| FreePCB User Guide | Version 1.2

PREV | Table of Contents | NEXT

5. PCB Layout (continued)

5.15 Copper Areas

Besides traces, copper areas can be used for connections on a PCB. These are commonly used for power and ground planes, in which case they may occupy an entire layer of the board. In FreePCB, all copper areas must be assigned to a net.

Copper areas are drawn as closed polylines (or polygons), similar to the board outline. They can be displayed as a simple outline, an outline with internal hatching, or an outline with a little bit of hatching along its inner edge. These hatch patterns are for visual reference only, as the actual copper area on the PCB will be solid copper. FreePCB will automatically create clearances around any pads or traces which pass through the copper area on the same layer. However, these clearances will not be displayed, but will be created in the Gerber files.

To create a new copper area, select Copper Area from the Add menu. The following dialog will appear.

Select the net for the copper area from the Net drop-down menu, or type the net name directly into the field. Select the layer from the Layer list. Choose the Hatch pattern. Then click OK to start drawing the area. The cursor will change to cross-hairs, and the Routing Grid will be in effect. Move to the desired position of the starting corner, and left-click to place it. Now you will be dragging the first side of the polyline. As with the board outline, you can change the style of the side from straight to a clockwise or counterclockwise arc by using the function-key menu. Continue left-clicking to place the rest of the corners, and right click to close the polyline. The copper area will then fill with a diagonal hatch pattern, to make it more visible.

An example of a small copper area on the inner 1 layer is shown below. This area was assigned to the GND net, and it uses the full hatch pattern.

Once created, a copper area can be edited by selecting corners or sides and using the function-key menu. This is exactly the same as editing the board outline, so you can just refer to Section 5.10: Board Outline for instructions. You can change the hatch pattern by selecting a side and right-clicking, then selecting Hatch style from the context menu.

Connections between parts and copper areas can be made two ways:

- Through-hole pins which pass through the copper area can connect using thermal reliefs. These will be placed automatically for pins on the same net as the copper area. They are indicated by an "X" drawn on the pin in the ratline color.

- SMT pads or through-hole pins which do not pass through the copper area can be connected using stub traces which terminate with vias. A thermal relief will be placed automatically on the via.

To illustrate, 4 parts have been placed, overlying the copper area in our previous example. Only the GND net has been made visible, which is the net assigned to the copper area. Note that pins Y1.4, JP2.2, JP2.3, JP2.4, JP2.6, JP2.8, JP2.10 have all been automatically connected to the copper area by thermal reliefs.

To connect R1.1 and C1.2, we will use stub traces. These have been added below. Note that the vias on the ends of the stubs have been connected with thermal reliefs. Now the entire GND net has been connected using the copper area.

The hatch pattern in the copper area is only intended as a visual aid, to show the extent of the area while allowing other features to show through. When the Gerber files are generated, the area will be solid copper with clearances for any non-connected pads and traces which pass through it.

In the tutorial, you will use copper areas to create power and ground planes which occupy entire layers of the PCB.

5.151 Copper Area Cutouts

Sometimes it is useful to "cut out" a portion of a copper area. This may be done to create an opening inside the copper area, or to modify its outline. To create a cutout, select a side or corner of the area and press F6 (Add Cutout). Then draw the cutout just as you would draw a new area. The image below shows our copper area with cutouts around Y1 and JP2.

Note: Actually, I cheated a bit to get the screen shot above. If you tried to add the cutouts directly to the area as shown, you would get an error message indicating that cutouts are not allowed in copper areas that use arcs. This is due to a limitation in the polygon clipping library that FreePCB uses, which only allows straight lines in polygons. Therefore, I converted the arcs to straight lines, added the cutouts, and then converted the straight lines back to arcs. Feel free to use this trick in your own designs.

PREV | Table of Contents | NEXT