This is only a preview of the May 2009 issue of Silicon Chip. You can view 31 of the 104 pages in the full issue, including the advertisments. For full access, purchase the issue for $10.00 or subscribe for access to the latest issues. Articles in this series:
Items relevant to "Dead-Accurate 6-Digit GPS-Locked Clock, Pt.1":
Items relevant to "230VAC 10A Full-Wave Motor Speed Controller":
Items relevant to "Precision 10V DC Reference For Checking DMMs":
Items relevant to "Input Attenuator For The Digital Audio Millivoltmeter":
Purchase a printed copy of this issue for $10.00. |
Give your circuit
that PROFESSION
When it comes to contributed projects or circuits, there are
few things more frustrating than finding the circuit has been
drawn (apparently) by “a thumbnail dipped in tar” – or near
equivalent. Here’s an easy way to make them look good!
N
ot only do poorly presented
circuit diagrams increase the
likelihood of errors, they also
make it more difficult to understand
the basic circuit operation.
And if those at SILICON CHIP cannot understand it, how are readers
going to?
The Editor will be much more impressed by a neatly laid out diagram
with standardised symbols, all components at right-angles and all the
components in scale.
How do you do it?
Many years ago Protel had a circuit
drawing package called Schematic.
Unfortunately it was less than acceptable – the frustration and poor results
with this program prompted me to
think about an alternative.
The one I use might sound a little
unusual at first glance. It’s the Protel
Autotrax PCB (Printed Circuit Board)
layout package which of course is
intended to lay out PC boards. But
I find gives excellent results when
drawing circuits – and as a bonus is
quite easy to use.
An even bigger bonus is that it won’t
cost you anything. Now well and truly
superseded, Protel Autotrax can be
downloaded free from www.altium.
com/altium/altiumsite/community/
downloads/altium-freeware-enduser-license-agreement/en/autotrax.cfm
If you find entering all that a bit
daunting, simply go to www.altium.
com and go to the “community” tab,
thence “downloads”!
This program was covered quite
thoroughly (mainly in its normal PC
board layout mode) in the February,
March & April 2004 editions of SILICON
CHIP. So I won’t go into all that detail
again but will cover aspects of using
it as a circuit drawing program.
Briefly, though, you need to know
that Protel Autotrax has two parts – the
first, the part you actually “draw” with,
is called TRAXEDIT.EXE. When you
want to print out your masterpiece,
you’ll need the second part, called
TRAXPLOT.EXE.
However, be warned: as Autotrax
is getting pretty long in the tooth (it’s
Which one looks better?
This one or the one on
the right? Unfortunately,
the example at left is
a positive masterpiece
compared to some which
we see!
72 Silicon Chip
siliconchip.com.au
diagrams
NAL look!
been around since the 1980s) video
and printer drivers can be problematic.
In fact, we seldom use Traxplot – at
SILICON CHIP we work mostly with
EPS (encapsulated Postscript) files and
use a little utility called “GRABEPS”
which converts Autotrax (*.PCB) files
directly into *.EPS files.
Grabeps can be downloaded from
www.electronicsaustralia.com.au
Will Autotrax
work on
XP and VISTA?
Being a DOS-based program,
Protel Autotrax performs best on a
computer operating under DOS.
However, that is not to say it
won’t operate under a Windows
command prompt because, in most
cases, it certainly will.
We have had no major problems
using Protel Autotrax on PCs running Windows 98, 2000, ME and
XP. As Rick Walters has mentioned
in this article, drivers for particular
printers and video cards might be
something of a problem; however
(so far!) not for us.
You might have noticed that the
list above doesn’t mention Windows
Vista. This is a whole new ballgame
because it works quite differently to
the earlier operating systems.
Unfortunately we haven’t had
the opportunity to test Autotrax on
Vista before going to press (like
many organisations, our computers
primarily operate under Windows
XP).
There is a fair amount of discussion on the net about operating old
DOS programs under Vista – the
majority suggest that using a program called DOSBox (or several
similar programs) will allow you to
use most DOS-based software on
a Vista machine.
by
Rick
Walters
find the folder labelled SCHEMATI
in the May 2009 section and click or
double-click on it. It will open, showing a single zipped file. Download and
save it to c:\schemati.
You will need to unzip them before
use – in the majority of cases, doubleclicking on a *.ZIP file will bring up
the appropriate unzip utility – but if it
doesn’t, there are numerous zip/unzip
utilities which you can download from
the web.
Before you start
Firstly we need a dedicated directory which I have (for obvious reasons) called SCHEMATI (DOS-based
programs cannot use directory or file
names with more than eight characters).
If you don’t know how to create a directory (now also called folders), check
the side panel. Create your directory
and call it SCHEMATI or whatever
8-letter name you desire.
It should now appear listed alphabetically under the C: drive. We have
placed all the files you will need in a
directory called SCHEMATI. Log onto
www.siliconchip.com.au/downloads
Drawing a circuit
Drawing a circuit, especially a large
and/or detailed one, is not a simple
task. Some of the larger ones you see
in SILICON CHIP may take many hours,
or even days, to draw.
As well as showing the interconnections between the various devices
the drawing tries to group relevant
components in reasonably close proximity, as well as tending to flow from
left to right with inputs on the left and
outputs on the right.
The area where this often does not
hold true is that we tend to bring power
+5V/+18V
100nMc
100nMc
1
2
3
4
5
6
7
Q12
Q13
16
Vcc
16
Q10
IC1
4060
Q14
2
13
Q6
R
Q5
CKin
CKO1
Q4
1
14
Q8
Q9
Q7
15
CKO2
16
IC2A
C
4518
CE
12
8
Q0
Q1
Q2
R
11
100u
100nMc
Q3
3
4
9
5
10
IC2B
C
Q1
CE
Q2
6
R
15
7
Q0
Q3
11
12
1
13
2
IC3A
C
4518
CE
Q1
Q2
14
8
Q0
R
7
Q3
3
Q0
4
9
5
10
C
IC3B
CE
Q1
Q2
6
R
15
Q3
11
12
13
14
10
9
E
22k
8
200Hz
1k
100Hz
10Hz
RESET
1Hz
0.1Hz
10M
3.2768MHz
TITLE
22p
270p X1
siliconchip.com.au
10p
SIMPLE FREQUENCY DIVIDER
A4H NUMBER
SIZE
DATE 040212 FILE
FDIV1
REV
0
DRAWN R.W.
May 2009 73
Protel Autotrax key commands
As an (old!) DOS program, Autotrax relies extensively
on keyboard commands instead of mouse clicks. Actually,
this works rather well, especially as you get more skilled
in using the program. Most of the letter codes are prettymuch self explanatory. The commands in red are the ones
you’ll use the most for circuits (you can virtually ignore
the rest unless, of course, you’re drawing PC boards!)
How they work
Typing the first character (as shown in bold below)
brings up the options list (which follows). For example,
when you type b (block) you will see a number of options. When you type the second letter, particular option
is invoked.
So bd would be block define (ie, tell Autotrax where the
block is), bm would be block move and so on. br (block
read) and bw (block write) allow you to save a block as a
file and read it back as a component. This is useful where,
for example, you may have six seven segment decoders
driving six LED displays. You draw it once, write it out to
a file, then read it back five times and place it.
The Autotrax commands
b block – allows you to “block off” areas of your diagram and do something with them: d define,
h hide, m move, c copy, i inside delete,
o outside delete, r read, w write.
c current – gives a list of the current setup
d delete – a arc, c component, f fill,
h highlight, p pad, s string, t track, v via
e edit – a arc, c component, p pad, s string,
t track, v via
f file – l load, s save, q quit, plus many more
g grid – s snap: 25, v visible: 100
h highlight – c connection, d duplicate, r reset
i information – c dimensions, c components, plus
others
j jump (to) – c component, c location, c net,
o origin, p pad, s string
l library – a add, b browse, c compact,
d delete, e explode, f file, l list, m merge,
n new, r rename
m move – a arc, b break, c component, d drag
end, f fill, p pad, s string, t track, v via
p place – a arc, c component, f fill, p pad,
s string, t track, v via
s setup – all the options for drawing, already setup for
you
u undelete – allows undeletes from 1 up
z zoom – see S PgUp and T PgDn below
Four arrow keys move the cursor in 25-thou steps
S (Page Up) – Zoom around mouse position
T (Page Down) – Shrink around mouse position
+ (Plus on keypad) – steps through Track Colours –
Red - Yellow - Brown
- (Minus on Keypad) – steps in reverse direction
to +
74 Silicon Chip
in on the right hand side.
An additional benefit of Autotrax is that the IC pins are
numbered with the pin function near the number. This
prevents transcription errors when going from an IC data
book to draft circuit to final circuit.
We will explain how to draw the Simple Frequency Divider Circuit on page 72. Start the program by clicking (or
double-clicking) on the “Traxedit” shortcut in the Schemati
folder. The shortcut tells Windows to run the program in
a window but it actually boots to full screen.
Once TRAXEDIT is loaded it appears on the opening
screen as AUTOTRAX with “Press a key to continue”.
Having pressed, you are presented with a light grey screen
with a grid of white dots.
Across the bottom of the screen (similar to the Windows
Taskbar) is a yellow bar with letters and numbers similar
to the following:
X:2000 – Y:1200 mils – L:Top Layer – a block of colour –
P:Round 50 – T:20 – S:60 – G:25.
In order these mean:
X and Y show the mouse co-ordinates at startup,
L is the layer you are working on,
The block of colour (Red, Brown or Yellow) indicates the
colour of the track you will draw on the screen,
P indicates the pad type and size,
T is the track width,
S is the string size and
G is the grid step.
If you are using the bottom layer, the yellow block of
colour melts into the yellow background, so you won’t be
able to see it.
You will note that after the Y position is the word mils,
which means 1/1000 of an inch, usually abbreviated to
“thou.” (however, for clarity, we generally leave the full
stop out – ie, “thou”).
Even with metrication, most components are based on an
imperial measurement – all through-hole ICs, for example,
have pins 100-mils (0.1”) apart.
Below the X: as you select functions a prompt will appear to assist you.
Drawing a circuit is much the same as “drawing” a PC
board pattern. Instead of pads and physical components,
you select circuit symbols. You join them using very fine
“tracks”, as you would the PC board pads etc.
The first step in drawing a circuit is to define the area in
which we can operate. While Autotrax allows the use of a
mouse it is far quicker to use a combination of the mouse
and keyboard keys.
In the following description (selecting a library) using a
mouse we would click the mouse, move to Library, click
the mouse, move to File and click. Using the keyboard we
would type (Library File).
In both cases the loaded library file will show but it is
obvious which is more efficient and usually much quicker.
Selecting a library
Type lf (or click the mouse as above). Normally we
will use SCHEMATI.LIB. If you can’t remember the library
name, press the keyboard question mark then K and
the libraries will be displayed.
At this stage you only have two, IC.LIB and SCHEMATI.
LIB. Select SCHEMATI.LIB. Type (Place Component)
then type (a horizontal A4 page).
siliconchip.com.au
This screen
grab shows
what you will
see running
Autotrax.
The type of
information
you get
on screen
(bottom strip)
is explained
in the text.
The nearlycompleted
circuit
diagram is
that which is
shown in its
printed-out
form on P73.
Every time you place a component you are asked for a
COMPONENT DESIGNATOR then a COMMENT. For this
component we want neither, so just press K, which gives
you a blank. Locate the A4H outline at 0,0 then press K,
then right click or press P (escape). Now type (Library Explode). The prompt on the bottom line will read
SELECT COMPONENT.
Move the mouse into the rectangle then click or press
K. This will leave a brown outline of the A4 page area
in which our circuit will need to be contained. You will
be asked to confirm.
We explode the library item to turn it into primitives
which means that Autotrax sees the brown outline as just
that and not a component, otherwise we would end up with
a lot of components inside a component and a myriad of
problems. Right click or press P to exit LE.
ESC
ESC
Placing the title block
Next we place the title block but before we do so you
need to zoom the active display, so press the S key on
the keypad twice. This should just about fill the screen
with the brown surround. Press pc (Place Component)
then overtype A4H with TITLE. Again no designator or
comment!
Move it where you prefer it. It’s normal practice to
place it at the bottom right (as you can see). We will come
back and enter some details later but let's keep placing
components.
Placing components
Overtype TITLE with CAP. Again, if you don’t know the
name of the component type a question mark, then press
K. A list of components will be displayed. My approach
is to keep the component name as short as possible, as long
as it is recognisable and identifiable.
Why waste time and effort typing CAPACITOR when CAP
will do? (But don’t be caught using names like “trans” – it
could be a transistor, a transformer, a transducer, a transmogrifier, a transcombobulator . . .)
siliconchip.com.au
As this is the first capacitor we type c1 for the component designator, then press K. For comment we type the
value of the capacitor, 100nmc for a 100nF monolithic
ceramic & press K.
The capacitor symbol will appear and can be moved
about with the mouse. A left click will place it. Repeat
Creating a directory (folder) in XP
Click or double-click (depending on how your computer
is set up) on the My Computer shortcut on your desktop. Click or double-click again on the C: drive (mine is
called WINDOWS_XP) but yours will possibly be named
differently. Click on FOLDERS to divide the screen.
Move the mouse to a blank area on the right hand panel
and Right-click. Move down to NEW, pause a moment,
then across and up to FOLDER. Left-click and a folder
called “New Folder” will be created. While New Folder is
hilighted blue, type SCHEMATI. This name should now
appear alphabetically listed in the left hand panel under
C:
Close My Computer.
Creating a shortcut to schematic
Click or double-click (depending on how your computer
is set up) on the My Computer shortcut on your desktop.
Click or double-click again on the C: drive (mine is called
WINDOWS_XP) but yours will probably be named differently. Find the SCHEMATI directory you have created.
Click on it to open it and the files will be listed in the right
hand panel. Hover over those named TRAXEDIT and find
the one that is TRAXEDIT with no suffix (blue bar at top
with XP). The size should be 170kB. Right click and move
to SEND TO then move to DESKTOP and click. It will be
named SHORTCUT TO TRAXEDIT. You can rename it if
you wish by right clicking and moving to Rename.
May 2009 75
the sequence twice. The capacitors will be sequentially
numbered and the description repeated. Next we will place
the electrolytic, so instead of CAP overtype electro.
It will need to be designated C4, as we have changed the
component type, and the comment will be 100u.
Now place the other three capacitors (CAP) 22p, 270p
and 10p. The crystal identity is XTAL, the designator X1,
the comment 3.2768MHz.
Rotating a component
You will notice that both the crystal and the 270pF
capacitor are rotated by 90° – but we don’t use special
components.
If placing the component, pressing the spacebar will
rotate it 90°; if it is already placed press mc (Move Component), click on it, then press the spacebar. Each press
rotates the component by 90° so four presses brings it back
to where you started!
Next place the three resistors. Their identity is RES,
the first designator R1 and the comment 1k, then 10M &
22k respectively. As previously explained, there are two
libraries: IC.LIB and SCHEMATI.LIB.
We have been using the SCHEMATI library but to place
ICs we have to use the IC library as there is a limit to the
number of components that a library can hold. Right click
to release PC then type lf (Library File), press K & C:\
SCHEMATI\SCHEMATI.LIB will show. Type ic, then
press K.
There is no need for the .LIB suffix but you may include
it if you wish. If you type ll (Library List) you will get a
list of all the ICs in the library. Press K to exit LL.
Placing integrated circuits
We wish to pc (Place Component) 4060, designator
IC1, comment 4060. Position it towards the LHS (you can
always move it later). Now PC 4518A, IC2A, 4518 to the
right of IC1. PC 4518B IC2B, (blank) to the right of IC2A.
Where an IC consists of two or more elements within
the one package (as in the 4518 above which is a dual
decade counter) I make it a practice to only identify the A
element with the type number. If you label them all, then
at a quick glance you might count four 4518s in the circuit
instead of two.
Repeat the layout for IC3A & IC3B. Your ICs will not be
numbered or identified. Press P, then ec (Edit Component).
ESC
Identifying integrated circuits
Click on IC1 the 4060, click on DESIGNATOR in the
panel, K, move down to HIDE, click, move to SHOW and
click. Follow with three right clicks or three Ps. IC1 will
now be displayed above 4060.
Do the same for IC2A & B and IC3A & B.P from EC and
type ms (move String). Ensure the task bar displays yellow then click on IC1 and position it to between Q12 &
Q13. Position 4060 between Q13 & Q14. Then move and
position the titles for IC2 & IC3.
You can identify any component but I usually don’t
identify resistors, capacitors and other miscellaneous bits.
Now all the ICs are placed we need to go back to our
SCHEMATI.LIB so press P (or right click) to get out of
Move String then lf, SCHEMATI.LIB then K.
We now have to place 13 ground symbols (GND) and nine
ESC
ESC
ESC
76 Silicon Chip
jumpers (JMP) but these are best left until later. For the best
appearance, ensure all the tops of the ICs are on the same
Y grid (ours is 4100). If not type mc (move component)
then move the mouse to the inside of the component and
click. Move it to the required location and click to lock it
in place. You are again prompted by the taskbar.
NOTE! You can only move components when the red or
yellow colour bar is displayed on the taskbar. They will
not move if the brown bar is showing.
Drawing the connections
Connections between components (remember, we are
using “tracks”) are always drawn in red. Draw the trace
from IC1/3 to IC2/2. If you are still in move component
mode, press P (or right click), ensure that you have the
red bar in the taskbar then type pt (Place Track). The
track width has been set to 20 thou in the initial setup you
downloaded and the visible grid to 100 thou The actual
step increment using the mouse or the four arrow keys on
the keyboard is 25 thou.
Move your mouse to the line from pin 3 and click. Move
the mouse to the left until you reach the grid then click
again, move the mouse vertically until you hit the grid
again, click, across, click, down, click then across to pin 2
of IC2A, click. Now press P (or right click). This disconnects the track from the mouse. You may need to zoom to
the area you are working in (plus key on keyboard).
Next move the mouse to IC1 pin 12, click and draw the
track to IC2 pin 7, clicking each time you want to change
direction. Right click to decouple the track from the mouse.
If you have previously laid out PC boards using Autotrax
these instructions will be instinctive.
Now join IC2b pin 15 to the junction of IC1/12 and IC2/7
and then to IC3/7 and IC3/15. Connect IC2A/3 to IC2B/10,
IC2A/14 to IC3/2 and IC3/6 to IC3/10.
Now draw the supply rail at the top of the ICs. Start at
the left and click to go towards IC1/16. Stop 50 thou past
the grid dot, then right click to break the track, move the
mouse down 100 thou and draw the track to the IC. Go back
up and join the pin 16s on IC2 and IC3, then continue the
track towards the right hand side. Right click twice (once
to release the track, the second to exit from PT) then type
pc (place component).
Placing miscellaneous components
Type join (K) accept its ID (K) and ensure the
comment is blank (K) them move your mouse to the sup-
ply line above IC1/16. Click and a dot will appear.
Move the mouse above IC2A/16 and click three times,
then place it. Another three clicks in the same vertical
plane as 100Hz and place, then three clicks and so on, for
each join. Next the four on the reset line, then the four on
the CE (clock enable) inputs. Knowing you need three for
the crystal area place three at random there.
The jumpers are placed in a similar manner. Type pc ,
when you see JOIN displayed type jmp (jumper). Place
the nine jumpers in like manner making sure the tracks
run right up to the start of the arc. The reason for this will
be explained shortly. Finally place the six ARROWS. They
will initially point to the right, so the RESET one will need
one press of the SPACEBAR to rotate it 90°, the others will
need three presses (270°). The COMMENT for each arrow
is 200Hz, 100Hz etc.
siliconchip.com.au
Using mc (move component) place the resistors, capacitors and crystal (click on each component, move it,
then click again to place it) in their correct locations. Now
draw the connections to pins 10 and 11 in IC1. The ground
symbol is GND so these (13) can now be placed and the
tracks drawn.
Checking the layout
To check your circuit for continuity and connections
place the mouse on the +5V/18V arrow and type hn
(highlight Net). All the Pin 16s should be connected.
The connections are obvious on this simple circuit but
in a complex one it is much harder to check. Place the
mouse on IC1 pin 3 and type hn. The track should be
continuous to 200Hz following the jumper. This is why
you need to take the track right up to the jumper arc to
ensure continuity.
Filling in the title block
Type ps (Place String), type simple freq
uency divider, click and move it to the title
space, then click to release it. The text will be too small (60
thou) so et (Edit Text) and try 80. Still a bit too small?
90 should just fit. Type a4h and move it to the SIZE
window, then fill in REV(ISION), DATE and DRAWN. File
is the name you will use to save the circuit.
If you use Autotrax to lay out your PC boards ensure that
the circuits are saved in the SCHEMATI directory and the
PC boards in a different directory, as both have the suffix
PCB and if you give them the same name (which is logical)
and put them in the same directory, one will overwrite
the other.
Creating a component
While you have a wide range of components available
you will probably need additional items in due course.
As an example, in the January 2009 issue of SILICON CHIP,
John Clarke used a 12F6754/P microprocessor. We don’t
have one in the library, but looking at the device it is an
8-pin integrated circuit similar to a PIC08. So we would
“create” a new IC using that.
Move the mouse to blank area of the screen, (making
sure you have IC LIB selected) type pc (Place Component)
PIC08 then press P or (right click). Then le (Library Explode), confirm yes. Press the plus key until you see Top
Overlay and the red or brown bar change to yellow (bottom
centre of screen). Type ds (Delete String), selecting each
description in turn. Next type ms (Move String) then
select and place the pin numbers in the correct position.
Finally type ps (Place String). The top left corner
displays what you are typing. Pressing K places the text
under the control of the mouse. Locate it and click to lock
ESC
1
Vcc
2
7
P00/SO
P-08
3
6
P04
P01
4
SI
P03
Gnd
8
P02
5
1
4
Vdd ---MCLR
5
6
GP2
GP1
12F6754/P
3
AN3
7 GPO
GP5 2
Vss
8
Creating a component is usually
much easier if you modify an
existing one. Don’t forget to
rename it!
siliconchip.com.au
Printing your circuit
In the drive for bigger, better and bloated programs,
support for old DOS-based software and printers is rapidly
(and probably not unreasonably) disappearing. Protel was
written to interface to brands of serial and parallel printers
which were popular at that time but now obsolete. Most
desktop computers and some laptops still have a parallel
output port but not for much longer, as new motherboards
are phasing it out. In a recent magazine issue only four
of the ten units reviewed had a parallel port.
If you have a parallel port on your computer and you
own an HP deskjet printer with parallel input, you are
ready to roll.
Protel’s output program is called Traxplot.You can create
a shortcut to it as we described for Traxedit. It appears that
all HP deskjets support laser 300 DPI (HP640c, HP649c
& HP948c all do) and the plot setup is for these printers.
My old HP649c packed up recently and on the advice of
my cartridge supplier, I went to the local Salvation Army
depot and purchased both an HP640c and an HP948c.
They were quite expensive though: $5.00 each with both
black & colour cartridges fairly full!
The print parameters are set up, so pressing fl (File
Load) will give you C:\SCHEMATI\*.PCB. Press ENTER
and select FDIV1.PCB. The file will load. Press P (escape)
o get back to the FILE menu then move down to print.
Press P or click. You will be asked to confirm PRINT, so
click or press y. A few seconds later you should have a
printout of your masterpiece.
If you don’t have an HP printer various other methods of printing were discussed in the April 2004 issue.
An updated version of Ghostscript has recently been
released.
it in place. If you want to move any strings then ms and
click will let you place them.
Once you are satisfied type bd (Block Define). Click
and move the mouse diagonally to encompass the device
and click. You are now asked for a reference point. For this
device I would use the left tip of the wire from GP2 and a
similar place for all ICs.
When placing the device in a circuit the mouse is located
at the reference point and you should always put this point
on a grid dot. Having defined the block it has to be saved
to the library. Type la (Library Add). You will be asked
for a name, then Autotrax checks to ensure this is not a
duplicate name then asks you to confirm the new name.
Before deleting the block place the new component and
make sure you are happy with it. Then type dc (Delete
Component) and click on the one just placed (unless you
plan to use it), then type bi (Block Inside Delete) and
confirm Yes, then when asked “all layers”, type a (ie,
biya).
Backup File
Protel periodically backs up the file you are working
on. With a modern computer it happens so quickly you
are unaware of the save. The file is named TRAXEDIT.
ABK. (which stands for AutoBacKup). Should you have a
computer crash, lockup or a power failure, once you are
running again, delete the file you were working on (FDIV1.
PCB) or rename it (FDIV1.BAK) then rename TRAXEDIT.
May 2009 77
So what do WE use?
We are often asked which software we use to draw
SILICON CHIP circuit diagrams.
We use Corel Draw but don’t use Corel’s symbols.
We have an extensive component library which we have
drawn up over many years (in fact, we created the Corel
Draw library from the pen-and-ink component library
which we drew when we started the magazine).
As we imply above, Corel Draw does contain its own
electronic component symbol library (among many other
libraries). There is nothing wrong with using this library
if you want to – we just believe ours looks much better!
The latest version of Corel Draw (X4) is a fairly expensive package (~$500-$800 or more, depending where
you get it) but we’ve seen earlier versions (eg V11)
legitimately downloadable from the net for very cheap
prices (eg, $US60!) – and you’d be able to do almost as
much with an earlier version.
ABK as FDIV1.PCB. When loaded, you will see that you
have only lost a few minutes’ work. If you wish you can
load each of the files and compare them.
Bill of Materials (BOM.EXE)
Once you have finished drawing your circuit you can
generate a bill of materials – or what we would call a parts
list. The Simple Frequency Divider circuit produced the
following BOM. It has been compressed to take less space.
78 Silicon Chip
_______________________________________________
FDIV1.PCB 9:21 9-1-2009 Bill of Material Summary
Page : 1
DESCRIPTION QUAN. COMPONENT DESIGNATOR(S)
43
A1
A2
A3
A4
A5 A7
A8
A9 A10
A11 A12 A13 A14 A15
A16 A17 A18 A19 A20
A21 A22 A23 A28 A29
A31 A32 A33 A34 A35
A36 A37 A38 A39 A40
A41 A42 A43 A45 A46
A48 A49 IC2B IC3B
+5V/+18V 1
A30
0.1HZ
1
A27
1HZ
1
A26
1K
1
R1
3.2768MHZ 1
X1
10HZ
1
A25
10M
1
R2
10P
1
C7
22K
1
R3
22P
1
C5
100HZ
1
A24
100NMC
3
C1
C2
C3
100U
1
C4
200HZ 1
A47
270P
1
C6
4060
1
IC1
4518
2
IC2A IC3A
RESET
1
A44
Obviously we can extract the components (R, C, X & IC)
SC
from the list.
siliconchip.com.au
|