skill
SPICE Simulation Skills
Public Made by Adomby adom
Pick, run and license the right SPICE simulator from an AI thread: ngspice in the container by default, LTspice and PSpice for TI on a Windows host for vendor models.
main
John Lauer
Publish 0.1.0
5442934
* Portable 12V->5V 1A sync buck - PSpice dialect (E VALUE, VSWITCH, probe resistor, CSDF output)
Vin vin 0 12
Vramp ramp 0 PULSE(0 1 0 1.98u 10n 10n 2u)
S1 vin sw hs 0 SWH
S2 sw 0 ls 0 SWL
L1 sw lx 15u
Rdcr lx vout 0.05
Cout vout ce 44u
Resr ce 0 5m
Rload vout 0 5
Sstep vout ld stp 0 SWH
Rld ld 0 5
Vstp stp 0 PULSE(0 1 3m 1u 1u 1 2)
Rtop vout fb 52.5k
Rbot fb 0 10k
Vref ref 0 PWL(0 0 1m 0.8)
Cff vout fb 1n
Gea 0 eo ref fb 200u
Rea eo 0 10Meg
Rc eo cz 10k
Cc cz 0 10n
Cp eo 0 100p
Dhi eo vhi DCLAMP
Vhi vhi 0 2
Dlo 0 eo DCLAMP
.model DCLAMP D(Is=1e-12 N=0.05)
Ecomp vc 0 VALUE={LIMIT(V(eo)*0.5,0.02,0.98)}
Ehs hs 0 VALUE={0.5+0.5*TANH(200*(V(vc)-V(ramp)))}
Els ls 0 VALUE={0.5-0.5*TANH(200*(V(vc)-V(ramp)))}
.model SWH VSWITCH(RON=0.1 ROFF=1MEG VON=0.501 VOFF=0.499)
.model SWL VSWITCH(RON=0.06 ROFF=1MEG VON=0.501 VOFF=0.499)
.TRAN 20n 5m 2.5m 20n
Rpv vout 0 1G
.PROBE/CSDF V(Rpv)
.END