|
FreePCB User
Guide |
Version 1.2 |
7. Tutorial (continued)
7.9 Routing
Ok, let's route our PCB. Before starting, you might want to
review Section 5.13: Nets, Ratlines and Routing.
- Optional: If you want to try some of the ratline editing features
that were
described in Section 5.13: Nets, Ratlines and Routing:
- Start by saving your project, so you can reload it if you screw
up.
- From the menus, select Project
> Nets...
to pop up the View/Edit Netlist
dialog. Make all of the nets invisible except GND.
- Select a ratline and delete it by pressing F7
("Delete Connect"). Then press F8 ("Recalc. Ratlines"),
and the ratline should reappear.
- You can add a new ratline between
pins on the same net by selecting one of the pins and using F4 ("Connect Pin"),
which allows you to draw a ratline to the other pin. Then press F3
("Lock Connect") to lock it. Now if you press F8 ("Recalc.
Ratlines"), some other ratline on the net should disappear.
- You can unlock the locked connection with F3. Then if you press F8 the
connections should revert back to their original state.
- OK, back to business. Use the View/Edit Netlist
dialog to make all of the nets visible.
- If necessary, use the View/Edit
Layers dialog to make the inner 1 and inner 2 copper layers
invisible
- Now your board should look something like:

- Select a reasonably small value for the routing grid such as 10 mils.
- We will be routing traces on the top and bottom copper layers, since inner
1 and inner 2 were used for the VCC and GND planes. The currently active
layer is shown on the status bar ("Top" in the screenshot above).
Press the "4" key to switch to the bottom layer (since there are 4
layers). Press the "1" key to switch back to the top layer. Keys
"2" and "3" would select the inner layers.
- Now select one of the longer ratlines, such as the one in the lower left from
JP4.8 to U1.14.
Press F4 ("Route Segment") to start routing. The cursor should
change to a cross-hair, and you will be dragging a trace segment from
whichever pin was closest to the cursor when you pressed F4. Since the
active layer is "Top", the trace segment will be colored green.
Notice that the angle of the segment will snap to multiples of 45 degrees.
- Place the first vertex in the trace by left-clicking the mouse. Now you
will be dragging a new segment from the vertex. Press "4" to
switch to the bottom layer. The segment will become red, and a via should
appear at the vertex.
- Continue adding segments until you are ready to complete the trace by
drawing a segment from the last vertex to the end pin. Press F4
("Complete Segment") to add the last segment, or just left-click
on the end pin. Your trace should look something like the screenshot below.
Notice that I have used a few more segments and vias than necessary.
- Now let's try editing the trace which you just drew. Select one of the
vertices by clicking on it. A small white box should appear around it to
indicate that it has been selected, and information about the vertex should
appear in the status bar. The editing options for a vertex are:
- F1 ("Set Position") - pop up a dialog to set the
X and Y coordinates of the vertex explicitly.
- F4 ("Move Vertex") - start moving the vertex by
dragging it with the mouse. The snap-angle will not be in effect, but
the routing grid will.
- F5 ("Delete Vertex") - remove the vertex, and
unroute the two adjacent segments, which will be replaced by a single
ratline segment.
- F6 ("Unroute trace") - unroute the entire trace,
which will revert to a ratline.
- F7 ("Delete Connect") - delete the trace,
without replacing it with a ratline.
- F8 ("Recalc. Ratlines") - regenerate the
ratlines for the net.
- Now select one of the trace segments, which should turn white indicating
that it has been selected. The editing options for a trace segment are:
- F1 ("Set Width") - pop up a dialog allowing you
to set the width of the net, trace or trace segment.
- F5 ("Unroute Segment") - replace the segment
with a ratline.
- F6 ("Unroute trace") - unroute the entire trace,
which will revert to a ratline.
- F7 ("Delete Connect") - delete the trace,
without replacing it with a ratline.
- F8 ("Recalc. Ratlines") - regenerate the
ratlines for the net.
- Most of these editing options are fairly self-explanatory, so
you can try them out on your own. Try deleting a vertex or trace segment,
and then re-routing the resulting ratline. Ratlines between vertices are
routed just like ratlines between pins.
- Now let's change the widths of some traces. Zoom in on the components in
the upper left corner, like this:

- The traces between JP6, D1, R3, C2 and U3 are power traces, so let's make
them wider than the default 10 mils. Select the ratline between JP6.1 and
D1.1. The status bar should indicate that this is net "N00534".
Press F1 ("Set Width"). The following dialog should pop up:

- The drop-down menu for Trace
width (mils) has two options, 10 and 15 mils. Lets use 20 mils
instead, by typing "20" directly into the text box. Click OK
to exit the dialog.
- Now route the trace. Since the D1 is an SMT part, the trace segment which
connects to D1.1 must be on the top layer. If you start routing from this
pin, the active layer will be automatically set to "Top". If you
start routing from JP6.1, which is a through-hole pin, you can start on
either "Top" or "Bottom" but you must be on
"Top" to complete the trace to D1.1.
- In similar fashion, set the width of the other power traces to 20 mils and
route them. Your board should look like:

- Now route the rest of the traces on the board. Feel free to get creative
with trace widths and routing if you like. If we were actually going to
produce the board, it might look something like this.
