Associate components with footprints

In this chapter we’ll create the component-footprint associations and then we will export the netlist file. Let’s begin with starting Cvpcb. If you are still in Pcbnew, click on the Cvpcb button:

Image

Start Cvpcb.

You will see the Cvpcb window, with the middle pane containing the components from the schematic.

Image

Cvpcb lists the schematic components in the middle pane.

We can start with the capacitor. For the capacitor, we’re looking for an SMDs type package. The one I would like to use is an electrolytic SMD aluminium capacitor, measuring 6.3 mm by 5.3 mm, like this one:

Image

An electrolytic SMD capacitor.

Select the Capacitors_SMD library from the left pane, and enable the Library filter. In the right pane there is a long list of candidate footprints. Scroll down until you find one that measures the correct dimensions:

Image

Select the library, filter, and look for the right footprint.

Confirm that you have the right footprint by looking at its preview:

Image

This is the footprint of an SMD electrolytic capacitor.

Double click to select this footprint and associate it wit the capacitor component.

For the LEDs, again I amlooking for an LED surface mounted device of 0805 type. Select the LEDs library, and inspect the list in the right pane.

Image

Candidate footprints for the LEDs.

There are several options for 3mm, 5mm, and 0805 here, among others. I am looking for the 0805, so double click on that to select it. Continue to double click until all LED have the 0805 footprint associated.

Image

The LED components are associated with the 0805 footprint.

Let’s skip the connector and work on the resistors next. Instead of selecting a library first, I will use the keyword and pin count filters to find the right footprint.

Image

With the keyword and pin count filter, I can quickly find the correct Resistor footprint.

Look for the 0805 type resistor, and double click several times to associate this footprint with all of the resistor components. Here is the end result:

Image

The resistor components are now associated with the 0805 footprint.

Let’s continue with the connector. Click on the CONN_01X05 component in the middle pane, and with the  filter settings unchanged, the suggested footprint in the right pane are just four. I’d like to use the straight header connector, so double click on the second option to select it.

Image

The options of the connector.

Image

The connector component is associated with the straight header.

Lastly, for the shift register, we need to look in the SMD package to find the appropriate footprint. Click on the library filter button, and click again on the other two filters to disable them. This part is more complicated than the resistor and capacitor, so I prefer more control over the browsing process. The integrated circuit I would like to use on the board comes in an SO16 package, so we need to find one of them in the right pane.

Image

Only the Library filter is used for the search for the SO16 package.

The correct footprint for our component is most likely the SO-16-N option. But because there are three varieties of this footprint, it is better to make sure we have the right one. Let’s bring up the footprint preview:

Image

The SO16-N footprint preview.

Measure the dimensions between the pads, between the rows, and of the package itself. The actual part that I have in my toolbox is this:

Image

The actual IC I would like to use comes in an SO16 package like this one.

I used my rule to measure the distances and found that the pitch between the pads is 1.27mm and that the distance between the two rows is 6.35mm. Use the measuring tool in the footprint previewer to make sure the the footprint you are about to select has the same measurements. This is the correct footprint, so double click to select it for both ICs:

Image

The shift registers are associated to the correct footprint.

We now have all our components associated with their footprints, so we can save the associations and return to Eeschema.

Before we close this chapter, let’s export the netlist file, store it in the project folder:

Image

Generate the netlist file.

Let’s continue with Pcbnew now and work on the layout and the wiring.

Back to top
« « Schematic wiring, Part 2 | Create the PCB in Pcbnew » »