Sch_Cmd-PlacePortPlacePort_AD

Applied Parameters: None

Summary

This command is used to place a Port object onto the active document. A port is an electrical design primitive. It is used to make an electrical connection between one schematic sheet and another sheet, or sheet symbol (through a corresponding sheet entry), in a design using multiple sheets (both flat and hierarchical designs). The name of the port defines the connection (i.e. a port on a schematic sheet connects to ports or sheet entries with the same name on other sheets in the project).

Access

Ports are available for placement in the Schematic Editor only, by:

• Choosing Place » Port from the Schematic Editor main menu.
• Locating and using the Port command () on the Active Bar.

• Clicking the  button on the Wiring toolbar.
• Right-clicking in the workspace and choosing Place » Port from the context menu.

Use

After launching the command, the cursor will change to a cross-hair and you will enter port placement mode. Placement is made by performing the following sequence of actions:

• Click or press Enter to anchor the left-hand edge of the port.
• Move the cursor to adjust the length of the port as required, then click or press Enter to complete placement of the port.
• Continue placing further ports or right-click or press Esc to exit placement mode.

Additional actions that can be performed during placement - while the port is still floating on the cursor, and before its left-hand edge is anchored - are:

• Press the Alt key to constrain the direction of movement to the horizontal or vertical axis, depending on the initial direction of movement.
• Press the Spacebar to rotate the port counterclockwise or Shift+Spacebar for clockwise rotation. Rotation is in steps of 90°.
• Press the X or Y keys to mirror the port along the X-axis or Y-axis respectively.

Tips

1. When compiling a schematic or generating a netlist, the relationship between ports and sheet symbols is determined by the Net Identifier Scope chosen for the project. This scope is defined by setting the Net Identifier Scope option, on the Options tab of the Options for Project dialog (Project » Project Options). When set to Flat or Global, all ports with the same name, within the same or different schematic documents, are considered to be electrically connected. When set to Hierarchical or Strict Hierarchical, ports only connect vertically to their corresponding sheet entries. They do not connect horizontally to other ports of the same name.
2. The I/O Type field in the Properties panel allows you to define the port's electrical type. Choose from either Input, Output, Bidirectional, or Unspecified.
3. To negate (include a bar over the top of) a port name, use one of the following methods:
   1. Include a backslash character after each character in the name (e.g. E\N\A\B\L\E).
   2. Enable the Single '\' Negation option on the Schematic - Graphical Editing page of the Preferences dialog, then include one backslash character at the start of the name (e.g. \ENABLE).
4. Port names are not used for naming nets. This means a system-generated net name will be used if no net label or power object is associated with that net.
5. When a Port is connected to a Signal Harness, the Port becomes a Harness object. By default, the Port will change color to match the color of the Signal Harness.
6. By default, the font used for the port's Name follows the global document-level font. This is set using the Document Font field, in the General section of the Properties panel (when no object is selected). This can be overridden at the individual port-level, using the control below the port's Name field (again, edited through the Properties panel) - allowing you to fully control the textual presentation of ports as needed.
7. For information on how a placed port object can be modified graphically, directly in the workspace, see Graphical Editing.
8. While attributes can be modified during placement (Tab to bring up the Properties panel), bear in mind that these will become the default settings for further placement unless the Permanent option on the Schematic - Defaults page of the Preferences dialog is enabled. When this option is enabled, changes made will affect only the object being placed and subsequent objects placed during the same placement session.