The Forward Annotation dialog allows you to execute forward annotation in eCADSTAR PCB Editor using a specified schematic design or RINF netlist (2D View mode only). It is launched by clicking Design > Design Changes > Forward Annotation on the ribbon.
Note
SPICE properties and pin assignments are not added to eCADSTAR PCB Editor when you execute the Forward Annotation command.
SPICE properties and pin assignments are not added to eCADSTAR PCB Editor when you execute the Forward Annotation command.
Command dialog
Schematic design
If selected, then you can specify the schematic design that is forward annotated to the current design in eCADSTAR PCB Editor. You can also specify the options that are applied in eCADSTAR PCB Editor.
| Value | Description | |
|---|---|---|
| Schematic box | Displays the schematic design that you want to forward annotate
to the current design in eCADSTAR PCB Editor.
Click  to select the required .sdes
file in the Open dialog.
Note Part data is provided by the schematic design, rather than the master library. Forward annotating from the schematic design and its associated library improves portability, as access to the master parts library is not required. |
|
|
|
Browse to a schematic design in the displayed Open dialog. The design that you specify is forward annotated to the current design in eCADSTAR PCB Editor. | |
| Update the association of the PCB design and the schematic | Allows you to link the current PCB design with the schematic design that you specify in the Schematic box. The specified schematic design is automatically displayed in the Schematic box when you execute the Forward Annotation command. By deselecting this box, you can execute the command for a different schematic design, without updating this link. | |
| Selected | The schematic design displayed in the Schematic
box is linked to the current PCB design. The specified
schematic design is automatically displayed when you execute the
Forward Annotation command.
To link to another schematic design, click the
button and browse to a different .sdes file.
The specified file is automatically displayed when you next execute
this command. |
|
| Not selected | Allows you to execute the Forward Annotation command for the schematic design that is displayed in the Schematic box, without creating a link to the specified design. The next time you to execute this command, the linked schematic design is displayed. | |
| Sheet range | Specify the start and end sheets in the schematic that you select in the Schematic box. The data in the specified schematic sheets is forward annotated to the current design in eCADSTAR PCB Editor. | |
| Customize variant component suffix | If a variant part has different footprints for each variant, then a new reference designator is created for each variant when the design is forward annotated. This setting allows you to specify the suffix for this reference designator. If selected, then you can customize the suffix that is added
to variant components in the specified schematic design file.
The Suffix of variant component
field is made available.
Note A license is required to access the variation functionality in eCADSTAR. |
|
| Selected | The Suffix of variant component box is made available. This allows you to customize the suffix that is added to variant components in the specified schematic design file. | |
| Not selected |
The Suffix of variant component box is made unavailable. |
|
| Suffix of variant component | Allows you to customize the suffix that is added to variant
components in the specified schematic design file. This field
is made available if Customize variant
component suffix is selected. If you do not enter a value
in this box, or Customize variant component
suffix is not selected, then variant components are displayed
as follows: [Variant]_1 [Variant]_2 [Variant]_3 If you enter an alphanumeric value in this box, then it is added before the existing suffix. For example, if you of enter a value of "X", then the names of the variant components are updated as follows: [Variant]_X1 [Variant]_X2 [Variant]_X3 |
|
| Load Clearance Class rules from schematic | Allows you to load the clearance classes into eCADSTAR PCB Editor that you specify in the Clearance Class Manager dialog in eCADSTAR Schematic Editor. | |
| Selected | The clearance classes are loaded into eCADSTAR PCB Editor that you specify in the Clearance Class Manager dialog in eCADSTAR Schematic Editor. | |
| Not selected | The clearance classes are not loaded into eCADSTAR PCB Editor that you specify in the Clearance Class Manager dialog in eCADSTAR Schematic Editor. | |
| Keep temporary track and jumper | Allows you to specify whether tracks that do not have a net defined ("no net" tracks), and jumpers are kept when you execute the Forward Annotation command in eCADSTAR PCB Editor. The setting that you specify is saved in the Forward Annotation dialog until eCADSTAR PCB Editor is restarted. | |
| Selected | Tracks that do not have a net defined, and jumpers are kept when you execute the Forward Annotation command. | |
| Not selected | Tracks that do not have a net defined, and jumpers are removed when you execute the Forward Annotation command. | |
| Use net color from schematic | Allows you to specify whether the net colors that are defined in the specified schematic are used in eCADSTAR PCB 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 Net Color in PCB column in the Basic tab. The setting that you specify is saved in the Forward Annotation dialog until eCADSTAR PCB Editor is restarted. | |
| Selected | If selected, the net colors that are defined in the specified schematic are used in eCADSTAR PCB Editor. | |
| Not selected | If selected, the net colors that are defined in the specified schematic are not used in eCADSTAR PCB Editor. |
Note
- If there are changes in the PCB design that have not been back annotated into the associated schematic design, then a confirmation dialog is displayed.
- To clear this information from the PCB design, click Yes in this dialog.
- To end the Forward Annotation command without executing forward annotation, click No.
- To apply these changes to the associated schematic design, execute the Back Annotation command in eCADSTAR Schematic Editor.
- If multiple users are working concurrently on a schematic design, then the Forward Annotation command cannot be executed.
- Changes to user-defined attributes in the specified schematic design are added to the current design in eCADSTAR PCB Editor. User-defined attributes are specified in the Attribute Manager dialog, in eCADSTAR Library Editor. The relevant values are set in the Library Editor Panel: Parts tab or the Part Editor Panel: Properties tab, User Part Attributes section.
- If a net is deleted during forward annotation, then any pin attributes are removed that are associated with it. A warning is displayed with details of the deleted net and pin attributes. If the net is subsequently reconnected to the pin, then the relevant pin attributes are readded.
- For a list of attributes in Constraint Browser which can be forward annotated and back annotated, see: Annotation matrix.pdf.
RINF netlist
If selected, then you can specify a RINF netlist that is forward annotated to the current design in eCADSTAR PCB Editor. The RINF netlist is a standard Zuken file format that can be output from schematic capture tools, including CADSTAR and OrCAD. Parts and footprints that are listed in the RINF file must be in the library, or the Forward Annotation process will fail.
Any new items and nets in the RINF file are added to the design, and items and nets that are absent from it are deleted from the design. The existing positions of items and net routing are retained if possible. A report is displayed that lists the changes that are made in the design. If there are errors that prevent the Forward Annotation process from finishing, then they are displayed in the report window.
Components are not permitted that are specified in the RINF file by footprint only. A part that matches the footprint name must also be available. The Create Parts From Selected Footprints and Create Parts From All Footprints commands allow you to create matching parts for footprints in Library Editor.
Note
The Create Parts From All Footprints command is not available by default, but can be added to the Quick Access Toolbar or ribbon.
The Create Parts From All Footprints command is not available by default, but can be added to the Quick Access Toolbar or ribbon.
| Value | Description | |
|---|---|---|
| Netlist box | Displays the RINF netlist that you want to forward annotate
to the current design in eCADSTAR PCB Editor.
Click to select the required .frs
or .net file in the Open
dialog. |
|
|
|
Allows you to browse to a .frs or .net file in the displayed Open dialog. The contents of the RINF netlist are forward annotated to the current design in eCADSTAR PCB Editor. If there is a problem with the specified file then a report dialog is displayed when you click Next. | |
| Update the association of the PCB design with the RINF netlist | Allows you to link the current PCB design with the RINF netlist that you specify in the Netlist box. The specified file is automatically displayed in the Netlist box when you execute the Forward Annotation command. By deselecting this box, you can execute the command for a different RINF netlist, without updating this link. | |
| Selected | The RINF netlist displayed in the Netlist
box is linked to the current PCB design. The specified
file is automatically displayed when you execute the Forward
Annotation command. To link to another RINF netlist, click
the button and browse to a different .frs or .net
file. The specified file is automatically displayed when you next
execute this command. |
|
| Not selected | Allows you to execute the Forward Annotation command for the RINF netlist that is displayed in the Netlist box, without creating a link to the specified design. The next time you execute this command, the linked RINF netlist is displayed. |
Note
- Attributes in the PCB design are preserved when forward annotation is performed using a RINF netlist. However, attributes are not currently supported in the RINF file.
- Back annotation to the RINF format is not currently supported in eCADSTAR.
- Pins can be specified in the RINF file by either index or pin name. The Forward Annotation process fails if a matching pin is not found on the part or footprint in eCADSTAR, and an error is displayed.
- Variants are not supported in the RINF file. Any variant items are removed from it, and a warning is displayed.
- The results of forward annotating from a RINF file may be inferior to those produced from a schematic design. Some tracks may become unrouted, and the position of components may be reset. E-Nets must be manually rebuilt.
Board configuration
Displays the settings that you specify in the Schematic section, and allows you to execute the Forward Annotation command by clicking Finish.
| Value | Description |
|---|---|
| Board configuration box | Displays the settings that you specify in the Schematic section of the Forward Annotation dialog. To change a setting, click Back to display the Schematic section. |
| Value | Description |
|---|---|
| Back | Displays the Schematic section in the Forward Annotation dialog. |
| Next | Displays the Board configuration section in the Forward Annotation dialog. If there is a problem with the RINF netlist that you specify, then a report dialog is displayed. |
| Finish | Executes Forward Annotation
using the settings specified in the Schematic
section. In the displayed confirmation dialog, click Yes
to continue. If no problems are discovered during this process,
then the View Design Changes
dialog is displayed. If problems are discovered, then the Forward Annotation dialog is displayed.
Relevant information and problems are listed in the dialog. You
can save the contents of the dialog in text format by clicking
 .
Click Close in this dialog to display
the View Design Changes
dialog. |
| Cancel | Closes the Forward Annotation dialog without executing Forward Annotation. |
