Home > Community > Blogs > RF Design > simulating mos transistor ft
 
Login with a Cadence account.
Not a member yet?
Create a permanent login account to make interactions with Cadence more conveniennt.

Register | Membership benefits
Get email delivery of the RF Design blog (individual posts).
 

Email

* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

Simulating MOS Transistor ft

Comments(14)Filed under: RF design, bipolar transistor, MOS transistorOne other question that you might ask is, this approach works for bipolars but what happens when you need to characterize a MOS transistor. Nothing changes, use the same testbench and measurements, see figure 1. In this testbench a MOS transistor is being compared to a bipolar transistor.


Figure 1: MOS and BJT Comparison


The simulation results are shown in Figure 2. The difference in the results is that the low frequency bipolar transistors current gain is limited by the base current, while the MOS transistor current gain is not limited. Note, in advanced node processes, MOS transistors do have significant gate leakage and the plot for the MOS transistor would look more like the plot for the bipolar transistor.


Figure 2: Comparison of current gain


So the same techniques that you would to characterize a bipolar transistor and also be applied to MOS transistor.

Comments(14)

By Guy on November 9, 2008
Hi,Can you send me a zoom for figure 1? I can't see device parameters in this screen. My email: guysari@gmail.com

By yves dufour on November 14, 2008
Hello, Allow me to react on the previous comment, Can you please add the netlist in the article so we can reproduce the analysis.  Thank you.Yves

By Yutao Liu on April 26, 2009
I don't understand which component you place between the gate terminal of the MOS and ground. It seems that it is not included in analoglib in spectre, right?

By Art Schaldenbrand on April 27, 2009
Yutao,
  The components is the current-controlled, current source, cccs, from the analogLib.
                                                                                                        Best Regards,
                                                                                                            Art Schaldenbrand

By Art3 on April 27, 2009
Hi,
  Sorry I should have posted the netlist sooner, it would have
avoided a lot of confusion for everyone.
                                                                     Best Regards,
                                                                        Art Schaldenbrand
simulator lang=spectre
global 0
parameters ICE=100u VCE=5
//
// these model files should be available in the samples directory
//
include "./models/NPNlower.scs"
include "./models/cornerMos.scs" section=TNTP
V0 (net014 0) vsource dc=VCE type=dc
// MOSFET ft
// NOTE: the element instance names have been changed
//            the default names are shown in the bjt section
//            IREFERENCE --> 0V voltage source
//            IFEEDBACK  --> current-controlled, current source
IIN (net014 net9) isource dc=ICE mag=1 type=dc
IREFERENCE (net6 0) vsource dc=0 type=dc
IFEEDBACK (net9 0) cccs gain=1.0 probe=IREFERENCE
NM0 (net014 net9 net6 0) nmos24 w=24u l=1.5u m=10
// BJT ft
I2 (net014 net025) isource dc=ICE mag=1 type=dc
V1 (net012 0) vsource dc=0 type=dc
F0 (net025 0) cccs gain=1.0 probe=IREF_BIPOLAR
Q0 (net014 net025 net012 0) NPNlower
ac ac start=1 stop=100G annotate=status
save NM0:g NM0:d Q0:c Q0:b

By Art3 on May 1, 2009
One more comment,
  Yutao has pointed a limitation of the testbench. This testbench should not be used
when the  Vds of the DUT, transistor is 0. Forcing the transistor to conduct constant current when Vds=0 causes convergence and accuracy issues. In general, this should
not be an issue since testbench is intended to measure the characteristics of devices biased in saturation: ft, gm, gds, ...
                                                                                                       Best Regards,
                                                                                                           Art Schaldenbrand

By greg on July 15, 2009
Hi, i tried to simulate ft of the mosfet.
I tried to rebuild the circuit you list and plot it.
dB20(IF("/M0/D")/IF("/M0/G"))
And it show a error. it can handle nil / nil.
Can you tell me how to simulate correctly? Thanks.

By Art Schaldenbrand on July 17, 2009
Greg,
  Sorry for the delay in replying, I have been at CDNLive! Japan this week.
It was fun but hectic!
  The issue is that the syntax example from the bipolar ft testbench is the
syntax for the bipolar ft schematic testbench simulation. In the testbench
schematic, the DUT is called Q0. In this netlist, the DUT is NM0.  So the
correct syntax would be
  dB20(i("NM0:d" ?result "ac-ac")/i("NM0:g" ?result "ac-ac"))
which matches the format used in the save command.
Also as mentioned in the bipolar append, it is easiest if you actually
build the expression yourself rather than trying to remember the syntax.
For example, if you are using ViVA:
1. Open the Results Browser
2. Select the output data directory, raw/psf/...
3. Select the results, ac-ac
4. Right mouse button on NM0:d and select calculator
5. Right mouse button on NM0:g and select calculator
6. Select divide, "/" from the calculator keypad
7. Select, dB20 from the "Math" functions
  Also, just noticed that there is a typo in the bipolar portion of the netlist.
The probe and the instance name are mismatched. The issue can be
resolved by renaming the instances,
simulator lang=spectre
global 0
parameters ICE=100u VCE=5
//
// these model files should be available in the samples directory
//
include "./models/NPNlower.scs"
include "./models/cornerMos.scs" section=TNTP
V0 (net014 0) vsource dc=VCE type=dc
// MOSFET ft
// NOTE: the element instance names have been changed
// the default names are shown in the bjt section
// IREFERENCE --> 0V voltage source
// IFEEDBACK --> current-controlled, current source
IIN (net014 net9) isource dc=ICE mag=1 type=dc
IREFERENCE (net6 0) vsource dc=0 type=dc
IFEEDBACK (net9 0) cccs gain=1.0 probe=IREFERENCE
NM0 (net014 net9 net6 0) nmos24 w=24u l=1.5u m=10
// BJT ft
IIN_BIPOLAR (net014 net025) isource dc=ICE mag=1 type=dc
IREF_BIPOLAR (net012 0) vsource dc=0 type=dc
IFDBK_BIPOLAR (net025 0) cccs gain=1.0 probe=IREF_BIPOLAR
Q0 (net014 net025 net012 0) NPNlower
ac ac start=1 stop=100G annotate=status
save NM0:g NM0:d Q0:c Q0:b
                                                              Best Regards,
                                                                Art Schaldenbrand

By bVenu on April 29, 2010
Hi Art,
Could you possibly put up a test bench to simulate the Fmax of a transistor too?
Thanks
Venu

By j m wincn on May 29, 2011
The BJT version of the test bench seems clear enough, but I fail to see how the MOS version will return a realistic result.  It's true that MOS devices have Gate-Drain and Gate-Source capacitance, and those elements will pass a measurable signal at sufficiently high frequency.  It's also true that latter-day MOS technology has significant Gate leakage, so there can be a realistic, non-zero, total Gate current value for any MOS device at sufficiently high frequency.  Excess capacitance at the Gate terminal will introduce a bandwidth limit, but MOSFET short-circuit current gain is -not- established by Gate current.  So a simulated ratio of Drain current to "Gate current" may return some kind of numeric result, and that result may not be entirely meaningless but it is not an accurate measure of MOSFET short-circuit current gain and thus not an accurate measure of MOSFET transition frequency.  An accurate measure of transition frequency will require a different set of metrics, for MOSFETs.

By G A S on November 21, 2012
Good afternoon! Can you please explain me, can test bench consist of dc voltage source in the Gate (for biasing) with some voltage AC magnitude parameter, dc voltage source for VDS, and transist frequency is simply measured as ft = (ac drain current) / (ac gate current) without any current sources.
Thanks!

By sreedevi baburaj on January 23, 2013
good afternoon sir.. i simulated a nmos transistor inverter in cadence. can u please tell me what are the values of the parameters of that nmos transistor. i want to know the capacitance (cox), mobility etc... can u tell me where can i find the model fuile

By Tawna on January 23, 2013
Hi folks,
Rather than post questions to blogs posted in the past (2008 in this case), please post new questions to the RF Community forum.  They have a much better chance of getting answered.
Also, you may want to contact http://support.cadence.com (Cadence Customer Support) for in-depth assistance.  
best regards,
Tawna

Leave a Comment


Name
E-mail (will not be published)
Comment
 I have read and agree to the Terms of use and Community Guidelines.
Community Guidelines
The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. 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. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.