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.
I want to short two nets (analog and digital ground) by a via. In schematic, how can I create such symbol which has one pin but attaching two different nets?Thanks in advance!
I don't know about in the schematic, but you can attach the "Net Short" property to the via in the board file.
Here is the source link solution number 11144408.this does work I have used it for a few years.Problem statement: I am creating my schematic design in Capture and using Allegro for my board layout. I have two nets "GND" and "AGND" in the schematic. I want to be able designate a specific point in the board layout where I will allow these two nets to be shorted (without generating a design rule error marker). I know how to use NET_SHORT in the ConceptHDL-to-Allegro flow to accomplish this. Can NET_SHORT also be used in the Capture-to-Allegro flow and, if so, how do I do this? Solution: You can use NET_SHORT in the Capture to Allegro flow also.In the following example I have a one pin component in my Capture schematic. The sole purpose of this one pin "component" is to provide a point where net "AGND" will be allowed to short to net "GND". The component has a reference designator of SP1 and a PCB Footprint of SHORTINGPOINT. Pin one of SP1 is tied to net "GND".1). Add the NET_SHORT propertyAdd the NET_SHORT property to the pin of the component instance. Take care to be sure to select the pin of the component rather than the attached wire or the component itself.Make the value of the NET_SHORT property GND:AGND. The first netname in the value string is the net that the pin is connected to (GND in this case). The second netname in the value string is the net (AGND) that I wish to allow to short to GND at this point. The netnames are separated by a colon.2). Set up the allegro.cfg fileSave the schematic and select Tools -> Create Netlist -> Allegro. Before netlisting select the Setup button on the Create Netlist form and choose the allegro.cfg file to be edited. The allegro.cfg file is loaded into a plain text editor. Locate the section called [pinprops] typically towards the bottom of the file. Add the line NET_SHORT = YES to this section. Save the allegro.cfg file and OK the Setup form. Then run the netlister by OK'ing the Create Netlist form.3). View the results in AllegroAfter netlisting is completed successfully, import the netlist into the Allegro board. Place component SP1 and place other components including pins of the net AGND. With Bubble Mode set to Off (instead of Hug Preferred or Shove Preferred) start a cline (add connect) at an AGND pin and draw the cline into the pin of component SP1. No DRC marker is reported even though the cline is on net AGND and the pin of SP1 is on net GND. Allegro ignores the violation because of the NET_SHORT property.Steve
Quite useful! Thanks a lot!
A further question is, the solution suggested by Swilber is only useful for shorting two nets on routing layer, how to make it work on power plane? Thanks!
What I do is create a test point footprint called shortpoint.Place a 1 pin connector for each (shape) point you want to short together in the schematic,such as Agnd and Dgnd and assign the shortpoint footprint to that part.Then I assign the net_short property as described previously.Place the footprint on the board. There are a couple of problem in allegro. 1) the second plane (positive) does not automatically connect. 2) You must go use a Cline that goes from the shape to the short point footprint. 3) And if you edit or connect to those planes the shortpoint cline is removed, (so I connect the shortpoint cline just before I generate the artwork).Steve