Spice model LM386 - Electronic Circuits Projects Diagrams Free

habbott · 9th August 2006, 11:01 AM

Hi looking for a spice model for the LM386 can't locate it on the web can anyone help.

Roff · 9th August 2006, 04:39 PM

No guarantees:

Code:

* lm386 subcircuit model follows:

************************************original* IC pins:     2   3   7   1   8   5   6   4
* IC pins:     1   2   3   4   5   6   7   8
*              |   |   |   |   |   |   |   |
.subckt lm386 g1  inn inp gnd out  vs byp g8
************************************original*.subckt lm386 inn inp byp  g1  g8 out  vs gnd

* input emitter-follower buffers:

q1 gnd inn 10011 ddpnp
r1 inn gnd 50k
q2 gnd inp 10012 ddpnp
r2 inp gnd 50k

* differential input stage, gain-setting
* resistors, and internal feedback resistor:

q3 10013 10011 10008 ddpnp
q4 10014 10012 g1 ddpnp
r3 vs byp 15k
r4 byp 10008 15k
r5 10008 g8 150
r6 g8 g1 1.35k
r7 g1 out 15k

* input stage current mirror:

q5 10013 10013 gnd ddnpn
q6 10014 10013 gnd ddnpn

* voltage gain stage & rolloff cap:

q7 10017 10014 gnd ddnpn
c1 10014 10017 15pf

* current mirror source for gain stage:

i1 10002 vs dc 5m
q8 10004 10002 vs ddpnp
q9 10002 10002 vs ddpnp

* Sziklai-connected push-pull output stage:

q10 10018 10017 out ddpnp
q11 10004 10004 10009 ddnpn 100
q12 10009 10009 10017 ddnpn 100
q13 vs 10004 out ddnpn 100
q14 out 10018 gnd ddnpn 100

* generic transistor models generated
* with MicroSim's PARTs utility, using
* default parameters except Bf:

.model ddnpn NPN(Is=10f Xti=3 Eg=1.11 Vaf=100
+ Bf=400 Ise=0 Ne=1.5 Ikf=0 Nk=.5 Xtb=1.5 Var=100
+ Br=1 Isc=0 Nc=2 Ikr=0 Rc=0 Cjc=2p Mjc=.3333
+ Vjc=.75 Fc=.5 Cje=5p Mje=.3333 Vje=.75 Tr=10n
+ Tf=1n Itf=1 Xtf=0 Vtf=10)

.model ddpnp PNP(Is=10f Xti=3 Eg=1.11 Vaf=100
+ Bf=200 Ise=0 Ne=1.5 Ikf=0 Nk=.5 Xtb=1.5 Var=100
+ Br=1 Isc=0 Nc=2 Ikr=0 Rc=0 Cjc=2p Mjc=.3333
+ Vjc=.75 Fc=.5 Cje=5p Mje=.3333 Vje=.75 Tr=10n
+ Tf=1n Itf=1 Xtf=0 Vtf=10)

.ends
*----------end of subcircuit model-----------

Optikon · 9th August 2006, 05:48 PM

FYI on that model

* 1. The following model behavior shows good agreement with the
* LM386 data sheet values:
*
* a) Quiescent power supply current;
* b) High frequency response at low gain setting;
* c) Power-supply rejection ratio, both bypassed and unbypassed;
* d) Voltage gain, both with pins 1&8 shorted and open; and
* e) Total harmonic distortion.
*
* 2. The model has the following discrepancies:
*
* f) High-gain frequency response looks somewhat more wideband
* than the actual device;
* g) Peak-to-peak output voltage swing is a bit more than the
* data sheet value- in other words, the model drives
* closer to the rails; and
* h) Input bias current in this model is only about 7 nA,
* compared with the 250 nA "typical" value mentioned in
* the data sheet.
*
* 3. The frequency response characteristics of this LM386 model
* can be adjusted somewhat by changing C1, the rolloff capacitor in
* the voltage gain stage. It could also be made more realistic by
* tweaking transistor model parameters Cjc, Cje, Tr and Tf,
* although this can get pretty hairy.
*
* 4. Likewise, output drive capability could be made more
* realistic by tweaking transistor model parameters; again, this is
* hairy.
*

habbott · 9th August 2006, 07:31 PM

Hi , thanks for the help but I am new to this. Has anyone got a complete model ready to go so I can just us it in my software program

Optikon · 10th August 2006, 05:36 PM

Quote:

Originally Posted by habbott

Hi , thanks for the help but I am new to this. Has anyone got a complete model ready to go so I can just us it in my software program

You were given a complete model that is ready to use by RonH.

If you don't know how to connect the model, that's a different problem but the model is as complete as it'll ever be.

philba · 10th August 2006, 06:47 PM

maybe the question should be what spice program are you using?

Hero999 · 29th December 2008, 03:21 PM

I'm having a couple of problems using this model.

I tried simulating it and got the following error:

Fatal Error: Unknown subcircuit called in:
xu1 n002 0 n007 0 n004 n001 n008 n003 lm386.sub

I'm using exactly the model posted by Roff, the symbol and schematic are attached.

Have I made an error with the symbol or schematic?

I've never drawn a sybol in LTSpice before so I just edited the generic op-amp file accordingly.

Symbol file:

Code:

Version 4
SymbolType CELL
LINE Normal -64 -63 64 0
LINE Normal -64 65 64 0
LINE Normal -64 -63 -64 65
LINE Normal -60 -48 -52 -48
LINE Normal -60 48 -52 48
LINE Normal -56 52 -56 44
LINE Normal -48 -80 -48 -55
LINE Normal -48 80 -48 57
LINE Normal -44 -68 -36 -68
LINE Normal -40 -72 -40 -64
LINE Normal -44 68 -36 68
LINE Normal -16 -39 -16 -64
LINE Normal 0 32 0 48
LINE Normal 48 -8 48 -32
TEXT -51 1 Left 0 LM386
SYMATTR Prefix X
SYMATTR Description Low power audio amplifier
SYMATTR ModelFile LM386.sub
SYMATTR SpiceModel LM386.sub
PIN -16 -64 LEFT 8
PINATTR PinName g1
PINATTR SpiceOrder 1
PIN -64 -48 NONE 0
PINATTR PinName In-
PINATTR SpiceOrder 2
PIN -64 48 NONE 0
PINATTR PinName In+
PINATTR SpiceOrder 3
PIN -48 80 NONE 0
PINATTR PinName V-
PINATTR SpiceOrder 4
PIN 64 0 NONE 0
PINATTR PinName OUT
PINATTR SpiceOrder 5
PIN -48 -80 NONE 0
PINATTR PinName V+
PINATTR SpiceOrder 6
PIN 0 48 LEFT 8
PINATTR PinName bp
PINATTR SpiceOrder 7
PIN 48 -32 LEFT 8
PINATTR PinName g8
PINATTR SpiceOrder 8

Roff · 29th December 2008, 04:38 PM

This seems to work:

Code:

Version 4
SymbolType CELL
LINE Normal -64 -63 64 0
LINE Normal -64 65 64 0
LINE Normal -64 -63 -64 65
LINE Normal -60 -48 -52 -48
LINE Normal -60 48 -52 48
LINE Normal -56 52 -56 44
LINE Normal -48 -80 -48 -55
LINE Normal -48 80 -48 57
LINE Normal -44 -68 -36 -68
LINE Normal -40 -72 -40 -64
LINE Normal -44 68 -36 68
LINE Normal -16 -39 -16 -64
LINE Normal 0 32 0 48
LINE Normal 48 -8 48 -32
SYMATTR Value LM386
SYMATTR Prefix X
SYMATTR ModelFile LM386.sub
SYMATTR Value2 LM386
SYMATTR Description Low power audio amplifier
PIN -16 -64 LEFT 8
PINATTR PinName g1
PINATTR SpiceOrder 1
PIN -64 -48 NONE 0
PINATTR PinName In-
PINATTR SpiceOrder 2
PIN -64 48 NONE 0
PINATTR PinName In+
PINATTR SpiceOrder 3
PIN -48 80 NONE 0
PINATTR PinName V-
PINATTR SpiceOrder 4
PIN 64 0 NONE 0
PINATTR PinName OUT
PINATTR SpiceOrder 5
PIN -48 -80 NONE 0
PINATTR PinName V+
PINATTR SpiceOrder 6
PIN 0 48 LEFT 8
PINATTR PinName bp
PINATTR SpiceOrder 7
PIN 48 -32 LEFT 8
PINATTR PinName g8
PINATTR SpiceOrder 8

You can also do it as in the attached file if you don't want to create a symbol. The 8 pin symbol is in the Misc library.

Hero999 · 29th December 2008, 09:08 PM

Thanks Roff.

Do you know where I had gone wrong (apart from not including a value for C4 which shouldn't have given me that error)?

MrAl · 29th December 2008, 09:14 PM

Hi,

I think what he meant was that he wants a model that actually models
all of the characteristics, not just some of them.

Hero999 · 29th December 2008, 09:47 PM

I think this is close enough for now.

The main discrepancy I've noticed is that this model only has a gain of about 168 rather than the 200 suggested on the datasheet.

Roff · 30th December 2008, 12:05 AM

Quote:

Originally Posted by Hero999

Thanks Roff.

Do you know where I had gone wrong (apart from not including a value for C4 which shouldn't have given me that error)?

Compare the file I gave you with the file you posted. I took yours and edited it until it looked like LM555.asy.

Thread Tools
Show Printable Version Email this Page
Display Modes
Linear Mode Switch to Hybrid Mode Switch to Threaded Mode

9th August 2006, 11:01 AM	(permalink)
habbott	Spice model LM386 Hi looking for a spice model for the LM386 can't locate it on the web can anyone help.

9th August 2006, 05:48 PM	(permalink)
Optikon	FYI on that model * 1. The following model behavior shows good agreement with the * LM386 data sheet values: * * a) Quiescent power supply current; * b) High frequency response at low gain setting; * c) Power-supply rejection ratio, both bypassed and unbypassed; * d) Voltage gain, both with pins 1&8 shorted and open; and * e) Total harmonic distortion. * * 2. The model has the following discrepancies: * * f) High-gain frequency response looks somewhat more wideband * than the actual device; * g) Peak-to-peak output voltage swing is a bit more than the * data sheet value- in other words, the model drives * closer to the rails; and * h) Input bias current in this model is only about 7 nA, * compared with the 250 nA "typical" value mentioned in * the data sheet. * * 3. The frequency response characteristics of this LM386 model * can be adjusted somewhat by changing C1, the rolloff capacitor in * the voltage gain stage. It could also be made more realistic by * tweaking transistor model parameters Cjc, Cje, Tr and Tf, * although this can get pretty hairy. * * 4. Likewise, output drive capability could be made more * realistic by tweaking transistor model parameters; again, this is * hairy. *

9th August 2006, 07:31 PM	(permalink)
habbott	Thanks Hi , thanks for the help but I am new to this. Has anyone got a complete model ready to go so I can just us it in my software program

10th August 2006, 06:47 PM	(permalink)
philba	maybe the question should be what spice program are you using?

29th December 2008, 09:08 PM	(permalink)
Hero999	Thanks Roff. Do you know where I had gone wrong (apart from not including a value for C4 which shouldn't have given me that error)? __________________ I also post at the following sites: http://www.stop-microsoft.org http://www.heated-debates.com Screen name: Aloone_Jonez And http://www.silicontronics.com, same screen name as here.

29th December 2008, 09:14 PM	(permalink)
MrAl	Hi, I think what he meant was that he wants a model that actually models all of the characteristics, not just some of them.

29th December 2008, 09:47 PM	(permalink)
Hero999	I think this is close enough for now. The main discrepancy I've noticed is that this model only has a gain of about 168 rather than the 200 suggested on the datasheet. __________________ I also post at the following sites: http://www.stop-microsoft.org http://www.heated-debates.com Screen name: Aloone_Jonez And http://www.silicontronics.com, same screen name as here.