LTSpice

[J4e8a16n]

Hi everyone,

Why cant I get 15 volts or so on the lm317 output?


       --- Operating Point ---

V(n001):    18    voltage
--------------------------------------     V(n002):    3.28882    voltage
V(n003):    2.55671    voltage
V(n008):    0.0112638    voltage
V(n004):    0.812597    voltage
V(n009):    1.58001    voltage
V(nc_01):    2.46341    voltage
-------------------------------------------V(out):    1.64052    voltage
V(nc_02):    0.812597    voltage
V(n006):    1.64046    voltage
V(n005):    1.64052    voltage
V(dumpingcap):    2.4602    voltage
V(n007):    1.63158    voltage
Ic(Q3):    -8.40439e-013    device_current
Ib(Q3):    8.3048e-013    device_current
Ie(Q3):    8.88178e-015    device_current
Ic(Q2):    1.66089e-012    device_current
Ib(Q2):    -1.65157e-012    device_current
Ie(Q2):    -1.11022e-014    device_current
Ic(Q1):    0.00121647    device_current
Ib(Q1):    0.00688217    device_current
Ie(Q1):    -0.00809864    device_current
I(C5):    2.47622e-017    device_current
I(C4):    8.19737e-016    device_current
I(C3):    8.2792e-020    device_current
I(C1):    1.8e-018    device_current
I(D3):    0.818979    device_current
I(D2):    0.818979    device_current
I(D1):    0.00121647    device_current
I(R3):    0.818979    device_current
I(R6):    8.07435e-020    device_current
I(R5):    0.000348823    device_current
I(R4):    0.000348823    device_current
I(R2):    0.00155767    device_current
---------------------------------------------------I(R1):    0.812597    device_current
I(V1):    -0.820696    device_current
Ix(u1:1):    0.820696    subckt_current
Ix(u1:2):    -7.61966e-006    subckt_current
Ix(u1:3):    -0.820688    subckt_current
Ix(u2:VN):    -8.25408e-006    subckt_current
Ix(u2:CONTROL):    -3.38813e-021    subckt_current
Ix(u2:VP):    8.25408e-006    subckt_current

Regards

JPD

[Ian.M]

What do you expect when you connect a LM317 to a load consisting of two diodes and a 1R resistor all in series?  With 16V across it the LM317 model I have here limits its output current to 400mA for short-circuit protection. 

You appear to be using a different LM317 model, and you haven't supplied your LMC555 CMOS 555 model.   When posting a LTspice sim here, if it relies on models and symbols not provided in a 'vanilla' LTspice IV install, make sure they are in the sim's folder and zip them up with the .asc simulation file.  As a poor alternative, at least provide links to the extra models and symbols you have used.

[Audioguru]

The voltage "doubler" with lots of ripple is overloading all the active devices since the R3 load is only 1 ohm.

[J4e8a16n]

I gather among my folders....

[mikerj]

The doubler may not even be running, just the two diode drops and the 1 ohm resistor is enough to drag the supply rail down before you even consider the effects of the doubler.

[Ian.M]

The models and symbols missing from your "Chargeur 12v.asc" aren't in that zip file. 
I found your LMC555 symbol and model on the LTSPICE wiki:
http://ltwiki.org/files/LTspiceIV/lib/sym/SBORKA/TIMER/LMC555.asy
http://ltwiki.org/files/LTspiceIV/lib/sub/Sborka.lib
I've got no idea where you got the LM317 model as the symbol size doesn't match the usual one from the Yahoo group.   Please locate the symbol "lLM317.asy" that you are using, and attach it and also open it in the LTspice symbol editor, do 'Edit Attributes' from the menu, and find whatever file is referenced on the 'ModelFile' line of the Symbol Attribute Editor and attach that.  Cancel out of the Symbol Attribute Editor and close the LM317.asy symbol without saving so you dont accidentally make any changes.

There may be a problem with the Vcc connection to the LMC555.  When I open "Chargeur 12v.asc", I notice the Vdd connection runs down the left edge of the LMC555 symbol.  Dragging it away from the symbol to bring the wire in to the pin at rightangles as is normal practice reveals it extended past the pin down the edge by another grid increment.   *PLEASE* don't draw wires to pins like that - its confusing at best and at worst may lead to the wrong pins being connected.  There are also problems with the Out and Adg pins of the LM317 and the base of Q1 where the wire connects to the pin then continues into the symbol and you should tidy those up as well.   If you have to, you can move the offending symbol out of the way with the 'Move' tool, grab the offending wire end by boxing it with the 'Drag' tool and drag it clear, move the symbol back the drag the wire end back onto the correct pin.

[J4e8a16n]

Hi,


The file was  lm317.sub

The corrected asc file.

[Ian.M]

Well, I've tidied it up a bit more and added a few net names and .op voltage and current labels, and its obvious that Q1 is hard on, and is dragging the LM317 Adj pin to one LED Vf drop above ground, thus limiting the output to a maximum of 3.28V

The diodes and R3 are dragging the regulator output down.  If you increase R3 to 100R, the regulator output goes up to 15.44V before the 555 and charge pump circuit drags it down.  However the LM317 model you are using doesn't seem to be very stable and the LMC555 model certainly doesn't like a rapidly varying supply voltage so the simulation time becomes unreasonably long - its a brute and probably indicates its behaviour would be unpredictable in real life.

I assume the 555 and charge pump circuit is meant to be a desulphator - you should get the basic CC/CV charging regulator circuit working first, then redesign the desulphator with a constant supply voltage to the 555, and maybe change to a pumped LC series resonance design powered by the incoming supply to the regulator so that it draws no net DC current from the battery.   A choke to isolate the desulphator pulse from the regulator would also be helpful.

Tidied up sim attached with all models and symbols reqquired.  Caution: its *S*L*O*W!