Ideal switch turn off gets delayed?

QSPICE
1

Hi All,

I am making a PCMC simulation,

image
image1267×592 29.8 KB

The actual PCMC is implemented in C-code with fixed current reference set at 1A to turn off the SWITCH.

// Automatically generated C++ file on Thu Oct 19 16:11:47 2023
//
// To build with Digital Mars C++ Compiler:
//
//    dmc -mn -WD study_pcmc.cpp kernel32.lib

union uData
{
   bool b;
   char c;
   unsigned char uc;
   short s;
   unsigned short us;
   int i;
   unsigned int ui;
   float f;
   double d;
   long long int i64;
   unsigned long long int ui64;
   char *str;
   unsigned char *bytes;
};

// int DllMain() must exist and return 1 for a process to load the .DLL
// See https://docs.microsoft.com/en-us/windows/win32/dlls/dllmain for more information.
int __stdcall DllMain(void *module, unsigned int reason, void *reserved) { return 1; }

// #undef pin names lest they collide with names in any header file(s) you might include.
#undef CLK
#undef OUT
#undef IL

double pwm;
double clk_prev;

extern "C" __declspec(dllexport) void study_pcmc(void **opaque, double t, union uData *data)
{
   double  CLK = data[0].d; // input
   double  IL  = data[1].d; // input
   double &OUT = data[2].d; // output

// Implement module evaluation code here:
   if((clk_prev<=0.5)&&(CLK>=0.5))
   {
      pwm = 5;
   }
   if(IL>1)
   {
      pwm = 0;
   }
   clk_prev = CLK;
   OUT = pwm;
}

The question is, why doest the inductor current L1 current increasing higher towards the end of simulation ? (to be clear, there is no need for me to run the sim for 1s, except for curiousity)

image
image1900×1028 36.5 KB

From detail in the waveform, it appears if there is significant simulation step delays between when the gate signal rise and inductor current increase as well as between gate signal fall and inductor current decrease. Why is it happened?

image
image1898×1027 56.6 KB

Looking for some clue…

Arief,

2

More detailed capture with ID, IL, and IS1 showing there is delay in S1 gate signal and actual response

image
image1895×1027 72.9 KB

3

I just solved the problem by setting the switch model to have Vh=-1

after reading following information from the Qspice documentation:

S. Voltage Controlled Switch

The switch turns on when the control voltage is VT + VH and off at VT - VH. TTOL allows one to determine how accurately the switch time should be found. If the hysteresis voltage, VH, is negative, the switch smoothly transitions between RON and ROFF as is the standard behavior in circuit simulation since most analog simulators can’t solve circuits with discontinuities.

image
image1210×526 27.6 KB

image
image1920×1030 60.9 KB

Though it works, I still cant really understand what it actually meant with negative Vh, how does it meant to be like this?

Thanks
Arief,

4

This is an explanation of +ve and -ve Vh
Normally, setup a simply test circuit and you should figure the meaning of parameter.

image
image1856×992 189 KB

2 Likes
5

@KSKelvin,
what is the syntax to plot Rsw() vs V(ctrl)?
Trying: .plot tran Rsw() V(Vg1) gives both Rsw() and V(Vg1) w.r.t. time on same plot window.

thanks!

6

There is no direct command to do this; you have to right-click on the X-axis in the waveform viewer and assign the quantity manually.
You can save the plot settings for the next simulation run, but currently, there is no method to pre-define the X-axis quantity.

1 Like