• Skip to primary navigation
  • Skip to main content
  • Skip to primary sidebar
  • Skip to footer

Electrical Engineering News and Products

Electronics Engineering Resources, Articles, Forums, Tear Down Videos and Technical Electronics How-To's

  • Products / Components
    • Analog ICs
    • Connectors
    • Microcontrollers
    • Power Electronics
    • Sensors
    • Test and Measurement
    • Wire / Cable
  • Applications
    • Automotive/Transportation
    • Industrial
    • IoT
    • Medical
    • Telecommunications
    • Wearables
    • Wireless
  • Resources
    • DesignFast
    • Digital Issues
    • Engineering Week
    • Oscilloscope Product Finder
    • Podcasts
    • Webinars / Digital Events
    • White Papers
    • Women in Engineering
  • Videos
    • Teschler’s Teardown Videos
    • EE Videos and Interviews
  • Learning Center
    • EE Classrooms
    • Design Guides
      • WiFi & the IOT Design Guide
      • Microcontrollers Design Guide
      • State of the Art Inductors Design Guide
    • FAQs
    • Ebooks / Tech Tips
  • EE Forums
    • EDABoard.com
    • Electro-Tech-Online.com
  • 5G

SPICE: how to choose an analysis

November 13, 2017 By Chris Francis Leave a Comment

SPICE is a very useful tool when used correctly and is used far beyond its original purpose — “Simulation Program with Integrated Circuit Emphasis.” It is now used for simulation of many non-integrated circuits. However, whichever type of circuit you use it for, you need to be aware of its limitations.

The modeling has been changed significantly over the years, as anyone who remembers the original basic MOSFET models will know. The newer models help to better model the smaller geometry devices in integrated circuits as the years progress. Of course, those simulator models are only useful if they match your actual devices. At a more fundamental level, when should you use the different types of simulation and does it matter which you use?

The main simulation types are transient, AC, DC, and noise. Additionally, there are transfer function, operating point and distortion analyses. One common misunderstanding is what the AC analysis does exactly so misinterpreting the results is a risk. An AC analysis is a small signal analysis which analyses the response to a very small input signal. That could be the same as the response to a large signal, but not necessarily. Take the following simple example.

SPICE

The gain should be 20dB. An AC analysis confirms that for low frequencies. At 200kHz the gain has dropped slightly to 19.92dB in the AC analysis because the gain bandwidth of the opamp is only 8MHz. A transient analysis with 0.4V peak-peak input results in 3.94V peak to peak out, compared to 3.96V which would be expected from the AC analysis. So, pretty close.

Here’s another example:

SPICE

This is not a “design” but a simple circuit to illustrate the problem. It is a tuned class C amplifier at around 50MHz. Conduct an AC analysis, and you will get the following:

SPICE

The peak gain is -25dB, so not much of an amplifier. Note that the transistor is biased, so it is turned off with 0.5V on the base. However, conduct a transient analysis with a 1V peak-peak 50MHz sine wave and you will get the following output:

SPICE

So, a peak-peak output of 9.4V – a gain of 19.5dB. The difference between the two simulations is the difference between small signal analysis and large signal analysis. The small signal (AC) analysis doesn’t show how the circuit will be used realistically ( i.e., with a large signal). You could duplicate the AC analysis results with the transient analysis but not the other way round.

If you change the input signal in the transient analysis to 1mV peak-peak rather than 1V, you will see only 57µV of peak-peak output signal. So the “gain” is -25dB or the same as the AC analysis. The reason the results are now the same is that by keeping the input signal very small, we are not altering the biasing of the transistor.

Unfortunately, there is no AC analysis for large signals (although there are tools specific to RF design more suited to such design problems) so you must use a transient analysis. It is not only RF design which will result in large signal problems. An audio amplifier or any circuit working with large signals could have similar problems depending on the design.

So, what of the other types of analysis? DC analysis is purely related to DC signals. You sweep a DC voltage (or a device parameter) and see how it affects the DC voltages in your circuit. A simple example would be the biasing of a transistor.

SPICE

If you sweep the input voltage V2, you will see the output voltage stay at 6V until the transistor starts to turn on when it will then rapidly drop to the saturation voltage. You can see that when V2 is around 0.93V the output voltage is at the mid rail point of 3V.

SPICE

A DC analysis can be useful in trying to work out why a circuit isn’t working as expected, particularly where the problem is the biasing. For example, if you have an amplifier design but it has no gain and/or the output is stuck at 0V or Vcc, a DC analysis could help to track down the error in your design/biasing. Another option is to sweep a resistor value with a fixed voltage. In addition to analyzing biasing, this option could be used to simulate the response of a circuit with a thermistor.

The noise analysis is usually treated as an extension of the AC analysis. It sums all the noise sources in a circuit (resistors and active devices) taking into account where they are in the circuit and the relevant gain (small signal transfer function) at the point at where the noise is injected. A resistor on the output of an amplifier will usually have a lot less effect on the total output noise than a resistor on the input. Some resistors will not contribute to the output noise if their effect is decoupled with a capacitor, for example. In fact, noise analysis is quite a subject in itself so … to be continued.

 

You may also like:

  • multi-level photonic IC
    Software models multi-level photonic IC designs
  • IBIS
    How IBIS models help with signal analysis

  • Getting started in electronics: core equipment
DesignFast Banner version: 03eceadf

Filed Under: FAQ, Featured, Tools Tagged With: basics, FAQ

Reader Interactions

Leave a Reply Cancel reply

You must be logged in to post a comment.

This site uses Akismet to reduce spam. Learn how your comment data is processed.

Primary Sidebar

EE Training Center Classrooms

EE Classrooms

Featured Resources

  • EE World Online Learning Center
  • CUI Devices – CUI Insights Blog
  • EE Classroom: Power Delivery
  • EE Classroom: Building Automation
  • EE Classroom: Aerospace & Defense
  • EE Classroom: Grid Infrastructure
Search Millions of Parts from Thousands of Suppliers.

Search Now!
design fast globle

R&D World Podcasts

R&D 100 Episode 7
See More >

Current Digital Issue

April 2022 Special Edition: Internet of Things Handbook

How to turn off a smart meter the hard way Potential cyber attacks have a lot of people worried thanks to the recent conflict in Ukraine. So it might be appropriate to review what happened when cybersecurity fi rm FireEye’s Mandiant team demonstrated how to infiltrate the network of a North American utility. During this…

Digital Edition Back Issues

Sponsored Content

Positioning in 5G NR – A look at the technology and related test aspects

Radar, NFC, UV Sensors, and Weather Kits are Some of the New RAKwireless Products for IoT

5G Connectors: Enabling the global 5G vision

Control EMI with I-PEX ZenShield™ Connectors

Speed-up time-to-tapeout with the Aprisa digital place-and-route system and Solido Characterization Suite

Siemens Analogue IC Design Simulation Flow

More Sponsored Content >>

RSS Current EDABoard.com discussions

  • Hotplugging UART
  • Capacitive Switches
  • Can I use 5000uF 50V instead of 4700uF 50V in Inverter 700VA output rating board ?
  • Full Bridge LLC converter, 4kW cannot be done with offtheshelf ferrite?
  • how capacitor in series with resistor to gnd forms a pole or zero ?

RSS Current Electro-Tech-Online.com Discussions

  • Rather misnomer on two: wifi transmitter & receiver
  • PCB Photo sensitizing options
  • ASM - Enhanced 16F and long calls - how?
  • I need a PROM CPU
  • Relaxation oscillator with neon or...

Oscilloscopes Product Finder

Footer

EE World Online

EE WORLD ONLINE NETWORK

  • 5G Technology World
  • Analog IC Tips
  • Battery Power Tips
  • Connector Tips
  • DesignFast
  • EDABoard Forums
  • Electro-Tech-Online Forums
  • Engineer's Garage
  • Microcontroller Tips
  • Power Electronic Tips
  • Sensor Tips
  • Test and Measurement Tips
  • Wire & Cable Tips

EE WORLD ONLINE

  • Subscribe to our newsletter
  • Lee's teardown videos
  • Advertise with us
  • Contact us
  • About Us
Follow us on TwitterAdd us on FacebookConnect with us on LinkedIn Follow us on YouTube Add us on Instagram

Copyright © 2022 · WTWH Media LLC and its licensors. All rights reserved.
The material on this site may not be reproduced, distributed, transmitted, cached or otherwise used, except with the prior written permission of WTWH Media.

Privacy Policy