Altium NEXUS Documentation

PlaceSheetEntry

Modified by Susan Riege on Feb 6, 2019

Parent page: Schematic Commands

The following pre-packaged resource, derived from this base command, is available:


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. 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 » Sheet Entry from the Schematic Editor main menu.
  • Locating and using the Sheet Entry command () on the Active Bar.
If the command has been recently used from the Active Bar, it will become the active/visible button. Where other commands are available, this is indicated by a triangle at the bottom-right corner of the button. Click and hold on the active button to access a menu of all associated commands for that grouping.
  • Clicking the  button on the Wiring toolbar.
  • Right-clicking in the workspace and choosing Place » 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:

  1. Move the sheet entry attached to the cursor over a placed sheet symbol on the schematic document.
  2. 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.
  3. 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 grayed-out and you will be prevented from placing it. 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, press the Tab key to access the Properties panel from where properties for the sheet entry can be changed on-the-fly. Pressing Tab pauses placement, allowing you to interact with the panel (or other area of the software) directly. To resume, click the pause symbol that appears over the workspace.

Tips

  1. 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.
  2. To negate (include a bar over the top of) a sheet entry 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).
  3. 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.
  4. For information on how a placed sheet entry object can be modified graphically directly in the workspace, see Graphical Editing.
  5. While attributes can be modified during placement (Tab to open the Properties panel), keep 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.

 

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
You are reporting an issue with the following selected text
and/or image within the active document:
ALTIUM DESIGNER FREE TRIAL
Altium Designer Free Trial
Let’s get started. First off, are you or your organization already using Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

In that case, why do you need an evaluation license?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You actually don’t need an evaluation license for that.

Click the button below to download the latest Altium Designer installer.

Download Altium Designer Installer

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Please fill out the form below to get a quote for a new seat of Altium Designer.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

If you are on Altium Subscription, you don’t need an evaluation license.

If you are not an active Altium Subscription member, please fill out the form below to get your free trial.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Why are you looking to evaluate Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

You came to the right place! Please fill out the form below to get your free trial started.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Great News!

Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

That’s great! Making things is awesome. We have the perfect program for you.

Upverter is a free community-driven platform designed specifically to meet the needs of makers like you.

Click here to give it a try!

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.