| FreePCB User Guide | Version 1.2

PREV | Table of Contents | NEXT

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 Projec t > 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.

PREV | Table of Contents | NEXT