Go Back   Home > Forums > >
Home Forums Rules Articles diyAudio Store Blogs Gallery Wiki Register Donations FAQ Calendar Search Today's Posts Mark Forums Read

Chip Amps Amplifiers based on integrated circuits

opa627 Spice Model vs Ideal Opamp Model
opa627 Spice Model vs Ideal Opamp Model
Please consider donating to help us continue to serve you.

Ads on/off / Custom Title / More PMs / More album space / Advanced printing & mass image saving
Reply
 
Thread Tools Search this Thread
Old 11th September 2013, 09:37 AM   #1
HiFiNutNut is offline HiFiNutNut  Australia
diyAudio Member
 
Join Date: May 2004
Location: Sydney
Default opa627 Spice Model vs Ideal Opamp Model

Refer to the attached simulation of a 2nd order high pass filter, the green curve is the result of using the opa627 PSpice model directly downloaded from Texas Instruments today, while the blue curve is the result of using the ideal opamp model.

I can't believe the difference. It is not possible to be that much different. What has gone wrong?

The asc file was created by Keantoken for me a while ago. I think I supplied him the TI downloaded model file, and he digged out a symbol and put it into an asc file for my use. Today I replaced the opa627 model file with the latest version from TI.

The asc file is attached. Unfortunately, I can't attach the MODEL file but you can get it from the TI site.

Regards,
Bill
Attached Images
File Type: png opa627_vs_ideal_opamp.PNG (54.7 KB, 209 views)
Attached Files
File Type: asc opa627_vs_ideal_opamp.asc (5.4 KB, 29 views)

Last edited by HiFiNutNut; 11th September 2013 at 09:41 AM.
  Reply With Quote
Old 12th September 2013, 04:30 AM   #2
dchisholm is offline dchisholm  United States
diyAudio Member
 
dchisholm's Avatar
 
Join Date: Mar 2011
Location: St Louis, Mo
Ummm . . . (mustering up my best "Sophomore Electronics Class" instructor's voice) . . . Which result is closest to what you were EXPECTING to see? Is there anything you readily notice about the difference between your expectations, and the simulation results? Do the answers to these questions provide a clue to the error you are looking for?

You have a SHORT CIRCUIT between the output of opamp U6 and the output of opamp U7. LENGTHEN IT.

(Probably a careless cut-and-paste error during editing.)

Dale
Attached Images
File Type: png Node_Name_Error.png (565.9 KB, 196 views)
Attached Files
File Type: asc opa627_vs_ideal_opamp_mod.asc (7.3 KB, 16 views)
  Reply With Quote
Old 12th September 2013, 09:43 AM   #3
HiFiNutNut is offline HiFiNutNut  Australia
diyAudio Member
 
Join Date: May 2004
Location: Sydney
Dale,

To me

To you

Thank you wholeheartedly

Bill

PS. Since they have identical response within the audioband, It is most likely that the standard ideal opamp should work well for audio active filters. I will check with 20MHz bandwidth though and make sure nothing bad happens at higher frequencies.
  Reply With Quote
Old 12th September 2013, 04:09 PM   #4
dchisholm is offline dchisholm  United States
diyAudio Member
 
dchisholm's Avatar
 
Join Date: Mar 2011
Location: St Louis, Mo
Quote:
Originally Posted by HiFiNutNut View Post
To me
In exchange for a serving of my favorite malt beverage, you can be certain that your supervisor (or instructor) will never hear of this incident from me.

Quote:
PS. Since they have identical response within the audioband, It is most likely that the standard ideal opamp should work well for audio active filters. I will check with 20MHz bandwidth though and make sure nothing bad happens at higher frequencies.
Why are you considering this approach? The LTSpice "simplified opamp" seems to be an accommodation intended primarily for conceptual investigations of an academic or tutorial nature. Its primary advantage is probably execution speed of a simulation, and even that won't be obvious (unless you're running a 486-class machine) for a realistic circuit with fewer than a dozen opamps.

If I had intentions of ever building this as a physical circuit, I'd simulate with the manufacturer's macromodels unless I had a good reason not to. Especially with active filters, even though the end-to-end behavior may appear rather undemanding, there may be things happening internal to the circuit that stress the opamp's capabilities. At the very least I'd want a model that accounted for finite slew rate, output clipping, and input capacitance effects.

As a general group, published opamp macromodels tend to be far short of what they COULD be if manufacturers would make the effort. Significant improvements to the accuracy and completeness of the Boyle/Cohen macromodel were documented and published in the early 1990's at Burr-Brown and Analog Devices but don't seem to have been widely adopted even within those organizations. Even so, a basic Boyle/Cohen model is MUCH more realistic than the LTSpice simplified approximations.

Dale
  Reply With Quote
Old 13th September 2013, 10:28 AM   #5
HiFiNutNut is offline HiFiNutNut  Australia
diyAudio Member
 
Join Date: May 2004
Location: Sydney
Dear Dale, the Sophomore Electronics Class Instructor,

You can have as much your favorite malt beverage as you like if you pass Sydney and this is your ticket. If you don't come this way then let me serve you some e-beverage in hope of getting one more free lesson.

Out of the 3 you listed (slew rate, output clipping, and input capacitance effects), I only know how to check output clipping. I think I can also check accurately current draw, power dissipation, or perhaps even rail noise injections, but I don't know how to check slew rate limit, and input capacitance effects.

There are more. For an example, I have been wondering how much compensation is needed for a non-inverting gain stage (cap from Vout to -Vin) to achieve the best transient response, i.e. minimal overshoot or undershoot. Could I simply generate some squire waves at 100kHz from the input and check the output? Or perhaps the marcomodel won't give me this level of accuracy and only a scope can provide the answer?

For another example, I would like to know how much isolation resistance is required for capacitive load. Attached is the real (i.e. almost real) circuit I am planning to use. I am learning to design the entire preamp/active crossover, as well as the input stage of the power amp. How would I know if C6 is too big to cause grief to the proceeding opa627, or if C6 can be increased to provide better RF noise suppression for the power amp, as the low pass corner frequency is really too high at the moment?

Of course, I wouldn't expect you to write a book for this lesson but if you could in the briefest way point me in the right direction that would be very much appreciated.

Regards,
Bill
Attached Images
File Type: png xo_to_poweramp.PNG (30.4 KB, 159 views)
Attached Files
File Type: asc xo_output_power_amp_input.asc (4.4 KB, 8 views)
  Reply With Quote
Old 13th September 2013, 11:00 PM   #6
HiFiNutNut is offline HiFiNutNut  Australia
diyAudio Member
 
Join Date: May 2004
Location: Sydney
Dale is not interested in e-beverage

  Reply With Quote
Old 16th September 2013, 05:41 AM   #7
dchisholm is offline dchisholm  United States
diyAudio Member
 
dchisholm's Avatar
 
Join Date: Mar 2011
Location: St Louis, Mo
Of course, your ability to find any performance shortcoming related to a device imperfection, and compensate or correct it, using simulation will depend on the completeness and accuracy of the simulation models. Some of the limitations of modeling techniques are discussed in the tutorial "Analog Circuit Simulation" at http://www.analog.com/static/importe...als/MT-099.pdf and especially Analog Devices' Application Note AN138, "SPICE-Compatible Op Amp Macro-Models" at
http://www.analog.com/static/importe...tes/AN-138.pdf . (Similar App Notes from Burr Brown are "Operational Amplifier Macromodels: A Comparison" at http://www.ti.com/lit/an/sboa027/sboa027.pdf and "SPICE Based Macromodels" at http://www.ti.com/lit/an/sbfa009/sbfa009.pdf .)

Quote:
Originally Posted by HiFiNutNut View Post
Out of the 3 you listed (slew rate, output clipping, and input capacitance effects), I only know how to check output clipping. I think I can also check accurately current draw, power dissipation, or perhaps even rail noise injections . . .
The original Boyle model topology was especially weak at modeling anything related to the power supplies. See the Analog Devices AN-138.

Quote:
. . . I don't know how to check slew rate limit, and input capacitance effects.
For slew rate, I'd apply the worst case input signal (highest frequency, highest amplitude) and look directly at the outputs of each individual opamp. If the simulation shows a slew rate faster than, say, half the opamp's data sheet value (or some other reasonable design margin) I would rework the design. (Usually, this approach can be used whether the model accurately accounts for slew rate or not.)

If you have confidence in the model's ability to accurately model slew rate, it may be easier to simulate with the worst-case input signal, and also with the same signal at lower amplitude (say, 1/10 the voltage). Then use the LTSpice trace math to scale and superimpose the two signals.

Input capacitance effects show up as perturbations in frequency response, peaking near the amplifier's upper cutoff frequency. How this affects overall circuit performance depends on topology and how close you're working to the opamp's capabilities. The algebra may appear formidable but the graphics in TI App Note SLOA013A "Effect of Parasitic Capacitance in Op Amp Circuits" at http://www.ti.com/lit/an/sloa013a/sloa013a.pdf give a general idea of what's happening.

Quote:
There are more. For an example, I have been wondering how much compensation is needed for a non-inverting gain stage (cap from Vout to -Vin) to achieve the best transient response, i.e. minimal overshoot or undershoot. Could I simply generate some squire waves at 100kHz from the input and check the output? Or perhaps the marcomodel won't give me this level of accuracy and only a scope can provide the answer?
This is one area where simulation should be quite useful. If the transient response is affected by output loading it will depend on the accuracy of the model's output section. The A-D MT-099 tutorial demonstrates this on page 7, and pages 11-12.

Quote:
For another example, I would like to know how much isolation resistance is required for capacitive load. Attached is the real (i.e. almost real) circuit I am planning to use. I am learning to design the entire preamp/active crossover, as well as the input stage of the power amp. How would I know if C6 is too big to cause grief to the proceeding opa627, or if C6 can be increased . . .
Many opamp data sheets give good guidelines on this. (The OPA627 data sheet seems to suggest that 20 ohms is adequate. See Fig 6.) TI App Note SLOA013A discusses this with greater theoretical analysis in Section 6.

Dale
  Reply With Quote
Old 16th September 2013, 11:40 PM   #8
HiFiNutNut is offline HiFiNutNut  Australia
diyAudio Member
 
Join Date: May 2004
Location: Sydney
Dale,

Your posts have been very much appreciated. For capacitance at the input or output of an opamp, I think I can follow the TI App Note SLOA013A closely. I should be able to get good result by doing that without relying on simulations. For the rest, it is always a good idea to use the macromodel, feed the opamp with maximum input voltage at the highest possible frequencies the opamps needs to deal with, and with fast rise time and check the results.

Regards,
Bill
  Reply With Quote

Reply


opa627 Spice Model vs Ideal Opamp ModelHide this!Advertise here!
Thread Tools Search this Thread
Search this Thread:

Advanced Search

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off

Forum Jump

Similar Threads
Thread Thread Starter Forum Replies Last Post
Spice Model for LME49830 KlaRa54 Chip Amps 0 28th August 2010 09:12 PM
BZX79C12V spice model nicholas1113 Solid State 1 29th December 2009 04:17 PM
Spice Macro Model for floating supply opamp rtarbell Solid State 2 21st June 2006 05:14 PM
SPICE model Prune Software Tools 6 16th October 2004 04:22 PM
Spice model doigtee Tubes / Valves 6 12th July 2003 12:42 PM


New To Site? Need Help?

All times are GMT. The time now is 06:40 PM.


Search Engine Optimisation provided by DragonByte SEO (Pro) - vBulletin Mods & Addons Copyright © 2018 DragonByte Technologies Ltd.
Resources saved on this page: MySQL 14.29%
vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2018 DragonByte Technologies Ltd.
Copyright ©1999-2018 diyAudio
Wiki