PCB Editor object properties are definable options that specify the visual style, content and behavior of the placed object. The property settings for each type of object are defined in two different ways:
Pre-placement settings – most Fill object properties, or those that can logically be pre-defined, are available as editable default settings on the PCB Editor - Defaults page of the Preferences dialog (access from the button at the top-right of the design space). Select the object in the Primitive List to reveal its options on the right.
Post-placement settings – all Fill object properties are available for editing in the Fill dialog and the Properties panel when a placed Fill is selected in the design space.
If the Double Click Runs Interactive Properties option is disabled (default) on the PCB Editor - General page of the Preferences dialog, when the primitive is double-clicked or you right-click on a selected primitive then choose Properties, the dialog will open. When the Double Click Runs Interactive Properties option is enabled, the Properties panel will open.
While the options are the same in the dialog and the panel, the order and placement of the options may differ slightly.
In the below properties listing, options that are not available as default settings in the Preferences dialog are noted as "Properties panel only".
Net Information (Properties panel only)
Net Name - the name of the selected net.
Net Class - the name of the selected net class.
Select the clickable clicks of the Net Name and Net Class from the FIll mode of the Properties panel to be redirected to the PCB - Nets panel, where you may view details of the nets associated.
Location (Properties panel only)
The icon to the right of this region must be displayed as (unlocked) in order to access the below fields. Toggle the lock/unlock icon to change its lock status.
X (first field) - the current X (horizontal) coordinate of the reference point of the fill, relative to the current design space origin. Edit to change the X position of the fill. The value can be entered in either metric or imperial, include the units when entering a value whose units are not the current default.
Y (second field) - The current Y (vertical) coordinate of the reference point of the fill, relative to the current origin. Edit to change the Y position of the fill. The value can be entered in either metric or imperial, include the units when entering a value whose units are not the current default.
Rotation - the fill's angle of rotation (in degrees), measured counterclockwise from zero (the 3 o'clock horizontal). Edit to change the rotation of the fill. Minimum angular resolution is 0.001°.
Net - use the drop-down to select the net to which this fill belongs. All nets for the active board design will be listed in the drop-down list. Select No Net to specify that the fill is not connected to any net. The Net property of a primitive is used by the Design Rule Checker to determine if a PCB object is legally placed. If there is no net, click the assign net button () to open the Net Name dialog, where you may quickly jump to a specific net within the design space by specifying the Net's name.
Layer - the layer on which the fill is placed. Fills can be placed on any layer other than the system layers. Use the drop-down to select a different layer.
Area - specifies the area value of the fill object.
Length - displays the length.
Width - displays the width.
Paste Mask Expansion
Rule - select to have the paste mask expansion for the fill follow the defined value in the applicable Paste Mask Expansion design rule. The associated expansion value will be disabled if this option is chosen.
Manual - select to override the applicable design rule and specify the paste mask expansion value for the fill in the field below.
Solder Mask Expansion
Rule - select the checkbox to have the solder mask expansion for the fill follow the defined value in the applicable Solder Mask Expansion design rule. The associated expansion value will be disabled if this option is chosen.
Manual - select the checkbox to override the applicable design rule and specify the solder mask expansion value for the fill in the field below.