Original question:
No simulation model for this chip after 4 years for tina ti
Hi Rangel,
Generally speaking, I would recommend to just hard-code the pulse for your simulations. To determine pulse width and other behavior of the real device, I recommend building a prototype using our EVMs and sample devices.
-
Generating a pulse in SPICE can be done many ways -- getting an accurate monostable multivibrator circuit is very difficult, but I can help you with a pulse generator circuit pretty easily.
My circuit just watches the input for a high state, then delays that in a second signal and combines the two with some logic (one inverted input AND gate) resulting in a pulse equal to the delay.
Here's the SPICE code:
* Pulse generator using RC delay element
.SUBCKT PULSE_GEN IN OUT VCC VEE
* Pulse width value is in nanoseconds
+ PARAMS:
+ PULSENS 100
* Input is buffered to avoid loading issues
* Threshold is set to VCC/2
EINBUF INBUF VEE VALUE = {IF(V(IN,VEE)>V(VCC,VEE)/2,1,0)}
* Threshold value for timer circuit (1 time constant)
VTHR VTH VEE 0.632119
* R*C provides delay for pulse generator
R1 INBUF TIMER {PULSENS}
C1 TIMER VEE 1E-9
* Delayed output from the timer
EDELAY DELAY VEE VALUE = {IF(V(TIMER,VEE)>V(VTH,VEE),1,0)}
* To get the delay, I multiply the input state (0 or 1) by the
* inverted delayed signal state (0 or 1) to get a short pulse
ELOGIC LOGIC VEE VALUE = {V(INBUF,VEE) * (1-V(DELAY,VEE))}
* I then use the VCC/VEE connections to determine the output voltage for the pulse:
EOUT OUT VEE VALUE = {V(VCC,VEE) * V(LOGIC,VEE)}
.ENDS
*$
And my Tina-TI example file: