Setting Up a Schematic Document

The options in this section of the panel determine which schematic objects may be selected in the design space.

• All - On button – select to remove object filtering so that all types of objects may be selected.
• Object buttons – toggle each object button to enable/disable the ability to select that object type.

• Units – select the desired unit. Choose either mm or mils.

  You can quickly verify the active units from the Status Bar, by looking at the Grid entry at the left-hand end of the bar.
  To toggle between the use of mils and mm measurement units for the active schematic sheet, you can also use the View » Toggle Units command from the main menus.
• Visible Grid – enter the desired grid. Use the or to show/hide the grid in the design space.
• Snap Grid – check the box to enable snap grids. Enter the desired grid in the text box or use the G shortcut to cycle through the different grids.
  • Snap to Electrical Object Hotspots – enable to use the snap grid to snap to an object's electrical hotspots or use the Shift+E shortcut.
• Snap Distance – when the cursor is within this distance from an enabled object snap point (and snapping is enabled for the active layer), the cursor will snap to that point.
• Document Font – set the font size, style and any additional font attributes that will be used for the text associated with all objects in the document sheet. For any given object, the font settings may be overridden in its corresponding Properties panel mode, which is enabled when that object is selected.
• Sheet Border – check the box to enable a sheet border then click the colored box to change the border color.
• Sheet Color – click the colored box to change the sheet color.

• Formatting and Size
  • Template mode – set the page size and format by selecting from a range of predefined schematic sheet templates. A schematic template is a document that holds user-defined sheet size, border and title block descriptions that can be referenced by (linked to) a schematic sheet negating the need to define these common attributes again and again. The list includes local and Workspace templates found in the location specified in the Data Management – Templates page of the Preferences dialog. Note that a default schematic sheet to be used for new schematic documents can be defined in the System – New Document Defaults page of the Preferences dialog.

    • Template – use the drop-down menu to select from a list of Workspace and local templates, and if required, use the button (or the Design » Templates »  Update Current Template command from the main menus) to refresh the template that may have had its information changed in some way. You can also use the Design » Sheet Templates » Local and Design » Sheet Templates » Server sub-menus from the main menus to select a template.

      After selecting a template (or refreshing the current template), the Update Template dialog opens in which you can update to the current template then an Information dialog opens displaying that the template was updated.

      To remove the current schematic template used, choose the Design » Templates » Remove Current Template command from the main menus. After launching the command, the Remove Template Graphics dialog will open. Use this dialog to define from which documents the current template will be removed - either the current document only, all schematic documents in the current (active) project, or all open schematic documents. After using this command, the entry for the currently used template will be blank.

      When removing the current template from all schematic documents in the current project, all documents that are currently closed will be opened as the removal is performed. When removing the current template from all open schematic documents, it is removed regardless of the project to which a document belongs.

      In addition, a Schematic Template Item can be used as a configuration data item in one or more defined Environment Configurations. When connected to the Workspace and using an environment configuration that does not control the use of schematic templates, you are free to manually choose a revision of a schematic template. To do so, use the Design » Sheet Templates » Set Template from server command. This presents the Choose Template dialog, from where you can browse to, and select the required template in the Workspace.

      For more information, see Environment Configuration Management (Altium 365 Workspace, Enterprise Server Workspace).

    • Width/Height – the dimensions of the current page size shown in the current document units (see the General section above).
  • Standard mode – set the sheet size to a standard page format.
    • Sheet Size – use the drop-down menu to select from a list of standard page dimensions.
    • Width/Height – the dimensions of the current page size in the current document units.
    • Orientation – use the drop-down to select the desired orientation.
    • Title Block – enable this option to display one of two predefined title blocks on the schematic sheet. Use the associated drop-down to choose from either a Standard or ANSI title block style.
  • Custom mode – set the sheet size to specified custom dimensions.
    • Width – enter the required sheet width measurement.
    • Height – enter the required sheet height measurement.
    • Orientation – use the drop-down to select the desired orientation.
    • Title Block – enable this option to display one of two predefined title blocks on the schematic sheet. Use the associated drop-down field to choose from either a Standard or ANSI title block style.
• Margin and Zones – defines the size of the sheet border graphics and its zone divisions. Uncheck the Show Zones box to hide the zone divisions in the border graphics.
  • Vertical – set the number of divisions (rows) in the vertical sheet margin. The alpha-numeric zone labeling type is defined by the Origin setting.
  • Horizontal – set the number of divisions (columns) in the horizontal sheet margin.
  • Origin – sets which corner of the document sheet(s) the perimeter zone alpha-numeric indicators will begin from (zone position A-1 or 1-A).
  • Margin Width – set the distance (in the current units) between the page edge and each of the four border lines as indicated by the arrows associated with each entry field.

The Properties panel Parameters tab lists all available Parameters and Rules available in the current project document.

• All button – select to view both Parameters and Rules.
• Parameters button – select to only view Parameters.
• Rules button – select to only view Rules.
• Parameters
  • Name and Value columns – lists the available parameters grouped by type.

• Rules
  • Name and Value columns – these list the current specified rules and their values.
• Add – use the drop-down menu to select to add a Parameter or a Rule. Selecting to add a new Rule will open the Choose Design Rule Type dialog to specify the type of rule to be used when adding a parameter as a rule to a supported design object in the schematic domain or a schematic document.
• – only accessible when a rule is selected. Click to open the Edit PCB Rule dialog to edit the selected rule.
• – click to delete the currently selected parameter or rule.