• State Resolved
  • Locked Locked
  • Replies 7 replies
  • Subscribers 41 subscribers
  • Views 6497 views
  • Users 0 members are here
Support feedback
Options
Options
Similar topics

This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

Faulty SPICE model of LM3886?

Klaus Strohhaecker
Prodigy 10 points
Other Parts Discussed in Thread: LM3886

Hi,

When checking the newly released (P)SPICE model for the LM3886 power amplifier at least two relevant problems were found :

1) The mute pin functionality is inverted : in the model the chip is ON when ZERO current is sunk out the MUTE pin, this is certainly wrong.

2) The open-loop mag/phase bode plot (derived from a closed loop AC analysis in the usual way by dividing Vout by the input differential (Vin+ - Vin-)) is severly off, indicating a unity stable opamp with a phase margin of 75deg! GBWP was found to be not the nominal 4MHz, rather the datasheet max. of 8Mhz was used, not a big deal but still questionable. However, the phase response is more than a decade off in its roll-off, way too high (for example, the real part and datasheet reads 900kHz for the 120deg open-loop phase point, model says 15Mhz... that's even above the UGBW!). Higher frequency poles are there of course, they just seem to be set at wrong, too high frequencies (note that I have developped a reliable AC model of the LM3886 which exactly matches the published graphs and has proven to be realistic in the real world, for stablility analysis). I'm pretty confident in ruling out user errors. Also the strange behaviour shows up with TINA, too, so it is not LTspice specific (I checked in LTspice, others tried in TINA).

3) Less severe but still annoying : Output current is NOT reflected in the supply pins, rather all current is sourced/sunk from the small-signal "GND" pin of the chip.

LTspice puts out the following warnings, maybe that is a hint :

WARNING: Node U1:AV1 is floating.
WARNING: Node U1:OVER_CLAMP is floating.
WARNING: Node U1:P0ZP1 is floating.
WARNING: Node U1:CLAW_CLAMP is floating.
WARNING: Node U1:VSENSE is floating.
WARNING: Node U1:P0Z is floating.
WARNING: Node U1:CL_CLAMP is floating.
WARNING: Node U1:UZ_N100 is floating.
WARNING: Node U1:UZ_N102 is floating.

Could TI/NS kindly check the issue? In the model description there is no statement that AC behaviour is precisely modelled at all except for unity gain BW. I know that TI uses the typical disclaimer in the model that they will take "no responsibility for anything" but publishing a model that questionable does not make any sense to me, honestly.

There is a discussion thread at DIYaudio.com for further information : http://www.diyaudio.com/forums/chip-amps/212805-ti-has-new-spice-models-lm3886-lm3875-et-all.html

  • 0
    TI__Mastermind 19290 points

    Hi Klaus,

    Thank you for giving feedback on this model. We will release a new model in the very near future that will

    take care of some of the  issues you mentioned, i.e, the polarity of MUTE pin, the dependency of current at the supply pin on load.

    The open loop gain was modeled as unloaded and the new model would be done with a typical load only.

    Our models  typically  are done and tested in PSPICE and /or TINA , please contact the Product Information

    Center at  support@ti.com for further assistance about requesting a new model.

    Thanks again for your feedback.

    Kind Regards,

     

    Arash Loloee

  • 0 in reply to Arash Loloee
    Prodigy 20 points

    Hi,

    Pspice model for LM3886 is encrypted, so it is of no use.

    Best, Ivo

  • 0 in reply to Ivo Klaric
    TI__Mastermind 19290 points

    Hi,

    An encrypted model should make no difference in its simulation . How  you  want to use the model that encryption is making it useless? May be I can assist you with that.

    Regards,

    Arash

  • 0 in reply to Arash Loloee
    Prodigy 20 points

    Hi Arash,

    Thank you for a quick replay...I use LTspice IV as simulation program for a long time, so I'm quite familiar with the definition of new devices in it. The previous .subckt model of LM3886 I used successfully, despite the shortcomings, but I'm not able to uploud new LM3886 encripted model in LTSpice IV successfully, it simply does not work. Also, old model had seven pins, while the new model has 6 pins ... GND pin is missing in new model?

    Regards, Ivo

  • 0 in reply to Ivo Klaric
    TI__Mastermind 19290 points

    Hello Ivo,

    Let me get back with you on the unencrypted version , I'll  see if I can post an unencrypted version of it.   If so,  you will see the new model posted in the next couple of weeks.

    The new model is using its own internal floating GND and thus no external GND pin was used. If the application requires a single supply operation, the negative supply pin  should be used as GND as before. 

    Kind Regards,

    Arash Loloee

  • 0 in reply to Arash Loloee
    Prodigy 20 points
    What does it mean when pspice generates error message saying "sub circuit lm3886 cannot be found?
  • 0 in reply to Arash Loloee
    Prodigy 20 points

    What does it mean when pspice generates error message saying "sub circuit lm3886 cannot be found"?