Backward Annotation

The Backward Annotation command allows you to add relevant changes in a specified PCB design to the current design in eCADSTAR Schematic Editor. The Design Library is updated. It also allows you to specify that any pending changes for the current design are ignored by eCADSTAR Schematic Editor. The results of the command are displayed in the Output panel. Launch the Backward Annotation command by clicking Design > Design Changes > Backward Annotation on the eCADSTAR Schematic Editor ribbon.

Dialog

Item		Description
PCB design		Displays the PCB design data file that you want to back annotate into eCADSTAR Schematic Editor. This is selected by clicking the button, and browsing to it in the displayed Open dialog. The specified design must be closed before you click OK.
		Displays the Open dialog. In the dialog, browse to a design data file (.pdes) and click Open. The specified PCB design file is back annotated to the current design in eCADSTAR Schematic Editor.
Update the association of the PCB design and the schematic		Allows you to link the current schematic design with the PCB design that you specify in the PCB design box. The specified PCB design is automatically displayed in the PCB design box when you execute the Backward Annotation command. By deselecting this box, you can execute the Backward Annotation command for a different PCB design, without updating this link.
	Selected	The PCB design displayed in the PCB design box is linked to the current schematic design. The specified PCB design is automatically displayed when you execute the Backward Annotation command. To link to another PCB design, click the button and browse to a different .pdes file. The specified file is automatically displayed when you next execute the Backward Annotation command.
	Not selected	Allows you to execute the Backward Annotation command for the PCB design that is displayed in the PCB design box, without creating a link to the specified design. The next time you to execute the Backward Annotation command, the linked PCB design is displayed.
Update schematic		Allows you to update the current schematic design with any relevant changes in the PCB design that is specified in the PCB design box. If both Update schematic and Clear Back Annotation Information from PCB are selected, then the schematic design is automatically saved after the back annotation is completed.
	Selected	When you execute the Backward Annotation command, any relevant changes in the specified PCB design are added to the current schematic design. The fields in the Schematic Sheet for the Placement of Added Parts and Connectivity sections are made available.
	Not selected	Allows you to execute the Backward Annotation command without adding relevant changes in the specified PCB design to the current schematic design. If this box is not selected, then you must specify that these changes are permanently ignored by eCADSTAR Schematic Editor after you execute the Backward Annotation command. This is done by selecting the Clear Back Annotation Information from PCB box. Before deselecting this box, either ensure that relevant changes have already been back annotated, and the current design has been saved, or that you want eCADSTAR Schematic Editor to permanently ignore relevant changes in the PCB design. You cannot execute the Backward Annotation command unless the Clear Back Annotation Information from PCB box is selected.
Schematic sheet for the placement of added parts		Allows you to specify the sheet in the current schematic design where parts are placed that have been added to the specified PCB design. You can select any sheet in the current schematic design.
	Specified sheet	Allows you to specify the sheet in the current schematic design where parts are placed that have been added to the specified PCB design. You can select any sheet in the top level circuit. Sheets in embedded circuits cannot be selected.
Distance between components		Allows you to specify the distance between connected components when parts and gates are added or removed, and when changes are made to connected components.
	X Offset	Allows you to specify the distance between connected components in the X direction.
	Y Offset	Allows you to specify the distance between connected components in the Y direction.
Connectivity		Allows you to specify the details for connected components when parts and gates are added or removed, and when changes to connected components are updated.
	Net length connected to added parts	Allows you to specify the maximum length of the net that connects to an added component.
	Global Symbol for signal nets	For components that are added to eCADSTAR Schematic Editor when you back annotate, the symbol name and symbol alternate is displayed for signal nets that are connected to the component's pins (the symbol alternate is shown in brackets). Click to specify these values in the Global Symbol for Signal Nets dialog.
		Displays the Global Symbol for Signal Nets dialog. This dialog allows you to specify the symbol name and symbol alternate for signal nets that are connected to the pins of added components.
	Global symbol for power nets	For components that are added to eCADSTAR Schematic Editor when you back annotate, the symbol name and symbol alternate is displayed for power nets that are connected to the component's pins (the symbol alternate is shown in brackets). Click to specify these values in the Global Symbol for Power Nets dialog.
		Displays the Global Symbol for Power Nets dialog. This dialog allows you to specify the symbol name and symbol alternate for power nets that are connected to the pins of added components.
	Global symbol for ground nets	For components that are added to eCADSTAR Schematic Editor when you back annotate, the symbol name and symbol alternate is displayed for ground nets that are connected to the component's pins (the symbol alternate is shown in brackets). Click to specify these values in the Global Symbol for Ground Nets dialog.
		Displays the Global Symbol for Ground Nets dialog. This dialog allows you to specify the symbol name and symbol alternate for ground nets that are connected to the pins of added components.
Use net color from PCB		Allows you to specify whether the net colors that are defined in the specified PCB are used in the eCADSTAR Schematic Editor. Define these colors in the Constraint Browser: Signals Section, Signals Tab or Constraint Browser: Signals Section, Classes/Groups tab. These are defined in the Color column in the Basic tab.
Clear Back Annotation information from PCB		Allows you to specify that any relevant changes in the PCB design that is specified in the PCB design box are permanently ignored by eCADSTAR Schematic Editor after you execute the Backward Annotation command. If the Update schematic box is not selected, then you must select this box or you cannot execute the Backward Annotation command. If both Update schematic and Clear Back Annotation Information from PCB are selected, then the schematic design is automatically saved after the back annotation is completed.
	Selected	Any relevant changes in the PCB design that is specified in the PCB design box are permanently ignored by eCADSTAR Schematic Editor after you execute the Backward Annotation command. You must close the relevant design in eCADSTAR PCB Editor before you execute the Backward Annotation command. If you do not close the design, then back annotation is not executed, and the following message is displayed in the Error tab, in the Output panel: "Cannot open PC board database file". If the Update schematic box deselected, then ensure that either the relevant changes have already been back annotated, and the current design has been saved, or that you want eCADSTAR Schematic Editor to permanently ignore the relevant changes in the PCB design.
	Not selected	Executing the Backward Annotation command with this setting deselected allows you to view the effects of the command, and re-execute it if necessary. Any relevant changes in the PCB design that is specified in the PCB design box remain at "pending" status. If you save the schematic design after executing the Backward Annotation command with Update schematic selected, then you must execute the command again with the Update schematic box deselected, and the Clear Back Annotation Information from PCB box selected. This must be done before you make any changes to the PCB design.
OK		Displays a confirmation dialog that lists the options that you specify in the Backward Annotation dialog. If you click OK in the dialog, backward annotation is executed for the current schematic design. Relevant changes in the specified PCB design are added to the schematic design. If Clear Back Annotation Information from PCB is selected, then any pending changes for the current design are permanently ignored by eCADSTAR Schematic Editor after back annotation is completed. The results of the Backward Annotation command are displayed in the Output panel.
Cancel		Closes the Backward Annotation dialog without adding changes in the specified PCB design to the current design in eCADSTAR Schematic Editor.