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.
Get email delivery of the Cadence blog featured here
The testbench is shown in Figure 1. The base of the bipolar transistor, the DUT, is grounded. The collector of the transistor is connected to a dc source, VBC, which is used to set the base-collector voltage of the transistor. The emitter is connected to a current source that sets the bias current, IE. An additional supply, VBE, is included to assure the base-emitter junction is always forward biased. For these tests, the dummy power supply voltage, VBE, is set to 5V.
Figure 1: Ft Testbench modified for fixed Vbc
To measure the ft, use the same methodology previously described:
1. Run a dc operating point analysis and save the collector current
2. Run an ac analysis, sweep the frequency beyond the maximum value of ft
a. In this case, the ac sweep was from 1Hz to 10GHz
b. Save the base and collector currents
3. Use the Virtuoso ViVA waveform calculator to measure the ac beta of the transistor
a. The ac beta is ic/ib, where ic and ib are the ac currents
4. Use the Virtuoso ViVA waveform calculator cross() function to measure the ft
a. Measure the frequency where the value of the ac beta=1, or 0dB
5. In Virtuoso Analog Design Environment, ADE, setup a parametric plot to sweep the emitter current
a. In this case the emitter current was swept from 100nA to 10mA
6. Run Parametric Analysis
7. Plot the collector current and the ft when the analysis completes
8. Use the Y vs Y option to plot the ft vs the collector current
Shown below is an example of the ft curves for the NPNupper transistor model used in the rfLib. The ft was measured for current sweeps using different values of Vbc: 0.5V, 1.0V, and 1.5V. As you can see, increasing the base-collector voltage delays the onset of saturation and allows the transistor to achieve higher ft.
Figure 2: ft vs Ic for a fixed Vbc
Please let me know if this post was useful, if you have any questions, or comments.
You can generate the same set of curves, and others quickly in a spreadsheet, by using the model's SPICE parameters. We know that fT = 1 / 2pi ( CJE VT/Ic + tau-F ), and we get the transit time tau-F from the SPICE-engine formula tau-F = TF * [ 1+ XTF * (Ic/Ic+ITF)^2 * exp (Vbc/1.44*VTF) ] entered into the spreadsheet cells. CJE, TF, ITF, VTF and XTF are the SPICE parameters.
Very useful test bench. Just a minor comment on the name "VBE" chosen for the 5 volt dummy supply. Let us call it VEE and reserve the VBE name for the bipolar device's voltage difference VBE = VB - VE (e.g. 0 V -(-0.7 V) = 0.7 V. The NPN is biased with an emitter current, so the voltage absorbed by the current source is VEE - VBE.