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.
using MMSIM 6.2 to run some Spectre simulations and I am having some
unexpected problems with the results. I am simulating files
netlistTRAN022.1x1.saveselected.PHC.scs. The only difference between
these files is the following options statement:
saveOptions options save=all pwr=all currents=all useprobes=yes
saveOptions options save=selected currents=selected useprobes=yes
but simulation results for the saved signals are completely different
depending on the scs file I run. As far as I understand, the above
options statements should not change the results of a simulation, only
the signals to be saved to HHDD, am I right?
Do you know which could be the problem?
If you take a look at the spectre output log file, in particular in the circuit inventory, you'll see a difference (I suspect) in the number of iprobes appearing in the circuit. This alters the size of the matrix being solved, and consequently it can affect the convergence. Normally the results may be very slightly different, but if bigger, it is normally indicative of the fact that you may have multiple stable operating points in your circuit (rather like hysterisis in a comparator, but it could be other things).
In the Simulation->Options->Analog you can enter "subcktiprobes=no" in the additional parameters field at the bottom of the form. If you do this it uses an alternative method for measuring currents (although I think if you set useprobes=yes it may stop this and still use iprobes). Is there a particular reason why you're using useprobes=yes? (it's normally only needed for currents in AC-type analyses).
In reply to Andrew Beckett:
Thank you very much Andrew, it looks like the problem was the useprobes option (I inhereted the script from another designer and, although I didn't need it, I thought that the useprobes option was harmless for my simulations...looks like I was wrong...again...:) ).
By the way, I have another problem. The circuit I am simulating is quite big, and if I use the save=all or save=allpub a file of 50GB is generated as the output of a tran analysis. If I select just a few signals of interest to be saved and use save=selected option the file is much smaller, but still measured in GB (about 7 - 8). The problem is that when I try to view the results with wavescan or ocean, sometimes, the application can not handle such big files. Do you know a way to overcame this problem?...maybe there is a way to separate the saved signals in several files instead of just only one...
In reply to yoyega:
See sourcelink solution 11264780
If using IC5141, then you'll need to do:
setenv PSF_WRITE_CHUNK_MODE_ON true
Thank you very much to both for your replies. I'm trying to consult sourlink solution 11264780 but it looks like I have a problem with my log in...I will try to solve it via cadence support...