| FreePCB User Guide | Version 1.2

PREV | Table of Contents | NEXT

7. Tutorial (continued)

7.8 Adding Copper Areas

In this section, we will create copper areas on the inner layers for power and ground planes.

- Select Project > Nets.... The View/Edit Netlist dialog should appear. If you are continuing from the last section, only the VCC and GND nets will be visible, as shown.

- Click on Make all visible/invisible one or two times to make all of the nets invisible. Then click on the GND checkbox to make only that net visible.
- Notice that the trace width for every net is "0". That means that the project default of 10 mils will be used. Let's change the trace width for GND to 15 mils.
- Select the GND net by clicking on its name, which should highlight it. Then click on the Change widths button. The following dialog should appear.

- Select "15" for the new width for the GND net by selecting that value from the drop-down menu, or enter "15" into the text box. Leave the Use default via for this trace width radio button selected. If we wanted to override the default via, we could select Set via widths instead, and set the via width and hole size explicitly in the text boxes. Click OK to exit the dialog.
- The View/Edit Netlist dialog should now look like:

- Click OK to exit the dialog. The layout window should now show only the ratlines for the GND net, as shown.

- Now we will add the copper area for the GND plane. First, set the routing grid to 50 mils. Then select Add > Copper Area. The following dialog should appear.

- We will use the "inner 1" copper layer for the GND plane. Select "GND" from the Net drop-down list, or type "GND" into the text box. Select "inner 1" from the Layer list. Set a hatch pattern of Full.

- Click OK to exit the dialog and start drawing the polyline for the copper area. The cursor should change to a cross-hair. We want to draw the outline of the copper area 50 mils inside the board outline. Place the cursor at the lower-left corner of the copper area, which will be at X = 50, Y = 50. Left-click to place the first corner. Then move the cursor to X = 50, Y = 1950 and left-click to place the second corner. Place the third corner at X = 2950, Y = 1950 and the fourth corner at X = 2950, Y = 50. After placing the fourth corner, right-click to close the polyline. Now your board should look like:

- Notice that the copper area has been drawn with a diagonal hatch pattern, in the color for layer "inner 1". Also, most of the ratlines for the GND net have disappeared, and X-shaped symbols in the ratline color have appeared on the through-hole pins in the net. These indicate internal connections of these pins to the GND copper area, using plated-through holes with thermal reliefs.
- We still have to connect the SMT pins to the GND copper area. For this, we will use stub traces, which are short traces that begin on a pin and end with a via to the GND plane.
- Let's start with the lower pin of C1. Select the pin by clicking on it. A white box with an "X" through it should appear around the pin, indicating that it has been selected, and the status bar should contain a description of the pin.
- Now start drawing the stub trace by pressing F3 ("Start Stub" ). The cursor should change to a cross-hair, and you will be dragging the end of a trace segment from the pin, on the top copper layer. You may wish to zoom in with the scroll wheel or the Page Up key. Move the cursor a short distance below the pin, and left-click to set a vertex. Then right-click to end the trace. A via should appear at the vertex, as shown. Notice that there is a thermal-relief symbol on the via, indicating an internal connection to the GND copper area.

- If you are unhappy with your trace, you can delete it by selecting the trace segment or the end via and pressing F7 ("Delete Connection"). You can move the end via by selecting it and pressing F4 ("Move Vertex"). You can add segments by selecting the end via and pressing F2 ("Add Segment").
- Since stub traces are usually used to connect pins to copper areas on other layers, the end via is added automatically when you end a stub trace. If you want, you can delete the via by selecting it and pressing F3 ("Delete Via"). This may be useful if you are connecting a pin to a copper area on the same layer, or if you are using a stub trace for some other purpose such as a shield trace.
- Now that you know how to do it, add stub traces to all of the SMT pins which have ratlines. You may need to move some of the reference designators to keep them free of the end vias, since it is generally a bad practice to have a silk-screen item overlapping a pad or via. Your board should look something like:

- Congratulations, you have now routed the entire GND net, which is by far the largest net in the design. The copper area made it easy.
- Since we won't be doing any routing on the "inner 1" copper layer, and since the hatch pattern may be annoying when we are working on other layers, let's make it invisible. Select Layers from the View menu to bring up the View/Edit Layers dialog, and uncheck the Visible checkbox next to Inner 1. Click OK, and the copper area should disappear. Alternatively, we could have changed the hatch pattern by selecting a side and right-clicking, then selecting Hatch style from the context menu.
- Now, let's add a copper area for net VCC on the "inner 2" copper layer. You just need to repeat the same steps that you performed for the GND area. These are:
  - Make the VCC net visible.
  - Change the VCC trace width to 15 mils.
  - Draw the VCC copper area on the "inner 2" layer (you can use the same corner positions as the GND area).
  - Add stub traces for all of the SMT pads on the VCC net. There should be four, on C1, C5, C6 and C7.
  - Make the "inner 2" layer invisible.
- Select Project > Nets... to launch the View/Edit Netlist dialog. Make both VCC and GND visible. Your board should look like:

In the next section we will route the rest of the nets on the top and bottom copper layers.

PREV | Table of Contents | NEXT