Spikes, surges and noise sources in LTSpice
You must be aware that one noise is not the other noise !?!?
OK, components in linear circuits (amplifiers for example) generate noise, mainly thermal noise and 1/f noise. This is type of noise is what I would call "small signal noise" meaning that these are small signals and you can evaluate them by using a linear representation of the circuit you're investigating. The noise properties of those two voltage sources concern this type of noise. Also you can only simulate the noise behavior of an amplifier by using the noise simulation, this is a variant of the AC simulation. If you would do a time (TRAN, transient) analysis of an amplifier, you CANNOT simulate the noise. OK, I use an advanced simulator called Cadence Spectre, it has a transient-noise simulation but I don't expect LTSpice to have this.

HOWEVER here we are dealing with a NON linear circuit ! It's a switching converter and therefore it has no "small signal transfer" like an amplifier would have. You can only simulate its behavior by running a transient (time) simulation. As I stated earlier, in a transient simulation you cannot simulate the noise.

Also, when talking about noise in relation to switched converters, that noise is not the thermal or 1/f noise of the individual components (see above). What is meant is the spurious content of the DC output voltage, so the variations that are on that DC voltage. Although it is called (switching) noise, it is different in that it mainly consists of spurious components (harmonics) of the switching frequency of the switched converter. "Proper noise" on the other hand (like thermal noise) consists of ALL frequencies.

The good thing is, you CAN simulate this switching noise by using a transient simulation. But the noise settings of the two voltage sources have no relation to this noise !

You want to know the suppression of the noise on the input voltage to the output voltage. This is called "line regulation". What I would do is place a sinewave source in series with one DC supply source (remove the pulse source, there's no use for it) and let it add a small (100 mV) ripple on the supply at a frequency of for example 10 kHz. Then at the output I expect to see peaks at multiples of the switching frequency with additional peaks at + and - 10 kHz around these peaks. The level of these additional peaks gives you an idea of the line regulation. Line regulation is frequency dependent so also try for other frequencies !