Making a new Schematic/PCB Part in Protel '99
by David Merrill
Q: What do I do if I want to use a part in my circuit that protel doesn't have in any of its libraries?
A: Make your own Schematic Library, and PCB Library documents for it, include your .ddb file in the list of libraries, then you can use it!
The situation came up because I wanted to make a circuit including the solenoid driver that I used for microcontroller week/ (see http://web.media.mit.edu/~dmerrill/mas863/micro.html, in the "Technical Details" section). I knew the following about it:
Part name: DRV101
Number of pins: 7
Usage of each pin: specified in the datasheet
Pin footprint: specified in the datasheet
So, first I made a schematic library for this part, so that I could use it in the schematic file I'm building. With my document open, I did the following:
- File -> New -> Schematic Library Document
- Tools -> New Component
- Gave it a name (DRV101)
- Make sure the "Drawing Toolbar" is present (find it in View -> Toolbars, if not)
- Draw the yellow box that will be the body of the part (the PlaceRectangle tool from the drawing toolbar)
- Draw the 7 pins (the PlacePin tool from the toolbar)
- make sure that the pins are in the proper orientation - the "knob" should be away from the body of the part,
since that end connects to the rest of the circuit. Press space to rotate
- Change the Name/Number of each pin to match the actual part characteristics (double-click the pin to get the dialog up)
- For instance, I made the following changes to the first pin I placed:
Name: 0 -> Input
Number: 0 -> 1
- and so forth for the rest of the pins
- Over in the group menu on the lefthand side of the screen, click "Description" and specify the:
- Default Designator: U? (the U is because it's an IC I think)
- Default Footprint (or Sheet Part Filename): TO220-7 (because the datasheet describes this thing as a 7-lead TO-220)
- Click the save button!
Now, I want to have the appropriate footprint so that I'll be able to lay out my PCB.
- File -> New -> PCB Library Document
- Tools -> New Component (you'll be welcomed to the PCB component wizard)
- For the component pattern I chose DIP, because it gave me something close
to what I wanted (i.e. a couple of rows of pins - you can tweak it all around
later)
- In the next screen, "Specify the pad dimensions", I made the hole diameters
40 mils (the datasheet shows a sample footprint and they are 40 there), and
the outer diameters 60 mils. This will leave a 10-mil ring around the holes, and
the modela should cut it OK since the diameter of the entire thing is 60 mils.
- In the next screen "Pad Spacing Values" put something reasonable here
- In the next screen "Outline Width" we don't care, since we'll draw our own outline.
- In the next screen "Total Number of Pads" I chose 8, since the actual part has 7
pins - we can remove the extra one.
- In the next screen "What is the name of this component" I put TO220-7, so that it
matches up with the schematic part we made.
- Finish
- Now, you can edit the part that it put down. Do the following:
- delete the yellow lines that it put there by default
- delete the 8th pin that I don't need
- change the x and/or y locations of the pins so that they line up
as needed by the actual footprint of the part.
- Click on the "top overlay" tab at the bottom of the screen, and click
on the line drawing tool.
- Draw a line around the footprint
- Save it!
Look at my final PCB footprint (with annotations that I put there to show the sizes of the parts)
Now, to actually use this stuff, you need to add the .dbb file to your Libraries list.
Other notes:
- If you can't find the particular microcontroller that you want to use
in the Microchip library, you can usually find one that's pin-for-pin
compatible with it.
-
Ari rumored that at one time there existed a
pin-for-pin compatibility chart somewhere at microchip.com, but I didn't
manage to find it myself. (although I didn't look too hard). Rather,
I just compared the datasheet for my PIC with the schematic parts that
are there in the Microchip library and found one that matched up.
-
In
case you're interested, here's my mapping:
I am using: PIC16F876 (it has 40 pins total)
I found this worked: PIC16C74-041/P(40)
(note - the 40 at the end designates the number of pins.. you could also
use whatever part you want, with a dip20 footprint)
- For things that I don't have schematic/layout for (3-pin crystal, for example)
- schematic design: use conX (connector, X pins - for example, I use con3 for my crystal)
- PCB footprint: sipX (single-inline-package, X pins - so I use sip3 for my crystal)
|