If you are a startup needing schematic and PCB design capabilities, or you are learning electronics, Kicad is an open source tool with everything you would need to get started. You can install it following the download instructions on the Kicad web site.

This tutorial will walk you through creating schematic design and PCB layout in Kicad to create some flashing LEDs, using an Astable Multivibrator design.

Select File->New->Project and name your project say LEDFlashAstable.

To start the schematic design double click on the LEDFlashAstable.sch file.

This will start the first schematic page, into which we will place and connect all components. The following is the final schematic we are aiming for.

Click on the schematic page to open the component library page. You will see a window and status bar while component libraries are loaded.

The first component we will place is the BJT transistor. Choosing a component is one of the subtle skills of an electronics engineer. There as so many to choose from and the wrong choice could be costly later. In this tutorial we will use Kicad to help us choose our component.

Typing in the filter box, will filter the components to suitable ones. BUT, take care as if you have a very large library set (as below with 16427 items loaded), typing a single character will take a long time to filter.

Instead, copy the text bjt from here and paste it into the filter box.

Then add dual to further narrow down our search.

As you can see in the search window Kicad conveniently gives you the voltage and current rating. A quick scan shows that almost all the voltages are high enough. Additional for the dual devices it seems the lowest current is 100mA, so we could chose any one at which point price may become the deciding factor. Additionally because most are SOT-363 (a 2x2mm package) the choice in Kicad is somewhat irrelevant as most will be pin for pin compatible.

The MBT3904DW would suit this circuit wo we will choose it.

To select the component into Kicad select Unit A of MBT3904DW and click ok.

Place the component by clicking on the page. To place the second half of the package/chip, click on the page again, which will open the library selection to the same location you just were. Click on Unit B, and then click OK.

While the image is ‘see through’, click Y (for mirror) so that the component faces the opposite direction (as per our example circuit).

Now what we want to do is choose the package that we want, which will define our foot print.

Hover the cursor over the resistor, and press ‘e’ for edit.

Click on the Footprints text box and then click the ‘book’ in the right corner. This will open the footprint library.

On the left scroll down to Resistor_SMD (surface mount resistor), and then on the right column scroll to and double click on R_0603_1608Metric.

We chose the 0603 SMD package as its big enough to work with manually using a soldering iron.

Then click ok to close the components edit window.

Now we want to repeat/copy this resistor, to place four resistors. This ensures each resistor will have the same footprint.

Hover your cursor over the same resistor and press ‘c’ for copy. This will ‘copy’ the component and allow you to place it. Repeat another two times to get the 4 resistors.

To move the first resistor placed (as it is out of line), hover over it and press ‘m’ for move. Then move it and click once positioned.

Now we need to place two capacitors.

In the component library, type c for capacitor or if you have a lot of symbols/libraries, copy and past capacitor to the filter box.

Select C for Unpolarized capacitor (though you could use a polarized capacitor), and click Ok.

Whilst the component is ‘see through’ move and place it by clicking the mouse key.

Hover over the capacitor symbol and press ‘e’ for edit, as done earlier for the resistor.

Click on the Footprint text box and then click the ‘books’ to open the foot print library.

This time scroll on the left to Capacitor_SMD and then scroll to and double click C_0603_1608Metric on the right list.

Then click on the Value text box and type 10u or 10uF.

Then Click Ok to save the edit.

Hover over the capacitor symbol and press ‘c’ to copy and then place a second by moving the copy and clicking to position it.

As noticed the capacitors are a little too close to the resistors. Click and hold the mouse button, starting top left of middle resistors and move to bottom right to select two resistors.

Then drag the components by moving the mouse to the new position and click the mouse button to place.

Now we add two LEDs in series with our outer most resistors.

Click on the screen/grid. Then type LED (or copy paste if you have a large number of symbols) and select LED and click Ok.

Press ‘r’ for rotate a few times to orient the LED as shown.

Click to place the LED.

Press ‘e’ to edit the component and click on Footprint text box and then the books on the right to open the footprint library.

Scroll on the left column to LED_SMD and in right column double click on LED_1206_3216Metric.

Then click Ok to close the symbol editor.

1206 is a fairly common SMD led size and should be a decent size for our purposes.

Now duplicate this LED by hovering over it and pressing ‘c’ for copy and placing it on the opposite side by moving it and clicking once positioned.

Now we need to draw the wires to create the circuit.

or hover over the top left LED pin (circle on component pins) and press ‘w’ for wire.

Then move the mouse to the pin to connect the wire to, the opposing LED…

… and click on the pin. Note the automatic creation of the connection points (big green circle) on each pin. This means all those components are connected to the same “NET” or circuit wire.

Do the same with the rest of the connections, to create the following circuit.

Take care with the four cross over wires which should NOT have a junction circle (green dots). If you find a junction is created automatically it will be because your wire crosses a ‘pin’, so move components as needed to avoid this.

Now we have a fairly complete circuit, but we still need power and ground.

Then click on the screen to open the selector. Scroll down, select GND and press Ok.

Place GND near the bottom.

Repeat this except place VDD at the top.

To ensure we have an easy way to connect power and ground, we also add a connector for power and ground.

Select the component symbol and click on the grid/screen.

Type ‘conn’ and scroll down to Connector_Generic and select Conn_01x02 and press Ok.

Place the component by clicking on the screen somewhere. The location is not important as we will keep it ‘separate’.

To set a footprint, hover over the connector component and click ‘e’ for edit. Then click on the Footprints text box and then click on the ‘books’ icon to open the footprint library.

Select Connector_Wire, SolderWirePad_1x02_P3.81mm_Drill0.8mm. This footprint may be too large, but before creating the PCB we are not sure, so select it as a starting point.

Now we will connect ground to pin 1 and Vdd to pin 2 of the connector.

Hover over the GND component at the bottom of the schematic and press ‘c’ for copy. Then move it to near pin 1 of the connector.

Then Hover over VDD component at the top of the schematic and press ‘c’ for copy. Then move it to near pin 2 of the connector.

Keeping VDD at the top and GND below which is a convention in electronic circuits.

To make the wire layout clean, hover over the connector, press ‘m’ for move and then press ‘r’ twice to rotate the component ‘upside down’. Then move it to the left and click to place it.

Now move cursor to the pins and click ‘w’ for wire and connect the wires.

That completes our circuit layout. Note how it looks like we have two circuits. This is because VDD and GND are ‘invisibly’ connected.

If you click the ‘Highlight net tool’ on the right (pink and grey lines) and then click on the top green wire, which is the ‘VDD NET’, you will see the ‘invisible connection’ in the pink lines on the circuit.

It is a convenient way to visually verify your circuit connections. The safest way though is to use the Electrical Rules Checker.

Electrical Rules Checker

Now we need to check our circuit. The Rule checker helps us by finding issues with our schematic before we go to design the PCB.

Click on the lady bird (bug) icon at top right of tool bar, then click Ok.

The ‘Messages box’ has a message Item not annotated. This is because we have not given each of our components unique identifiers, which is necessary.

Press Close to close the window.

We can manually annotate if we want, but we can automate this, especially useful with larger circuits.

You can control what is annotated, but for our purposes default settings are fine, so press Annotate button to give each component an identifier.

Press Close to close the annotate window.

Now you will see all the components have an ID and the ? marks are gone.

Press the lady bird button at the top right again, and Press Run in the popup window.

As you can see there are three messages, and three green arrows on the schematic to show where the error is.

The first error is telling us that the connector pin for GND is not connected. If you zoom in, it certainly looks connected and no different to the VDD connector.

To work around this (which may be an issue with the component itself), we can try add a junction.

Then move the cursor to the join, and click to add the junction. Press Run on the Rule Checker window again to check. (Note, you can move the window to the right so it is always there while you fix the circuit, for convenience).

That has corrected the warning, though technically this one should not have been necessary.

The last two errors are related to Kicad noticing the circuit does not have any ‘driving’ components. This is because we have a passive circuit that will be connected to a battery or other power source, which is not defined in the schematic.

To hide these warnings we can add what Kicad calls a ‘power flag’.

Select PWR_FLAG and press OK.

Place this component near the connector’s VDD. Then hover over it and press ‘c’ to copy it and move it near the GND.

Finally go to the pin and press ‘w’ for wire and create a wire from the PWR_FLAG to the GND and VDD NETs.

Another Run of the Electrical Rules Checker now will show no warnings or errors.

Finally lets chose the resistors to use. For the maths behind choosing resistor and capacitor values, refer to Astable Multivibrator.

We have two load resistors in series with the LEDs (on the same ‘line’). These we can make 100ohms and are responsible to ensure the current through the LEDs is not too high.

Hover over the resistor and press ‘e’ to edit. Change the Value to 100.

The remaining two resistors R2&R3 we will set to 33kOhms.

The result of this circuit is a flashing rate of just under a second.

Congratulations, one flashing LED circuit.

Exercises

1. Test your skills and add a second LED in parallel to each existing LED. i.e. one led to right of D2 and another LED to left of D1.
2. This circuit has no input protection, so if someone were to supply a high voltage, components would be damaged. Add a current limiting resistor and Zener diode to provide some simple protection to your circuit.

For theory refer to Designing a Simple Over-Voltage Protection Circuit using Zener, which is effectively a Voltage Regulator.