PCB Design Software Tutorial


PCB is a free software tool for the UNIX operating system that is used to lay out printed-circuit boards.  PCB does not, however, include a tool for creating circuit schematics.  Because the PCBs we will design have a relatively small number of components, we will forgo the latter step and just build the layout directly.

To load PCB, at the command prompt type:

      /tools1/pcb/bin/pcb

This will bring up the PCB interface.  Before starting your layout, read chapters 1-3 and 8 from the user guide.  This will familiarize you with some of the basic commands and techniques using the software.  The manual can be found at:

    /tools1/pcb/share/pcb/pcb.pdf

In addition, an example pcb layout can be found in

        /tools1/pcb/share/pcb/tutorial/tut1.pcb

You can use this to experiment with the software before beginning your own layout.

Designing Your Own PCB

The following tutorial will allow you to become better acquainted with the PCB software.

1.  We will be designing a two-layer PCB only.  Therefore, specify the layers as shown in the figure below.  Do this by selecting Settings -> Edit layer groupings from the top menu.  We will assume that all power lines will be routed on the top (component side) of the board, while GND wires and planes will be present on the bottom (solder side).

layer groups window


2.  Set the board size by selecting Edit -> Change board size.  Set the PCB width and height to 6000.00 and 3000.00, respectively.  This size should be sufficient for your board.  Note that all measurements are in units of "mils" (0.001 in.).

3.  Set the zoom setting in the Screen menu to 1:2 and select Display grid.  Also change the grid setting to 1 mil.

4.  We will now place a few component "footprints" on the board and wire them up.  A footprint contains all the pads on which a real component will sit.  We will use BNC connectors to route power and GND signals.  Go to the ~connector group in the PCB library menu and select the "1, right angle BNC" component.  Place it anywhere in the layout.  Now obtain the MOSIS_DIP28_ele component by accessing File -> Load element data to paste-buffer and then selecting the directory where this component resides.  Place this near the DIP connector.  Note that these components are known as "through-hole" because their pins physically pass through the PCB.

5.  Go to the ~genericsmt library and select the "6400, 3200, 750, SMT type capacitor/resistor" footprint.  Place two of these on the board.  This footprint is known as a "surface-mount" component because it contains pins that sit on the top (or bottom) surface of the PCB.  Arrange the components so that they look similar to the figure shown below.


Arranged components


6.  Now we must name each of the components in our layout.  Select the BNC connector, click the right mouse button, and then choose Edit Name from the list.  Name the connector "BNC1".  You will see this name appear on the footprint.  Name the DIP package "IC", and the top and bottom resistors "RES1" and "RES2", respectively.

7.  To view the pin numbers of each component, select the component and hit "<Esc>D".  You may have to zoom in to see these better.

8.  Before we begin drawing the wires, select Sizes and increase the line width to 20.00.  Then make sure the active layer on the left is set to "component".  Select the LINE tool and then draw a wire from pin 15 of the DIP footprint to the left pad of RES1.  Your layout should look similar to that shown in the figure below.


onewire


9.  Now we will connect a wire from the left pad of resistor RES2 to pin 18 of the DIP.  To do this, first drop a via between the resistor pad and the previously drawn wire.  Using the VIA tool on the left to do this.  Then draw a short piece of wire from the resistor pad to the via using the component layer.  Now change the active layer to solder and draw another wire from the via to pin 18 of the DIP.  Your layout should look similar to that shown below.


crossedwires


10.  Often, power and ground signals are routed using a "plane" rather than a wire.  We will place the power planes on the component side of the board and the ground plane on the solder side.  To define a power plane, select the RECT tool on  the left and make sure the active layer is set to power.   Draw a power plane that covers the components in the layout as shown below.


powerplane


Pin 1 of the BNC connector footprint is used to route the power signal.  Therefore, we must connect this to the power plane.  Do this by selecting the THRM (thermal) tool and making sure the active layer is still set to power.  Press the left mouse button over pin 1 of the BNC connector.  Your layout should now look as shown below.


connectpowerplane


To define a GND plane, press <TAB> to view the solder side of the board.  Then set the active layer to GND and select the RECT tool.  Draw a plane similar to that shown in the figure below.  Connect pin 2 of the BNC connector to the plane using the THRM tool as before.

groundplane


11.  When we have finished laying out and connecting all the components, we must perform a DRC check to ensure that there are no spacing or width violations.  Before doing this, go to Sizes and reduce the DRC minimum silkwidth to 1.00.  Now go to Connects -> Design Rule Checker to perform the DRC.  The checker will stop and notify you every time it finds a DRC violation.  These errors appear in the program's log window.  Fix any DRC errors before continuing.

12.  The PCB is fabricated by an external manufacturer.  The manufacturer receives a number of text files created by the PCB design software that contain physical layout data.  To generate these files, go to File ->  Print Layout.  Fill in the form as shown below.  In the enter filename box, type in your directory and the name of your layout.  Hit OK when you are done.


gerber


Additional Information

1.  Most of the footprints for components you will need can be found in the various libraries that come with PCB.  If you cannot find an appropriate footprint, you will  need to make your own.  For information on how to do this, see section 8.2 on page 69 of the user's manual.

2.  For a list of through-hole and surface-mount components, go to www.digikey.com and browse through their catalogues.  These usually come with mechanical drawings from which you can more easily make your own footprints.

3.  You can use "rat" lines to logically connect pins from different components before actually routing wires.  This allows you to optimize the placement and orientation of components without the inconvenience of moving or deleting PCB traces.  The Netlist layer is used for this purpose.  See the user's manual for more information.