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.
Hey all.I am trying to create models for two different circuit components. The first is a single pin test node. Basically the schematic symbol has one and only one pin. I need to create a espice or ibis model of this and have been having a really tough time. All I really want this to be is a small capacitiance to ground. This seems to be quite elusive.The second model I am trying to create is for a rnet. The schematic symbol has three sections. Two sections of bussed resistors and one section of power pins. For some reason when I try to apply a si model to any one section I cant "hook it up" to the other sections or to VCC. Some help here??Matt Skogmo
Hi Matt,Some times it's the little custom things that are the hardest.We likely need you to clarify a couple things before we're able to answer.1) Are you working in SigXp or PCB_SI? I'm guessing PCB_SI?2) The second question is not clear. Maybe we need a diagram? ...or at least more description.Donald
Donald, We use both SigXp and PCB_SI. At this point, we are extracting the net topology off of the schematic through constraint manager. When we try to extract any net that has one of these test nodes, SigXp complains that all discrete components need models and bails out.I am including a little .gif of the resistor nets. In this particular shot, the three components are labeled RN1,2,3 but in reality, they would all be part of the same network... Notice the pin numbers.
Matt:If you need to model the test point, you can create an IBIS model using the CDSDefaultProbe and add a package capacitance that corresponds to the capacitance of the pad which you can calculate from the parallel plate capacitance formula using the Area, Dk, and distance to the adjacent plane. Use some small value for R and L. This works OK but slows down your simulations if you are running long lists of nets as the tool will now be trying to measure the signal at the test points and since the default probe has no thresholds, you will get NAs for most of the parameters in the reports. If you can determine the test point is negligible, it is better to change the test points to type IO from type IC (which they usually are) and then they will appear as a connector and not be used in the simulation. I think you are asking how to create an espice model of a resistor pack that has common pins. The sourcelink doc describes this but here is a sample for a 10 pin with pins 5 and 10 common.("RN_51Ohm" ("ESpice" ".subckt RN_51Ohm 5 1 2 3 4 6 7 8 9 10R1 1 5 51R2 2 5 51R3 3 5 51R4 4 5 51R5 6 5 51R6 7 5 51R7 8 5 51R8 9 5 51.ends RN_51Ohm") ("PinConnections" ("1" "5" "10") ("2" "5" "10") ("3" "5" "10") ("4" "5" "10") ("6" "5" "10") ("7" "5" "10") ("8" "5" "10") ("9" "5" "10") ))
Why would you create two logical parts from 1 physical part? Why not call RN1 the whole 10 pin resistor network. Your BOM will be very interesting and you will have 2 logical symbols for 1 physical symbol.
Perhaps I chose a poor picture. The way the library part is designed, there are three sections, one section for the "common pins" one section each for the resistor nets. I understand how to make an espice device if the part is all together on one symbol... just like your previous post showed. However if I were to try to stick that espice part onto one of my resistor nets, the pins would not match up because the symbol is logically different than the espice model. Another picture included to try to clarify... Note all are RN1
Hi, Matt,Per your last explanation, you will have to model RN1 all 10 pins in one discrete part in order to be extracted into Sigxp successfully.Here is the espice part for it:.subckt RN1 1 2 3 4 5 6 7 8 9 10x5_10 5 10 2pinsx1_2_3_4 1 2 3 4 4pinx6_7_8_9 6 7 8 9 4pin.subckt 2pin 1 2r5_10 5 10 4.7k.ends 2pin.subckt 4pin 1 2 3 4 ra 1 99 4.7krb 2 99 4.7krc 3 99 4.7krd 4 99 4.7k .ends 4pin.ends RN1I assume the common node for 4pin is not connected to GND. Otherwise, you need to change node 99 to 0also, you might want to make sure DML Pin Connection lists correct connection combinations. This will beef up the extraction performance as well.Hope this helps,Lance WangIO Methodology Inc.