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 am trying to get an idea as to what a device model parameter represents.
Can anyone please suggest where i can get the list for it.
I am specifically looking for the parameters like mobility, Cox,
subthreshold factor, TC of threshold voltage, Vth0 of the device etc.
Also i am trying to plot the threshold voltage of a device as per my DC sweep parameter. Can anyone please tell me how should i do that?
Did you consider reading the documentation? There's a whole manual on the device model equations, plus documentation on the parameters available for each mode. Run "cdnshelp" from <MMSIMinstDir>/tools/bin to get to the documentation.
If you want to plot the threshold voltage, the best thing to do is to create an include file, called (say) save.scs with the contents:
and then reference this file from Setup->Model Libraries or Setup->Simulation Files. Then you can see this parameter from the Results browser after your dc sweep. Of course, change M1 to be whatever the device name is in your case.
In reply to Andrew Beckett:
I went through this thread and am interested in plot vth through DC sweep. But I received this warning：
WARNING (SPECTRE-8282): `M1a' is not a device or subcircuit instance name.
WARNING (SPECTRE-8287): Ignoring invalid item `M1a:vth' in save statement.
WARNING (SPECTRE-8282): `M6' is not a device or subcircuit instance name.
WARNING (SPECTRE-8287): Ignoring invalid item `M6:vth' in save statement.
I am sure the name is correct and is copied from schematic instance name field.
Do you know how to fix it?
In reply to Alex Liao:
Presumably the name is not correct, or you've not given the correct hierarchical path to the instance. Look at the netlist itself - that's the best bet.
You can refer my snap cut. The naming is correct. I do not know how to check that hierarchical path. But the netlist is enough I think.
The transistors you're trying to save the vth for are inside the _sub0 subckt, and you didn't tell it the hierarchical path to them. Since there is only one instance of that subckt, ie instance I0, you'd need:
(assuming that the model pch is not a subckt itself).
In my case I have seen that subckt _sub0. But wher is the instance info? As you exampled, the instance I0, what is the only instance name in my design from previous snapshoot?
All I did was read your netlist in your post. It's not difficult!
I have no warning now. I assume that I have saved vth of M6 by including "save I0.M6.vth". But this thread mentioned plot this variance by DC sweeping. How can I plot it with the help of result browser. You can point it out direct in this figure .
Firstly it would be "save I0.M6:vth" (note the colon) - check the spectre output as it will tell you if you have got it wrong.
Secondly, you're looking at the dcOp output there, not the dc sweep output. That's the (initial) DC operating point. You'd need to look in the "dc-dc" output in the results browser, and then you should be able to plot a waveform of I0.M6:vth versus the swept parameter.
Thank you so much. Now I have my desired plot.
I am trying to plot Vth vs L like the same manner as described in your post. I gave a variable name in length field of transistor and chose dc analysis. In that i selected design variable as sweep variable and added the variable name. But when im running the simulation i am getting the following error. Even if i give save M0:vth , im getting error and in the results browser (dc-dc) there is no Vth of the tansistor. Please help me in this regard.
In reply to Arjun RP:
Please read the forum guidelines - these tell you not to double post (especially when you already have your own thread on this subject). I answered your other post here.