a Device, there is a set of data associated with
it. These data describe the following:
The type of I/O. The Fan In and Fan Out capabilities. If it is a
power pin, the voltage it is at. If it is a Pseudo Pin, the special
characteristic.
Refer to "Defining Library Parts" for more information.
Plot :
Enter schematic Plotting mode. Refer to Section "Printing and
Plotting".
Post :
Enter Post-Processing operation. When IFK-Post is selected, a
list of options is given to you; you can select Net, BOM, Map,
PgRef, ErrChk, and the disk drive where the results should go.
The list of schematic files are also given to you on the screen,
if you choose a page of a schematic, the whole schematic (all
pages) will be included in the Post Processing. All schematic
files having the same filename (with different numeric
extensions, e.g. xxx.1, xxx.2, etc.) are considered part of the
schematic.
Please refer to Section 3.8 : "How to generate the Net List,
BOM etc".
Print :
Enter schematic Print out operation. Refer to Section
"Printing and Plotting".
Recall :
In DefDev/Attr/PinAtt (Define Device/Attribute/Pin Attribute)
mode, IFK-Recall is used to call out the Pin Attributes
previously defined. The display shows blank entries for
whichever Pin Attributes not defined previously. You can use
the IFK-Next to scan through all pins of the Device being
defined.
Rename :
In the File mode, this IFK-Rename is used to change the
name of a schematic file. Note that when you change the
name of any one page of the schematic, all pages of the same
schematic will have their named changed also.
Please refer to IFK-Copy.
Repeat :
In Line Mode, after you draw one line segment at a pin, if you
press Repeat, the same line segment will appear on another
pin (of the same IC), if any, below the current pin.
Rotate :
To Rotate the Device. When you call out a Device and before it
is settled, the Device is rotated by 90 degree every time you
press this IFK-Rotate.
Rubber :
You can perform a rubber-band Move (Rubber Move) by
selecting IFK-Rubber. Rubber Move allows you to move a
Device without breaking its connections. You can only Rubber
move one Device at a time. After the Rubber Move, you can
enter the IFK-Line/Adjust mode to Adjust the Lines (refer to
IFK-Adjust).
SavDev :
After you finish defining a Device, this IFK-SavDev (Save
Device) allows you to Save the Device under a filename given
by you.
Same Device using different Symbols can be Saved under
different filename.
Save :
Edit/More/Save saves the schematic. In Edit mode, You can
also Save the schematic simply by pressing <ESC> several
times until the Entry at the bottom of the screen says 'Quit,
Save, or Continue', press 'S' to Save the schematic and then
quit the Edit.
SavPin :
After all Attributes of a Device Pin are defined, you can use
this IFK-SavPin to save the attributes to a Pin, at this time, you
can also key in another pin number having the same pin
attributes and save it.
Please Refer to Section "Defining Library Parts".
SavSym :
Symbols are defined under DefLib/DefSym, after you finish
defining the Symbol, pressing this IFK allows you to save the
Symbol.
There is another way to Save the Symbol, you can keep
pressing <ESC> until you see a question on the entry line
asking whether you would like to Save, Quit or Continue. If the
answer is a 's', the Symbol will be saved.
SetRef :
In DefLib/DefSym mode, this IFK-SetRef allows you to set one
reference point on the screen, the relative positions of other
points with respect to this point is shown as X, Y coordinates
(relative) in units of Pixels. 3 Pixels is equal to 1 mm, and
Symbols are drawn to the size of 3/8 Template (ANSI Y32.14,
MIL-STD-860).
Signal :
Add or delete Signal Name of a line. Enter Signal Name and
click (Add button) at line to add or click (Delete button) at
Signal Name to delete. You can put the signal name above
the line (IFK-Above), below the line (IFK-Below), or at the end
of the line with a box around it (IFK-Conn, normally used for
connectors).
Small :
Select small size Text.
Step @ :
Step down (IFK-Down) or up (IFK-Up) the number embedded
in the Signal name and place it at the next lower line.
Stripe :
In Edit/Note/Stripe mode, add or delete Stripes as Notes.
In DefLib/DefSym mode, add or delete Stripes as part of the
Symbol, the Stripes of a Symbol can not be modified during
schematic capture (Edit) mode. Stripes has no effect to the
Net List. Unlike Lines, Stripes can go in any directions, and
when two orthogonal stripes is jointed together, Dot is not
added in automatically.
SubDir :
Look into the Sub-Directory of a Library.
To view the library. The list of all libraries are shown on the
screen. You can select one of the libraries and browse its
content.
SymDir :
When you try to call a Symbol (IFK-CalSym) and forgot the
name of the Symbol, you can use this IFK-SymDir to browse
the Directory of the Symbol Library.
System :
This IFK-System is used to select some system options such
as :
The disk drive in which you put the Library Disk, the disk
drive in you put the Data (User or Schematic) Disk. You also
have control over the Grid display, Grid Snap, and Grid Size.
Text :
In Edit/Note/Text mode, enter Text as notes, the Text can be
added or deleted at will.
In DefLib/DefSym, enter Text as part of the symbol, the Text
can not be modified during schematic capture (Edit) mode.
Title :
Used to Call a Title Block from the library. Title Blocks have
many different forms. For example, a title block may include a
title area, part number area, revision level area, signature area,
mechanical tolerance area, and outline of the drawing, etc. Or,
the title block may include a part number area only. You can
define Title Block in DefLib/DefSym as if you were defining a
Symbol; the difference are: (1) When you draw the bound for
the Title, you must make the bound exactly the same size as
your outline of the Title Block. (2) When you save the Title
Block, you must use a Symbol name "SymName.title". The
SymName is any name assigned by you and ".title" is
mandatory. You can find some Title block examples in the
Symbol Library.
ToDf0: :
Tell the Post Processing where to put its result, IFK-ToDf0:
directs the result to floppy drive 0.
ToDf1: :
Tell the Post Processing where to put its result, IFK-ToDf1:
directs the result to floppy drive 1.
ToDh0: :
Tell the Post Processing where to put its result, IFK-ToDh0:
directs the result to hard drive 0.
Up :
When IFK-Signal is active, IFK-Up forces the number
embedded in the Signal label to increment by one (1) every
time IFK-Step@ is pressed.
Zoom Up by 2X (Devices are 2 times as big as what is
currently shown. First Zoom-Up may be smaller than 2X
depending on the paper size.
Value :
Allows you to enter the values of Passive Devices when you
are entering the schematic. You do this by clicking at the
Device Name Label (the color of the Label will be changed).
V-Ref :
When this mode is selected, clicking the Add (left) button of
the mouse will add in an Vertical line on screen. This line is of
type NOTE (see NOTE mode); which has no effect to the
connections between Devices (i.e. no effect on the NET-LIST).
It is used for alignment purposes such as lining up the Signal
Name, or the position of Devices, etc.
Reference lines are not printed or plotted.
Weight :
To assign the priority of the line in routing. Heavier means
higher priority in routing.
Lines without weights are defaulted to have 0 priority.
Priorities range from 0 to 999.
Weights can be placed above (IFK-Above) or below (IFK-
Below) the line.
Weights are all hiddenng Wide Stripes.
Yes :
The answer to your question, my friend, is 'YES'.
Zone-1, 2, and 3 :
These IFK's are used optionally to optimize the automatic
Device Number assignment.
The concept behind this Zone control feature is based on :
- Physically far apart Devices should not reside in the same
package (e.g. IC).
- logically adjacent Devices in the schematic are likely to be
physical adjacent on the PCB also.
If you know the approximate locations of different sections of
the logics (such as Input, Processing, and Output) on the PCB
before you draw the schematic, then you can optimize the
Auto Device Number assignment by selecting one of the
Zones before calling out a Device from the Library.
By doing so, you have avoided the situation where a section
of an IC is used in one area of the PCB, while another section
of the same IC is used in another area that is far apart from the
first area.
You can change your mind later by swapping gates or by
changing the Zone assigned to a device. These are done in
Modify/Label.
ZoneX :
To assign Device Numbers manually, select ZoneX. This is
most commonly used when the Device Numbers are known in
advance. For example, when you are entering an old
schematic.
Zoom :
First time you hit zoom, the pictures shrinks so that you can
see more. After that, you have the choices of Zoom Down
(IFK-Down), or Zoom Up (IFK-Up).
IFK-Norm always brings you back to the normal
LIBRARY PARTS:
Sub-libraries
PRONET Library is made up of sub-libraries such as TTL, CMOS etc.
Sub-libraries must be opened before they can be used.
Sub-libraries are opened when you create a new schematic page. You
can also open or close Sub-libraries under the Device screen.
Please refer to Section "Directory Structure" under "Terms and
Conventions".
User Library
To increase speed, the user may want to copy part of the libraries to
one library and add to it whatever he/she wants. In this case, the parts
PRONET needs to search are substantially reduced, and only one
library need be opened at all times.
Library structure
Each part that you call out from the library to the schematic is call a
Device. The Device consists of two parts: the Symbol and the Device
Specific Information (Info, in short). Their relationships is depicted as
follow:
Symbol + Info = Device
where:
Symbol contains the graphic description of the Device(s). A Symbol
could be used by many different Devices as long as they have the
same graphics. The user can define the Symbol under DefLib/Defsym
(Define Library/Define Symbol).
Info contains Device specific information such as pin number
assignments, pin attributes, current consumption of the Device, etc.
Besides pin number, normally, the rest of the information cannot be
shared by different Devices. The user can define the Info under
DefLib/DefDev (Define Library/Define Device).
DEFINING LIBRARY PARTS:
When you are in the Library define mode, unlike in schematic capture
mode, the template size is fixed at 3/8 (MIL STANDARD 860);
therefore, the grid sizes are also fixed. The grid #1, #2, #3, #4 sizes
are 1 mm, 2mm, 4mm, 8mm respectively.
In the DefLib (Define Library) mode, the IFK-DefSym and the IFK-
DefDev are used for defining the Symbol and the Device, respectively.
There is also an utility program that comes with PRO-NET, so that you
can copy Devices from one library to another.
NOTE THAT YOU CAN NOT COPY DEVICES USING AMIGA DOS FILE
COPY COMMAND, SINCE PRO-NET MAINTAINS ITS OWN
DIRECTORY (FOR SPEED PURPOSES). COPY DEVICES BETWEEN
SUB-LIBRARIES USING AMIGA DOS FILE COPY COMMAND WILL
CORRUPT THE PRO-NET DIRECTORY SYSTEM.
How to Define Symbol
Basically, to define a Symbol is to draw the picture that represents the
Device.
There are two ways to define a Symbol:
(a) By Modifying an existing Symbol: You can call out an old
symbol, modify it to form a new Symbol, or You can combine
some old symbols to form a new Complex Symbol. However,
you cannot call out an old Complex Symbol and try to modify
it.
(b) By Drawing the Symbol: You can create the Symbol using
tools provided to you under DefSym. In the DefSym screen,
you can find a set of IFK's to help you draw the Symbol. These
IFK's are the Text, Stripe, Box, Circle, Arc, CalSym, Bound,
Save, SetRef, and System. Refer to the Command Description
section for the details of each IFK.
You could use the hot keys (refer to the CONVENTION section) to
control the grid size and grid snapping, etc. We recommend that you
select grid Snap whenever possible, this will make drawing the
schematic even easier.
Before you save the Symbol, you have to define the Bound (Boundary)
of the Symbol.
You must observe the following rules:
RULE #1
Bound MUST pass through the tip of every pin on the Symbol
or, if that side of the Device Body has no pin(s), must be
bigger than the Device by one #2 grid (2 mm).
RULE #2
The body (outline) of the Device must be of Wide Stripes
(lines) in order that you have the option of printing/plotting the
Device using narrow lines or wide lines.
RULE #3
When you call out an existing Symbol to be modified to
another Symbol, you may not call out complex Symbols. All
complex Symbols have the extension of ".C".
Also, experience tells us that if you adhere to the following
guide lines in defining symbols, you can draw the schematic
easier, faster, and better. Nevertheless, these remain guide
lines, no errors will result if you don't follow them :
GUIDE #1
Keep in mind that the gates (such as 7400) are defined using
3/8 template (MIL-STD-860 or ANSI Y32.14 standard) and that
the smallest grid (grid #1) equals 1 mm, try to draw the
Symbol as small as possible while as big as needed to show
all necessary details (such as the "D", "Q" etc. inside the
symbol of 7474) of the symbol.
Note that grid #2, #3, #4 are 2 mm, 4 mm, 8 mm respectively
when the template is 3/8 inch.
GUIDE #2
Use grid Snap whenever possible -- even if you have to bump
down the grid size to a smaller one.
Normally you should try to stay on #2 grid.
GUIDE #3
If you are using a floppy disk system, Library is distributed on
several floppies, every Library disk has one or more Device
Sub-libraries AND a Symbol sub-library. Therefore, if you
change or add a Symbol, not only that you have to save the
Symbol to the floppy disk (that holds the sub-library) that you
are working on, but also ALL other sub-library disks. If you
delete a Symbol (which is unlikely), you need to do the same
on ALL sub-library disks.
If you have a hard disk system, you only have one Symbol
Library in one place, therefore, you only need to update that
one library when you modify Symbol.
How to Define Device
Basically, to define a Device is to specify all the Device
specific information of that Device. This information includes:
-- the Symbol to use
-- the location of each pin
-- the Device Name.
-- the default location of the Device Name Label.
-- the Device Number label.
-- the default location of the Device Number label.
-- the Symbol to be used for the DeMorgan equivalence
(if any) of the Device.
-- (you may want to save the Device at this point and do
something else for a while, see HINT below).
-- the characteristics (attributes) of each pin.
-- the current consumption of this Device.
HINT :
For example, if you are defining Device 74LS00, you may want
to save all the information to 74LS00, then also save to 74S00,
74F00, 74AS00 --- etc. Note that this is alright because up to
this point, all the information you have entered for 74LS00 is
shared by the corresponding Device in the other families.
To define a new Device or to edit an existing Device in the
Library, the steps are:
1. from Level 1 screen, Select DefLib (define library)
2. select DefDev (Define Device)
3. select the Sub-Library in which you want to find the old
Device to edit or to store the new Device. Press IFK-OK.
4. A list of Device in the selected Sub-Library is displayed,
you can scroll up and down to find the Device you want to
edit or you can select IFK-New and specify a new Device
Name to define a new Device.
5. At this point, you start to specify all the Device specific
information; type in the Symbol Name if you know which
Symbol to use for this Device. Or, you can choose a
Symbol from a list under DefDev/Calsym/Index.
6. After the symbol is retrieved, select IFK-Pin, enter the pin
number you want to associate a line (graphic of the pin)
with, then click at one of the four quadrants of the tip of the
pin. The pin number will appear in that quadrant near the
tip of the pin as follows:
q1, q2, q3, q4 represent the four quadrants of the tip of the
pin. All you need to do is enter the pin number and click
close to the pin in the quadrant you want the pin number to
appear in.
Repeat the process until all pins are specified.
If you don't like what you have just defined, you can clear
all pin definitions by selecting IFK-AllClr. Pin number could
also be hidden (not shown in schematic) in which case,
you have to select IFK-Hidden before specifying pin
location.
If the Device has several sections, you could go to the next
section by using IFK-NxtSct.
7. The next thing you want to do is to specify the Labels.
Select IFK-Label, then IFK-DevNam, See if the Device name
in the entry line is exactly what you want, if so, click the
mouse to place the DevNam at the desire location.
Or, if the Device name in the entry line is not what you
want, just retype the Device Name, then click the left
mouse button to place it at the desired location.
Again, the Device name could be hidden.
8. Now you want to enter the Device Number, it is not really a
number, rather, it is the Prefix of the Device Number.
Select DefDev/Label/DevNum, enter the Device Number
(prefix), click the mouse left button to place it at the desired
location.
For example, for an IC, we normally call it 'U' something. In
that case, enter 'U' and click the left mouse button to place
it at the desired place.
Again, the Device Number can be hidden.
9. If the Device has a negative logic symbol (DeMorgan
equivalence), and you have already defined it using Define
Symbol, then you can select IFK--Logic, enter the Symbol
name, and <CR>.
10. Now, you are almost done, the remaining task is to define
the Attributes of the Device. This is necessary if you want
PRONET to perform Loading Analysis for you or to perform
the Power Consumption Calculation for you.
Under Attr (Attributes), there are the Icc (Icc) Attribute and
the PinAtt (Pin Attribute).
-- In Icc, enter (or reenter) theÿ Worst Case Current
consumption of the whole Device.
-- In PinAtt, basically you call (Recall) the attributes of a pin on
the screen, then modify existing attributes or enter new
attributes. You do this one pin at a time until all the pins of
the Device are done. You could check them by using IFK-
Next to scan through all pins, make sure they are correct,
then save the pin attributes using IFK-SavPin. The following
IFK's help you accomplish these tasks:
IFK-Recall
When this IFK is selected, you could enter the
pin number and recall the attributes that you
have defined previously.
IFK-Next
Display the attribution of the next pin.
IFK-Modify
If you do not like the attributes displayed, you
can use this IFK to modify them.
To define the pin attribute, normally you refer to the Data book of
the Device.
<A> Device Pin
Select one from the following list in line 1.
I specify that this is an Input pin.
O a totem pole Output pin.
B a Bidirectional pin (including a pin of a
passive device with current attributes).
C an open Collector pin. a
T Tri-state pin.
P a pin of a Passive Device with no current
attributes.
V a Voltage pin such as Vcc Pin or Gnd (0 V)
pin.
<B> Driving Capability of the pin
Fill in the WORSE CASE value of the current sunk
or sourced by the pin under consideration.
Specify Iih, Iil when the pin is an Input pin.
Specify Ioh, Iol when the pin is an Output pin.
Specify all Iih, Iil, Ioh, Iol when the pin is a
Bidirectional pin.
If it is Voltage pin, specify what voltage the pin is at.
For example:
If the pin is a 5V pin, key in a "5". If the pin is a GND
pin, key in a "0".
If it is a pin for a passive part, the current entries
are normally ignored since the value (e.g. 1K ohm)
of a passive part is entered during the schematic
capture phase (when you are drawing the
schematic); without the value and without knowing
the exact situation in which the passive part will be
used, the current attributes can not be specified.
The loading analysis will flag a warning message in
the .ERR (error) file saying that the passive part is
not accounted for and that the manual verification
for the node (that has the passive part) is needed.
HINT:
To reduce the amount of manual verification, you
can predetermine the value and the current
attributes of a passive device during DefDev and
limit its usage to a particular application. This
allows the PRONET to include the passive device
in the loading analysis automatically. To do this,
you need to define the pin of the passive device as
'B'(Bidirectional) rather than 'P'(Passive).
For example :
A pull up resistor SIP, if it is pulled up to +5V, and
the value is 1K ohm, then, each pin of the resistor
SIP is of type 'B' and the current attributes are:
Iil = 5 mA
Iih = 0
Iol = 0
Ioh = 5 mA
The loading analysis will take this SIP into account
automatically.
<C> Prolific specific characteristics
This is a numeric number, each value specifies a
special characteristics of the Device (or its pin):
VALUE MEANING
1. Pseudo Device, for Surface Trace purpose. (see
Section 9.1 Surface-Power-trace and Surface-
Ground)
2. Pseudo Device, for Power Planes direct
connection (Refer to section 9.1).
3.
undefine
| |
| |
| |
11. Save the Device definition. Two ways to do it are :
<A> After defining the Pin Attributes, hit <ESC> to back up to
one higher IFK level. Then use IFK-SavDev (Save
Device) to save the Device definition.
<B> Keep hitting <ESC> until you see a question in the entry
line asking whether you would like to Save, quit or
continue. If the answer is an "S", the Device definition
will be saved.
PRINTING
The printer you use is selected in the AMIGA preference.
Your drawing size and template size is determined in the design rule
you choose when you create that drawing.
When the drawing size is bigger than the printer's printing area, PRO-
NET automatically divide the drawing into sections, and print them
one at a time until all done.
EPSON OR EPSON COMPATIBLE PRINTERS :
Interface Protocol:
Centronic Style Parallel Interface
Interface Cable:
-- For AMIGA 1000, use a cable as follow :
Centronic type AMIGA 1000
36 pin male DB 25S (female)
1 STROBE- ------------ 1
2 DATA 0 ------------ 2
3 DATA 1 ------------ 3
4 DATA 2 ------------ 4
5 DATA 3 ------------ 5
6 DATA 4 ------------ 6
7 DATA 5 ------------ 7
8 DATA 6 ------------ 8
9 DATA 7 ------------ 9
10 ACK- ------------ 10
11 BUSY ------------ 11
12 PE ------------ 12
13 SELECT (PWR ON) ------- 13
14 AUTO-FEED-
15
16 LOGIC GND ------------ 16
17 CHASSIS GND
18 +5 V
19 GND ------------ 14
| | --multiple-- |
30 GND ------------ 22
31 INIT- ------------ 25
32 ERROR-
33 GND
34
35
36 SELECT-
-- For AMIGA 500/2000 use a cable as follow :
Centronic type AMIGA 1000
36 pin male DB 25P (male)
1 STROBE- ------------ 1
2 DATA 0 ------------ 2
3 DATA 1 ------------ 3
4 DATA 2 ------------ 4
5 DATA 3 ------------ 5
6 DATA 4 ------------ 6
7 DATA 5 ------------ 7
8 DATA 6 ------------ 8
9 DATA 7 ------------ 9
10 ACK- ------------ 10
11 BUSY ------------ 11
12 PE ------------ 12
13 SELECT (PWR ON) ------- 13
14 AUTO-FEED-
15
16 LOGIC GND ------------ 16
17 CHASSIS GND
18 +5 V
19 GND ------------ 14
| | --multiple-- |
30 GND ------------ 22
31 INIT- ------------ 25
32 ERROR-
33 GND
34
35
36 SELECT-
9.0 PLOTTING
The model number of the plotter you use is selected when you
configure (IFK-Config) PRO-NET.
The paper size and template size are selected in the Design Rule
which you have chosen when you start (IFK-Edit/New) drawing that
page. You could review what you have selected by using IFK-
Device/ChgLib.
PRO-NET does not allow you to plot a page that is bigger than
what your plotter can handle.
9.1 HOUSTON INSTRUMENT (H.I.) PLOTTERS
All H.I. Plotters should be set up as follow:
Interface Protocol:
RS232 Serial
Baud Rate : 2400
# of Bits : 7 Bits
Bit 8 : always logic 1 (high)
Parity : no parity
Handshake : XOn/XOff
Set both the plotter and the AMIGA preference to the above Serial
protocol.
Note that to set the plotter to XON/XOFF mode, you need to use the
plotter panel and set ?? RTS/CTS to always high which means that
XON/XOFF is selected . Also you may want to set the Text Font to
Simple type for higher plotting speed.
9.1.1 H.I. Model 695, 695A
Paper Size: A size 8.5 X 11 inches
B size 11 X 17 inches
Plotting Area: A size 7 X 9.5 inches
B size 9.5 X 15.5 inches
Pen recommended :
H.I.--
MA-17 Adaptor
MP-815 .35 mm stainless steel tip
KOH-I-NOOR--
7009WOP Adaptor
63TB-00/.30 .30 mm Tungsten tip
63TB-0/.35 .35 mm Tungsten tip
63TB-2/.60 .60 mm Tungsten tip
63TB-2.5/.70 .70 mm Tungsten tip
Interface Cable:
-- For AMIGA 1000, use the H.I. cable 375-98 :
Plotter Side AMIGA 1000 Side
RJ12 6 pin plug DB25P (male)
1 (not used)
2 TxD ------------ 3 RxD
3 RxD ------------ 2 TxD
4 GND ------------ 7 GND
* 5 DTR ------------ 5 CTS
6 (not used) 6,8,20,22
tie together
others pins
not used
* actually not used by PRO-NET
-- For AMIGA 500/2000, use the H.I. cable 375-99 :
Plotter Side AMIGA 500/2000 Side
RJ12 6 pin plug DB25S (female)
1 (not used)
2 TxD ------------ 3 RxD
3 RxD ------------ 2 TxD
4 GND ------------ 7 GND
* 5 DTR ------------ 5 CTS
6 (not used) 6,8,20,22
tie together
others pins
not used
* actually not used by PRO-NET
8.1.2 H.I. Model DMP-41, DMP-42, DMP-51, DMP-52, DMP-56 :
Paper Size:
A size 8.5 X 11 inches
(DMP-56 only)
B size 11 X 17 inches
(DMP-56 only)
C size 17 X 22 inches
D size 22 X 34 inches
E size 34 X 44 inches
(DMP-56 only)
Plotting Area:
A size 7 X 9.5 inches
(DMP-56 only)
B size 9.5 X 15.5 inches
(DMP-56 only)
C size 15 X 20 inches
D size 20 X 32 inches
E size 34 X 44 inches
(DMP-56 only)
Pen recommended :
H.I. (Non-refillable)--
MA-15 Adaptor
MP-729 to 776 .35 mm stainless steel tips
MP-737 to 783 .70 mm stainless steel tips
KOH-I-NOOR (Refillable)--
7006WOP Adaptor
63TB-00/.30 .30 mm Tungsten tip
63TB-0/.35 .35 mm Tungsten tip
63TB-2/.60 .60 mm Tungsten tip
63TB-2.5/.70 .70 mm Tungsten tip
Interface Cable:
- For AMIGA 1000, use a cable as follow :
Plotter Side AMIGA 1000 Side
DB25S (female) DB25P (male)
2 TxD ------------ 3 RxD
3 RxD ------------ 2 TxD
7 GND ------------ 7 GND
6,8,20,22
tie together
others pins
not used
-- For AMIGA 500/2000, use the H.I. cable HR29-316 or H.I. Smart
Cable 825 or a cable as follow :
Plotter Side AMIGA 500/2000 Side
DB25S (female) DB25S (female)
2 TxD ------------ 3 RxD
3 RxD ------------ 2 TxD
7 GND ------------ 7 GND
6,8,20,22
tie together
others pins
not used
10.0 ADVANCED TECHNIQUES:
10.1 Surface-Power-trace and Surface-Ground
PROBLEM DESCRIPTION:
IC pins sometimes are tied to power supply lines such as +5V or
Ground. For a PCB that has a power plane and a Ground plane, there
are two ways you could tie them. First, you could tie those power
supply pins directly to the Power or Ground plane. Second, you could
tie those non-power-supply spare pins (that should be tied to power or
ground) to Power or ground through surface traces on the solder side.
The reason for the second method is such that engineers could
modify (let's face it, this is inevitable!) the design by cut and jump
those pins. Although the above approaches are common practice
among engineers, it is traditionally a problem not taken care of even
by those schematic capture and PCB layout CAD systems that cost 50
times more than PRO-NET and PRO-BOARD. In those cases, PCB
designers have to patch up Net list, put in special traces which may be
forgotten in the next round of PCB update.
SOLUTIONS:
PRO-NET and PRO-BOARD work hand in hand to solve the problem.
Now, using PRO-NET, you could draw schematics that carry enough
information such that the Layout program PRO-BOARD could create
those surface power and surface ground traces automatically if
desired.
Using the user definable attribute feature of the library parts (see
Chapter 5), we have defined some special Devices in the library. They
are called the Surface PoWer (Ground), and PoWeR (Ground). They
are defined as follow:
1. SPWR+5VN : Surface PoWeR +5V at North Side -
* indicates non-display label
Prolific Special attribute = 1
indicates that this is a pseudo Device of type Surface power
or surface ground.
2. SPWR+5VS : Surface PoWeR +5V at South Side -
* indicates non-display label
Prolific Special attribute = 1
Indicates that this is a pseudo Device of type Surface power
or surface ground.
3. SPWR0VS : Surface PoWeR 0 V at South Side -
* indicates non-display label
Prolific Special attribute = 1
Indicates that this is a pseudo Device of type Surface power
or surface ground.
4. PWR+5VN : PoWeR +5V at North Side -
* indicates non-display label
Prolific Special attribute = 1
Indicates that this is a pseudo Device of type Surface power
or surface ground.
5. SPWR+5VS : Surface PoWeR +5V at South Side -
* indicates non-display label
Prolific Special attribute = 1
Indicates that this is a pseudo Device of type Surface power
or surface ground.
6. SPWR0VS : Surface PoWeR 0 V at South Side -
* indicates non-display label
Prolific Special attribute = 1
Indicates that this is a pseudo Device of type Surface power
or surface ground.
7. Similarly, user could define other power supply pin of other
voltage.
If you connect some pins of an ordinary Device to the above pseudo
Device, PRO-NET understands that you want these pins to be tied to
power or ground through surface traces instead of the power or
ground planes directly.
10.2 Scattered Connector
PROBLEM DESCRIPTION:
Traditionally there are several ways of drawing a connector in a
schematics:
1. The connector is drawn on one page with signal
names and page references. Each pin of the
connector is connected to another page or pages
through the signal names alone.
2. The connector is broken up into pieces of single pin
or groups of pins and scattered among pages of the
schematic.
3. The connector is drawn once in method 1, and again
in method 2.
Method 1 is best suited for schematic capture program, since the
connector could be defined as one library part.
Method 2 is normally difficult for schematic capture program because
a connector of 100 pins require the user to define 100 different library
parts, each has one pin.
Another problem of drawing a connector is when the connector has
pin numbers other than numerics. This presents a problem both to
schematic capture and to PCB layout program. In this case, pro-net
(and pro-board) requires that you use method 1 or method 3 to draw
the connector.
SOLUTIONS:
Pro-Net allows user to draw connectors in all three methods listed in
above with certain limitations. If some of the connector pins are
designated by alphanumerics other than pure numerics, then either
method 1 or method 3 must be used.
When Pro-Net is producing the Net List, it will perform two things on
the connector:
a. Connect pins of Devices to pins of the connector
together through matching of the signal label.
b. Connect pins of Devices to pins of the connector
according to the connector label if and only if the pin
number portion of the connector label is pure
numerics.
If you use method 1 (connector in one place) to draw the connector,
correct net list is produced by step a above.
If you use method 2 (scattered) to draw the connector, correct net list
is produced by step b above.
If you use method 3 (both ways) to draw the connector, the correct net
list is produced by step a as well as step b if the designation (label) of
the connector pin is purely numerical. If designation is not purely
numerics, method a is used to produce the correct net list.
By now, you should be confuse enough to demand for some
examples. As you wish, here are some examples:
EXAMPLE 1:
A VME bus Euro-Din connector is used in a design. The connector
pins are designated as J4 (say) -A1, J4-A2... J4-C1, -C2, -C3......etc.
The correct way to draw this connector is by method 1 (in one place)
or method 3 (both ways), since the pin designation is not purely
numerics. ..page Method 1: On page 20 (say) of the schematic, call
out the library part which looks like:
J4 is analogous to the U number of an IC. A1, A2 etc. are analogous to
the pin function label of, say, the "Q" label in symbol 7474. "name 1",
"name 2" etc. are signal names of lines. Connector pin 1 is defined to
be the pin labeled by A1, pin 2 is A2, pin 32 is A32, pin 33 is C1, pin 63
is C31, pin 64 is C32 etc.
However, all pin numbers are defined with attribute "hidden" and thus
not shown on display or print out of the schematic.
On Page 7 (for example) of the schematic, some pins of the connector
are connected to different circuits:
Method 3: On page 20 (for example) of the schematic, call out the
library part which looks like:
J4 is analogous to the U number of an IC. A1, A2 etc. are analogous to
the pin function label of, say, the "Q" label in symbol 7474. "name 1",
"name 2" etc. are signal names of lines. Connector pin 1 is defined to
be the pin labeled by A1, pin 2 is A2, pin 32 is A32, pin 33 is C1, pin 63
is C31, pin 64 is C32 etc.
However, all pin numbers are defined with attribute "hidden" and thus
not shown on display or print out of the schematic.
On Page 7 (for example) of the schematic, some pins of the connector
are connected to different circuits. The connector symbol (box
around pin label) is created by using IFK "Conn" (connector), press
"Conn", then type in the connector pin label such as "J4-A2", then
click at the end of the line where you want the connector symbol to
occur.
Here, since the pin number part of the pin function label is not purely
numerics, for example, the "C31" in the connector pin function label
"J4-C31" is not purely numeric, therefore, Pro-Net could not use the
connector pin function label to create the correct net.
In this example, Pro-Net uses the signal label "name 63" to match the
one that occur on page 20, where "name 63" is the signal name for
the line that is connected to connector pin 63. The pin number label
"63" is defined as "hidden" and whose pin function label is defined as
"C31". Therefore, Pro-Net produce a net which specifies the
connection of U22 pin 5 to J4 pin 63.
EXAMPLE 2:
A 50 pin D type connector is used in a design, the pin numbers of this
type of connector are all pure numerics, therefore, all three methods
listed in beginning of this section could be used. Method 1 and
Method 3 are similar to example one. The following describes the
method 2.
Method 2: Only scattered connector symbol are used.
On Page 7 (for example) of the schematic, some pins of the connector
are connected to different circuits. The connector symbol (box
around pin label) is created by using IFK "Conn" (connector), press
"Conn", then type in the connector pin label such as "J4-A2", then
click at the end of the line where you want the connector symbol to
occur.
Here, Pro-Net uses the pin number that is embedded in the connector
pin label to generate the net list connections. Thus J4 pin 2 is
connected to U15 pin 12.