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.
The Cadence Academic Network helps build strong relationships between academia and industry, and promotes the proliferation of leading-edge technologies and methodologies at universities renowned for their engineering and design excellence.
Participate in CDNLive
A huge knowledge exchange platform for academia to network with industry. We are looking for academic speakers to talk about their research to the industry attendees at the Academic Track at CDNLive EMEA and Silicon Valley.
Come & Meet Us @ Events
A huge knowledge exchange platform for academia. We are looking for academic speakers to talk about their research to industry attendees.
Americas University Software Program
Join the 250+ qualified Americas member universities who have already incorporated Cadence EDA software into their classrooms and academic research projects.
EMEA University Software Program
In EMEA, Cadence works with EUROPRACTICE to ensure cost-effective availability of our extensive electronic design automation (EDA) tools for non-commercial activities.
Apply Now For Jobs
If you are a recent college graduate or a student looking for internship. Visit our exclusive job search page for interns and recent college graduate jobs.
Cadence is a Great Place to do great work
Learn more about our internship program and visit our careers page to do meaningful work and make a great impact.
Get the most out of your investment in Cadence technologies through a wide range of training offerings.
Overview All Courses Asia Pacific EMEANorth America
Instructor-led training [ILT] are live classes that are offered in our state-of-the-art classrooms at our worldwide training centers, at your site, or as a Virtual classroom.
Online Training is delivered over the web to let you proceed at your own pace, anytime and anywhere.
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.
Get email delivery of the Cadence blog featured here
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