• Skip to main content
  • Skip to search
  • Skip to footer
Cadence Home
  • This search text may be transcribed, used, stored, or accessed by our third-party service providers per our Cookie Policy and Privacy Policy.

  1. Blogs
  2. RF Engineering
  3. Measuring Transistor fmax
Art3
Art3

Community Member

Blog Activity
Options
  • Subscribe by email
  • More
  • Cancel
CDNS - RequestDemo

Try Cadence Software for your next design!

Free Trials

Measuring Transistor fmax

7 Dec 2010 • 3 minute read

There were several questions about measuring transistor fmax in comments posted to my previous Measuring Transistor ft and Simulating MOS Transistor ft blog posts. So in this posting we will look at simulating transistor s-parameters and device characteristics including fmax, noise, and distortion. There are two parts to the characterizing a device -- creating the testbench and performing the measurement.

First, we will look at creating a testbench to measure transistor s-parameters. While we can't directly use the ft testbench to measure s-parameters, it will serve as the basis for the s-parameter testbench. The current feedback loop from the ft testbench will be used to define the transistor's dc operating point. Then we will add ports to the testbench in order to measure the transistor's s-parameters. The ports define the reference impedance and the port number for s-parameter analysis. The complexity is that we need to isolate the current feedback to stabilize the dc operating point from the ports used for s-parameter analysis. To isolate the dc and the ac signal paths, the dc paths include shorts and the ac paths include capacitors. The corner frequency of LC network is set low enough so that frequency sweeps can be performed from frequencies as low as 1Hz (see Figure 1).

 fmax testbench

 Figure 1: fmax Testbench

Next, let's talk a little bit about how to perform the fmax measurement using Virtuoso Analog Design Environment (ADE). We will use Spectre's s-parameter analysis to simulate the transistor's s-parameters and then calculate fmax from the s-parameter data. We will calculate the fmax from the s-parameters using Mason's Unilateral Power Gain. Let's look at the process step-by-step.

1)       First, we will perform s-parameter analysis. We will start by selecting the input and output ports, in this case port1 and port2.

  S-parameter Analysis

                     Figure 2: Setting Up s-parameter analysis

2)      In order to improve the accuracy of the measurement, we will use 100 points/decade instead of the default value, 20 points/decade. Increasing the number of points reduces the interpolation error when we make the fmax measurement using the cross() function.

3)      ADE can calculate the Unilateral Power Gain from the device's s-parameters. The Maximum Unilateral Power Gain measurement is available from either of the following options:

a.        From ADE select Results --> Direct Plot --> Main Form..., then in the sp analysis section choose Gumx

 

 Direct Plot Form dialog box

 

                            Figure 3: S-parameter Direct Plot

b.      From ADE select Tools --> Calculator...,  then select gumx from RF functions

4)      In our case, we will use the ViVA Calculator because we want to know the frequency now that the Unilateral Power Gain is 0dB. This measurement can be done using the cross() function. In this case, we have saved Maximum Unilateral Power Gain and the fmax measurement, and the cross(dB10(Gumx() 0 1 "falling" nil nil) as outputs in ADE.

  VIVA Calculator

 

Figure 4: ADE with fmax measurement

5)      If you have ever done the measurement in the lab, you probably did not measure the 0dB crossing -- you extrapolated from a higher level to the 0dB crossing due to measurement noise. Simulating fmax is different than measuring fmax and as a result, when simulating, we can directly measure fmax. We do not need to extrapolate to estimate the 0dB crossing as you would in the lab.

6)      On the other hand, the accuracy of the fmax simulation is affected by how well you model the actual device. For example, using a BSIM4 model with gate resistance, substrate resistance, ...

Once the simulation is complete we can begin to measure the fmax from the Gumx gain plot (see Figure 5).

 

 Gumx Gain Plot

 

Figure 5: Calculating fmax from Gumx

Using ADE's Parametric Plotting function (see the Measure Twice, Cut Once post for details) we can sweep the operating conditions and see the effect on fmax (see Figure 6). Designers can use this information to optimize the speed/performance of their design.

ADE's parametric plotting function

 

Figure 6: fmax vs. collector current

To review, in this post we have looked at how to simulate the fmax of a transistor. This testbench and methodology is based on s-parameter simulation. Any transistor parameter that you might wish to measure using s-parameters can be simulated -- for example, noise figure or IIP3.  

I hope you found this post useful. Please let me know if you have any questions.

Best Regards,

Art Schaldenbrand

Related Resources:

  • Virtuoso Analog Design Environment
  • Virtuoso ADE Product Suite

CDNS - RequestDemo

Have a question? Need more information?

Contact Us

© 2025 Cadence Design Systems, Inc. All Rights Reserved.

  • Terms of Use
  • Privacy
  • Cookie Policy
  • US Trademarks
  • Do Not Sell or Share My Personal Information