| FreePCB User Guide | Version 1.2

PREV | Table of Contents | NEXT

5. PCB Layout (continued)

5.9 PCB Elements

5.91 Individual Elements

The representation of the PCB in the layout window consists of various items, which are listed in this section. Note that most of these may be selected by clicking on them. Once an item has been selected, operations can be performed on it by pressing a function key or by right-clicking and making a selection from the context menu. If the operation involves dragging the item, function keys can sometimes be used to perform additional operations while dragging.

The elements of the PCB are listed below, along with their associated function key operations.

- Origin: This is a symbol that identifies the origin of the PCB coordinate system (i.e. the point where X = 0 and Y = 0). It looks like a cross with a small circle at its center. It is always visible, and cannot be selected. It can be moved using Tools > Move origin.
- Visible grid: Dots in a regularly-spaced array, used for visual reference. The grid spacing is set by a drop-down menu in the taskbar.
- Board outline: This is a closed polyline, consisting of a set of points (corners), with lines between them (sides). The sides may be straight lines or arcs. The corners and sides are selectable, and may be edited as follows:
  - Corner:
    - F1 (Set Position) - pop up a dialog that allows you to edit the X and Y coordinates of the corner explicitly
    - F4 (Move Corner) - start dragging the corner with the cursor
    - F5 (Delete Corner) - remove the corner
    - F7 (Delete Outline) - remove the entire board outline
  - Side:
    - F1 (Straight Line) - make the side a straight line
    - F2 (Arc CW) - make the side a clockwise arc
    - F3 (Arc CCW) - make the side a counterclockwise arc
    - F4 (Add Corner) - insert a corner into the side and starts dragging it
    - F7 (Delete Outline) - remove the entire outline
- Part footprint: This is a compound symbol consisting of a set of copper pads, a part outline, a text string for the reference designator of the part, and possibly other text strings. The entire footprint, a single pad or the reference designator may be selected for editing.
  - Entire footprint:
    - F1 (Edit Part) - pop up a dialog to edit the properties of the part
    - F2 (Edit Footprint) - switch to the Footprint Editor window, with the footprint of the part already imported for editing
    - F3 (Glue/Unglue Part) - a "glued" part can't be moved without "ungluing" it
    - F4 (Move Part) - start dragging the footprint to move it
      - While dragging:
        - F2 - flip part from one side of the board to the other
        - F3 - rotate part 90 degrees clockwise
    - F7 (Delete Part) - remove the part from the PCB and the partlist
    - F8 (Recalc. Ratlines) - reassign ratlines for all nets which connect to the part to minimize their length
  - Pad:
    - F1 (Set Net) - pop up a dialog to assign the pad to a net
    - F3 (Start Stub) - start dragging a new stub trace
    - F4 (Connect Pin) - start dragging a ratline to another pad
    - F8 (Recalc. Ratlines) - reassign ratlines for the net which connects to this pad to minimize their length
  - Reference designator text:
    - F1 (Set Size) - pop up a dialog that lets you change the size and direction of the text string
    - F4 (Move Ref Text) - start dragging the text string to move it
      - While dragging:
        - F3 (Rotate Ref Text) - rotate the text string 90 degrees clockwise
- Trace: This is a polyline representing a connection between two pads. It consists of one or more straight-line segments with vertices between the segments. The segments may be routed (i.e. physically present on a copper layer) or unrouted. Unrouted segments are called ratlines.
  - Ratline: This is a line representing an unrouted segment of a trace.
    - F1 (Set Width) - pop up a dialog that lets you set the change the trace and via widths of the trace or net
    - F3 (Lock/Unlock Connect) - a locked ratline can't be eliminated by the "Recalc. Ratlines" operation
    - F4 (Route Segment) - start dragging the endpoint of a routed segment to replace the ratline
      - While dragging:
        - F4 (Complete Segment) - extend the routed segment being dragged to the endpoint of the ratline
    - F5 (Change Pin) - change the pin to which the ratline is connected
    - F7 (Delete Connect) - remove the connection (start_pin to end_pin) from the net
    - F8 (Recalc. Ratlines) - reassign ratlines for the net to minimize their length
  - Segment: This is a line representing a routed segment of a trace.
    - F1 (Set Width) - see above
    - F5 (Unroute Segment) - unroute the segment, converting it to a ratline
    - F6 (Unroute Trace) - unroute the entire trace, converting it to a ratline
    - F7 (Delete Connect) - remove the connection (start_pin to end_pin) from the net
    - F8 (Recalc. Ratlines) - reassign ratlines for the net to minimize their length
  - Vertex: This is a point at the junction of two segments, or a segment and a ratline. If both segments are routed on different layers, there will be a via at the vertex.
    - F1 (Set Position) - pop up a dialog that allows you to edit the X and Y coordinates of the vertex explicitly
    - F4 (Move Vertex) - start dragging the vertex to move it
    - F5 (Delete Vertex) - remove vertex, unrouting the adjacent segments
    - F6 (Unroute Trace) - unroute the entire trace
    - F7 (Delete Connect) - remove the connection (start_pin to end_pin)
    - F8 (Recalc. Ratlines) - reassign ratlines for the net to minimize their length
- Stub Trace: A stub trace starts on a pad but doesn't end on a pad. It usually ends with a via, which is used to connect the trace to a copper area on another layer. It may contain ratlines, segments and vertices like a regular trace, but the last segment and last vertex are treated specially.
  - End Segment: The last routed segment.
    - F1 (Set Width) -
    - F5 (Delete Segment) - remove the segment
    - F7 (Delete Connect) - remove the entire stub trace
    - F8 (Recalc. Ratlines) - reassign ratlines for the net to minimize their length.
  - End Vertex: The last vertex (i.e. the end-point of the stub trace).
    - F1 (Set Position) - pop up a dialog that allows you to edit the X and Y coordinates of the vertex explicitly
    - F2 (Add Segment) - start dragging a new segment to extend the stub trace
    - F3 (Add/Delete Via) - add or remove a via at the end of the stub trace
    - F4 (Move Vertex) - start dragging the end vertex to move
    - F5 (Delete Vertex) - remove the segment
    - F7 (Delete Connect) - remove the entire stub trace
    - F8 (Recalc. Ratlines) - reassign ratlines for the net to minimize their length
- Copper Area: This is a closed polyline which defines an area of solid or patterned copper on one of the copper layers. It is used to created ground planes, heatsinks, etc. It consists of a set of corners with sides between the corners. It is filled with a hatch pattern of diagonal lines. Note that this hatch pattern is for visual identification of the area only, and does not represent the actual copper pattern which will be applied to the PCB. It may also contain cutouts, which are "holes" in the copper area. Cutouts are edited just like copper areas.
  - Corner:
    - F1 (Set Position) - pop up a dialog to set the corner position explicitly
    - F4 (Move Corner) - start dragging the corner to move it
    - F5 (Delete Corner) - remove the corner
    - F6 (Add Cutout) - start drawing a new polygon for a cutout in the copper area
    - F7 (Delete Area) - remove the entire area
  - Side:
    - F1 (Straight Line) - if the side is an arc, convert to straight line
    - F2 (Arc (CW) ) - convert side to clockwise arc
    - F3 (Arc (CCW) ) - convert side to counterclockwise arc
    - F4 (Add Corner) - add a new corner and start dragging it
    - F6 (Add Cutout) - start drawing a new polygon for a cutout in the copper area
    - F7 (Delete Area) - remove the entire copper area
- Text String: This is a string of alphanumeric characters, used for adding labels, copyright notices, etc. It may be placed on a silk-screen or copper layer.
  - F1 (Edit Text) - pop up a dialog to edit the string and its properties, such as size and stroke width
  - F4 (Move Text) - start dragging the string to move it
  - F7 (Delete Text) - remove the entire string

- Solder Mask Cutout: This is a closed polyline that defines a cutout in a solder mask layer.
  - Corner:
    - F1 (Set Position) - pop up a dialog to set the corner position explicitly
    - F4 (Move Corner) - start dragging the corner to move it
    - F5 (Delete Corner) - remove the corner
    - F6 (Add Cutout) - start drawing a new polygon for a cutout in the copper area
    - F7 (Delete Area) - remove the entire area
  - Side:
    - F1 (Straight Line) - make the side a straight line
    - F2 (Arc CW) - make the side a clockwise arc
    - F3 (Arc CCW) - make the side a counterclockwise arc
    - F4 (Add Corner) - add a new corner and start dragging it
    - F6 (Add Cutout) - start drawing a new polygon for a cutout in the copper area
    - F7 (Delete Area) - remove the entire copper area

5.92 Groups of Elements

A group of elements can be selected by drawing a rectangle around them with the mouse. All of the items in the group will be highlighted. Individual items can be added to the group or removed from the group by clicking on them with the Ctrl key held down. Currently, the only operation that can be performed on the group is F4(MoveGroup), which allows you to drag the group to a new position with the mouse.

5.93 Moving items or groups with the arrow keys

When an item or group is selected, you can move it by selecting a move operation with the function keys or context-menu, and then dragging it with the mouse. Most items and groups can also be moved by pressing the arrow keys on the keyboard. Pressing an arrow key will move the item or group a distance equal to the current setting of the placement grid or routing grid, depending on the item selected. Smaller movements can be made by holding down the Shift key when pressing the arrow key, which will move the item 1 mil or 0.01 mm, depending on the units in use.

PREV | Table of Contents | NEXT