"Time step too small" error in LTspice.

[Flyback]

Hello,
Do you know how I can get this simulation working?, it gives the above error.

 

[ericgibbs]

hi,
It work for me,
Goto Tools/Control Panel,,, select Alternate NOT Normal
E

 

[Flyback]

tried alternate 1 and 2, and runs for a bit but then stops and gives the error...I am using windows 8

 

[ericgibbs]

I am using XP Pro.

You didnt add the TLV431_ti model to your file so I used my TL431, it should be the same.

Could your TLV model be the problem.?

 

[Flyback]

The tlv431 model I used is from Helmut sennewald on the ltspice forum, as attached

the model worked fine in other sims with less nodes.

 

[ericgibbs]

hi,
With your model and Trtol=1 it never solves the sim!, change Trtol = 7 [ on the same Tools window as 'Alternate]

It runs slow but it will solve
E

EDIT:
Sometimes it fails! There is a problem with your model

 

[Flyback]

trtol to 7 and it still doesnt work

 

[ronv]

Try this spice directive.

.options gmin=1e-10

If not.

**********************************************************************************
* Model developed by Eugene Dvoskin "https://www.audio-perfection.com" 02/05/2012
* This TL431 model has been developed from schematic in the datasheet
* https://www.ti.com/lit/ds/symlink/tl431.pdf
* It matches most of DC, AC, Transient, Stability and Noise performance of TI TL431
* No attempts were made to cover Temperature dependences
*********************************************************************************
.SUBCKT TL431ED CATHODE ANODE REF
Q1 CATHODE REF N005 QN_ED
R4 N005 N009 3.28k
R2 N009 N012 2.4k
R3 N009 N010 7.2k
Q2 N012 N012 ANODE QN_ED area=1.2
Q3 N010 N012 N014 QN_ED area=2.2
R1 N014 ANODE 800
Q4 N003 N005 N006 QN_ED
R5 N006 N011 4k
Q5 N011 N010 ANODE QN_ED
Q6 N004 N013 ANODE QN_ED area=0.5
Q7 N003 N003 N001 QP_ED
Q8 N004 N003 N002 QP_ED
R7 CATHODE N001 800
R8 CATHODE N002 800
Q9 CATHODE N004 N007 QN_ED
R9 N008 N007 150
Q10 CATHODE N008 ANODE QN_ED area=5
R10 N008 ANODE 10k
Q11 N004 N004 REF QN_ED
D1 ANODE N004 D_ED
R6 N013 N012 1k
D2 ANODE CATHODE D_ED
C1 CATHODE N004 10p
C2 N010 N011 20p
.model QN_ED NPN(BF=140 Cje=1p Cjc=2p Rb=40 VAF=80 VAR=50 KF=3.2e-16 AF=1)
.model QP_ED PNP(BF=60 Cje=1p Cjc=3p Rb=80 VAF=70 VAR=40)
.MODEL D_ED D(Rs=5 CJ0=4.0p)
.ends TL431ED

 

[ericgibbs]

hi Flyback,
This zip has all my LTS TL431 information.
The asc file uses my TL431 model, it runs in LTS.
E

 

[Flyback]

thanks, I should say though, that this is TLV431

Thanks, but ".options gmin=1e-10" doesnt make it work.

The really weird thing is that if I run the simulation with V1 set to 12V, the simulation runs fine

 

[alec_t]

I often get that error message with sims. Sometimes the alternatesolver, or trtol, or gmin trick works; sometimes not. For reasons I haven't sussed, just changing a component value slightly can sometimes get it working. Schematics with inductors or high value caps seem to be the main types which trigger the error.
There's an option to select the maximum time step; shame there's no way to set the minimum .

 

[Flyback]

OK thanks all, you got me on the right track saying about the TLV431 model.....that was the problem,

here they are on ltspice yahoo groups "analogspiceman" is telling it and giving solution...I used his model...

As for the reason your original simulation was balky, you can blame the poorly written model from TI. It contains stiff (voltage source) elements with problematic discontinuities (either within the function directly or within its derivative). Replace it with a better model properly written to enhance convergence performance and your simulation will run fine (search the files archive for TLV431AS.sub).

I changed to his tlv431as and it is fine......................

 

[ericgibbs]

hi,
Thats good news, when you have a minute please post the TLV431AS data.
E

 

[Flyback]

ok

 

[ericgibbs]

Got it, thanks.

 

[eTech]

Hi

I tried your schematic in LTSpice. It failed with "Timestep too small"

1. The TLV431.asy symbol attributes are incorrect. The only attibutes values should be:
Prefix=X
Value = TLV431
Modelfile = tlv431.lib

all others should be blank (except description if you like)
Once I did this I had to remove and replace all TLV431's in the schematic.

2. I was able to run the sim longer if I used this option:

.options cshunt=1e-15

not good..

I would start by removing all the serial resistance values from all caps..