Annotate

Parent page: WorkspaceManager Dialogs

The Annotate... Dialog.

Summary

The Annotate dialog allows you to systematically assign designators to all or selected parts in selected sheets of your current project, ensuring designators are unique and ordered based on their position. You can customize your annotation to package multi-part components, set Index and Suffix options, Reset Schematic Designators including any duplicate designators and Back Annotate from PCB.

Access

Use the Tools » Annotate Schematics command which brings up the Annotate dialog

Options/Controls

Order of Processing

Positional annotation is directed through the Order of Processing control. As you select one of each of the four positional annotation methods available, the graphical representation dynamically updates to illustrate how the components will be annotated.

• Across then down - In this mode, scanning will start at the top left of the schematic sheet and move left to right until all components are designated.
• Up then across - In this mode, scanning will start at the bottom left of the schematic sheet and move bottom to top until all components are designated.
• Down then across - In this mode, scanning will start at the top left of the schematic sheet and move top to bottom until all components are designated.
• Across then up - In this mode, scanning will start at the bottom left of the schematic sheet and move left to right until all components are designated.

Process Location of

• Designator - Choose Designator to process location by Designator
• Part - Choose this to process location by Part

Matching Options

• Complete Existing Packages - To configure your Matching Options, first select how you would like to Complete Existing Packages. This control lets you decide how and if parts that are not annotated will be included in existing packages. Choose from:
  • None - existing packages will not be completed and all new parts will be placed into new packages
  • Per Sheet - existing packages will only include new parts from the same Schematic Sheet
  • Whole Project - existing packages will include new parts from any of the Schematic Sheets in your project.

• Component Parameter - Select the Component Parameters to package your components by. The default settings in the Annotate dialog are to complete existing packages by Library Reference and Comment. A Component Parameter helps you identify and match multi-part components based on common properties. The parameters listed reflect all of the parameters available across the components in the design. These are defined in the Parameters region of the Component Properties dialog.
  Selecting any parameter in this column means that you will be using this parameter to match your parts into packages. If multi-part components share the enabled parameters and a common value, then they will be packaged together.
• Strictly - If the Strictly checkbox is enabled for a Component Parameter, all components must have that parameter to be matched into a package. Components that do not have this parameter are annotated as individual components and are not packaged. 

Schematic Sheets To Annotate - You can annotate the designators for all or selected Schematic Sheets within the current project. Enable or disable the checkbox before the Schematic Sheet name to include or exclude the sheets from annotation

• Schematic Sheet - Selet which schematic to annotate
• Annotation Scope - Set your Annotation Scope, choose from one of the following:
  • All - All parts in the Schematic Sheet will be annotated
  • Ignore Selected Parts - All parts except those selected will be annotated
  • Only Selected Parts - Only the parts selected will be annotated

• Order of Annotation - Configure the order in which the Schematic Sheets are to be annotated using the Order field. Type the Order directly into the field or use the arrows which appear once you click in the field to scroll to your preference.

Designator Index Control

• Start Index - Enable the Start Index checkbox and choose a numerical value to start the numbering from. For example, if you choose a Start Index
  of 100 and your first Designator is C?, it will be annotated to C100, the next C101 and so on.

Add Suffix

• Suffix - Choose a Suffix you wish to append to your designator. Alpha (A, B, C...) numerical (1, 2, 3...) and non numerical (_ * . %...) suffixes are supported including a combination of these.

Proposed Change List 

The Proposed Change List displays the effect of every annotation option selected for your design before you commit to the changes

• Current - Display the current designator of components
• Proposed - Display the proposed designator of components after annoataion
• Location of Part - Shows where the part locates

Update Changes List - Click on the Update Changes List button to load your proposed changes into this list.

Reset All - If you are re-annotating, click on the Reset All button to reset either all or duplicate designators and then click on the Update Changes List button to load your proposed changes into this list.

Back Annotate - You can Back Annotate from PCB to the Editor View (the logical Schematic design) in Schematics through the Annotate dialog using the Back Annotate button. This command updates the designators of components in the Schematic Sheets of the active project with changes made in the PCB document. These changes are applied using a WAS-IS file that is generated when re-annotating designators in the PCB environment.
The feature is useful when it is not possible to have the schematic and PCB open at the same time, for example, when they are being designed by different people in different locations. Otherwise, it is best practice to use Design » Update to push annotation changes from the PCB back to the schematic.

Accept Changes(Create ECO) - After reviewing proposed changes, click the Accept Changes (Create ECO) button. The Engineering Change Order dialog will appear, listing the proposed changes as modifications with a modification category, Annotate Component. Use this dialog to validate, report and execute the ECO, completing the Annotation Process at the Schematic level

All On - When pressed, the All On button ticks the Enabled checkbox for all Schematic Sheets in the project, including them in annotation.

All Off - The All Off button disables the Enabled checkbox for all Schematic Sheets in the project, excluding them from annotation