Search In: Doc:Documentation: Altium Designer
Altium DesignerAltium 365Altium MCAD CoDesignerAltium On-Prem Enterprise ServerAltium CircuitMakerAltium CircuitStudioCompany DashboardAltium Infrastructure Server
Ver: Version: 22.0
17.117.016.116.015.1
Close
Search Search on Documentation
Documentation Altium Designer Documentation ... Dialog Reference S to Z

Sheet Symbol

Created: June 08, 2017 | Updated: June 18, 2017 | Applies to version: 17.1
Now reading version 22.0. For the latest, read: Sheet Symbol for version 17.1


The Properties tab of the Sheet Symbol dialog.

Summary

This dialog allows the designer to specify the properties of a Sheet Symbol object. A sheet symbol is an electrical design primitive. It is used to represent a sub-sheet in a multi-sheet hierarchical design. Sheet symbols include sheet entries, which provide a connection point for signals between the parent and child sheets, similar to the way that Ports provide connections between sheets in a flat-sheet design.

For information on how a placed sheet symbol object can be modified graphically, directly in the workspace, see the Graphical Editing section of the Sheet Symbol object page.

Access

The Sheet Symbol dialog can be accessed during placement by pressing the Tab key.

After placement, the dialog can be accessed in one of the following ways:

  • Double-clicking on the placed sheet symbol object.
  • Placing the cursor over the sheet symbol object, right-clicking, and choosing Properties from the context menu.

Properties Tab


Sheet Symbol dialog - Properties tab.

Use the dialog's Properties tab to modify graphical properties of the sheet symbol object.

Options/Controls

  • Location - the current X (horizontal) and Y (vertical) coordinates for the top-left corner of the sheet symbol (X is the top value, Y is the bottom value). Edit these values to change the position of the sheet symbol in the horizontal and/or vertical planes respectively.
  • X-Size - the current length of the sheet symbol in the horizontal plane.
  • Y-Size - the current length of the sheet symbol in the vertical plane.
  • Border Color - click the color sample to change the border color for the sheet symbol, using the standard Choose Color dialog.
  • Draw Solid - if this option is enabled, the sheet symbol is filled with the color set in the Fill Color field. If this option is disabled, the sheet symbol is drawn in outline only.
  • Fill Color - click the color sample to change the fill color for the sheet symbol, using the standard Choose Color dialog. The Draw Solid option must be enabled for the sheet symbol to be filled.
  • Border Width - the width of the border used to draw the outline of the rectangular shape. Available widths are: Smallest, Small, Medium, and Large.

Properties

  • Designator - the current name for the sheet symbol. This field is used to provide the sheet symbol with a meaningful name that will distinguish it from other sheet symbols placed on the same schematic sheet. Typically the name will reflect the overall function of the schematic sub-sheet that the symbol represents.
  • Filename - the current schematic document referenced by the symbol. It is this field that provides the link between the sheet symbol and the schematic sub-sheet that the symbol represents. Either enter the name of the target schematic sheet directly in the field, or click the  button to the right, to access the Choose Document to Reference dialog. This dialog presents a listing of all source schematic sheets in the project (with the exception of the sheet upon which the symbol is currently placed). Use it to choose the required target sub-sheet.
Multiple sub-sheets may be referenced by a single sheet symbol. Separate each filename by a semi-colon in the Filename field. With the effective use of off-sheet connectors placed on the sub-sheets, you can effectively spread a section of your design over multiple sheets, treated as though they were one giant (flat) sheet. Note, however, that use of off-sheet connectors is only possible for sheets referenced by the same sheet symbol.
  • Unique Id - the current unique identifier for the sheet symbol. The Unique ID (UID) is a system generated value that uniquely identifies this current sheet symbol. A new UID value can be entered directly into this field.
    • Reset - click this button to have the system generate a new UID for the sheet symbol.
  • Show Hidden Text Fields - enable this option to reveal any text fields associated with the sheet symbol (designator, filename, parameters) that have been hidden.
  • Locked - enable this option to protect the sheet symbol from being edited graphically.
An object that has its Locked property enabled cannot be selected or graphically edited. Double click on the locked object directly and disable the Locked property, to graphically edit the object.

Parameters Tab


Sheet Symbol dialog - Parameters tab.

Use the dialog's Parameters tab to manage parameters attached to the currently selected sheet symbol object. You can also add rule-based parameters.

Adding a parameter (as a rule) to a sheet symbol on the schematic results in a PCB design rule being generated - when the design is transferred to the PCB document - with a scope that targets a Component Class, the members of which are the components on the sheet referenced by the sheet symbol.

Options/Controls

  • Parameters Grid - the main region of the tab lists all of the parameters currently defined for the sheet symbol, in terms of:
    • Visible - use this option to determine the visibility of the parameter's value in the workspace. Note that this does not relate to the visibility of the parameter's Name, which can be determined, for a standard (non-rule) parameter only, in the Parameter Properties dialog.
    • Name - the name of the parameter. For a rule-type parameter, this entry will be locked as Rule.
    • Value - the value of the parameter. For a rule-type parameter, the entry will reflect the rule type, along with a listing of its defined constraints.
    • Type - the type of parameter, which determines the valid entries that can be used for its value. Available types are: STRING, BOOLEAN, INTEGER, and FLOAT. For a rule-type parameter, this entry is always STRING.
A standard parameter (non-rule) can be modified with respect to any of these attributes directly in the grid. However, attempting to change a locked Name and/or Value attribute will raise an error and you will need to press Esc to abandon such changes.
A parameter added as a rule can not be edited directly in the grid with respect to its Name, Value, or Type. Its Name and Type are set to Rule and STRING respectively and are always uneditable. Its Value can only be edited by changing the constraints of the rule. To do this, select and edit the parameter, and click the Edit Rules Button in the Parameter Properties dialog. This will give access to the Edit PCB Rule (From Schematic) dialog, from where the changes to the constraints can be made.
  • Add - click this button to add a new parameter to the list. The Parameter Properties dialog will appear. Use this to define the parameter, especially its Name, Value, Type, and whether or not it's value is to be visible in the workspace.
  • Remove - click this button to delete the selected parameter(s) from the list of parameters.
  • Edit - click this button to modify the currently selected parameter. The Parameter Properties dialog will appear, with which to do so.
  • Add as Rule - click this button to add a new design rule directive parameter to the list. The Parameter Properties dialog will appear, but this time will contain the Edit Rule Values button, which in turn gives access to the Choose Design Rule Type dialog, from where you can choose, and subsequently define, the constraints of the required rule type.

Right-Click Menu

The Parameters Grid right-click menu offers the following commands:

  • All On - use this command to quickly enable the Visible option for all parameters in the list.
  • All Off - use this command to quickly disable the Visible option for all parameters in the list.
  • Selected On - use this command to quickly enable the Visible option for all currently selected parameters in the list.
  • Selected Off - use this command to quickly disable the Visible option for all currently selected parameters in the list.
  • Add - use this command to add a new standard (non-rule) parameter to the list.
  • Remove - use this command to remove the currently selected parameter(s) in the list.
  • Edit - use this command to edit the currently selected parameter in the list.
  • Select All - use this command to quickly select all parameters in the list.
  • Select None - use this command to quickly deselect all parameters in the list.
If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.
Note

The features available depend on your Altium product access level. Compare features included in the various levels of Altium Designer Software Subscription and functionality delivered through applications provided by the Altium 365 platform.

If you don’t see a discussed feature in your software, contact Altium Sales to find out more.