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.
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
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
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.
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