Applied Parameters: None
Summary
This command is used to place a Sheet Entry object within the bounds of an existing sheet symbol object on the active document. A sheet entry is an electrical design primitive that belongs within a sheet symbol (and device sheet symbol and managed sheet instance symbol). It is placed within a sheet symbol to designate input/output ports for the symbol. The sheet entries correspond to ports placed in the source schematic sub-sheet that the symbol represents.
For detailed information about this object type, see
Sheet Entry.
Access
Sheet entries are available for placement in the Schematic Editor only, by:
- Choosing Place » Add Sheet Entry from the Schematic Editor main menu.
- Clicking the
button on the Wiring toolbar.
- Right-clicking in the workspace and choosing Place » Add Sheet Entry from the context menu.
Use
After launching the command, the cursor will change to a cross-hair and you will enter sheet entry placement mode. Placement is made by performing the following sequence of actions:
- Move the sheet entry attached to the cursor over a placed sheet symbol on the sheet.
- Adjust the position of the sheet entry in relation to an edge of the sheet symbol, then click or press Enter to anchor the sheet entry to the required edge, and complete placement.
- Continue placing further sheet entries, or right-click or press Esc to exit placement mode.
The coloring of the sheet entry will aid in its correct placement. While outside of a sheet symbol, the entry will appear greyed-out, and you will be prevented from placing. When over a sheet symbol, the entry will turn blue, indicating it can validly be placed at that location. Once placed, the entry will revert to its true coloring, as defined by its Fill Color property.
While the sheet entry is still floating on the cursor, and while it is within the bounds of a sheet symbol, press the
Tab key to access the
Sheet Entry dialog, from where properties for the sheet entry can be changed on-the-fly.
Tips
- When a Sheet Entry is connected to a Signal Harness, the Sheet Entry becomes a Harness object. By default, the Sheet Entry will change color to match the color of the Signal Harness. Disable the option, Sheet Entries and Ports use Harness Color on the Schematic - Graphical Editing page of the Preferences dialog to specify your own color for Sheet Entries, or to use the default color.
- When a Sheet Entry is connected to a Harness Connector by a Signal Harness, the Harness Type in the Sheet Entry dialog is automatically populated with the Harness Type of the Harness Connector. When a Sheet Entry is connected to a Port by a Signal Harness and the Port has a Harness Type declared, the Sheet Entry will become a Harness object and change to the color of the Signal Harness. If you move the Sheet Entry away from the Harness Connector and the Harness Type field is not populated, the Sheet Entry will revert back to the default color.
- To negate (include a bar over the top of) a sheet entry name, use one of the following methods:
- Include a backslash character after each character in the name (e.g. E\N\A\B\L\E).
- 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).
- When instantiating multiple channels from the same sheet symbol, certain signals are repeated and sent individually to each instantiated channel. With respect to a sheet entry, a signal is repeated by using the Repeat keyword in the sheet entry's name (e.g. Repeat(Headphone)). The sheet entry is then wired to a bus, which in turn carries the individual signals to their correspondingly instantiated destinations.
- For information on how a placed sheet entry object can be modified graphically, directly in the workspace, see Graphical Editing.
- While attributes can be modified during placement (Tab to bring up associated properties dialog), bear in mind that these will become the default settings for further placement unless the Permanent option on the Schematic – Default Primitives 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.
Altium Designer Documentation
...
((Command Reference))_AD
((Sch Commands))_AD