Allegro Front to Back User Guide

Allegro Front-to-Back User Guide Getting Logical Design Ready for Physical Layout October 2019 46 Product Version 17.4-2019 © 1999-2019 All Rights Reserved. The constraints in the schematic are synchronized with the constraints in the board. If you now start Constraint Manager from Design Entry HDL, all the electrical constraints that you captured in Allegro PCB and Package or Allegro SI will appear in Constraint Manager. Passing Properties from the Layout to Schematic While updating the schematic in Design Entry HDL with the changes in the board file in PCB Editor, you can use Packager Setup to specify which of the properties need to be modified and which properties need to be added to the schematic. You can make the following changes: 1. Define the feedback properties. By default, all feedback properties replace the corresponding properties in the schematic. You can, however, specify that certain feedback properties will not replace (win) the properties in the schematic. ❑ Add a property in the No Feedback Properties list box to insure that it will not replace the schematic property. ❑ Click Remove in the No Feedback Properties list box to delete any property from it. A property removed from the No Feedback Properties list box is fed back to the schematic. 2. Run Packager-XL in the feedback mode. By default, the None radio button is selected signifying that Packager-XL will run only in the forward mode. To run Packager-XL in the feedback mode, click either the Allegro PCB Editor radio button or the 3rd Party radio button to specify the source of feedback files. 3. Annotate properties. You can define the objects in the design that should be backannotated. You can select body, pin, net, or physical net name for backannotation. To choose any object for backannotation, select the respective check boxes under the Options radio button. 4. Manage hard properties. You can manage the packaging of hard properties (user-defined properties) by selecting the Do not Update Hard Location, Section and Pin numbers on schematic check box. By default, Packager-XL updates only soft properties in the feedback mode. 5. Accept the changes.

• Cover
• c contents - Contents
• Preface
• About the Front-to-Back Flow
• How This Book is Organized
• Creating and Managing Libraries
• Allegro Front-end Tools Libraries
• Library Structure
• Creating and Managing Libraries
• OrCAD Libraries
• Capturing Logical Design
• Creating Project Using Allegro Tools
• System Capture
• You can also perform other page manipulation operations, such as creating a new page or deleting an existing page from the Project viewer. You can drag and move the pages up and down to change their order in the Project viewer.
• Allegro Design Entry HDL
• Creating Project Using OrCAD Capture
• Creating a Schematic
• Designing Schematic Using System Capture
• Creating Schematic Using OrCAD Capture
• Capturing Logical Designs using DE-HDL
• Capturing Logical Design Constraints
• Why Constraint Manager?
• Using Constraint Manager with Design Capture Tools
• All the constraints are stored in the Constraint Manager Database (CMDB) and saved in the dictionary and constraints file designname.dcf.
• Constraints in System Capture
• Capturing Constraints in Design Entry HDL
• Capturing Constraints in OrCAD Capture
• Creating Variants of Your Design
• Managing Variants in System Capture
• Creating Variants using Variant Editor
• Getting Logical Design Ready for Physical Layout
• Preparing a System Capture Design for Physical Layout
• Preparing a DE-HDL Design for Physical Layout
• Exporting a DE-HDL Design
• Forward Mode
• Preparing an OrCAD Capture Design for Physical Layout
• Exporting an OrCAD Capture
• Annotating the Design
• Packaging Your Design (Advanced)
• Generating a Bill of Materials
• Updating the Schematic With the Changes in the Board
• Passing Properties from the Layout to Schematic
• Designing Layout
• Physical Layout using OrCAD PCB Editor
• Creating a Board Outline
• Creating Symbols and Padstacks
• Importing Logic
• Defining Layers
• Defining Constraints
• Placement
• Routing
• Design Synchronization
• Physical Layout using OrCAD Capture
• Preparing the Schematic for Layout
• Property Flow from Capture to PCB Editor
• Generating Initial Board File
• Backannotation from PCB Editor
• Running Design Rules Check - Physical Rules
• Capturing Physical Constraints
• Using Constraint Manager with PCB Editor
• Synchronizing Schematics and Boards
• Need for Synchronization
• Design Synchronization Tasks
• Feedback Mode