The LSSP spectre simulation (Cadence 5) fails with the following error

The first error is because you're using too old a version of Spectre. My guess is that maybe you're using the spectre from IC5141 (which is not a good idea because it hasn't really been updated since 2004, when we split off spectre into a separate stream, initially MMSIM but later the SPECTRE stream; there have been 16 major releases of the simulator since then. As far as I can tell, the LSSP support was added later (I can't quite remember because this was a long time ago), and I think it needs spectre version 11.1 or later (coming from the MMSIM11.1 stream). I tried with the spectre from IC5141 and get the failure you do, but if I use 11.1 then it works fine (just make sure you have the <MMSIM>/tools.lnx86/bin in your path before the path for the IC5141 software.

I can't answer your second question because I don't know what your simulation set up is, but I suspect you're not comparing like with like with respect to ADS.

Andrew.

The first error is because you're using too old a version of Spectre. My guess is that maybe you're using the spectre from IC5141 (which is not a good idea because it hasn't really been updated since 2004, when we split off spectre into a separate stream, initially MMSIM but later the SPECTRE stream; there have been 16 major releases of the simulator since then. As far as I can tell, the LSSP support was added later (I can't quite remember because this was a long time ago), and I think it needs spectre version 11.1 or later (coming from the MMSIM11.1 stream). I tried with the spectre from IC5141 and get the failure you do, but if I use 11.1 then it works fine (just make sure you have the <MMSIM>/tools.lnx86/bin in your path before the path for the IC5141 software.

I can't answer your second question because I don't know what your simulation set up is, but I suspect you're not comparing like with like with respect to ADS.

Andrew.

Firstly, Thanks for your clear answer.

for the 2nd question 

I actually applied the SP analysis and it gives approximately the same results of ADS.

when I applied the PSP analysis for lower power level (-5 dBm at the linear region of my power amplifier), it gives these weird results as mentioned before.

So, what is the possible problem for that? and what is the main difference between SP and PSP analysis?

or I can satisfied with the SP analysis for the PA

The sp analysis computes the s-parameters around a single dc operating point. So no "power level" can be involved, because there's no time varying signal and it's a completely linear analysis. The psp analysis first computes a periodic steady state (a time-varying operating point over the period) and then does a linearisation of the circuit equations over the time-varying operating point - so it is a time-varying linearisation. This means that signals can be translated in frequency by that time-variant operating point. When you run a psp analysis, you specify a "virtual port" (the port number and the sideband for that port) so that it can compute s21 between different frequencies.

When psp is applied to a PA though, what you are doing is computing the linear s-parameters (swept over frequency, usually) when there is a large-signal (maybe a blocker). This is different from what LSSP does/ With psp it's like having a second small-signal input together with the large signal altering the behaviour of the PA; with LSSP, the s-parameters are computed with just a single frequency applied - the large signal.

I cannot explain why you're getting these weird results. As I said earlier, I can't see your simulation setup - it would be best to ask this to customer support so that we can see your data (even though you're running an ancient version of Virtuoso). Whether sp is sufficient for your PA rather depends on what you are hoping to measure!

Andrew.

Thanks for your efforts in answering m 

When I make a PSS analysis at Cadence SpectreRF, it gives me some warnings related to the breakdown voltage, as follows

However when I test the transient response of the voltage signal between the two related nodes (drain and gate), I found that the voltage does not exceed this value (4.08), as shown in the following figures.

Thus, I do not know about the meaning of this error and if the transistor is fabricated it will go to its breakdown region

Sometimes these messages occur as PSS is trying to converge. The Shooting Newton method is trying to solve for the final settled steady state of the circuit, and sometimes as it is iterating towards a solution, it will move the operating region outside the correct place and then you might see these breakdown type messages. Usually you wouldn't expect to see that in the final iteration though when it reaches convergence - you should check the time domain waveforms from the final PSS solution to see if they appear to be in the correct region (it would be odd for it to converge in an invalid region though unless the models are non-physical). So usually this is nothing to worry about, just an indication that the circuit is a little problematic to converge.

Regards,

Andrew.