|
FreePCB User
Guide |
Version 1.2 |
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.