will be under maintenance from Friday, Oct. 3rd at 6pm (PST) thru Sunday, Oct 5th at 11pm (PST). login, registration, community posting and commenting functionalities will be disabled.
Home > Community > Blogs > PCB Design > what s good about differential impedance in allegro constraint manager it s in spb16 3
Login with a Cadence account.
Not a member yet?
Create a permanent login account to make interactions with Cadence more convenient.

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 Differential Impedance in Allegro Constraint Manager? It's in SPB16.3!

Comments(3)Filed under: PCB Signal and power integrity, PCB design, Differential Pair Support, Allegro PCB Editor, RF, SI, Signal Intregrity, SiP, Power, PCB, SPB 16.3, DRC, Allegro 16.3, PCB SI, Digital SiP design, SPB16.3, SI analysis and modeling, design

The ability to constrain or report Differential Impedance from within Constraint Manager (CM) has been a long standing request. The SPB16.3 Allegro PCB Editor Advanced Constraints feature allows customization of a user-defined differential impedance constraint in CM.

Constraint Manager has the ability to report and Design Rule Check (DRC) single-ended impedance in the Electrical domain, Net — Routing — Impedance worksheet. Differential impedance can be added as a user-defined constraint to a new or existing worksheet.

Read more for how to use this new capability.

1. Open the Electrical domain in Constraint Manager (CM).

2. Right mouse button (RMB) click on the Net folder in the tree view and select Customize Worksheet. This will put CM in Customize Mode.

This is indicated by the extra plus signs in the tree view and the check mark next to Customize Worksheet as seen in the graphic below.

3. RMB on the Net folder again and select Add New Workbook.

4. If desired, click on the new Workbook/Worksheet you just added and rename them.

5. Open the new Worksheet you created.

6. RMB on the new Worksheet and select Add Column.

This launches the Add Column dialog, which can be used to add pre-defined and user-defined columns throughout CM and can also be used as a launching pad for creating user-defined columns for things like Measurements, Properties, or User-Defined Constraint Bundles.


7. Change the Type: pulldown to Pre-defined and scroll down in the window until the DIFF... entries are seen.

The items in the Pre-defined list are all of the Cadence attributes in the database and columns in CM. The DIFF_IMPEDANCE_RULE is an example of optional customization that is made available to users.

8. Select DIFF_IMPEDANCE_RULE in the list and OK the Add Column dialog.

9. OK the confirmer that appears. This is merely an indication that the attribute you are adding is enabled for Objects that are not available in the current worksheet.

CM should look something like the following:

The column header and individual columns look like any other constraint in CM. As user-defined constraints, they have the limitation of indicating pass/fail solely within CM. There will be no DRC markers associated with these.

This constraint has a default value of 100 +/- 5 ohms.

10. RMB on the column header and select Analyze to update the worksheet. The values in the Actual column are the min and max values from the range of values found along the differential pair -- similar to the way single ended impedance is reported.

Please share how you're using this new capability in the SPB16.3 release.

Jerry "GenPart" Grzenia


By FoxVictorWang on September 28, 2010
Thanks.but I have a question, why the result is difference between using the cross -section calculate the impedance and using the Analyze -Transmission line calculator , and different between Si9000

By Jerry GenPart on September 28, 2010
Hi Victor,

I asked one of our PCB SI experts and here's what they about your question -

The cross-section impedance is calculated with the field solver, so it will be more accurate than the Transmission line calculator, which uses empirical formulas to calculate the impedance. I can't comment on why it might be different from Si9000, since this is not our tool. I do not know how they calculate impedance.


By Juniper on October 10, 2010
Most of PCB shops we are dealing with use Polar tools to create stack-ups for the required impedances. I'm also seeing the difference in the results between Polar SI9000 and Allegro cross-section. It would be very helpfull if Cadence can provide an appnote of comparing these two tools and how to tweak the parameters (ie dielectric thickness or etch factor) in cross-section to get the same results as Polar

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.