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'm currently simulating a big mixed signal block, consisting of two big blocks. The instance block I0 is
pure digital logic, instance I1 is mainly analog but also includes some digital parts. I'm using Ultrasim
for verification but due to the analog parts I'm forced to use a quite strict accuracy setting to get the
results about right. However this setting is killing the digital part ...
I know that some other simulators offer the possibility to define accuracy levels for each instance in
a design, e.g. set I0 to Digital Fast and I1 to Analog. Is something like this possible with Ultrasim ?
This can be done in the hierarchy editor. Create a config view (File->New->CellView and pick your lib cell view and set the Type to be "config". Then when this opens, hit Use Template and pick "spectre". Make sure that the top cellView is pointing to your schematic and OK that form.
You'll then get a Table view showing Cell Bindings and a Tree View showing instance bindings - this is how you control which views are used for each cell or instance with greater control than just a view list and stop list which is applied everywhere.
For Ultrasim usage, use View->Properties. You'll see some additional columns appear in the table and tree view, including sim_mode and speed. You can click on these for a particular cell, or a particular instance. sim_mode is a cyclic with the various sim_mod choices (e.g. s, a, ms, da, df, dx) - and you can also set the speed.
Save your setup, and then you can hit the Open button in the hierarchy editor to open the configured schematic, From here, launch ADE (you'll see ADE shows the config as being the view being simulated) and then if Ultrasim is the simulator, it will take this information and add it to the netlist so that Ultrasim knows the per-cell or per-instance mode and speed settings.
Hope that helps,
In reply to Andrew Beckett:
Thank you very much. Found it and trying it right now.
However I'm puzzled by one simulator output. Even though I set one instance to df and one to s
the device model statistics reports only devices set to spice. Shouldn't there also be devices listed
that are set to df ? I'm using MMSIM 12.11.115
In reply to baenischfau:
I suggest you contact customer support - I don't have time to check this out myself right now.
Hi Andrew, I am currently using AMS simulator with ultrasim solver. I have a question. If I mention sim_mode and speed for a sub-block which is digital block(verilog view) then will this digital block solved by analog(ultrasim) solver, or the simulator will just ignore the sim_mode and speed option specified for this block and block will be simulated by digital solver? And for a analog block I do not mention any of sim_mode or speed, then what is the default mode the simulator will consider?
In reply to Jagdish23:
You probably should have started a new thread, but any settings for a digital block will be ignored (this doesn't influence the partitioning between the two solvers). If you don't specify the sim_mode or speed, then it will use whatever has been set on Simulation->Options->FastSPICE (UltraSim) on the Main tab.
Not sure if this was resolved, but for anyone else coming across this, there is actually a magic button that you have to set to make this work.
After you set the config view the way you like it, go back to ADE (or ADEXL) and go to Simulation->Options->FastSpice->Miscellaneous. Click "Allow usim_opt in HED." Now it should work.
Also, the option directly above allows you to specify usim_opt's on the schematic instead. For example, you can "q" schematic instances and add a user variable "usim_opt" and specifying strings like "sim_mode=s speed=1"...
For what it's worth, in simulating large mixed signal designs with Ultrasim, another critical option for me was judicious use of the "Voltage regulator" option if you have any VR's, or in my case, for power gating switches. From what I understand, this is because Ultrasim is not able to take advantage of the simplified MOS models if it doesn't see sources of devices connected to stable supplies (like vdc's or gnds), so the 1000's of digital transistors connected to a power switch (or VR) will be simulated at much higher accuracy than they need to be. When I finally realized I should apply this option, I received a very large speed-up.