Numbering Your Schematic Sheets in Altium Designer

Numbering schematic sheets in a project allows you to take control of the sheet designation and store them as parameters within the respective schematic documents. The special string feature (=SheetNumber, =DocumentNumber, =SheetTotal) can then be used to display these values on the sheet (in the sheet's title block, for example) as text objects. The numbering does not alter component designators but rather schematic sheet designators (numbers) and is, therefore, related to the general concept of design annotation.

Sheet Numbering

Sheet numbering is accessed by clicking Tools » Annotation » Number Schematic Sheets from the main menus to open the Sheet Numbering For Project dialog.

Use the Sheet Numbering For Project dialog to number and organize the schematic sheets in a project.
Use the Sheet Numbering For Project dialog to number and organize the schematic sheets in a project.

Schematic Sheet Numbering and Device Sheets

Sheet or Document Numbers cannot be configured for Device Sheets when they are read-only (the default state). In the Sheet Numbering For Project dialog, they will be cross-hatched to indicate they cannot be updated, as shown in the image below. When Device Sheets are set as editable, the cross-hatching is removed, and numbering can be configured as usual.

Automatic Sheet Numbering

The automatic sheet numbering feature can be enabled/disabled using the Automatic Sheet Numbering option on the Options tab of the Project Options dialog and the Automatic Sheet Numbering (Project Option) option in the Sheet Numbering For Project dialog. The option needs to be enabled only in one of the dialogs for automatic sheet numbering to occur. If the option is disabled in both dialogs, the sheets can be manually numbered. 

If one of the above-mentioned options is enabled, automatic sheet numbering can be applied to schematic sheets directly in the Projects panel. To change the numbering, drag and drop schematic sheets in the panel. The sheet numbering is displayed to the left of the schematic sheet name.

Annotating Compiled Sheets

Annotating compiled sheets allows you to take control over how compiled sheets (physical instances of a sheet) are numbered, similar to the way Sheet Numbering controls how logical sheets are numbered.

For example, consider a design that includes a schematic document called Input channel.SchDoc. The circuitry in that sheet is used eight times within the design so after design compilation, the Input channel.SchDoc will be instantiated eight times (i.e., once for each instance of the circuitry on the physical PCB). Sheet numbering is used to number the Input channel.SchDoc sheet within the logical structure of the design; annotating compiled sheets is done to number the individual instances of that sheet in the physical (compiled) view of the design.

Annotating compiled sheets is accomplished in the Annotate Compiled Sheets dialog, which is accessed by selecting the Tools » Annotation » Annotate Compiled Sheets command from the main menus.

The dialog lists all compiled sheets of the current project. You can create custom names for your compiled sheets by typing directly into the Sheet Number field. Use any combination of characters (alphanumeric or non-alphanumeric), and then click OK to implement your custom annotation.

Click the Annotate Sheet button to annotate the sheet(s) after selecting the options accessed by clicking the associated down arrow. (Refer to the Sheet Numbering section for field descriptions, if needed.) The SheetNumber will be updated to match your selections.

Sheet numbers updated by the dialog are stored in the project's *.Annotation file under the Settings\Annotation Documents subfolder in the Projects panel. This ensures that annotation information and settings are remembered across project editing sessions.

The Annotate Compiled Sheets dialog treats Device Sheets like any other sheet in the design project and annotates them according to the Annotation options.
The Sheet Number allocated by the Annotate Compiled Sheets dialog can be referenced on printed outputs of the compiled (Physical) sheet using the =SheetNumber special string. This will then be updated in any printed outputs of the design.

Using Compiled Sheet Annotation in Board Level Annotation

Once the compiled sheets have been annotated through the Annotate Compiled Sheets dialog, the $SheetNumber keyword can be used as part of the Naming Scheme in the Board Level Annotation Options dialog. If the project's compiled sheets have not yet been annotated, the sheet numbering defined in the Sheet Numbering For Project dialog will be used by default.

For more information about Board Level Annotation, see the Board Level Annotation page.

Using Compiled Sheet Annotation in a Project

Once you have annotated your compiled sheets, you can place the SheetNumber special string in your project to reference this information.

  • The special string is always displayed; if null, then the parameter name is displayed. 

  • Place a special string where the value =SheetNumber to use your Compiled Sheet Annotation values. You can use special strings in the values of parameter properties, text strings, net labels, etc.

  • The Sheet Number allocated by the dialog can be referenced on printed outputs of the compiled (Physical) sheet using the =SheetNumber special string. This will then be updated in any printed outputs of the design.

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.

Content