Strange result when simulating RF low pass filter with Pspice
You should add a label at least for the plotted waveforms because nobody can tell which node is N002 &amp; co. Also, using passive elements means there is no gain, and thus the output will always be less than the input. What you have there is a voltage divider, followed by another, etc. Even if those are ideal LC elements, the resistive divider formed by the input and output cannot be avoided.

If you mean that you should see the 6 dB at the lowest frequency, then you should simulate to include DC (or closest to it). And, since your filter goes into hundreds of MHz, then a linear scale is better (in the comments I proposed log scale to match the one in the example): .ac lin 1001 1m 1g will allow you to see what you've missed. Using dec (log scale) means every decade there are N points. Using lin (linear) means from start to finish there are N points. Since for this case you want to see pretty much from DC to light, then lin makes more sense, but .AC analysis go very fast and, if you're really in dire need of points, you can choose dec with 10k points; it's overkill for this case, but it's not forbidden or impossible.



If you're expecting the response to be as in the picture you provided, as I said in the comments, they are showing the response of the mathematical formula, which does not include the attenuation given by the I/O impedances:



Not lastly, there are some builtin parasitics that may affect the response, but not in this case. If you really want to go pedantic about it, then you can set Rser, Rpar and Cpar for all elements to zero, and for capacitors Lser and Rshunt, too. Also, this is LTspice, not PSpice, and the results are accurate for the given input (same in other SPICE programs).