Allegro Front to Back User Guide

Allegro Front-to-Back User Guide Designing Layout October 2019 56 Product Version 17.4-2019 © 1999-2019 All Rights Reserved. Cross Probing for PCB Editor After creating the board file, you place and route the board. This includes placing the parts in PCB Editor/Allegro SI/PCB Editor, APD and routing the nets. Sometimes, you may also require to swap pins or sections/functions to make routing easier. You can select the components from the Select elements for placement list in the Placement dialog box and then place them directly on the board. You can also place the components directly from the Capture schematic design. This feature is called cross probing. Between Capture and PCB Editor, there are two cross probing functions: cross highlighting and cross selection. Cross selecting between Capture and Allegro PCB Editor If you are placing parts in PCB Editor using Place - Manually command, then select one or more parts in Capture and the corresponding parts will be selected in the Placement dialog box in PCB Editor. This option is only available when PCB Editor is active (running) and Intertool Communication (ITC) is enabled in Capture. Cross highlighting between Capture and PCB Editor Cross highlighting applies to three different types of objects: parts, nets and pins. Following are the general rules of cross probing: ■ If PCB Editor is in highlight mode, you can select an object in PCB Editor, and the corresponding logical element in Capture is highlighted. ■ If PCB Editor is in dehighlight mode, when you dehighlight a physical object, the corresponding logical element is dehighlighted in Capture. Deselecting an element in Capture dehighlights the corresponding element in PCB Editor. ■ In Capture, when you select a component, its corresponding physical part is only highlighted in PCB Editor if you are in PCB Editor highlight mode. Otherwise, selection in Capture has no effect in PCB Editor, unless you are using cross selection. Locking Components during Cross-Probing When you cross probe between Capture and PCB Editor, you need to keep selecting components in your design to place them on your board. In many cases, you create elaborate design with a large number of components and intricate connectivity. So when you keep selecting the components and nets on your design, you might inadvertently shift a component. This shift, in some cases, might even cause issues of connectivity.

• 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