Home > Community > Blogs > PCB Design > what s good about pcb si design setup and audit 16 5 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 Design Setup and Audit? 16.5 Has MANY New Enhancements!

Comments(0)Filed under: PCB Signal and power integrity, PCB design, PCB Editor, SI, IC Packaging and SiP Design, Signal Intregrity, SiP, SigXP UI, PCB SI, "PCB design", SI analysis and modeling, "PCB SI", SPB16.5, Allegro 16.5, Allegro PCB SI

Many of the problems that customers encounter today when running a signal integrity (SI) analysis tool are caused by the design not being properly set up. The Allegro PCB SI tools require information that is specific to the tool, and it must be available before the tool will function correctly.

Today there is a Setup Advisor command whose purpose is to help you set up the design correctly. Although this command is useful, it ignores much of the setup data. There are also several SI Audit commands that look for errors in the design setup. These commands create a lengthy report that show possible errors. As with the Setup Advisor, the Audit commands fail to check much of the required setup data and they offer little help in fixing the problems that are detected.

Two new commands are available in the SPB 16.5 release that replace the existing Setup Advisor and SI Audit commands. One of these commands is a new SI Design Setup and the other is an SI Design Audit. Both of these commands invoke wizards that walk you through the steps that are necessary to do the setup or audit.

Read on for more details …

Design Audit

Currently, the Analysis > SI/EMI Sim menu contains four Audit commands. They are:
Design Audit               Runs an audit on all nets in the design
Net Audit                    Runs an audit on selected nets in the design
Audit One Library        Runs dmlcheck on a selected dml file
Audit List of Libraries   Runs dmlcheck on a list of dml files

The two commands the run dmlcheck are no longer needed since we now have the ability to run dmlcheck on a dml library from the Library Mgmt dialog that is available in the SI Model Browser. The other two net-based audit commands have been replaced with one new audit command.

The new SI Design Audit command replaces the two net audit commands described above. It is available using the menu pick Setup > SI Design Audit. This command opens a wizard with three pages. The function of each page is:

Page 1     Used to control which tests are to be performed
Page 2     Used to select the Xnets and nets to be audited
Page 3     Shows the errors that were found and alls you to resolve these errors

Page 1 — Controlling Tests to be Run

The first page of the SI Design Audit wizard allows you to control the tests that are to be run by the audit. This page is shown below:


This tree shows all of the tests that can be performed by the Audit. The tests are organized into categories, such as Cross-Section, Power & Ground Nets and Components. Under each category is a list of each test in that category. Next to each item in the tree is a box. If the box contains a check mark the item is selected; if the box is empty the item is not selected. Picking a box will reverse its selection. By picking the boxes next to the items in the tree, you can turn off or on any individual test, all of the tests in a category, or all tests.

The list of tests to be run is saved with the drawing so the next time this command is run, the test selection will be in the same state as it was in the last time this command was used.

Page 2 — Selecting Xnets and Nets to Audit

The purpose of the second page is to allow you to select the Xnets and nets in the design that are to be audited. This page is skipped if you have disabled all of the Xnet/net-based tests, such as those in the Components, Xnets, InterConnect, SI Models and Diff Pairs categories. In general you will only want to audit the high speed Xnets/nets that will be simulated. This page is shown below:


This dialog allows you to select (or unselect) the Xnets and nets that are to be audited. The Xnets and nets can be selected individually, by bus, by diff pair or for an entire design. The above example shows a single design (named test) but if a multi-board system is active, each of the designs in the system will be shown.

By default, Xnets and nets that are members of buses or diff pairs will be shown as members of the bus or diff pair. You can turn off the display of buses and diff pairs by changing the Show Buses and Show Diff Pairs options that are at the top of the page.

The Import Xnets/Nets to be Selected button allows you to specify a file of Xnets and nets that are to be selected. The file must contain each Xnet and net name on a separate line. The result will be that all Xnets and nets will be unselected except for those specified in the file.

The Export Selected Xnets/Nets button will create a file that contains the names of each net and Xnet that is currently selected.

The first time the SI Design Audit command is run, all Xnets and nets will be selected by default. Once the Next button is picked, the list of selected Xnets and nets is saved in the drawing. The next time the SI Design Audit command is run, the Xnet/net selection will start in the same state it was in the last time the command was run.

Page 3 — Audit Errors

Picking the Next button on the Xnet/net selection page causes the selected audit tests to be run on the specified Xnets and nets. The results are shown on the next page of the wizard that will look as shown below:


A list of the audit errors is shown. For each error there is a message that describes the error and a Status column that shows the status of the error. There are three status values:

Unresolved    The error still exists
Resolved       The error has been resolved
Ignored         The error is to be ignored

There are several ways to change the status for any error. First is the pulldown on each cell in the Status column. Depending upon the current state of the error, this pulldown can have the following values:

Resolve Error     An attempt will be made to automatically resolve the error. If the error can be resolved, the status will change to Resolved. If it can't be resolved then a confirmer is shown that tells you that no automatic resolution is possible and the status will remain Unresolved.
Ignore Error     Causes the system to ignore this error. The status will change to Ignored. The errors that are ignored are saved with the drawing so the next time this command is run this error will be displayed with a status of Ignored.
Set to Unresolved     This option is available for Ignored errors. The status will be reset to Unresolved.

Another way to resolve errors is by using the three buttons under the Resolve Errors heading. They will perform the following functions:

All             All unresolved errors that can be automatically resolved will be resolved
Selected    All of the selected errors will be automatically resolved, if possible
Manually    Depending upon the type of error, a separate dialog is opened that shows the selected error and allows you to correct it. When the separate dialog is closed, the error is retested. If the error no longer exists then the status of the error is changed to Resolved.

The two buttons under the Ignore Errors heading allow you another method to ignore errors. These buttons perform the following functions:

All             All unresolved errors will be changed to Ignored
Selected    All selected and unresolved errors will be changed to Ignored

The Show Resolution button displays a message that describes how the selected error was resolved. The Report button creates a report that shows each error with its status and test category. This report is shown in a text window that allows you to save the report to a file or to print the report.

The three fields at the top of the dialog allow you to control the display of errors. They are:

Status Filter     Optionally restricts the list of errors to only show Unresolved, Resolved or Ignored errors
Test Filter         Optionally restricts the list of errors to only show errors of a specific test category
Sort By            Sorts the list of errors by either test category or status

Design Setup

The existing Tools > Setup Advisor command has been replaced by the new Setup > SI Design Setup command. This command invokes a wizard that will lead you through the steps necessary to set up the design to do SI simulations.The pages of this wizard are described below.

Page 1 — Selecting Setup Categories to be Performed

The first page of the SI Design Setup command lists the setup categories that can be performed by the wizard. The page is shown below:

This list is similar to the test categories that are shown by the Design Audit command. Normally it is expected that all of the setup operations will be performed, but this page allows you to optionally turn any of them off. One use for this might be if Setup has been previously run. In this case you might know that only certain operations need to be performed again.

The Turn On All Setup Categories and Turn Off All Setup Categories buttons are provided as a quick way to turn on or off all categories.

As described below, at the completion of setting up items in a category, an audit of the data in that category is run by default. The errors found by this audit are shown by the dialog described the Audit Errors section above. You can disable this automatic running of this audit by turning off the Run Audit upon completion of each setup category button.

Page 2 — Selecting Xnets and Nets to Setup

This page is similar to the Xnet and net selection page shown for the SI Design Audit command. It allows you to select the Xnets and nets on which the setup operations are to be run. The Xnets/nets that are selected are saved with the drawing the same way they are for SI Design Audit. If the Audit command has been previously run then the initial state of this page will reflect the state it was in when Audit was run. Likewise the Xnets/nets that are selected for Setup will be the same Xnets/nets that will be selected if the Audit command is later run.

Performing Setup Operations

Each setup category has one or more pages that contain fields that allow you to perform the requested setup. The example below shows one of the pages that is part of the Power and Ground Net setup:

This dialog shows both the nets that have been marked as DC nets and also the nets that are possible DC nets. It allows you to assign a voltage to any of the possible DC nets or to change the voltage that has been assigned to a DC net.

Once setup has been completed for any setup category, a pick of the Next button will, by default, cause an audit to be run. As described above, this feature can be turned off. Only the audit tests associated with the category just completed will be run. If any errors are found then the Audit Errors dialog will be displayed. As described in that section, this dialog allows you to optionally resolve any of these errors or to mark them as being ignored.

Once the Audit Errors dialog is completed, the audit tests are run again. If any errors still remain, you are warned and asked whether or not you would like to continue to the next setup category.

After each selected setup category has been processed, the final page of the setup wizard is as shown below:

As the text on this page says, this gives you one more chance to do an audit of the design. Picking the Run SI Design Audit button will run the audit tests for all the setup categories that were selected and show any errors found in the errors dialog.

I look forward to your feedback on using this new 16.5 capability.

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.