| FreePCB User Guide | Version 1.2

PREV | Table of Contents | NEXT

7. Tutorial (continued)

7.7 Adding Parts and Editing Nets

Modifying a PCB design by adding, replacing or deleting parts or changing the netlist is sometimes referred to as "on-the-fly" editing. FreePCB gives you virtually unlimited freedom for this type of editing. However, you should use this freedom carefully. Keep in mind that by modifying the partlist and netlist, you are creating a discrepancy between your PCB layout and the original schematic. If you make any significant changes you should carefully back-annotate them to the schematic, otherwise troubleshooting the PCB can be a nightmare. In general, "on-the-fly" editing is best used for relatively minor changes. If you need to perform more extensive redesign, you should probably go back to your schematic editor and create a new netlist file.

In this section, we will add three bypass capacitors to our PCB, one for each of the DIP ICs. We will connect them to the VCC and GND nets. Since FreePCB provides several methods for doing this, we will try them all.

- Set the placement grid to a reasonable value for surface-mount capacitors such as 50 mils.
- Select Parts... from the Project menu. The View/Edit Part List dialog should appear.

- Note that the last capacitor in the part list is C4. We will add C5, C6 and C7.
- Click on Add New Part. This will bring up the Add/Edit Part dialog.

- Expand the library sm_capacitor.fpl by clicking on the "+" sign next to it.
- Select the footprint "C1206" by clicking on it. The Footprint field should change to "C1206".
- Enter "C5" in the Reference field. Now you should see:

- Click OK to add the part to the partlist.
- Now you will be back in the View/Edit Part List dialog. Click OK to exit. Your new capacitor C5 will be visible just to the left of the origin.

- Select C5 by clicking on it, and move it near the top of Y1. Move the reference designator text if necessary so that it will be visible.

- Now we will connect the pins of C5. Lets start by making only the nets VCC and GND visible. Select Project > Nets... to bring up the View/Edit Netlist dialog.

- Click the Make all visible/invisible button twice, to clear all of the checkboxes and make all of the nets invisible. Then click on the boxes for VCC and GND, to make these nets visible. Then click OK. Now only the VCC and GND ratlines are visible, as shown.

- Click on the right-most pad of C5 to select it. This will be pin 2, unless you rotated the part. Press F1 ("Set Net") to pop up the following dialog:

- From the drop-down menu, select VCC, or just type "VCC" into the text box. Click OK to connect the pin. Press F8 ("Recalc. Ratlines") to recalculate the ratlines for VCC to include the new pin C5.2.
- Now select the left-most pad of C5, and repeat the above procedure to connect it to GND. Now you should see ratlines to both pads of C5.

- Let's use a slightly different method to add C6. Select Add > Part. The Add/Edit Part dialog will pop up. This is the same dialog that you invoked previously from the View/Edit Partlist dialog, except that the Drag to position button is now enabled and selected. This time, select C0805 for the footprint of the new part. Enter C6 into the Reference field.

- Press OK. You should find yourself dragging the outline for C6. Place it near pins 19 and 20 of U1, as shown.

- We will connect C6 to the VCC and GND nets by drawing ratlines between pins. Select the upper pad of C6 by clicking on it. Then press F4 ("Connect Pin"). You should start dragging a ratline from the pad. Move the cursor over the pad for pin 20 of U1 (which is attached to net VCC) and click to connect the ratline to this pin. In similar fashion, connect the lower pad of C6 to pin U1.19. Select C6 by clicking on it, and press F8 ("Recalc. Ratlines") to recalculate the ratlines for C6. Your layout should look like this:

- Finally, add C7 using Add > Part, the same way we added C6. Place it near the top of U2, similarly to the way we placed C5 near the top of Y1.
- Now let's connect it to VCC and GND by using Project > Nets..., to pop up the View/Edit Netlist dialog. Then select the VCC net by clicking on it, as shown.

- Now click on Edit selection. The Add/Edit Net dialog will appear.

- Enter C7.2 into the text box next to the Add Pin button. Then click on Add Pin. C7.2 should be added to the Pin list. Click OK to accept it. This will return you to the View/Edit Netlist dialog.
- Now select the GND net by clicking on it, and edit the pin list just as you did for VCC, this time adding C7.1.
- Tip: When you add a pin to a net using the Add/Edit Net dialog, be sure that you click on Add Pin. Don't just click on OK, which exits the dialog without adding the pin.
- Press F8 ("Recalc. Ratlines") to add ratlines to the newly added pins. The layout should now look like:

In the next section we will use copper areas and stub traces to create power and ground planes for VCC and GND.

PREV | Table of Contents | NEXT