Home > Community > Blogs > PCB Design > what s good about pcb si setup audit 16 6 has many new enhancements
Login with a Cadence account.
Not a member yet?
Create a permanent login account to make interactions with Cadence more conveniennt.

Register | Membership benefits
Get email delivery of the PCB Design blog (individual posts).


* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

What's Good About PCB SI Setup/Audit? 16.6 has Many New Enhancements!

Comments(0)Filed under: PCB Signal and power integrity, PCB design, Differential Pair Support, Allegro, SI, Signal Intregrity, Power, PCB, SigXP UI, DRC, PCB SI, SI analysis and modeling, design, differential pairs, diff pairs, "PCB SI", "PCB PI", High Speed, PCB power integrity, Allegro PCB SI, signal integrity, Grzenia, diff pair, differential pair, Allegro 16.6, 16.6, setup/audit, setup, audit

The Allegro PCB SI Signal Setup and Audit commands were introduced in the 16.5 release. Enhancements have been made to these commands in the 16.6 release.

Read on for more details…

Selection of all Components in Component Class Setup

A new top level has been added to the tree display with a label of All Classes. Selecting the All Classes item will cause all of the visible classes and components to be selected:


More Flexibility In Creating Differential Pairs

This enhancement allows for more control over what nets or Xnets get selected to form differential pairs. You can now specify the Xnet name suffixes and differential pair name prefix as is currently allowed by the Auto Generate button on the Logic > Assign Differential Pair dialog. A new button, named Create Diff Pairs From User Defined Rules has been added to the Diff Pairs page of the SI Setup wizard:

When this button is selected, the following new dialog appears:

This dialog works the same as the Auto Generate button on the Assign Differential Pairs command. Once the two suffixes have been defined, selecting OK on this dialog causes the Setup command to look for pairs of selected Xnets that have the same base name and also have the two suffixes. A user defined differential pair will be created from these pairs of Xnets. The name of each differential pair will be the specified Diff Pair Name Prefix string followed by the base name of the Xnets. These diff pairs are then shown in the Setup Diff Pairs page of the setup wizard. You can then use the Change Selected Diff Pair to Model Defined button on this page to convert these diff pairs from user defined to model defined.

This command also handles Xnet or net names that use the bus bit format, that is, names that end with a <#>. For example, a name of DATA<3> indicates bit three in the DATA bus. When this format is used the diff pair suffixes that are specified in the above form will come before the bit number in the Xnet name. For example, there might be two Xnet names such as DATA_P<3> and DATA_N<3>. If diff pair Xnet suffixes of _P and _N are specified and the Diff Pair Name Prefix is DP_ then a diff pair named DP_DATA3 will be created from these two Xnets. This is consistent with how this case is handled by the Auto Generate button on the Assign Differential Pairs command.

User Control Over Possible Power/Ground Nets Selection

The Power and Ground Setup page of the SI Setup command shows a list of possible power and ground nets that aren’t currently marked with a VOLTAGE property. The following rules are currently used to select these nets -

•    A net that is part of a diff pair is not considered to be a voltage net.
•    A single pin net is not considered to be a voltage net.
•    If the name of the net contains any of the following strings, then the net is considered as a possible voltage net: VCC, GND, VEE, VTT.
•    If the net contains any pins that have a POWER or GROUND pin use then the net is considered to be a possible voltage net.
•    If the net contains more than a specified number of pins then it is considered to be a possible voltage net. By default this number is 25 but can be changed with the MAX_PINS_IN_NET environment variable.

The following change has been made to give you more control over how the possible power and ground nets are selected. A new button, labeled Define Possible Voltage Net Rules has been added to the Setup Power and Ground Nets page of the SI Setup wizard. This page is shown below:

When this new button is selected, the following dialog appears:

This form allows you to set up your own list of strings that will be matched against net names to find possible voltage nets. The Add and Delete buttons allow you to add new strings and delete existing ones.

The Include nets that contain power or ground pins check box allows you to turn on and off this feature. Likewise, the Include nets that contain more than XXX pins check box allows you to control this feature. The field showing the number of pins can also be updated.

The data from this form is saved with the active drawing as an invisible property on the design so they will be reused each time the drawing is opened.

Another command that looks for possible voltage nets is the Logic > DC Nets command. This command lists the nets in the design but attempts to put the nets that are most likely voltage nets at the top of the list. A new button, labeled Possible Voltage Net Rules, has been added to this form. This button opens the same form as shown above to allow you to set the rules for selecting possible voltage nets:


Improvements to Audit of Dangling Lines

This enhancement improves the audit on clines ending at a via that is a test point, as this should not be considered a dangling cline. Also dangling clines should be referred to as stubs to avoid confusion with the Dangling Lines, Via and Antenna report that is currently available.

The SI Audit command has been updated to now refer to clines that have an end point that has no connections as stubs. Also, a cline that ends at a via that has been marked as a test point will no longer be considered a stub.

Model Assignment from Assignment Map Files

The SI Model Assignment command allows you to output a record of assigned SI models into a file. There are two file formats supported - one organized by component refdes, and the other by component device type. This enhancement allows you to perform model assignments from these assignment map files.

To accomplish this, the Assign Models to Components page of the Setup wizard has been updated as shown below:

A new button, labeled Load Assignments From a File, has been added to this page. This button prompts you to select an assignment map file. Either type of assignment file format will be accepted, that is, a file organized by refdes or by device type. The assignments defined by the selected file are loaded. At the completion of this process a text window appear that shows the model assignments that were made and list any errors (such as model not found) that were detected. The Assign Models to Components page of the wizard will then be updated to remove all the components that now have assigned models.

Highlight Power and Ground Errors in Audit

This enhancement allows for the ability to highlight a net that has been flagged with a missing voltage property error. The RMB popup over an error shown in the Audit dialog contains a More Info About Error option for Power and Ground errors. Selecting this option provides more information about the selected error, such as why Audit thinks this net should be a power or ground net. When More Info is requested, in addition to providing the information in a confirmer, the net will be highlighted in PCB SI:

Warn User When Manually Resolving Many Audit Errors

When multiple errors have been selected in the Audit command and the Manual Resolve button is picked, you are faced with resolving each of the selected errors one at a time. The command has been enhanced to first display a confirmer that tells you how many errors have been selected and warns you that they will be resolved one at a time.

Import Errors to be Ignored in Audit

This enhancement allows for the ability to transfer the list of ignored errors from one drawing to another. To accomplish this a new button, labeled Import Report, has been added to the Audit errors page. This is shown below:

This button opens a file browser asking for an errors report file. This is a file that was created by the “Report” button on this same dialog. An attempt will be made to find each ignored error in the report file in the current errors list. If found and the error is currently Unresolved, its state will be changed to Ignored. This allows you to transfer the ignored errors from one drawing to another.

Edit Model Defined Differential Pairs in Setup

Currently the Setup command only allows you to update user defined differential pairs. You now have the ability to edit model defined diff pairs.

Two radio buttons have been added to the Diff Pair page of the Setup command. These buttons control whether user defined or model defined diff pairs will be listed. By default, user defined diff pairs will be displayed. By picking the Show Model Defined Diff Pairs button, model defined diff pairs will be shown. A new button, labeled Edit Model Defined Diff Pair, will be visible when a model defined diff pair is selected from the list:

When the Edit Model Defined Diff Pair button is selected, the pins of this diff pair are shown in the following form:

This is the same form that is currently available when you do a manual resolve of a diff pair connection error that is found in Audit.

Collapse/Expand Levels in the Xnet Selection Tree

This enhancement allows for the ability to expand or collapse all the items in the Xnet selection tree.

Both the Setup and the Audit commands have a page that allows you to select the Xnets. This tree can have many different levels - designs, buses, diff pairs and Xnets. If you open a number of these levels it can become difficult to find items. A right-mouse-button popup has been added that is available over any item in the tree. There are two options on the popup - Collapse All and Expand All. Selecting Collapse All will collapse the tree for the selected item as well as all of the sub-items under the selected item. Selecting Expand All will expand the selected item as well as all of its sub-items:


I look forward to you sharing your experiences using these new features.

Jerry "GenPart" Grzenia


Leave a Comment

E-mail (will not be published)
 I have read and agree to the Terms of use and Community Guidelines.
Community Guidelines
The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. 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. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.