series resonant dc-dc converter (pspice to capture) HELP

[cokokerem]

series resonant converter

hi..!!
i want to circuit design psice command to capture
my circuit name is SERIES SESONANT DC-DC CONVERTER...
i'm drawing this circuit but, circuit waves is not true
this is commands
SERIES RESONANT DC-DC CONVERTER (sresdc.cir)

.PARAM F = 120k
.PARAM CR = .08uF
.PARAM LR = 30uH
.PARAM RL = 10
.PARAM CO = 100UF
.PARAM VS = 100
.PARAM TRF = 10NS
VS1 1 2 DC {VS/2}
VS2 2 0 DC {VS/2}
*SWITCHES ( unidirectional )
S1 1 13 20 0 SMOD
DS1 13 3 DMOD
S2 3 12 10 0 SMOD
DS2 12 0 DMOD


VCONTROL 10 0 PULSE(-2 2 0 {TRF} {TRF} {.5/F} {1/F})
VCONT2 20 0 PULSE(2 -2 0 {TRF} {TRF} {.5/F} {1/F})

*FEEDBACK DIODES:
D2 0 3 DMOD
D1 3 1 DMOD

*RESONANT LC
LR 3 4 {LR} IC=-4
CR 4 5 {CR} IC =-80

*RECTIFIER DIODES
DR1 5 6 DMOD
DR2 7 2 DMOD
DR3 2 6 DMOD
DR4 7 5 DMOD
c1 5 6 1n ;small capacitors help convergence
c2 7 2 1n
c3 2 6 1n
c4 7 5 1n

*LOAD:
RL 6 7 {RL}
CO 6 7 {CO} IC = 40

*MODELS:
.MODEL DMOD D(N=1E-2) ;idealized diodes
.MODEL SMOD VSWITCH(RON=.01)
*CONTROL STATEMENTS:
.PROBE
.TRAN 0.05MS .1MS UIC
.OPTIONS NOPAGE reltol = .0001
.END


this is my drawing circuit (in attach)

 

[eem2am]

resonant dc-dc converter

i dont think its practical to simulate resonant converters as the sim time is too long.

unless its a very simplified sim

 

[cokokerem]

resonant dc dc converter

thanks for interested my problem ...

 

[FvM]

series resanance converter pspice

circuit waves is not true

What is wrong?

i dont think its practical to simulate resonant converters as the sim time is too long.

SPICE simulators are a good tool to simulate different aspects of power converter behaviour to my opinion. You get valuable insights in a fair simulation time, some minutes at maximum, a few ten seconds in typical cases.

Of course, the simulation setup should be choosen appropriately. It's not about a "very simplified" setup rather than a suitable level of abstraction. According to the schematic, cokokerem did this by using SPICE switches instead of real transistors. This setup implies, that you are not interested to evaluate transistor switching behaviour (e.g. current rise time and switching losses) in this case rather than overall behaviour of the converter.

I have done a lot of similar simulations, e.g. of resonant converters or multiphase PWM converters, including PWM generation and control loops.

PS.: I see three points, that unsuitale for a real resonant converter, to my opinion.
1. The resonant circuit impedance is too high, I would scale it down e.g. by a factor of 10.
2. A loss resistance, always present in a real circuit and required for stable operation should be added.
3. The converter should be driven somewhat below the series resonance.

I got meaningful waveforms with F=95k, LR=3uH, CR=0.8uF, RR=0.05

PPS: The said F < fr dimensioning causes a small dead-time in resonant circuit current. It's also usual, to blank the switch drive during this interval. This mainly creates a margin for resonant frequency variation and avoids high current transients. Duty cycle ramping furthermore is a means in starting the resonant converter with limited current.