Lm13700 LTSpice Sim Help

bobtech · May 8, 2017

Hi guys,

I'm having an issue simulating the LM13700 in LTSpice.... I have trawled through the net to no avail.

It's a standard setup for the LM13700 from the data sheet (Square/Triangle VCO) and I have some initial conditions which can be seen in LTSpice, to help kick it into oscillation (it stays flat at 0V and -1.3V otherwise) .... and the output I get is below (only runs for a fraction of a micro second)

any ideas on where to go with this, why doesn't it display the waveform for longer? I'm stumped..

Alec_t · May 8, 2017

Please post your .asc file here.

bobtech · May 8, 2017

there was a small mistake in the original, where I hadn't connected the capacitor to ground....
I've fixed it but now it doesn't do anything

I also attached the asc file.

bobtech · May 8, 2017

update: although no errors show when I run the sim, when I check the error log, I do get this error... any ideas?

Direct Newton iteration failed to find .op point. (Use ".option noopiter" to skip.)
Starting Gmin stepping
Gmin = 10
vernier = 0.5
vernier = 0.25
vernier = 0.125
Gmin = 2.62144
vernier = 0.0625
vernier = 0.03125
vernier = 0.015625
vernier = 0.0078125
vernier = 0.00390625
vernier = 0.00195313
vernier = 0.000976563
Gmin = 2.61952
vernier = 0.00130208
vernier = 0.00173611
Gmin = 2.61087
vernier = 0.00231481
Gmin = 2.59731
vernier = 0.00308642
vernier = 0.00411522
Gmin = 2.5747
vernier = 0.00548696
vernier = 0.00731595
Gmin = 2.53907
vernier = 0.00975459
Gmin = 2.48401
vernier = 0.0130061
vernier = 0.0173415
Gmin = 2.39431
vernier = 0.023122
vernier = 0.0308293
Gmin = 2.25805
vernier = 0.0411057
Gmin = 2.05947
vernier = 0.0548076
vernier = 0.0730768
Gmin = 1.7654
vernier = 0.0974357
vernier = 0.129914
Gmin = 1.38243
vernier = 0.0649571
vernier = 0.0324786
Gmin = 1.27537
vernier = 0.0433047
vernier = 0.0216524
Gmin = 1.21165
vernier = 0.0288698
vernier = 0.0144349
vernier = 0.0192465
Gmin = 1.17301
vernier = 0.00962327
vernier = 0.012831
Gmin = 1.14791
vernier = 0.00641551
vernier = 0.00320776
vernier = 0.00160388
vernier = 0.000801939
vernier = 0.000400969
Gmin = 1.15148
Gmin = 0
Gmin stepping succeeded in finding the operating point.

Date: Mon May 08 20:03:53 2017
Total elapsed time: 0.909 seconds.

tnom = 27
temp = 27
method = modified trap
totiter = 7152
traniter = 2082
tranpoints = 1042
accept = 1042
rejected = 0
matrix size = 54
fillins = 178
solver = Normal
Thread vector: 11.3/6.9[2] 5.8/4.1[2] 3.9/2.5[2] 0.4/1.2[1] 2592/500
Matrix Compiler1: 638 opcodes 4.1/[2.4]/284.4
Matrix Compiler2: 7.65 KB object code size 1.2/1.2/[0.8]
Click to expand...

bobtech · May 8, 2017

Ok, so taking the advice of the logfile, I skipped the.op point.... however I get a new problem...

Direct Newton iteration for .op point skipped.
Starting Gmin stepping
Gmin = 10
vernier = 0.5
vernier = 0.25
vernier = 0.125
Gmin = 2.62144
vernier = 0.0625
vernier = 0.03125
vernier = 0.015625
vernier = 0.0078125
vernier = 0.00390625
vernier = 0.00195313
vernier = 0.000976563
Gmin = 2.61952
vernier = 0.00130208
vernier = 0.00173611
Gmin = 2.61087
vernier = 0.00231481
Gmin = 2.59731
vernier = 0.00308642
vernier = 0.00411522
Gmin = 2.5747
vernier = 0.00548696
vernier = 0.00731595
Gmin = 2.53907
vernier = 0.00975459
Gmin = 2.48401
vernier = 0.0130061
vernier = 0.0173415
Gmin = 2.39431
vernier = 0.023122
vernier = 0.0308293
Gmin = 2.25805
vernier = 0.0411057
Gmin = 2.05947
vernier = 0.0548076
vernier = 0.0730768
Gmin = 1.7654
vernier = 0.0974357
vernier = 0.129914
Gmin = 1.38243
vernier = 0.0649571
vernier = 0.0324786
Gmin = 1.27537
vernier = 0.0433047
vernier = 0.0216524
Gmin = 1.21165
vernier = 0.0288698
vernier = 0.0144349
vernier = 0.0192465
Gmin = 1.17301
vernier = 0.00962327
vernier = 0.012831
Gmin = 1.14791
vernier = 0.00641551
vernier = 0.00320776
vernier = 0.00160388
vernier = 0.000801939
vernier = 0.000400969
Gmin = 1.15148
Singular matrix: Check nodes u2:27 and v:u2:3#branch
Iteration No. 15
Gmin = 0
Singular matrix: Check nodes u2:27 and v:u2:3#branch
Iteration No. 1
Gmin stepping failed

Starting source stepping with srcstepmethod=0
Source Step = 3.0303%
Source Step = 33.3333%
Source Step = 63.6364%
Source Step = 93.9394%
Source stepping succeeded in finding the operating point.

Date: Mon May 08 20:29:04 2017
Total elapsed time: 1.923 seconds.

tnom = 27
temp = 27
method = modified trap
totiter = 7552
traniter = 2290
tranpoints = 1082
accept = 1074
rejected = 8
matrix size = 54
fillins = 225
solver = Normal
Thread vector: 21.3/12.9[2] 5.2/3.6[2] 7.6/3.0[2] 1.1/2.1[1] 2592/500
Matrix Compiler1: 20.11 KB object code size 5.7/4.3/[2.4]
Matrix Compiler2: 8.30 KB object code size 6.4/6.7/[1.5]
Click to expand...

Harald Kapp · May 9, 2017

Have a look at our ressources. Especially:
- How to deal with LTSPICE error messages
- Simulating (absolutely) symmetrical circuits
If you want us to check you ASC file you should kindly post the model file(s) for the LM13700, too, as they are not a part of the LTSPICE standard libraries.

Alec_t · May 9, 2017

Like you, I failed to get your sim of the VCO in the datasheet to run. However, it can be made to run with the following changes (I daresay other changes would work too):-
1) Reduce V3 to 1V,
2) Increase C1 to 100n,
3) Add the directive ".options gmin=1e-7" to the schematic.

bobtech · May 9, 2017

Harald Kapp said:

Have a look at our ressources. Especially:
- How to deal with LTSPICE error messages
- Simulating (absolutely) symmetrical circuits
If you want us to check you ASC file you should kindly post the model file(s) for the LM13700, too, as they are not a part of the LTSPICE standard libraries.
Click to expand...

Sorry, the model is take from the Texas instruments site directly, and loaded into LTSpice

Here vvvvvv
http://www.ti.com/product/LM13700/toolssoftware

Alec_t said:

Like you, I failed to get your sim of the VCO in the datasheet to run. However, it can be made to run with the following changes (I daresay other changes would work too):-
1) Reduce V3 to 1V,
2) Increase C1 to 100n,
3) Add the directive ".options gmin=1e-7" to the schematic.
Click to expand...

would the 1e-7 not give false results? (I remember reading somewhere not to really go past 1e-9)

Harald Kapp · May 9, 2017

bobtech said:

would the 1e-7 not give false results? (I remember reading somewhere not to really go past 1e-9)
Click to expand...

Better some error with 1e-7 than no simulation at all with 1e-9.
As with all simulations you have to take the result with a grain of salt anyway. The simulation can be only as good as the models used and who guarantees the model of the amplifier is as accurate as you expect?

My personal stance is that the simulation is only there to verify there's no fatal flaw in the design calculations. A prototype will show the real world behavior much better than any simulation, including hard to simulate parameters such as e.g. noise, PCB Layout parasitics etc.

eetech00 · May 16, 2017

Hi

The input offset current is modeled with an F device poly which doesn't converge very well.

Change the following in the subcircuit definition:

IS:
F1 4 3 POLY(1) V6 1E-10 5.129E-2 -1.189E4 1.123E9

Change to:
*F1 4 3 POLY(1) V6 1E-10 5.129E-2 -1.189E4 1.123E9 <--comment this out
B1 4 3 I=If(V(11)>1.4v,100nA,0)

eT

Lm13700 LTSpice Sim Help

bobtech

Alec_t

bobtech

Attached Files:

sqr_tri.asc

bobtech

bobtech

Harald Kapp Moderator Moderator

Alec_t

bobtech

Harald Kapp Moderator Moderator

eetech00

LM13700 sim in TINA-TI help!

LTSpice LM13700 Simulation Error

LM13700 strange simulation problem on LTSpice

LTSpice Help

SIM Module

LTSpice simulation help

Keep Blowing lm13700's

LM13700 Amplifier/VCO Circuit