Look in

Browse the hierarchical drive and directory structure for your system.

File name

Select or type the name of the project or file(s) that you want to add to the Project Folder.

Files of type

Filter files by extension.

Name

Displays the name of the new property column or row to add in the property editor.

Value

Displays the value of the new property column or row to add to selected objects and in the property editor. If you enter the name of an existing property in the Name text box, its current value appears in this text box.

Display [ON/OFF]

Select the check box to display the Display Properties dialog box.

Always show this column/row in this filter

Select the check box to save the new column/row in the current filter. You cannot save a new column or row in the <Current properties> filter.

Annotate parts and group parts together that have common characteristics. Packaging is a key step that should be done before netlisting to a PCB board design tool such as PCB Editor.

Generate a reuse module or renumber the reference designators in a reuse module in Capture. Reuse modules may be netlisted then used in PCB Editor or used in Capture as library parts or as hierarchical blocks.

Refdes control required

Check this option, if you want to specify a part reference range for each schematic page or a hierarchical block in the root-level of your design.

For more description about how to use this option to specify a part reference range for a schematic page or a hierarchical block, see Customizing part references in a design.

Scope

• Update entire design
• Update selection

Specify whether to ll the part references in the design (or library), or just the selected schematic pages.

• Schematic Pages
• Hierarchical Blocks

Grid (for specifying part reference range)

• Pages or H-Blocks column

Displays all the schematic pages or hierarchical blocks in the root schematic folder of your design depending on whether your design is a flat design or a hierarchical design.

• Start Value and End Value columns

Specify a numeric value greater than 0 in the cell corresponding to the schematic page name or hierarchical block name.

You can also use the Arrow keys to move around in the grid.

You can use the column handle () to resize the rows and columns in the grid.

Action

Incremental reference update

If checked, Capture incrementally updates parts with a question mark in the part reference. For example, parts with reference designators of U?A will be numbered U1A, U1B, U1C, and so on. Part reference and package information is not updated on existing parts.

Unconditional reference update

If checked, Capture updates all parts in the selected schematic pages. Both part reference and package information may be updated on existing parts. Parts on different schematic pages are not packaged together.

Reset part references to “?”

Specifies to reset all the part references to "U?"

Add intersheet references

Specifies to add intersheet references to the design.

Delete intersheet references

Specifies to remove all intersheet references from the design.

Annotation Type

Specifies the sequence in which the components on the design are annotated.

The Annotation Sequence list contains three options that you can use to decide the sequence in which the objects on your design are annotated - Default, Left to Right & Top to Bottom.

Mode

Specifies to update either instances or occurrences. Capture automatically sets this option based on the project type. All designs default to use instances. If a PCB or schematic design is complex or has occurrence properties, the default shifts to occurrences. Capture recommends the preferred mode, which you can override.

Physical Packaging

Specifies the properties that must match for Capture to group parts into a single package. Value and Source Library properties are the default property string, but you can use any combination you like.

The value in Additionally From INI is updated using the value specified by you in the Capture.ini file AnnotateAdditionalPropertyString property. For example, to specify PartGroup as the value, set it in Capture.ini as AnnotateAdditionalPropertyString={PartGroup}. You can also specify more than one value such as {Value}{Source Package}. If you change this value in the field, Capture.ini will be updated accordingly.

For example, you might want to use Value and Voltage. Say your design uses both Tantalum capacitors and ceramic disk capacitors. First, you could assign ".01uF" to the part Value property for all the capacitors. Then, you could define a user property called "Voltage" for all capacitors in the design, and assign it the value "100V" or "25V" as appropriate. To annotate your design, type "{Value} {Voltage}" (without the quotation marks) in the Part Value property combine text box.

In this example, Capture groups the parts with "C?" as the part reference, and ".01uF" as the part value, but it separates the 100V Tantalum capacitors from the 25V ceramic disk capacitors.

Additionally From INI

Specifies a combined property string that gets added in the Capture.ini file under the Preferences section, such as AnnotateAdditionalPropertyString=<property name>. For example, adding {ROOM} in the Additionally From INI field has the following entry under the Preferences section: AnnotateAdditionalPropertyString={ROOM}

Once added, any project opened in Capture will have this property.

Reset reference numbers to begin at 1 in each page

Specify whether to number parts within the context of the schematic folder. When this option is selected, Capture begins numbering parts at 1 for every selected page. Otherwise, Capture continues numbering after the highest referenced part in the selected schematic pages.

Annotate as per PM page ordering

Specify whether to perform the annotation on the basis of order of pages/ folders in the Project Manager window. If there are multiple folders and multiple pages in each folder then the root folder is annotated first followed by its pages. Alphabetic order is followed to determine the sequence of pages in a folder.

Annotate as per page ordering in the title blocks

Specify whether to perform annotation according to numbers on the page numbers specified in the title blocks of the schematic pages.

Do not change the page number

Check this option if you have chosen to annotate as per page ordering in the title blocks option, changed the page numbers in the title blocks, but do not want to change the page ordering on reannotation.

Include non-primitive parts

Specifies whether to annotate non-primitive parts or to reset non-primitive part references to “?”. Select this option to avoid netlisting duplicate reference errors when you want to simulate a design or generate a new part.

Preserve designator

Specifies that the designator information of a homogeneous part during unconditional or reset annotation is to be preserved.

Preserve User Assigned Valid References

Specifies that the user assigned reference designator during annotation is to be preserved.

Library files

• • Profile-level model libraries are archived under their respective profiles and referenced as .\<library_name>.lib. For example, when a profile; AC containing a model library diode.lib is archived, the diode.lib is copied under the folder AC and the simulation settings is modified as: .\diode.lib.

• • Design-level model libraries are archived under .\<design_name-pspicefiles>\<design_name>\<library_name>.lib. For example, when a design called histo containing a model library bipolar.lib is archived, the model library bipolar.lib is copied under folder histo-pspicefiles\histo and the simulation settings is modified as: .\histo-pspicefiles\histo\bipolar.lib.
  • In case of global-level model libraries:
    • a copy of model library is created under the existing <design_name>.lib, if it exists
    • a new <design_name>.lib file is created and a copy of model library is added to the <design_name>lib and the simulation setting is modified as design-level library.

Include TestBench

Include any testbench which is part of the current project.

Output files

Archive output files generated by Capture tools.

For example, cross reference reports (*.XRF files), EDIF netlists (*.EDN files) and PSpice project .DAT files, would be archived.

Referenced projects

Recursively save any projects referenced from within the current project.

Archive directory

Specify the drive and directory for the project to be archived in.

Use the ... button to display the Select Directory dialog box where you can locate and select a new drive, directory, or both.

Create single archive file

Activate the File name text box for specifying the name of the compressed archive file.

File name

Specify a name for the compressed archive file. The default name is <projectname-current date>.

Add more files

Add more files and folders to be archived.

Browse for

Specify whether you want to add more files or directories to your archive.

Select the Directories option to add a directory or the Files option to add more files to your archive.

Additional Files/Directories

Specify files and directories you want to be archived.

Use the ... button to select the files and directories you want to archive.

Implementation Type

Specify the type of implementation from one of the following:

Schematic View Indicates that the attached implementation is a schematic. Capture automatically generates the appropriate hierarchical pins for the hierarchical block based on the hierarchical ports.

VHDL Indicates that the attached implementation is a VHDL entity. Capture automatically generates the appropriate hierarchical pins for the hierarchical block based on the port declarations in the VHDL entity.

Verilog Indicates that the attached implementation is a Verilog model. Capture automatically generates the appropriate hierarchical pins for the hierarchical block based on the port declarations in the Verilog model.

EDIF Indicates that the attached implementation is an EDIF netlist. If your design includes EDIF implementations for hierarchical blocks, you must specify the hierarchical pins for the hierarchical block; Capture will not generate them from the EDIF netlist. Also, if your design includes EDIF implementations, you can simulate them, but you cannot compile or build them.

Project Indicates that the attached implementation is a Capture programmable logic project. You must specify the hierarchical pins for the hierarchical block; Capture will not generate them.

Attaching an implementation does not automatically add that file, project, or schematic folder to the project. You must specifically add the implementation to the project with the Project command.

Implementation

Specify the name of the attached object.

Implementation Path

Specify the path and name of the library or file where the attached object is located.

Design Hierarchy

Select the Design Hierarchy option to select a design or its pages to apply advanced annotation.

Property Block

Select a property from the drop-sown list to apply advanced annotation on those objects that have the selected property in their properties.

Reference Range for

Prefix

Specify the Part Prefix

Instance Count

Specify the number of instances that have the same prefix

Start

Specify the start of the Reference Range

End

Specify the end of the Reference Range

Auto Fill Prefix

Automatically fills all the prefixes that are present in the design

Add Row

Adds a row to define Prefix, Instance Count, Start, and End

Delete Row

Deletes a row that contains Prefix, Instance Count, Start, and End

Delete All

Delete all the rows that contains Prefix, Instance Count, Start, and End

Apply

Applies the changes made to the selected

Inherited Ranges

Specifies the inherited ranges from the top-level, such as Capture design

Action

Incremental reference update

If checked, Capture incrementally updates parts with a question mark in the part reference. For example, parts with reference designators of U?A will be numbered U1A, U1B, U1C, and so on. Part reference and package information is not updated on existing parts.

Unconditional reference update

If checked, Capture updates all parts in the selected schematic pages. Both part reference and package information may be updated on existing parts. Parts on different schematic pages are not packaged together.

Reset part references to “?”

Specifies to reset all the part references to "U?"

Annotation Type

Specifies the sequence in which the components on the design are annotated.

The Annotation Sequence list contains three options that you can use to decide the sequence in which the objects on your design are annotated - Default, Left to Right & Top to Bottom.

Annotation Scheme

Annotate as per page ordering in the title blocks

Specify whether to perform annotation according to numbers on the page numbers specified in the title blocks of the schematic pages.

Annotate as per page ordering in the title blocks

Specify whether to perform annotation according to numbers on the page numbers specified in the title blocks of the schematic pages.

Combined Property String

Specifies the properties that must match for Capture to group parts into a single package. Value and Source Library properties are the default property string, but you can use any combination you like.

For example, you might want to use Value and Voltage. Say your design uses both Tantalum capacitors and ceramic disk capacitors. First, you could assign ".01uF" to the part Value property for all the capacitors. Then, you could define a user property called "Voltage" for all capacitors in the design, and assign it the value "100V" or "25V" as appropriate. To annotate your design, type "{Value} {Voltage}" (without the quotation marks) in the Part Value property combine text box.

In this example, Capture groups the parts with "C?" as the part reference, and ".01uF" as the part value, but it separates the 100V Tantalum capacitors from the 25V ceramic disk capacitors.

Additional from INI

Include Non-Primitive Parts

Specifies whether to annotate non-primitive parts or to reset non-primitive part references to “?”. Select this option to avoid netlisting duplicate reference errors when you want to simulate a design or generate a new part.

Preserve Designator

Specifies that the designator information of a homogeneous part during unconditional or reset annotation is to be preserved.

Preserve User Assigned Valid References

Specifies that the user assigned reference designator during annotation is to be preserved.

You can explicitly mark a reference as user assigned by choosing User Assigned Flag – Set from the pop-up menu for the Reference property in the Property Editor or from the pop-up menu of a part in the schematic page. Any references changed using Property Editor, Schematic Editor, or during backannotation are marked as changed and are preserved on selecting this and the previous option.