Electronic – spice plot resolution – sinusoid does not look continuous

spice

Problem

How does one increase the resolution of a SPICE plot? My sinusoidal signal doesn't look continuous, it looks very 'pointy'. I am using MACSPICE3 to simulate a non-inverting op-amp by using a dependent source (VCVS). Changing the step parameter of the tran command has not helped.

I understand that results data is stored in a construct called a plot, which is comprised of vectors. Is this pointy phenomena linked to the data in these constructs, or the graphical representation?

Example of a pointy plot

Pointy SPICE plot

Netlist

Basic Non-Inverting OpAmp

V1 2 0 AC sin(0 10 50 0 0) DC 0

RBogus 2 0 10K

e 3 0 2 1 999K

R1 3 1 10K

R2 1 0 10K

.control

delete all

tran 1.0ns 100ms

plot v(1) v(2) v(3)

op

display

print all

show all

.endc

.end

Note:

RBogus exists to create a closed loop for the ac source.

Best Answer

The syntax is

.TRAN TSTEP TSTOP [ [ TSTART ] TMAX ] [ UIC ]

Changing

tran 1.0ns 100ms

To

tran 1us 100ms 0 1us

has solved the issue. In the user guide, note that the TSTEP doesn't exclusively control the step size. TMAX must also be set. The boldface text explains why.

  • TSTEP is the printing or plotting increment for line-printer output. For use with the post-processor, TSTEP is the suggested computing increment.
  • TSTOP is the final time
  • TSTART is the initial time. If TSTART is omitted, it is assumed to be zero. The transient analysis always begins at time zero. In the interval , the circuit is analyzed (to reach a steady state), but no outputs are stored. In the interval , the circuit is analyzed and outputs are stored.
  • TMAX is the maximum step-size that SPICE uses; for default, the program chooses either TSTEP or (TSTOP-TSTART)/50.0, whichever is larger. TMAX is useful when one wishes to guarantee a computing interval which is smaller than the printer increment, TSTEP. enter image description here http://www.macspice.com/ug/sec4.html#s4.3.9
Related Topic