Cadence® system design and verification solutions, integrated under our System Development Suite, provide the simulation, acceleration, emulation, and management capabilities.
Verification 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.
Get email delivery of the Cadence blog featured here
The SPB16.2 release now has new MOSFET device Model BSIM4 Support in PSpice
PSpice designers had been requesting support for the BSIM4 Mosfet Model. The BSIM4 model addresses the MOSFET physical effects into sub-100nm regime. It is a physics-based, accurate, scalable, robust and predictive MOSFET spice model for circuit simulation and CMOS technology development.
BSIM4 finds wide application in RF circuits since it's a physical device model.
The BSIM4 model supported by PSpice is BSIM4 version 4.1.0. To use the BSIM4 equations you need to use the keyword LEVEL=8 inside the model file.
Here's an example:
.MODEL N1 NMOS+Level=8+VERSION = 4.1.0
As specified by University of California, Berkeley, BSIM4 has the following major improvements and enhancements over BSIM3 model:
1. A new accurate channel thermal noise model and a noise partition model for the induced gate noise.
Complete noise model includes flicker noise (also known as 1/f noise), channel thermal noise and induced gate noise and their correlation, thermal noise due to physical resistances such as the source/ drain, gate electrode, and substrate resistances, and shot noise due to the gate dielectric tunneling current.
2. An accurate gate direct tunneling model
In BSIM4, the gate tunneling current components include the tunneling current between gate and substrate (Igb), and the current between gate and channel (Igc), which is partitioned between the source and drain terminals by Igc = Igcs + Igcd. The third component happens between gate and source/drain diffusion regions (Igs and Igd).
The figure below shows the schematic gate tunneling current flows.
3. A better model for pocket-implanted devices in Vth, bulk charge effect model, and Rout
BSIM4 uses Abulk to model the bulk charge effect. Several model parameters are introduced to account for the channel length and width dependences and bias effects.
Abulk is formulated by
4. An asymmetrical and bias-dependent source/drain resistance, either internal or external to the intrinsic MOSFET, at the user’s discretion
BSIM4 models source/drain resistances in two components: bias-independent diffusion resistance (sheet resistance) and bias-dependent LDD resistance. Accurate modeling of the bias-dependent LDD resistances is important for deep submicron CMOS technologies. In BSIM3 models, the LDD source/drain resistance Rds(V) is modeled internally through the I-V equation and symmetry is assumed for the source and drain sides. In addition, BSIM4 allows the source LDD resistance Rs(V) and the drain LDD resistance Rd(V) to be external and asymmetric (i.e. Rs(V) and Rd(V) can be connected between the external and internal source and drain nodes, respectively; furthermore, Rs(V) does not have to be equal to Rd(V)). This feature makes accurate RF CMOS simulation possible.
The following figure shows the schematic of source/drain resistance connection
5. The quantum mechanical charge-layer-thickness model for both IV and CV
As the gate oxide thickness is vigorously scaled down, the finite charge-layer thickness can not be ignored . BSIM4 models this by accepting two of the following three as the model inputs:
the electrical gate oxide thickness TOXE,
the physical gate oxide thickness TOXP,
and their difference DTOX = TOXE - TOXP.
Based on these parameters, the effect of effective gate oxide on IV and CV is modeled.
6. A more accurate mobility model for predictive modeling
A good mobility model is critical to the accuracy of a MOSFET model. Mobility depends on the gate oxide thickness, substrate doping concentration, threshold voltage, gate and substrate voltages. BSIM4 provides three different models of the effective mobility. The mobMod = 0 and 1 models are from BSIM3v3.2.2; the new mobMod = 2, a universal mobility model, is more accurate and suitable for predictive modeling.
7. A gate-induced drain leakage (GIDL) current model, available in BSIM for the first time
The Gate induced drain leakage current and its body bias effect are modeled by
where AGIDL, BGIDL, CGIDL, and EGIDL are model parameters .CGIDL accounts for the body-bias dependence of IGIDL.WeffCJ and Nf are the effective width of the source/drain diffusions and the number of fingers.
8. Different diode IV and CV characteristics for source and drain junctions
Junction Diode IV Model
In BSIM4, there are three junction diode IV models:
1. When the IV model selector dioMod is set to 0 ("resistance-free"), the diode IV is modeled as resistance-free with or without breakdown depending on the parameter values of XJBVS or XJBVD.
2. When dioMod is set to 1 ("breakdown-free"), the diode is modeled exactly the same way as in BSIM3v3.2 with current-limiting feature in the forward-bias region through the limiting current parameters IJTHSFWD or IJTHDFWD; diode breakdown is not modeled for dioMod = 1 and XJBVS, XJBVD, BVS, and BVD parameters all have no effect.
3. When dioMod is set to 2 ("resistance-and-breakdown"), BSIM4 models the diode breakdown with current limiting in both forward and reverse operations.
In general, setting dioMod to 1 produces fast convergence.
Junction Diode CV Model
Source and drain junction capacitances consist of three components: the bottom junction capacitance, sidewall junction capacitance along the isolation edge, and sidewall junction capacitance along the gate edge. An analogous set of equations are used for both sides but each side has a separate set of model parameters
Typical BSIM4 characteristics
IV Characteristics :
a) Ids vs. Vds @ Vgs=1.5V (deep-inversion) Vbs sweep
b) Ids vs. Vds @ Vbs=0.0V; Vgs sweep to test Impact-ionization
CV Characteristics :
Cgd vs. Vgd @ CAPMOD=2 (Vbs=0.0; Vgs=1.0 and 2.0)
So, how many AMS Simulator designers will be taking advantage of these new model capabilities? I'm interested in hearing from you.
Hi vijayakumar s
Your question may best be answered by contacting our Customer Support team at http://support.cadence.com and filing a new Case.
Hello sir..can anybody say how to create symbol of spatial wave function feild effect transistor (swsfet) from bsim model in orcad pspice.....please help sir.......
Hi sita - it's best if you contact one of your local Cadence Customer Support AEs who can assist you with this. Please file a new case at - http://support.cadence.com.
Hi ,where can i download >lib file for BSIM models.I need for my simulation.Please help me.
Currently, there is no direct method to plot a CV plot for MOSFETs in PSpice. One possible way is to create a circuit where one of the node voltages or branch current (or
it's expression) represents the Capacitance. Now you can plot this node voltage or current to get the desired plot.
I am trying to create a pspice model (pretty basic, level1or2 may be) for my mosfet, from the results obtained from SILVACO device simulator. How do I cross-check parasitic capacitances? I cannot generate CV plot by ramping up DC voltage (VGS). Is there any way I can do that? Or any other method where by I can set ac parameters???