Applied Parameters: None
This command is used to access a dialog with which to specify various properties for the active footprint in the current PCB Library document.
This command is accessed from the PCB Library Editor by:
- Choosing the Tools » Footprint Properties command, from the main menus.
- Double-clicking on the entry for the footprint in the Footprints region of the PCB Library panel.
- Right-clicking in the Footprints region of the PCB Library panel, and choosing the Footprint Properties command from the context menu.
First, ensure that the footprint whose properties you wish to browse/change is selected in the Footprints list in the PCB Library panel (and is therefore the active footprint in the main design window).
After launching the command, the PCB Library Footprint dialog will appear, from where you can change the name for the footprint and give it a meaningful description. You can set the height of the component (accommodated by the footprint), and also the type of that component. Choose from the following types:
- Standard - standard electrical component loaded onto board. Always synchronized, always in BOM.
- Mechanical - non-electrical component, e.g. heat sink or mounting bracket. Synchronized if exists on both schematic and PCB documents, always in BOM.
- Graphical - non-electrical component used for company logo, title block, etc. Never synchronized and not included in BOM.
- Net Tie (In BOM) - for shorting two (or more) nets together in the routing. Typically used if a jumper type component needs to be fitted and also provide shorting in the same location. Always synchronized and included in BOM.
- Net Tie - as above but designed so you couldn't tell a component existed at the location where the shorting is to occur. Always synchronized but not included in BOM. When placing components of this type, use the Verify Shorting Copper option in the Design Rule Checker dialog (when performing a DRC in the PCB), to verify the short (i.e. that no unconnected copper exists in the component).
- Standard (No BOM) - standard electrical component loaded onto board. Always synchronized, not included in BOM.
- Jumper - used to represent a wire link, typically used on a single-sided board. On the schematic, Jumper-type components do not need to be wired in, they are only included to ensure that the Jumpers get included in the BOM. On the PCB, set the jumper pads to share the same non-zero JumperID value; the software recognizes this state, adds a symbolic link between the jumper pads to represent the wire link, and factors the link into design rule checks.
After editing the properties as required, click OK to effect the changes. If the name for the footprint has been changed, the Footprints list (in the PCB Library panel) will update accordingly to reflect this.
- The value specified for the height (the height of the component accommodated by the footprint) is used by the Height design rule (part of the Placement category of rules).
- The Type setting allows you to set the type for a footprint that is placed directly from the PCB Library onto the PCB design document. However, if the component has been placed on the schematic side and brought across to the PCB through the synchronization process, then the Type setting defined for that component - on the schematic side - will always take precedence.