EXPRESS PCB TUTORIAL

Revised 1/11/2010

This tutorial leads you through the design of a PCB using layout software from ExpressPCB, which is freeware available at www.expresspcb.com.    Before beginning you should make sure your computer has both ExpressPCB and ExpressSCH, if not than you should download the software.   Before beginning the PCB process, you should come up with the initial design, build it and test it on a breadboard, fix any errors, and determine specific components.  It is also useful to have datasheets and dimensions for all of the “special” components such as transistors, ICs, sensors, actuators, etc., on hand.  For this tutorial, we will use a drawer burglar alarm circuit, which had the following form after testing on a breadboard:

There are two stages remaining in the process to creating the circuit board.  In the first stage, you build the schematic using the ExpressPCB schematic editor.  In the second stage you layout the circuit board.  It is possible to skip directly to the layout editor.  However, doing the schematic first will allow you to link the schematic into the layout editor reducing the probability of error.

Entering the Schematic into ExpressSCH

1. Open ExpressSCH to create a fresh schematic.  The first time you start ExpressSCH you will get a dialog box with a link to a quick start guide for ExpressSCH.  This can be useful if you want to get a general overview for the tool.  Once you are ready to start, close the dialog box to view the empty schematic.

2. Click on Op-Amp-like symbol to place components.  To place the resistors, select “Passive-Resistor” in the text box in the upper right corner.

3. Then click on the schematic for the 4 resistors (not including the photoresistor or potentiometer) in roughly the location you want them to display.  Then zoom in using the magnifying glass tool (or the wheel on the mouse) and pan the display (using the sliding bars) to improve your view.

4. Now you need to give each of the resistors unique identifiers.  Right click on a resistor and choose “Set component properties.”  In the Component Properties box, under “Component ID,” select “Auto assign Part ID.”  The program should assign this resistor to be R1.  Set its value 10k in the “Part Name” field and hit OK.  Repeat this process to identify and label   R2 (10k), R3 (100k), and R4 (10k).

5. Rotate R4 by right clicking on it, selecting “Rotate component” and then “Body left 90º”

6. Now add the capacitor, potentiometer, comparator, and transistor to the circuit by first clicking back on the component placement tool (the red op-amp symbol) and using the component names “Passive-Capacitor polarized,” “Passive- Potentiometer,” “IC – National  - LM311 – Comparator – DIP-8,” and “Semiconductor – Transistor NPN.”  Use “set component properties” to assign all of these parts Part IDs, label them and position them (using the arrow tool) in a logical manner.

7. Now we need to add some components (the photoresistor and the buzzer) that don’t exist in the library.  Let’s start with the photoresistor.  The easiest way to make new parts is to start with a symbol that’s already close to what you want and modify it.  Place a regular resistor on the layout (using the placement tool with ‘Passive – Resistor’).  Go to the selection tool (the arrow), choose that resistor and go to the “Component” menu at the top and select “Ungroup component”

8. Using the circle shaped tool from the tool menu, draw a circle around the resistor.

9. Select the whole object (using the arrow tool), and choose “Component” -> “Group to make component”

10. In the component properties box that appears, assign the photoresistor a unique part ID, such as “PR1”.

11. For future use, save this as a custom component by selecting “Component” -> “Save custom component” and then in the dialog box that appears give the component a name such as “photoresistor.”  (If someone else has already completed the tutorial on this computer, the part may already exist, in that case you should either save this component with a unique name, or save your component on top of the one already existing)

12. Move the photoresistor to the spot you want it in the circuit.
13. Now we will create the buzzer.  The buzzer is a polarized device, so a good starting point is a polarized capacitor.  Go to the component selector, choose a polarized capacitor, ungroup the capacitor, and then add a circle to the symbol to distinguish it as a buzzer.  Group the entire object as a component with part ID, “BZ1,” and label “CEP-2224” and save the component as a “Buzzer” under custom components.  At the last step, you’re display will be as follows:

14. Now we need to add our connections to power and ground.  Let’s start with ground.  Go to the “symbol or signal label” tool, which looks like a ground, and select “Power – ground” from the text box in the upper right. 

15. Place 5 grounds into the circuit, at the bottom of R2, near pins 1 and 4 of the LM311, near the bottom of the capacitor, at the emitter of the BJT, and at the bottom of the potentiometer.

16. Repeat this process, but using “Power – Voltage Supply +9V” to put 5 power connections in at the top of R1, the photoresistor, pin 8 of the LM311, the top of R3 and the top of the buzzer.

17. Now let’s add in our battery connection.  Place a battery into the circuit, using “Misc – Battery.” Assign the battery the part ID “B1” and give it the label “9V.” Then, use the symbol tool to add a ground connection and a +9V network connection (this will link the positive terminal of the battery with every other point in the circuit that should go to 9V—if you wanted to add a switch to the circuit, you would add it between the + terminal of the battery and the ‘+9V’ symbol.)

18. Now select the wire tool, and wire your circuit together. The left-click starts the wire and sets a bend, and the right click ends a wire.  After wiring, the schematic should appear as follows:

19. Save your work, using “Save As..” to create a unique filename.
20. Check your file for netlist errors using “File” -> “Check schematic for netlist errors”

21. The pins inside of the BJT are not specified (this is because pin assignments vary for different BJTs) so you will probably will get an error message, like that shown below:

22. Hit “cancel” on the error message, and then as that message suggested, select the part and choose “Component” and then “Ungroup Component.”  This example uses the 2n1711 BJT in the little tin can (the TO-39 package).  For this package the base is pin 2, the emitter is pin 1, and the collector is pin 3.  To set this in the schematic, double click on just the collector pin, and assign it to pin 3.

23. In a similar fashion, assign “2” to the base, and “1” to the emitter.  Then select the entire component (this takes a lot of shift-clicking—be sure to get all the little parts), choose “Group to make component” from the Component menu, and assign the part ID to be Q1.

24. If you’re going to be using the transistor again, it’s probably a good idea to then click on it, select “Component” -> “Save custom component” and save it as the transistor name, which in this case is 2n1711. 

25. Now check your file for netlist errors again, using “File” -> “Check schematic for netlist errors,”  you might get an error like that shown below (if not skip to #28)

26. The cause of this error is that the wire isn’t really connected.  The “snap-to-grid” function has prevented you from making a connection.   Hit continue to exit the netlist check.  Then toggle the “snap-to-grid” function off, select the errant line end(s) and move it (them) into the correct position.  Repeat this process until all the lines are properly connected.

 

27. Reattempt the netlist error check.
28. Once the netlist error check runs clean, you will be asked to save your file, which you should definitely do.  The final schematic should look like this:

29. Print your schematic to reference as you work on your layout.  At this point, you should review your schematic carefully to check for errors.  Once you are satisfied that the schematic is correct, close ExpressSCH.