Using Python scripts to create Eagle parts

I dread creating part models in Eagle – it’s time consuming and error prone.

Over the years I have used scripting languages to help with the tedious work. It’s quite easy to create basic part footprint algorithms given the mechanical drawing. Much more tedious would be drawing a picture on graph paper and using your calculator.

If you’ve ever made a circuit board and made a very basic error that caused you to have to remanufacture your board, you’ll understand the value of getting it right the first time around.

Take this extremely simple script for example:

#!/usr/bin/python
x=0.0
y=0.0
pins=24
print 'EDIT TSSOP_' + str(pins) + '.pac'
for p in range(1, pins/2+1):
 x = (p-1)*0.5
 y = -4.15
 print 'SMD 0.27 1.0 \'' + str(p) + '\' (' + str(x) +' ' + str(y) + ');'
 print 'SMD 0.27 1.0 \'' + str(pins+1-p) + '\' (' + str(x) +' ' + str(-y) + ');'

You could really write this in any language and it would be about the same length. There’s no reason it has to be done in Python. The value is in what it prints out:

EDIT TSSOP_24.pac
SMD 0.27 1.0 '1' (0.0 -4.15);
SMD 0.27 1.0 '24' (0.0 4.15);
SMD 0.27 1.0 '2' (0.5 -4.15);
SMD 0.27 1.0 '23' (0.5 4.15);
SMD 0.27 1.0 '3' (1.0 -4.15);
SMD 0.27 1.0 '22' (1.0 4.15);
SMD 0.27 1.0 '4' (1.5 -4.15);
SMD 0.27 1.0 '21' (1.5 4.15);
SMD 0.27 1.0 '5' (2.0 -4.15);
SMD 0.27 1.0 '20' (2.0 4.15);
SMD 0.27 1.0 '6' (2.5 -4.15);
SMD 0.27 1.0 '19' (2.5 4.15);
SMD 0.27 1.0 '7' (3.0 -4.15);
SMD 0.27 1.0 '18' (3.0 4.15);
SMD 0.27 1.0 '8' (3.5 -4.15);
SMD 0.27 1.0 '17' (3.5 4.15);
SMD 0.27 1.0 '9' (4.0 -4.15);
SMD 0.27 1.0 '16' (4.0 4.15);
SMD 0.27 1.0 '10' (4.5 -4.15);
SMD 0.27 1.0 '15' (4.5 4.15);
SMD 0.27 1.0 '11' (5.0 -4.15);
SMD 0.27 1.0 '14' (5.0 4.15);
SMD 0.27 1.0 '12' (5.5 -4.15);
SMD 0.27 1.0 '13' (5.5 4.15);

If you open up the EAGLE Library editor and paste this script into the command console, you get this:

Not a bad start.

The same technique applies for much larger parts. Imagine how much time you’ll save when you’re creating a part model for a 256+ ball grid array?

I must say I don’t claim to be an expert Python coder – I have my own specialties and I’m really a low-level embedded systems guy. If you need a turn-key shoe-phone (that’s a joke) or a radio watch (if you don’t get the joke you’re too young) or an accelerometer based movement tracker with 6 months battery life, I’m your man.

I’m just rambling – back on topic: there’s another script I wrote that you can access via pastebin (click “see original”)
[iframe src=”http://pastebin.com/embed_iframe.php?i=2RqWXs83″ style=”border:none;width:100%”][/iframe]

This script takes a CSV file and a model name as command line options, i.e:

$ ~/bin/csv2model.py sn74.csv sn74vme22501a

And produces helpful Eagle SCR data that you can call from Eagle to make a schematic symbol, and also to CONNECT the schematic part model PINs to the physical layout PADs. i.e:

EDIT sn74vme22501a.sym;
PIN '1OEBY' Short (0 0.0)
PIN '1A' Short (0 -0.1)
PIN '1Y' Short (0 -0.2)
PIN 'GND' Short (0 -0.3)
PIN '2A' Short (0 -0.4)
PIN '2Y' Short (0 -0.5)
PIN 'VCC' Short (0 -0.6)
PIN '!2OEBY' Short (0 -0.7)
PIN '3A1' Short (0 -0.8)
PIN 'GND_2' Short (0 -0.9)
PIN 'LE' Short (0 -1.0)
PIN '3A2' Short (0 -1.1)
PIN '3A3' Short (0 -1.2)
PIN 'OE' Short (0 -1.3)
PIN 'GND_3' Short (0 -1.4)

and:

CONNECT sn74vme22501a.1OEBY 1;
CONNECT sn74vme22501a.1A 2;
CONNECT sn74vme22501a.1Y 3;
CONNECT sn74vme22501a.GND 4;
CONNECT sn74vme22501a.2A 5;
CONNECT sn74vme22501a.2Y 6;
CONNECT sn74vme22501a.VCC 7;
CONNECT sn74vme22501a.!2OEBY 8;
CONNECT sn74vme22501a.3A1 9;
CONNECT sn74vme22501a.GND_2 10;
CONNECT sn74vme22501a.LE 11;
CONNECT sn74vme22501a.3A2 12;
CONNECT sn74vme22501a.3A3 13;
CONNECT sn74vme22501a.OE 14;
CONNECT sn74vme22501a.GND_3 15;

The CSV file contains (partially):

PIN,NAME
1,1OEBY
2,1A
3,1Y
4,GND
5,2A
6,2Y
7,VCC
8,!2OEBY
9,3A1
10,GND
11,LE
12,3A2
13,3A3
14,OE
15,GND

 

 


Here’s another script I generated for the FT256 / FTG256 package which is used by some Xilinx FPGAs:

#!/usr/bin/python
# Create BGA SCR for Eagle 5.x
print 'GRID MM;'
rows = ['A', 'B', 'C', 'D', 'E', 'F', 'G', 'H', 'J', 'K', 'L', 'M', 'N', 'P', 'R', 'T']
cols = ['1', '2', '3', '4', '5', '6', '7', '8', '9' ,'10', '11', '12', '13', '14', '15', '16']
nrows = 16
ncols = 16
pitch = 1.0 # ball spacing in millimeters
padsize = 0.4 # SMD pad size in millimeters
xstart = -(nrows - 1) / 2.0
ystart = (ncols - 1) / 2.0
x = xstart
y = ystart
for row in rows:
 x=xstart
 for col in cols:
 print 'SMD ' + str(padsize) + ' ' + str(padsize) + ' -100 \'' + row + col + '\' (' + str(x) +' ' + str(y) + ');'
 x=x+pitch
 y=y-pitch
print 'LAYER 21;' #tplace
print 'WIRE .254MM (' + str(x) + ' ' + str(y) + ') (' + str(-x) + ' ' + str(y) + '); '
print 'WIRE .254MM (' + str(-x) + ' ' + str(y) + ') (' + str(-x) + ' ' + str(-y) + '); '
print 'WIRE .254MM (' + str(-x) + ' ' + str(-y) + ') (' + str(x) + ' ' + str(-y) + '); '
print 'WIRE .254MM (' + str(x) + ' ' + str(-y) + ') (' + str(x) + ' ' + str(y) + '); '
 
print 'LAYER 25; \n\
TEXT \'>NAME\' ('+ str(-x) +' '+ str(-y+.5) +'); \n\
CHANGE SIZE 0.05IN ('+ str(-x) +' '+ str(-y+.5) +'); \n\
CHANGE RATIO 20% ('+ str(-x) +' '+ str(-y+.5) +'); \n\
CHANGE FONT VECTOR ('+ str(-x) +' '+ str(-y+.5) +'); \n\
LAYER 27; \n\
TEXT \'>VALUE\' ('+ str(-x) +' '+ str(-y+2.5) +'); \n\
CHANGE SIZE 0.05IN ('+ str(-x) +' '+ str(-y+2.5) +');\n\
CHANGE RATIO 20% ('+ str(-x) +' '+ str(-y+2.5) +'); \n\
CHANGE FONT VECTOR ('+ str(-x) +' '+ str(-y+2.5) +');\n\
LAYER 51; \n\
TEXT \'>NAME\' (0 0); \n\
CHANGE SIZE 0.03IN (0 0); \n\
CHANGE RATIO 10% (0 0); \n\
CHANGE FONT VECTOR (0 0); \n\
'

[iframe src=”http://pastebin.com/embed_iframe.php?i=0RSLWxWM” style=”border:none;width:100%”][/iframe]

And here’s what it produces, which can be run right in the Eagle Library editor:

[iframe src=”http://pastebin.com/embed_iframe.php?i=VMTYQPnK” style=”border:none;width:100%”][/iframe]

 
Which produces this in Eagle 5.x:

 

E96 Resistor values

A common annoyance I have is that I’ll design a gadget: make the schematic, figure out how big the board can be, design the board – all of these so far are creative tasks requiring ┬ásome skilled input as to the technical details.

Then you order the board (a task let’s set aside for now)

Then you have to make a bill of materials and order parts. The most annoying, time consuming part of designing hardware.

I use Eagle from Cadsoft, so my answers may not apply to you. Is your EDA software a lot better? Let me know, I’d like to hear about it. I’d also be interested to know how much it costs. Eagle is relatively inexpensive when it comes to EDA tools. Industry-standard Mentor Graphics (among others) are many thousands of dollars. That’s just not possible for me.

But back on topic: how do you take your schematic and create a BOM? Well, Eagle has a ULP you can run that will produce a rudimentary BOM (bom.ulp) . It sucks.

I’ve tried to improve it a bit by post-processing the CSV with my own Perl script. I use Cygwin on Windows to run this by the way.

[click here to see the code]

The Perl script is called eagle.bom.pl and it attempts to produce a usable BOM. It tries to combine all of your 1K resistors into one line item, for example.

 

Now that you have a BOM that doesn’t require two hours of manual formatting to complete, my next problem is that I often have numerous different resistor values that I have to look up at Digi-Key or Mouser (or Newark) and make sure I picked a real value, find the part number, and add it to my spreadsheet.

A partial solution I have is that I made a Python script that will print out all E96 resistor values for Stackpole electronics’ RMCF series. This is very specific, but I’ve picked a manufacturer that literally has thousands of parts at Digi-Key, with millions in stock.

Now that I have a list, I can scroll through and find the one I want, and simply copy and paste the part number into my BOM.

The next step would be integrating this into my BOM script. This will get you started though.

Making table legs

Here it is in gallery form. Click on an image to see a larger version.