Overview

You have explored circuit design and prototyping through breadboards and perfboards. This time, you will explore the manufacturing of more sophisticated circuit prototypes and finished products: You will create a printed circuit board (PCB) of the all-too-familiar 555 Blinker circuit with the software KiCad.

Concepts

Printed Circuit Boards (PCB)

When electronics are more complex or are ready for production, we typically use printed circuit boards or PCBs. Nearly every device, from a digital alarm clock to laptop computer, uses a PCB. It is a board designed with CAD software that connects individual components.

The benefits of PCBs over prototyping boards are numerous: They're more compact, more reliable, and enable complex circuit design. Above all, they are easy to mass produce.

To learn more about PCBs and how they are constructed, view the lecture material here.

PCB Design Overview

When it is time to design your PCB, there are two major components of the operation: (1) Schematic capture - converting your prototyped design and circuit drawings into a digital schematic. (2) PCB Layout Design - placing components and routing conductive tracks in a virtual layout of your PCB. You can learn exactly how this process works in the KiCad EDA software by viewing our PCB Design with KiCad workshop material here.

Installing KiCAD 7.0

To complete this project, you will download the PCB design software KiCad (version 7.0.11).

Windows	Download
Mac	Download

1. Download the installer from the link appropriate to your OS.
2. Launch the installer. Click Next.
   
3. When the Choose Components dialog appears, make sure all but the “Help files” components are selected. Then, click Next.
   
4. Select the Install Location. The default setting is usually acceptable. Then, click Install.
   
5. The installation is complete! The fun starts now.

Requirements

For readers who are enrolled in the course: In order to receive full marks on your project submission, make sure it meets the following minimum requirements.

• You must create a full schematic that replicates the provided 555 Blinker Circuit diagram
  • The schematic must pass the Electronic Rules Check (ERC) for all but the error: “Input Power pin not driven by any Output Power pins.”
• You must design a PCB from the 555 Blinker Circuit schematic you create
  • The PCB layout must pass the Design Rules Check (DRC)
• The symbols and footprints used in the schematic and PCB must match those listed in the Parts section of the project specification
• Optional Challenge: The PCB must have no traces on the bottom copper layer and no vias

Parts

This is not a physical parts list. The followig parts will be used in the PCB EDA application.

Schematics

Instructions

Each checkpoint guides you through the process of designing the 555 Blinker circuit, which should look something like this upon completion:

Make sure to save your progress frequently. Nothing is more infuriating than trying to recover lost data and lost time.

You should also do yourself the favor of using a mouse. Suffice to say, KiCad is unkind to touchpad users (and if you are using a pointing stick, something is wrong with you.)

And with that, let's get started!

Checkpoint 1

1. Open KiCad 7.0 to launch the Project Manager and create a new project. Name the project file using the following format: “ops_project8_lastname_firstname.kicad_pro”
   
2. Now that you have created a project, open the Schematic Editor (or press Ctrl+E, Mac: ⌘+E) to launch the schematic capture application.
   
3. Click on Add Power Symbol (or press P) to add the +9V (VCC) and Earth schematic symbols.
   
   Need to zoom in or out? Use the mouse scroll wheel or select one of the following options from the menu bar at the top of the application:

   
4. Click on Add Symbol (or press A) and add each of the schematic symbols listed in the Parts section of the project specification.
   
   Moving Symbols: You can move symbols by selecting them, then holding down the left mouse button, and moving the cursor. You can also select the symbol, press M, then move the cursor.
5. For each valued component (resistors, capacitor, LED), right click on the component, and select Properties (or press E).
   
   Edit the Value field in the Symbol Properties dialog to be the corresponding component value in Ohms, Farads, etc.
   
   The value scheme is as follows:
   {base value} {scale} {unit}
   scale (power of 10): p: -12, n: -9, u: -6, m: -3, k: 3, M: 6, G: 9
   unit: Capacitors: F, Inductors: H, Resistors: None
6. Open the Footprint Assignment tool. For each component symbol, assign a footprint. The symbols' footprints (and their footprint libraries) are defined in the Parts section of the project specification.
   
   After assigning each component, select Apply, Save Schematic & Continue to save your progress.
   
   After footprints are assigned to symbols, you can copy (Ctrl+C, Mac: ⌘+E) and paste (Ctrl+V, Mac: ⌘+V) symbols and their footprint assignments will be copied over as well
7. Move symbols and rotate them in preparation to connect them with wires. If a symbol is in the wrong orientation right click on the component and select Rotate Counterclockwise (or press R) to rotate it 90 degrees counterclockwise.
   
8. Complete the circuit defined by the provided schematic. Select the Wire button (or press W) to create connections between components and other wires. Connections between two wires are indicated by a dot.
   
9. Add net labels to avoid crossing wires. Net labels are basically invisible connections; they help clean up the schematic.
   
10. Add no-connection flags to indicate which pins/leads are to be left unconnected. This is important for when we run verification tools later.
    
    Run the Annotate Schematic tool

Checkpoint 2

1. Open the Annotate Schematic tool and select Annotate to name the remaining symbols which have been marked erroneously with “?”.
   
2. You will now verify the schematic. Open the Electrical Rules Check (ERC) tool and select Run ERC
   
   There should be no violations except for Error: Input Power pin not driven by any Output Power pins.

Checkpoint 3

10. Return to the Project Manager window and open the PCB Editor (or press Ctrl+P, Mac: ⌘+P).
    
11. Though this step is not required for your project, you can configure the stackup and add manufacturer design constraints by selecting File → Board settings
    
12. To generate the components specified by your schematic, open the Update PCB tool (or press F8) and select Update PCB
    
    The component footprints will then be generated and follow your cursor until you left click to confirm their initial placement.
    
13. Now, you need to set the track and via sizes. Disable the Use Existing Track Width.. option by selecting the button until it is no longer highlighted. Then, open the Track use netclass width dropdown and select Edit Pre-defined Sizes
    
    Add the following pre-defined sizes:

    Tracks (Width)	Vias (Diameter/Hole)
    40 mil	30mil/20mil
    30 mil

    Traces with 40 mil width must be used for power and ground lines.
    Traces with 30 mil width must be used for signal lines
    
    Vist the Track use netclass width and Via use netclass sizesropdowns and select one of the newly populated options. (Change between the options as necessary when you route the traces.)
    
14. Create the board outline. Select the Edge.Cuts layer then use one of the shapes tools to create the outline. Remember to return to the F.Cu (Front Copper) layer when done.
    
15. Create the traces. Select Route Tracks (or press X) and begin drawing traces between pads which are connected via the ratsnets.
    
    Remember to change the trace width according its use case. Power/Ground lines should be larger width than signal lines.
    Leave the ground pads unconnected.
16. In the event two traces on the same layer must cross paths, you may instead create one of the traces on the B.Cu (Back Copper) layer.
    
    Use the Add Via tool (or press Ctrl+Shift+V, Mac: ⌘+Shift+V) to place vias which may connect traces of different layers.
    
17. With all but the ground pads connected, you will create the ground fill. Select Add Fill Zone (or press Ctrl+Shift+Z Mac: ⌘+Shift+Z). A dialog will appear:
    
    Select both the F.Cu and B.Cu layers as well as the Earth net. Then, select Ok.
    
    Now, left click to draw the closed area in which the fill will be created.
    
    When the fill zone is created, press B to fill.
    
18. If you wish to add text to the PCB, select the F.Silkscreen layer. Then, use the Add Text Item tool (or press Ctrl+Shift+T, Mac: ⌘+Shift+T) to generate and place textboxes on the silkscreen.
    
    Alternatively, you may write text to the back of the PCB by selecting the B.Silkscreen layer instead.
    

Checkpoint 4

10. Now to verify the PCB layout. Open the Design Rules Checker (DRC) tool and select Run DRC. There should be no violations.
    

Checkpoint 5

10. As a final checkpoint, you will generate the manufacturing files for your project. Select the Plot tool. Then, choose an Output directory. It should be a new folder called “gbr” in your project folder.
    
    Now, select Plot tool. Then, select Generate Drill Files… to open a new dialog where you will select Generate Drill Files again.
    
    Close all the dialogs. You are done!
    

Deliverables (Enrolled Students Only)

Students enrolled in the course must submit the following deliverables to the corresponding Canvas course assignment.

Compress the KiCad project folder as a .zip. It must contain the following:

• KiCad Project File (.kicad_pro)
• KiCad PCB File (.kicad_pcb)
• KiCad Schematic File (.kicad_sch)
• Folder containing the manufacturing and drill files

Rename the zip file using the format “ops_project8_lastname_firstname.zip” Then, submit the zip file to the Project 8 Canvas assignment.