This tab of the Project Options dialog enables you to specify the output path and related options for generated outputs for the project. You can also specify various netlisting options and the Net Identifier Scope.
This is one of the multiple tabs available when configuring the options for a project accessed from within the Project Options dialog. To access this dialog:
*.SchDoc) for the project.
<FolderName> Date Timewhere the
<FolderName>is specified in the Output Path field and
Timeare in the same format as your system settings.
Append Sheet Numbers to Local Net – enable to append the value for a schematic document's Sheet Number parameter (a document-level parameter) to nets that are local to that sheet. A local net is a net that does not leave the sheet. For a net that does leave the sheet (and is therefore not local), this option does not apply.
Power Port Names Take Priority – the software has the ability to localize a global power net by wiring a power port to a normal port. This would force all pins on that sheet connected to that power port to be in a separate net. Enabling this option would force net naming using the name of the net assigned to the power port.
Multi-sheet designs are defined at the electrical (or connective) level by Net Identifiers. Net identifiers (net labels, ports, sheet entries, power ports, and hidden pins) create logical connections between points in the same net. This can be within a sheet or across multiple sheets. Physical connections exist when one object is attached directly to another electrical object by a wire. Logical connections are created when two net identifiers of the same type (e.g., two net labels) have the same Net property.
When the connectivity model of the design is created, you must define how you want net identifiers to connect to each other – this is known as setting the Net Identifier Scope. There are essentially two ways of connecting sheets in a multi-sheet design: either horizontally, directly from one sheet to another sheet to another sheet, etc., or vertically, from a sub-sheet to the sheet symbol that represents it on the parent sheet. In horizontal connectivity, the connections are from port to port (net label to net label is also available). In vertical connectivity, the connections are from sheet entry to port.
Use the drop-down list to choose from the following scopes:
Automatic (Based on project contents) – this mode automatically selects which of the net identifier modes to use based on the following criteria: if there are sheet entries on the top sheet, then Hierarchical is used; if there are no sheet entries, but there are ports present, then Flat is used; if there are no sheet entries and no ports, then Global is used.
In the PCB editor, Pin, Differential Pair and Part swaps are performed by exchanging nets on component pads and their corresponding copper. When the changes are merged into the schematics, there are two ways that a pin swap can be handled:
Adding / Removing Net-Labels – enable to allow swapping of pins on a component symbol. Performing the swap on the schematic by swapping net labels can only be done if the connectivity is established through the net labels, i.e. if the pins are not hardwired together.
Changing Schematic Pins – enable to allow swapping of net labels on the wires attached to the pins of a component. Swapping Pins will be the only option available when nets have been physically hardwired to a component. This method can be used on simple components (such as a resistor array) or where there is no alternative because of the structure of the schematic design.
Automatic Cross References – enable this option to automatically add port and off sheet connectors cross-referencing information to all source schematic documents in the active project. This feature helps trace net connectivity in a non-hierarchical design.
Sheet Style – choose one of the following sheet styles for the cross referencing of ports on a schematic sheet or schematic sheets within a project.
None– no sheet style is added in the cross reference string of all ports.
Name– names of the sheets that the ports are linked to are added in the cross reference strings.
Number– the sheet numbers of the sheets that the ports are linked to are added in the cross reference strings.
Location Style – choose one of the following location styles for the cross referencing of ports on a schematic sheet or schematic sheets within a project.
None– no location style is added in the cross reference string of all ports.
Zone– the reference zone numbering (the sheet borders have the zones) is added in the cross reference strings of all ports that are associated with the parent objects such as the location of sheet symbols.
Location X,Y– the locations of the ports are published in brackets in the cross reference strings for all ports that are associated with the parent objects such as the location of sheet symbols.