Protel Tutorial Notes

Note for non-Media Lab people: I am happy that you find this tutorial useful (asuming you do). However, I will not send you a license number and I am way too busy to answer your miscellaneous questions via email. Don't bother.

NEW!!!!11/9/00 Download the finished design database from the tutorial. (tutorial.zip WINZIP format).
You must unzip it, have Protel installed and a floating license (Media-Labbers email ayb@media.mit.edu for the access code) in order to view the tutorial.

Usually you do a PCB layout once you already have designed the circuit and it is fairly stable. It's usually a schematic you get from the back of a napkin. Here are notes on creating both a schematic and PCB layout.

First, read Ari's Protel notes at  http://www.media.mit.edu/physics/pedagogy/fab/pcb99/index.html
You can find it off the class page under PCB layout. It will tell you how to :
    Install protel
    Make a design database
    Get the relevant part libraries

We create a pcb of a circuit that gets input from a microphone and gives it to an A/D converter on a PIC.

The program we are using (protel) is called Design Explorer. It is a mega-program that contains all the libraries, pcbs, schematics in one

Ari says, "First we create the schematic"

Steps to create the schematic:

1. Click to place the Electret Mic (the electret microphone) from the phm-sch library. Left click will put down the part. Right click will cancel.
2. Place a MAX475 op-amp. It is a quad op-amp package ( there are 4 op-amps on the chip). Change the second op-amp piece to Part 2 in properties, so you are using a different part of the op-amp.
3. Use the standard Designator U? for op-amps.
4. Add a resistor using the add part graphic (looks like an AND gate).Library reference for a resistor is "RES1". Edit the part type for the actual value.
5. Connect to 5V and GND. The upside down tree icon adds the powerport. Double-click and edit the Net names to either 5V or GND. All 5V references  will be recognized as the same thing by protel and connected together, similarly, all GND references will be ground.
6. Hook up a capacitor. We will need a polarized capacitor. Go to the Miscellaneous Devices library provided by Protel.  Select "CAPACITOR POL", and place your cap.
7. Add a coupling capacitor "CAP".  Edit the properties so that it is 0.1uF.
8. Make a voltage divider to source the op-amp using 2 resistors, 5v and GND.  Make another port off the divider called "2.5V".
9. Connect the circuit to a PIC microcontroller.  Some vendors provide a library that you can get the part from. Go to Add/Remove Libraries, and get the libraries from the mfg we want-- Microchip. Doubleclick to add. From the library, we get the PICK16C73A20I/JW28. It gives you a pinout and footprint for the chip.
10. Note that there are no power and grounds on this chip.  Power and ground are hidden. Doubleclick on the part and select "Hidden Pins". Click this.  Now power (Vdd) and ground pins (Vss) appear, connect them up.
11. Add a crystal for the PIC.
12. We need a serial line driver.  We don't have one in our libraries, but know someone who does. To use some else's schematic:
13. Open up another design file *.ddb. Select the parts you want and copy it under Edit->Copy. Go to your previous board *.ddb, and paste it in. Then wire it in.
14. Add Footprints. Now we can give all our RES1 type resistors footprints.
15. Match the library references and change the footprint sizes using the Global button.
16. Annotate to number the parts for your PCB layout using Tools -> Annotate...
17. Now we have a full schematic. The next step is to make this into a full PCB.

Usage notes

Open by doubleclicking on  the .SCH file schematic to edit it.
The Libraries are on the "Browse Schematic" tab.  It will show you the parts available.

Part Properties
Lib Ref- The name for this part from the library. Protel uses this to recognize types of parts. Examples of this are RES1, MAX475, ELECTRET MIC,...
Footprint- the size/shape that this part takes up on the PCB.
Designator- letters and a number that name each part on your schematic

As you hover, a big, black dot will appear at places where you may possibly connect a part to the existing schematic.

When it is not clear to Protel what you are clicking on, Protel will show a dropdown list so you can choose.

If parts are floating in space, use the wiring tool (a parallel squiggle ont he upper left of the Wiring Tools box).. DO NOT use the Drawing Tools, which will draw lines, but not be electrical connections. Left click to put down a wire, right click to stop wiring.

Drag a bounding box to select an area to copy. When you copy, you get a cursor. Pick the "handle" that you will use to paste the part later. We copied the whole microphone-opamp circuit so we can have two inputs.

Protel doesn't automatically deselect items. To deselect items you have to shift-click or use the "deselect all" button.

Wires are only connected if they have a dot between them. You can select the junction tool to manually put a connection in.

Footprint conventions come from libraries. Here are some example footprints:
axial- axial means it lies on the surface. axial 0.4 -- 0.4" spacing between the holes.
rad- radial means it sticks out of the surface.. rad0.1 means 0.1" between the pads.
polar cap- means direction matters. polar0.2- \0.2" space between the holes and polarity matters

for chips:
sip- single inline pin- a row of holes. sip3 means 3 pins. use this for the electret mic.
dip- dual- inline pin. 2 rows of holes. dip14 means 14 pins. usually parts from library, or other peoples schematics already have this done for you.
xtal1 - footprint for the crystal
This is also a highly incomplete list available.

See Ari to create a footprint for chips you can't find. Ask him for questions, if you have them.

Creating the PCB from a Schematic file

If you are missing a library listing, look at the pcb footprints library. You have to explicitly add the library in the PCB window. See the instructions linked to above.

Click EXECUTE to try to generate a PCB file.
Unmatched reference components - things on the SCH
Unmatched target components- things on the PCB
You can manually manually match it

When there are no errors, execute to put the parts in the PCB layout.

All the parts are lined up by type. Every part has a rubberbanding wire (green) that show the closest connections between the pin and something it is connected to.

If you bring parts too close, they turn green. You're violating the design rules.

Place your components:
Untangle the rats nest by: vaguely clumping together the parts. Again, use the spacebars to rotate your pieces.

Hide the ground and power nets, for simplicity right now. Click Browse-> Nets and click the 5V and GND nets and check the box to hide them.

Before we autoRoute, we set a design rule so that the traces that carry ground and power to be thicker than the other ones (to reduce their resistance). We only worry about Width constraint and Clearance constraint. For us, it is usually 10 mils. The standard trace rule is also 10 mils. This is the standard 10-10 rule. Very tight layouts use 7-7. At some point it will cost you $$.
Use the Max-Min Width rule for 5V net and Ground Net filter 25 mil.
Click Route All. "OK" does nothing (great, isn't it! NOT!). It routes stuff on both sides for no reason and doesn't do a great job. So we'll use manual route.

Manual Layout
First select placement tool, select a start point, you can see the look aheads that try to help you route the connections.  A connection will appear as a large circle around a pin.

It won't let you make bad routes. You are forced to route only the nets.

When you're done, go and route the 5V  net.  Unhide the net  using the browse window. Route +5V on top of board. Manually route. Note that the trace is automatically 25 mils thick.

Make a ground mesh around your circuit.
Go to place polygon
remove dead copper, track width 8mils, 45 degree hatch
draw any box around your circuit.
A hashed mesh is drawn.

Are we done?
Run the design rules to check that you've done everything.

Select Tools->Design Rule Check... Click RunDRC.
Change to make min allowable width 8mil.

If you've neglected to wire things, your Design rules will catch that for you by saying you have a BROKEN NET.

Run again. When you're done, you're done.

APC (Alberta Printed Circuits) www.apcircuits.com:
Cheapo boards--> 3 days if you get it to them by 1PM.--> Less than $100.
We usually use the Proto1 service. Not all the drill sizes are free.

Drill hole sizes
28 mil is a free size
32 mil isn't... so change those to 35 mil using Edit->Hole Size Editor.
Ari sez: "Never make the hole smaller!"

6/26/01 Anj--> For things like connectors, the through hole sizes often need to be edited to .125 mil. Just click on them and edit them manually.
For all the other drill hole sizes, use the drill hole editor.
[View APCIRCUIT's free hole sizes]

Use APClient to package stuff and ftp it to them. "It's wonderful!"

Make Files for Print house: NC Drill file, Gerber files, GTL, GBL (Gerber Bottom Layer), etc.
Make a CAM file using the File->CAM Manager. Next->2:4 format is probably the best. We want Top and Bottom layer only. Don't mirror any layers or get any of the weird stuff. Click Finish.

Some Definitions