LTSpice: How do make a Schmitt oscillator run?

[Joerg]

Ok, simple circuit: Schmitt inverter, 10K resistor from output to input,
1000pF capacitor from input to ground. Vh set to about 20% of Vhigh.
Should happily oscillate but I get the error message "Time step too
small". Also there is a noted dip in voltage down to about 80%,
something which should even be possible with a digital behavioral device.

What gives? How can I fix that and make it run? Does it need some kind
of kicker?

 

[Helmut Sennewald]

Ok, simple circuit: Schmitt inverter, 10K resistor from output to input,
1000pF capacitor from input to ground. Vh set to about 20% of Vhigh.
Should happily oscillate but I get the error message "Time step too
small". Also there is a noted dip in voltage down to about 80%, something
which should even be possible with a digital behavioral device.

What gives? How can I fix that and make it run? Does it need some kind of
kicker?

Hallo Joerg,

I don't know what you did wrong.
Have you set the trigger levels vt and vh?

hysteresis: vh
trigger levels:
v1 = vt+vh
v2 = vt-vh

Example: Right-mouse-click on teh schmitt device.
Vhigh=5 Vt=2.5 Vh=1
td=5n

"osc.asc"-file:

Version 4
SHEET 1 880 680
WIRE 144 0 96 0
WIRE 288 0 224 0
WIRE 96 96 96 0
WIRE 128 96 96 96
WIRE 176 96 128 96
WIRE 288 96 288 0
WIRE 288 96 240 96
WIRE 320 96 288 96
WIRE 96 112 96 96
WIRE 96 192 96 176
FLAG 96 192 0
FLAG 320 96 out
FLAG 128 96 rc
SYMBOL Digital\\schmtinv 176 32 R0
SYMATTR InstName A2
SYMATTR Value2 Vhigh=5 Vt=2.5 Vh=1
SYMATTR SpiceLine Td=5n
SYMBOL cap 80 112 R0
SYMATTR InstName C1
SYMATTR Value 1n
SYMBOL res 128 16 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R1
SYMATTR Value 10k
TEXT 80 -104 Left 0 !.tran 0 100u 0 100n

 

[Joerg]

Hallo Joerg,

I don't know what you did wrong.
Have you set the trigger levels vt and vh?

hysteresis: vh
trigger levels:
v1 = vt+vh
v2 = vt-vh

Example: Right-mouse-click on teh schmitt device.
Vhigh=5 Vt=2.5 Vh=1
td=5n

"osc.asc"-file:

Version 4
SHEET 1 880 680
WIRE 144 0 96 0
WIRE 288 0 224 0
WIRE 96 96 96 0
WIRE 128 96 96 96
WIRE 176 96 128 96
WIRE 288 96 288 0
WIRE 288 96 240 96
WIRE 320 96 288 96
WIRE 96 112 96 96
WIRE 96 192 96 176
FLAG 96 192 0
FLAG 320 96 out
FLAG 128 96 rc
SYMBOL Digital\\schmtinv 176 32 R0
SYMATTR InstName A2
SYMATTR Value2 Vhigh=5 Vt=2.5 Vh=1
SYMATTR SpiceLine Td=5n
SYMBOL cap 80 112 R0
SYMATTR InstName C1
SYMATTR Value 1n
SYMBOL res 128 16 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R1
SYMATTR Value 10k
TEXT 80 -104 Left 0 !.tran 0 100u 0 100n

Thanks, Helmut. I did have everything in there except td since it wasn't
mentioned in the LTSpice manual. That did it. But I still have a weak
output, dips about 3V from the rails with Vhigh=12 with some serious
inductive load and 2ohms in series. Somehow that doesn't look normal. Do
they have a finite output current capability?

When I tried to open your file I got a syntax error.

 

[Helmut Sennewald]

Thanks, Helmut. I did have everything in there except td since it wasn't
mentioned in the LTSpice manual. That did it. But I still have a weak
output, dips about 3V from the rails with Vhigh=12 with some serious
inductive load and 2ohms in series. Somehow that doesn't look normal. Do
they have a finite output current capability?

When I tried to open your file I got a syntax error.

Hello Joerg,

I copied my attached circuit into a file "osc.asc" and it worked.
You should copy the text from line "Version 4" to the end.
(The line "Version 4" is already part of the schematic file osc.asc.)


Version 4
.....
TEXT 80 -104 Left 0 !.tran 0 100u 0 100n


I think it has 1 Ohm output resistance.
Please add an E-source with gain 1 at the ouput to get a low output
impedance.

Best regards,
Helmut

 

[Joerg]

Hello Joerg,

I copied my attached circuit into a file "osc.asc" and it worked.
You should copy the text from line "Version 4" to the end.
(The line "Version 4" is already part of the schematic file osc.asc.)

That is what I tried.

Version 4
....
TEXT 80 -104 Left 0 !.tran 0 100u 0 100n


I think it has 1 Ohm output resistance.

Aha! Thanks. That explains it.

Please add an E-source with gain 1 at the ouput to get a low output
impedance.

Well, a 1ohm Z Out is pretty much what my final driver will have so
it'll be ok this time.

Thanks for your help, Helmut.

 

[Helmut Sennewald]

Add something like "vhigh=5 trise=10n". Essentially the 'trise' adds a
bit
of time reality to the gate. The help file is particularly obtuse in this
area. I've still to discover what that "ref" thing is there for.

Hello,

"ref" is the threshold for normal digital devices like AND and OR.
If you don't specify "ref", it's (vhigh+vlow)/2

The threshold for Schmitt trigger devices is "vt" and "vh", but not "ref".

Helmut

 

[jonathanscottjames]

schmit trigger oscelator. is there some kind of update that can fix all that?

i was using the free trial of multisim and it's schmit trigger works normaly. but lt threw me.
i tried t o uninstall it from xp pro sp3 in add/remove and it just blinkes. restarted and same..
at least now i can try to rtemodel its schmit trigger. thanks.
is there any other models that have to be altered t o make them do their functions?

 

[jonathanscottjames]

i meant to say ltspice4.08 works but won't uninstall. reinstalling didn't help

i meant to say ltspice4.08 works but won't uninstall. reinstalling didn't help