| FreePCB User Guide | Version 1.2

PREV | Table of Contents | NEXT

7. Tutorial (continued)

7.3 Importing the Netlist File

The netlist file that we will be using is listed in Section 5.14: Importing Netlist Files. You might want to review that section before continuing. The package for U2 was intentionally left incorrect, so we will have to fix it after the file is imported.

- Select Import from the File menu. A dialog called Open will pop up.

- If necessary, navigate to the "motor" project folder. Select file motor.net.
- Select Parts and Nets in the Import section of the dialog.
- Select PADS-PCB in the Format section of the dialog.
- Click the Open button.
- FreePCB will open a Log window and import the netlist, describing its progress in the Log. You should see a message indicating that a footprint was not found for U2. Click OK to dismiss the Log.
- All of the imported parts will be stacked up just to the left of the origin symbol in the layout window. Select View > All Parts (or press the "Home" key) to see them. Connections between the pins will be shown as ratlines.

- Now we will fix the missing footprint. Select Parts... from the Project menu. The View/Edit Part List dialog should appear:

- This dialog shows a list of all of the parts which were imported, with their reference designators, package identifiers and footprints.
- Note that the footprint for U2 is shown as "??????", indicating that the package identifier "dip14" does not match any of FreePCB's footprints. We need to fix this.
- Select the line for U2 by clicking on it.
- Click the Edit Selection(s) button. The Add/Edit Part dialog should appear as shown below.

- This dialog allows you to edit the parameters for part U2, including its footprint. All of the available footprint libraries are shown in the large tree control occupying most of the dialog. The first entry is "local cache", which is not actually a library but which contains all of the footprints which are currently loaded into FreePCB.
- Expand the "th_dip.fpl" library by clicking on the "+" next to it. This library contains footprints for DIP packages. Its name begins with "th_" to indicate that it contains through-hole footprints.
- Select "14DIP300" from the library by clicking on it. An image of the footprint will appear in the preview window, and "14DIP300" should replace "??????" in the Footprint field. Now the dialog should look like like:

- Click on OK.
- A message box should appear asking whether you want to replace all instances of "dip14" with "14DIP300", or just U2. Since there is only one instance, you can click on either YES or NO.
- This should return you to the View/Edit Partlist dialog, with "??????" replaced with "14DIP300" for part U2.
- Click OK. U2 should now have a footprint, placed at position (0,0), as shown below.

- OK, now all of the footprints are loaded. Save your work. In the next section, we will create the board outline.

PREV | Table of Contents | NEXT