Board Level Annotate

Parent page: WorkspaceManager Dialogs

Summary

The Board Level Annotate dialog allows you to either name your components based on a number of Naming Schemes, Back Annotate from PCB documents to the Compiled Documents or specify custom names. Board Level Annotation is also useful if you are implementing Device Sheets in your project since Board Level Annotation is the annotation of the Compiled Documents not the source document, which in the case of Device Sheets, is read-only by default.. 

Access

Select Tools » Board Level Annotate (CTRL + L) which brings up the Board Level Annotate dialog. 

Options/Controls

Filter Options

The left hand side of the Board Level Annotate dialog allows you to control the scope of annotation at the Sheet, Channel and Part Level. The columns in the Filter Options control do not change.

• Schematic Sheet - The Schematic Sheet column lists all of the Schematic Documents in your project. A Schematic Document may be listed more than once if your design includes multiple channels.
• Channel Name - The Channel Name column lists all of the relevant channels in your design. If there are no channels in the design, this column will be populated with the Schematic Sheet name.
• Enabled - Tick the check box to include the Schematic Sheet for a specific Channel in this Board Level Annotation. Uncheck the box to exclude this sheet from Board Level Annotation.
• Annotation Scope - Choose from the following to set the scope for the parts to be annotated:
  
  • 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

• 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.

Proposed Change List

The right hand side of the Board Level Annotate dialog allows you to view Schematic Source Components (highlighted in pink), view Calculated Design Data used in the current naming scheme whether this is the default names for compiled components or the applied naming scheme, (highlighted in green), apply a Naming Scheme and view the resultant PCB Component Instance.

• Schematic Source Component - The Schematic Source Component section is made up of three columns:
• Hierarchy Path - the path of the Schematic Source, in the format Filename\Channel
• Prefix - the alphabetical prefix extracted from the Schematic Level Designator e.g if your Schematic Level Designator is R13, the Prefix is R.
• Local Index - the index you have specified following the alphabetical prefix, extracted from the Schematic Level Designator e.g if the Schematic Level Designator is R13, the Local Index is 13.

• Calculated Design Data - Upon first opening the Board Level Annotate Dialog, the Calculated Design Data section displays the Room Name column, which corresponds to the default Annotate Option selected.
  Once you have performed a Board Level Annotation, the columns displayed in the Calculated Design Data represent the keywords selected in your naming scheme for annotation in your Annotate Options. These columns are updated dynamically based on your selection. For example, if you select your Naming Scheme to be $GlobalIndex.$SheetDesignator, the columns displayed will be Global Index and Sheet Designator.
• Naming Scheme - Tick the check box to enable the Naming Scheme for this component. Uncheck the box to disable the Naming Scheme for this component. Note that when this field is unchecked, the PCB Component Instance column can be edited so you can specify a custom designator for your component.
• PCB Component Instance - The PCB Component Instance column displays the proposed designator. This field is dictated by either the Naming Scheme selected or a custom value which can only be specified when the Naming Scheme field is unchecked. The custom name can contain any combination of alphanumeric and non-alphanumeric characters.
• Annotate Options - The Annotate Options allows you to further customize your Annotation using either predefined or custom Naming Schemes.
• Annotate - Click on the Annotate drop down and choose whether you want to Annotate Undesignated, Annotate All or Annotate Selected
• Reset All - Use the Reset All button to reset all of the designators back to the default names for Compiled Components. These default names are configured in the Project Options dialog accessed through the Project menu. Once components have been reset, The Prefix column will display a component icon with a question mark  _{to show that the component is now undesignated.}
• _{Back Annotate - Click the Back Annotate button to synchronize changes from your PCB design to the Compiled Documents in the Schematic Editor. After clicking the Back Annotate button, the Choose WAS-IS File for Back-Annotation from PCB dialog appears. Choose your file for Back Annotation.
  Back Annotation for Board Level Annotation performs the same way as it does for Schematic Level Annotation.}