PSRR Analysis in LTSpice

Question

I am performing PSRR analysis in LTSpice from this online tutorial. It shows PSRR analysis of LT 3042.

Here is my LTSpice schematic:

The thing is no matter how much I try, I only get data till 10kHz. What am I doing wrong?

P.S. Let me know, I will attach my .asc file if needed.

EDIT 1: When I change the .tran stop time to 2 sec, it shows the initial missing data, still the range is stuck at 10kHz.

Answer 1

The problem is your .step statement

.step dec param freq 10kHz 80MHz 100

In the SPICE Error Log (see below) you can see that the freq starts from 0.08 which is not what you intended. 80MHz seems to be interpreted as 80mHz i.e., 0.08 and the frequency starts at 0.08Hz and goes upto 10kHz. This is the problem.

To fix this, change the statement to
.step dec param freq 10e3 80e6 100

You can then simulate and see that the sweep starts from freq = 10kHz and goes higher like what you want

Answer 2

In LTSpice, 'M' is not a recognised suffix, you have to use 'meg'.

So your sim statement should say .step dec param freq 10kHz 80meg 6

Correction from @qrk: 'm' gets recognised as e-3, which is why you have to use 'meg'