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.
Dear all, I'm using freq_meter component from ahdlLib
to calculate instantaneous frequency of an oscillator. While doing
Spectre simulation, I'm getting the error as ========================================================== Error found by spectre at time = 20.6089 ns during transient analysis `tran'. Signal FF(FREQ_OUT) = 2.18688 GHz exceeds the blowup limit for the quantity `FF' which is (1 GHz). It is likely that the circuit is unstable. If you really want signals this large, set the `blowup' parameter of this quantity to a larger value. ========================================================== Please let me know how to resolve this issue.
Take a copy of the freq_meter model, and change the section at the top which creates a nature Frequency to the following:nature Frequency abstol = 1; access = FF; blowup = 1e12; units = "Hz";endnatureThe default blowup is 1G, which is a little small if you're measuring frequencies around 1GHz. Note I also increased abstol, since the accuracy requirements shouldn't be so tight if you have GHz signals. Even 1 might be a bit small (normal practice is to set abstol to a millionth of a typical signal level).Regards,Andrew.
Hi,I normally find no fault with Andrew's contributions, but I would like to point out that propagating an altered copy of a quasi-standard device from a common library can cause problems if you ever share your schematic with others that don't have access to where you placed the altered copy. Fortunately, there is another solution which avoids this problem!Here's the steps:1. Create a small text file that contains the following lines. simulator lang=spectre
defineLrgFreq quantity \ name="FF" \ units="Hz" \ abstol=1e-3 \ description="Frequency in Hz" \ huge=100e92. Save the file with a name like "frequency_nature.scs" in a path that would be accessible to anyone that may end up using your schematic.3. In ADE, do Setup->Simulation Files... Add the path of the file in Include Path and the name of the file in Defintion Files.Now, just leave the freq_meter as is and referenced from the standard ahdlLib. Netlist and Run will produce a netlist that lets the freq_meter operate at a higher frequency! Then save a state so that others can recall it and get your modification included already.
My practice is to make a local library for the modified elements from bmslib.. and any new ones I create.. so my first step in making a mod is to copy from bmslib to my local (corporate) lib and make the changes.. so if they instantiate from the standard lib they get the standard one, otherwise they the the corporate verilog-A/AMS block.(which is, of course, under revision control) jbd