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.
Can anyone please help me with a very simple circuit of three capacitors in series. Attaching its netlist below:
// Library name: FloatingGate // Cell name: cap //
View name: schematic
C8 (net5 0) capacitor
C10 (net05 0)
capacitor c=1p ic=1
C11 (net5 net05)
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27 \
tnom=27 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 \
digits=5 cols=80 pivrel=1e-3 sensfile="../psf/sens.output" \
tran tran stop=1 errpreset=moderate
writefinal="spectre.fc" annotate=status maxiters=5
finalTimeOP info what=oppoint where=rawfile
modelParameter info what=models
outputParameter info what=output
designParamVals info what=parameters
subckts info what=subckts where=rawfile
saveOptions options save=allpub
With my knowlegde of circuit and experience on spice simulator of Tanner, I expect net5=1v and net05=1v
However, Output in cadence the voltage at net5 and net05 start with 1v and decreased exponentialy wo zero.
The capacitor is enable to retain its charge.
This issue looks simple but it is creating issue in all my designs, which are working well in TSpice.
Please help me
Hopeful for quick reply from some expert
This is because of the gmin conductance that is added from floating nodes to ground. Nodes in reality are never entirely floating - there's always some leakage path. The issue is for a circuit simulator, that floating nodes can cause a convergence problem, because it leads to an ill-conditioned matrix (effectively there are potentially an infinite number of solutions for a floating node). To help with floating nodes and off junctions, spectre inserts a gmin conductance to ground (for floating nodes), or across the off junction. The default value of gmin is 1e-12 Siemens (i.e. 1e12 ohms) - and is explicitly stated in your netlist. With a 1pF cap, that's a 1 second time constant - hence, the decay you're seeing over a 1 second simulation. You could set gmin=0 in this case (Simulation->Options->Analog in ADE, or the simulatorOptions line in the netlist above), and you'll then get no decay, but be warned in general gmin helps avoid convergence problems (most circuit simulators do similar things; this is not unique to spectre).