Add a capacitor to the schematic using Eeschema

The first version of the breakout is a good start, but considering how the nRF24 module is normally used, I realized that it can be improved. An obvious improvement is the inclusion of  a capacitor on the breakout PCB, so that we don’t have to plug one on the breadboard. The capacitor is used to help smooth out any ripple effects from the power supply that feeds the module. It also stores energy which is used for for when the power supply can’t provide enough. That’s used for when you connect the module to a small Arduino or battery powered applications.

Two more things I would like to do in order to improve our design, is to add a copper fill for ground. The copper fill is simply an area on the board that is covered by copper, and connected to the ground pads. Ground copper fills (also known as “ground planes”) have certain benefits, including reducing the amount of chemicals used in etching the copper from the board during manufacturing. Having a ground plane can make routing easy since a return path for the current can always be found nearby.

I would also like to adjust the width of the Vcc track, so that it’s a little bit larger than the rest, again so, that it provides a bigger path with a lower impedance for current to flow through.

Both improvements are not strictly needed for this small project. They actually are not going to make any difference to the way that the circuit will behave, but they are a good common practice for any PCB design, regardless, and it takes very little effort to do, anyway.

Let’s go ahead and add the capacitor first.

First, we will update our schematic with the new component in Eeschema, then create a new netlist. After that, we will start Pcbnew and import the new netlist. This will, in effect, insert the new component to the layout editor, place it on the canvas, and do the wiring.

Start Eeschema and hit the ‘A’ key to add a new component.

Let’s search for a capacitor. I would like to use an electrolytic capacitor. The component chooser gives us a few options. Some of them are non-polarised capacitors, some others are polarised. Our electrolytic capacitor is polarised, so I will choose an option with the appropriate symbol.

Image

We will add a polarised capacitor; be careful to select the appropriate component.

Double-click on this option to insert this component to the canvas.

Image

The new component is on the canvas now. Notice the “+” sign indicating the polarity of the capacitor, and the designator that contains a question mark.

You can see that the designator is got a question mark still, so it hasn’t been given a number yet.

Image

The capacitor is connected to the rest of the circuit.

Let’s do the connections. Use the ‘W’ key to create a wire. Connect the negative pin of the capacitor to pin 0 of the nRF24 component. Connect the positive pin of the capacitor to pin 7 of the nRF24 component. To confirm that two wires are properly connected, look for a solid green dot at the junction of the two wires. If there is no dot, then the two wires are simply crossing, but not connected.

Don’t forget to save your new schematic.

Let’s continue with the the annotation.

Image

The annotation tool button.

Click on the ‘Annotate Tool’.

Image

The Annotate Schematic window. The defaults are usually good to use.

The default options in the Annotate Schematic window are good as they are, so click ‘Annotate’.

Image

We only want to annotate unannotated components anyway.

You will see an information box explaining that only unannotated components will be annotated. This is exactly what we want, so click on OK to complete the process.

Image

The capacitor now has a unique designator.

So, there’s the designator for the capacitor, it’s now C1. I would also like to assign the capacitor with a value, so that will show up on the schematic.

Image

You can edit the value of a component by accessing it’s Edit Value Field window.

Hit the ‘V’ key, as your cursor is over the capacitor. The Edit Value window will come up. Type the value “10 μF” in the Text box, and click OK.

Image

The capacitor value is showing in the schematic.

You could also have done the same thing by hitting the ‘E’ key.

Image

Typing “E” will bring up the properties window for the component. You can edit the component value, as well as various other properties.

This would take you to the component’s properties window.

Next, let’s do the associations of this schematic component with a footprint. Start the Cvpcb tool to do this.

Image

In Cvpcb, you can see that the capacitor does not have an association yet.

You can see here that the new component does not have an association. Let’s look for a footprint for the capacitor. We need to find something that will have the appropriate size on the board.

Image

Find a footprint that has the right dimensions for the component.

Our capacitor is a through-hole component. You can use a ruler to measure the distance between the pins and the diameter at its base.  You can see this in the photograph, that this capacitor is a radial capacitor with a diameter of 10 mm. You can look for a footprint in the Capacitors_Throughole library. The contents of this library have footprints with the sizes included in the filename. This is very convenient! Look for one with “D10” in its name (for “Diameter”), and there is a good chance that this is the footprint you need.

Image

Click on the preview button to see the selected footprint.

Image

Inspect the footprint to ensure it is the right one for the component.

You can also look at the footprint preview in order to ensure that it is the right one for your component. You can have a look at the way that it looks like.

Double-click on the footprint titled “Capacitors_Throughhole:C_Radial_D10_L16_P5” to select it, and the association is complete.

Save the footprint associations and go back to Eeschema. Let’s generate the new netlist.

Image

Click to generate a new netlist.

The Netlist dialogue, click on Generate. It is ok to overwrite the previous netlist.

Image

Click “Generate”. It is ok to overwrite the old netlist file since now it is out of date.

We now have a new netlist, so we can exit Eeschema and get into Pcbnew to do the layout and the wiring. We will do this in the next chapter.

Back to top
« « Section introduction | Add a capacitor to the layout in Pcbnew » »