Villanova University 48 of 52 Villanova Electronics Inventors Club
College of Engineering PCB Layout Design Tutorial for the Novice
Dept. of Electrical & Computer Engineering Ralph Alfano, Frank Mercede, Chris Thajudeen
Introduction
The purpose of this tutorial is to provide a step-by-step introduction to the EAGLE PCB-Design Package by way of a simple example. We assume that the reader has downloaded the freeware version of the software from the developer's website at http://www.cadsoftusa.com/.
Since the author is a novice to PCB layout design, the procedure outlined below is neither necessarily efficient nor all-inclusive. The subject of PCB layout design is a field unto itself and requires considerably more study and experience than that provided in this document.
References
The following references were quite helpful in surmounting the learning curve in preparation for this seminar.
[1] David L. Jones, PCB Design Tutorial, Revision A - June 29, 2004, http://alternatezone.com/electronics/pcbdesign.htm
This publication provides an excellent general introduction to PCB design.
[2] CadSoft Computer, Inc., EAGLE Tutorial - Version 5, second edition, 2008
This publication is included with the download of the EAGLE PCB-Design Package.
[3] ECE 445: Senior Design Wiki, CadSoft Eagle Tutorial, http://courses.ece.uiuc.edu/ece445/wiki/?n=Topics.CadsoftEagle
This Department of Electrical and Computer Engineering site at the University of Illinois at Urban-Champaign provides an excellent introduction to the EAGLE package.
[4] instructables website, Draw Electronic Schematics with CadSoft EAGLE, http://www.instructables.com/id/Draw-Electronic-Schematics-with-CadSoft-EAGLE/
This site provides a very helpful step-by-step introduction to the Schematic Editor of the EAGLE PCB-Design Package.
[5] instructables website, Turn your EAGLE schematic into a PCB, http://www.instructables.com/id/Turn-your-EAGLE-schematic-into-a-PCB/
This site provides a very helpful step-by-step introduction to PCB layout with the EAGLE package.
[6] instructables website, Make hobbyist PCBs with professional CAD tools by modifying Design Rules, http://www.instructables.com/id/Make-hobbyist-PCBs-with-professional-CAD-tools-by-/
This site provides important guidelines on how to modify the Design Rules defaults for the auto router to achieve a PCB layout that is easily manufactured by a hobbyist.
Tutorial Example
The procedure of this tutorial is based on the circuit below. The circuit employs a 555 timer IC to generate a square waveform, a potentiometer to adjust the audio frequency of the waveform, and a transistor circuit to enable the waveform to drive an 8 ohm speaker.
Open a New Schematic
In the EAGLE Control Panel select File → New → Schematic. You will be greeted with a screen that looks something like the following.
Add Circuit Components from Pre-defined Parts in Library
Now, click the Add button in the command toolbar on the left-hand side of the screen. You will be greeted by a window that shows a list of libraries which contain pre-defined parts that can be used for schematics and boards.
In the window below, the rcl library is highlighted. This library contains various packages of resistors, capacitors, and inductors.
Clicking alongside the R-US_ designation will open the menu of American-symbol resistors.
Consulting the Jameco Electronics catalog, I learned that the body length of a 1/4 watt carbon resistor is 0.25 inch (6.35 mm). Thus, as shown below, I chose the 0207/10 package located within the R-US_ menu of the rcl library. I am hoping that the 10 mm grid of this package will provide sufficient leeway for the resistor body to lay flush on the board after the leads have been pushed through its holes. Clicking OK will enable you to put this part onto the schematic.
Our schematic employs five of this type of resistor. Simply click the chosen resistor part five times at different places in the schematic editor window, and then click the STOP button to conclude this command and dismiss the phantom image of the resistor part.
In general, the STOP button can be clicked to conclude the command currently in effect, clicking the Copy button and then clicking the crosshair of any part will produce a copy of that part, and clicking the Move button and then clicking the crosshair of any part will enable it to be moved to any location in the schematic editor window.
In general, the Name and Value buttons in the command toolbar are used to assign the name and value of any part, respectively.
For instance, the ohmic value of a resistor is assigned by clicking the Value button, clicking on the crosshair of the resistor, and entering the resistor value in the value field of the pop-up window.
Now, at this point it is advantageous to mention the Zoom commands located at the top of the schematic editor window in the action toolbar. Click the Zoom In or Zoom Out button to zoom into or out of the drawing, respectively. Click the Fit button to display the drawing full size to fit the screen. To display a particular region of a drawing, such as resistor R3 in our previous schematic, click the Select button, mark the region by dragging the cursor while the left mouse button is pressed, and release the mouse button. The result is shown below. Finally, during certain actions, objects in a drawing could disappear or become corrupted. Clicking the Redraw button to refresh the screen will alleviate this anomaly.
Let us proceed to add more parts to the schematic by clicking the Add button in the command toolbar.
The C-US menu within the rcl library will be accessed to select the package for the 0.1 mF and 0.01 mF ceramic disc capacitors of our circuit. Clicking alongside the C-US designation will open the menu of American-symbol (non-polarized) capacitors.
Consulting the Jameco Electronics catalog, I decided to use a radial ceramic disc capacitor with a 25 volt rating and 6 mm "diameter" (i.e. width or lead spacing) for the 0.1 mF and 0.01 mF ceramic disc capacitors of our circuit. (Please note that other diameter sizes are available; so, be sure about which size is in stock before choosing the part.) Since the diameter of the ceramic disc capacitor is 6 mm, I chose the C075-032X103 package from the C-US menu located in the rcl library. I believe that the 7.5 mm grid of the package is sufficient for the capacitor leads to fit comfortably through its holes. Clicking OK will enable you to put this part onto the schematic.
Our circuit employs two of this type of capacitor. Simply click the chosen capacitor part two times at different places in the schematic editor window, and then click the STOP button to conclude this command and dismiss the phantom image of the part.
In general, the STOP button can be clicked to conclude the command currently in effect, clicking the Copy button and then clicking the crosshair of any part will produce a copy of that part, and clicking the Move button and then clicking the crosshair of any part will enable it to be moved to any location in the editor window.
In general, the Name and Value buttons are used to assign the name and value of any part, respectively.
For instance, the value of a capacitor is assigned by clicking the Value button, clicking on the crosshair of the capacitor, and entering the capacitor value in the value field of the pop-up window.
The package for the 555 timer IC is located in the linear library. Clicking alongside the linear designation will expose the menus of the linear devices.
Select the LM555N dual in line package, located within the *555 TIMER menu of the linear library. Click OK to put this part onto the schematic.
Our circuit employs one 555 timer IC. Simply click the chosen part one time in the schematic editor window, and then click the STOP button to conclude this command and dismiss the phantom image of the IC. Clicking the Move button and then clicking the crosshair of this part will enable it to be moved to any location in the editor window.
Referring to the Jameco Electronics catalog, I chose the Bourns 3362P 10 kW, 1/2-watt, 1/4 inch square trimming potentiometer with top adjust and Y-layout solder pins (Jameco Part No. 182837). Unfortunately, this particular model is not provided in any of the EAGLE libraries. Rather than developing a custom part from the data sheet, I decided to employ the TRIM_US-B25P part, located in the TRIM_US- menu of the pot library. This B.I. (Beckman) 25P part is compatible with the Bourns 3362P trimmer.
Clicking OK will enable you to put this part onto the schematic.
Our circuit employs one of this potentiometer. Simply click the chosen part one time in the schematic editor window, and then click the STOP button to conclude this command and dismiss the phantom image of the part. Click the Value button, click on the crosshair of the potentiometer, and enter the 10K value in the value field of the pop-up window. Clicking the Move button and then clicking the crosshair of this part will enable it to be moved to any location in the editor window.
Next, let us add a red LED with a 3.0 mm diameter to our schematic. Click the Add button in the command toolbar, and select the LED3MM part located within the LED menu of the led library. (Please note ...
olek210