Cadence® system design and verification solutions, integrated under our System Development Suite, provide the simulation, acceleration, emulation, and management capabilities.
System Development Suite Related Products A-Z
Cadence® digital design and signoff solutions provide a fast path to design closure and better predictability, helping you meet your power, performance, and area (PPA) targets.
Full-Flow Digital Solution Related Products A-Z
Cadence® custom, analog, and RF design solutions can help you save time by automating many routine tasks, from block-level and mixed-signal simulation to routing and library characterization.
Overview Related Products A-Z
Driving efficiency and accuracy in advanced packaging, system planning, and multi-fabric interoperability, Cadence® package implementation products deliver the automation and accuracy.
Cadence® PCB design solutions enable shorter, more predictable design cycles with greater integration of component design and system-level simulation for a constraint-driven flow.
An open IP platform for you to customize your app-driven SoC design.
Comprehensive solutions and methodologies.
Helping you meet your broader business goals.
A global customer support infrastructure with around-the-clock help.
24/7 Support - Cadence Online Support
Locate the latest software updates, service request, technical documentation, solutions and more in your personalized environment.
Cadence offers various software services for download. This page describes our offerings, including the Allegro FREE Physical Viewer.
Get the most out of your investment in Cadence technologies through a wide range of training offerings.
This course combines our Allegro PCB Editor Basic Techniques, followed by Allegro PCB Editor Intermediate Techniques.
Virtuoso Analog Design Environment Verifier 16.7
Learn learn to perform requirements-driven analog verification using the Virtuoso ADE Verifier tool.
Exchange ideas, news, technical information, and best practices.
The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information.
It's not all about the technlogy. Here we exchange ideas on the Cadence Academic Network and other subjects of general interest.
Cadence is a leading provider of system design tools, software, IP, and services.
Assigning reference designators for the schematic instances is a very vital part of the entire PCB flow. This can sometimes become very cumbersome, and in some cases users allocate a major portion of their time and effort to get the assignments correct and optimized.
Annotation is the automated process of assigning reference designators in Allegro Design Entry CIS, also known as OrCAD Capture. The following AppNote clarifies the fundamentals of the Instance and occurrence modes of annotation in a Capture based design. It explains various aspects of annotation and simplifies the concept behind Instance and Occurrence modes.
What are Instance and Occurrence Modes?
These two modes essentially determine how a design is annotated. The Annotate dialog, as shown in Fig.2, provides the option to annotate a design in Instance or Occurrence modes. The recommended mode of annotation is determined based on the conditions specified in the following table:
Table.1 - Recommended annotation modes
Fig.2 - Annotate Dialog Box
The property editor for any part in a Capture design has a white column and one or more yellow columns. The white column is the instance column and yellow columns are occurrence columns.
Flat and Simple Hierarchical Design
With the above explanation, we can deduce that no part contains duplicate occurrence in a flat or simple hierarchical design. The property editor contains one white and one yellow column for every part and both contain the same value for all the properties. By default, the yellow column is hidden for an INSTANCE mode design. You can click the plus sign to expand the yellow column.
Fig. 3 - Property Editor of a Part in a Flat/Simple-Hierarchical Design
For Complex Designs
The property editor includes a yellow column for each occurrence of a part. If a design contains 3 duplicate hierarchical blocks, for all the parts within that hierarchical block, the property editor will contain one white and three yellow columns.
The Part Reference of parts in yellow columns (at the Occurrence level) must be unique after correct annotation of the design.
Fig.4 - Property Editor of a Part in a Complex Hierarchical Design
In Fig.4, observe that capacitors have four occurrences in the design. C1 has four occurrences, C1, C5, C9 and C13.
Annotation is the automated process of assigning reference designators to all the parts placed in the design. Under ideal conditions, annotation must be done as shown in Table1.However, you can select the desired radio button in Fig.2 for any type of design. So, let's understand what exactly happens when the INSTANCE or OCCURRENCE radio buttons are selected.
When a design is annotated in the Instance mode, the part reference is assigned/modified in the white column, representing the instance mode, of the property editor. As a flat or simple hierarchical design is expected to have the same values in the white and yellow columns, this is the preferred mode of annotation for a flat or simple hierarchical design.
When a design is annotated in the Occurrence mode:
Fig 5 - Occurrence mode annotation
Note: As a part will have more than one occurrence in a complex hierarchical design, it is essential that all these occurrences have a unique reference designator in the design. For this, the yellow columns for the parts must have unique reference designator. Therefore, for a complex hierarchical design, the preferred mode of annotation is Occurrence. This ensures that each occurrence gets a unique reference designator.
You can also perform controlled annotation in a multi-page design or a design which contains hierarchical blocks. You can specify the range of reference designator under a hierarchical block or a page. To do this, use the Refdes control required option in the Annotate dialog. Selecting this option gives an additional control to specify range for reference designators as per the hierarchical block or schematic pages.
Fig 6 - options for controlled annotation
For hierarchical designs, you can define a range for each hierarchical block. For flat designs, you can define a range for schematic pages.
Exception in Design Annotation Modes
Sometimes it can be seen that for a flat or simple hierarchical design, the preferred annotation mode is Occurrence. This is the case when any property value has been manually modified in the yellow column (occurrence level). Even adding a space in a property value at the occurrence level will make the preferred mode change from occurrence to instance. In such cases, the preferred mode can be changed using the Accessories > Transfer Occ. Prop. to Instance > Push Occ. Prop into Instance command. Sometimes it can be seen that for a flat or simple hierarchical design, the preferred annotation mode is Occurrence. This is the case when any property value has been manually modified in the yellow column (occurrence level). Even adding a space in a property value at the occurrence level will make the preferred mode change from occurrence to instance. In such cases, the preferred mode can be changed using the Accessories > Transfer Occ. Prop. to Instance > Push Occ. Prop into Instance command.
This will transfer all the yellow column property values (occurrence level properties) to white column (Instance), making both the same and switching the design back to the Instance mode.
Refer the following AppNote for the detailed understanding of these modes in the Capture - Allegro PCB Editor flow.
Click here for the AppNote.
Note: The above link can only be accessed by Cadence customers who have valid login credentials for Cadence Online Support (http://support.cadence.com/).
Naveen KonchadaCadence Customer Support
for multipage schematic, how can change the starting no of reference from 1 to onther number (e.g. 101)?, i don't want set the number range in each page, just whole schematic use same start ref. no.
How to add intersheet references when there are multiple schematics each having multiple pages. I found the intersheet references got added only on the root schematic folder.
I have a complex hierarchical design, now if I annotate the design, i got two different references for one part, one for OCCURRENCES and another for INSTANCES. How can I solve this issue..? please help.
PLEASE DEFINE TERMS USED! OCCURANCES..INSTANCES...NO EXAMPLES...JUST DEFINITIONS PLEASE PLEASE
IT WOULD BE A WONDERFUL IDEA IF TERMS USED WERE 'DEFINED'. FOR INSTANCE "INSTANCES" OR OCCUDRRENCE" ARE BOTH USED OFTEN BUT NEVER IS THERE A DEFINITION FOR THES TERMS. THIS HAS BEEN A PROBLEM FOR OUR USERS FOR YEARS. WHERE CAN THE DEFINITIONS BE FOUND????????