|
FreePCB User
Guide |
Version 1.2 |
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.