The Periodic Steady State is a large signal calculation. This means that non-linear behaviour is part of the math. The DC simulation calculates the bias point (e.g. gm of a transistor) and then the AC simulates with the values calculated in DC (this is a linearisation of the circuit).

When a large signal is applied the bias point change with the time, hence a simple DC is not enough. For example imagine a MOS transistor with a large signal applied on top of a bias voltage on the gate, the Vgs varies with time and until the voltage explore the linear zone (saturation) of the MOS, a DC+AC is ok. Now if the signal is large enough for a certain time the MOS will be off and for the other time ON. This means that the gm is not constant and then a PSS is needed.

Now for your questions:

1. The DC is not calculated for each time but the circuit is resolved in time domain shooting simulation) like for a step response. Of course there are two limitation: the signal should be periodic and linear as explained in spectreRFTheory document.

2.Typically for IIP3 simulation the power of the PSS tone and the power of the PAC tone vary together, so you should put a variable and then sweep in PSS domain. With direct plot you should select variable instead of spectrum and then plot the 1st and 3rd harmonic from IPN curves tab.

3.The IIP3 should not change with the input power. Check if you setting correctly the simulation. Or let me know if you need some explanation on that.

BR,

Ivan

Hi guys I have a problem regarding IIP3 plots. My IIP3 is not rising by 3dB. As I am designing a passive like attenuator and dealing with very low voltages, PSS an PAC simulators does not function properly when transistor Vds is close to zero. I have done the transient, reduced power and pretty confident that the circuit is working fine. But I really need to find a trust worthy way to generate the IIP3 curves as PSS and PAC analysis cannot be trusted. Now I am trying to apply a small bias voltage at the drain just to get the curves but that is getting things very complicated. Sorry for writing in your Post but I landed here while I was searching for solutions and thought I ask. Best regards.

Hi,

you can try to increase the power sweep range of the PSS signal and also the absolute values. You can also try to put both signal in PSS. The simulation time will be much longer but you should have better results.

Last chance is to run a transient simulation, apply Fourier transform to the output and "measure" the power difference between linear signal and IM3. With that you can have the IIP3. Repeat for different power and you can plot a curve.

Anyway, what does it mean a "passive like" attenuator? If your circuit is purely passive you cannot have any kind of non-linearities.

Thank you for the fast reply. I am actually applying the transient now. And I can get the values but I was hoping for a simpler solution as my final goal is to get the curve for IIP3 VS Attenuation which depends on a control voltage which I apply to the shunt transistors.

By passive like I mean that the transistors in the attenuator are in their triode region and are working as variable resistors. The idea is to use the inherent linearity but I will have to generate the linearity curves to show that it is actually inherently more linear than a VGA and also how we can improve the linearity.

I applied a bit of bias voltage at the drain of the transistor to forcefully make it work and the PSS and PAC analysis are working but the operation for obvious reasons is varying even though the variation is negligible.

Since you seem to already have a good grasp about the techniques of measuring the IIP3 my question to you is that now that I have forcefully got the VDS a bit higher do you think the curves generated are accurate (as the operation and attenuation curve is varying very slightly due to the biasing voltage). Ps. bro because of technical difficulties I cant go further even though my design is almost done. Thank you once again and best regards.

Hi Shashwata,

the problem is that you're exploring a discontinuity in the model representation of the MOS. Probably you're getting some curve going up and down. This is what typically happen with passive MOS if the PSS signal is too large (e.g. mixers). 

I think it's not accurate to simulate the IIP3 imposing an offset based on my experience with mixers. But you can run a parametric analysis sweeping the power as variable and plotting the results of the IIP3 formula. This should simplify the work. Anyway try also to increase the PSS accuracy may could work.

BR,

     Ivan

Hey Fabiano,

Thank you for the suggestion and you are right the PSS and PAC is not reliable with biasing. On a different note now my supervisor for my thesis is super suspicious about all the simulations. He now wants me check the S parameters (211 and S21) in transient. I can see that the circuit is working by a simple transient analysis but he wants  me to generate the s parameter curves by using transient as transient analysis is the only one trusts. I cannot seem to generate the S parameter curves. Any suggestions?

Hi Shashwata,

From transient simulation you should get V/I and calculate real and imaginary part. Typically you want to see the S-parameter across a frequency range. You should run a parametric to sweep it.

My suggestion is to try the Harmonic Balance simulation. It works like PSS, so you need to run a hb and then the others simulations. Try it for IIP3 (hb+ hbac) and S-par (hb+hbsp). Remember to increase the accuracy (also for PSS).

BR,

Hey Fabiano, thankyou for the insight. Much appreciated. But now it turns out even the transient cannot be trusted. I spoke to some of the Cadence guys and it turns out that the transistor model is at fault. Anyway on a different note need help on a one last thing. I am new to op-amp design and my question is do you think a sigle stage op-amp is enough for generating a voltage just to match the circuit to a 50ohm load as I dont require it to amplify anything I just need it to basically work as a feedback amplifier to get the voltages at the inverting and noninverting same by generating a matching voltage. I used a default amp for the design but my supervisor said that I have to design my own amp. Here is the image of a ciruit similar to what I have designed. I know it's a silly question but just wanted to check if A single stage opamp is fine for the application.

http://snag.gy/UDHjD.jpg

I think it's better if you create a new question for the Op-Amp.

Hi Fabiano,

                  Sorry that I am replying after long time. Still my IIP3 problem is not solved yet. 1-dB compression point is coming fine but IIP3 is varying depending on the input signal magnitude. LNA is for 5.5 Ghz, I am following these steps to simulate IIP3 performance.

1. First setting PSS: Two tones are considered to be separated for 50 MHz (besides, on what basis two tone separation is decided? ). So I selected my beat frequency as 50 MHz. Accordingly, selected array of indices are 90 100 110 and 111.

2.PAC setting: Single point input frequency is set at 5.55 GHZ i.e. is f2. Maximum sideband is selected as 3. PAC magnitude is set to -50dbm bcz 1-dB resulted is -13dB.

3.Plotting IIP3: Single input power value is set to -50 dBm. 1st order harmonic f1 as 5.5 GHz and 3rd order harmonic 2f1-f2= 4.5 GHz.

When I plot these, I am getting IIP3 of -1.82 dBm.

I ran same thing for PAC magnitude of -40 dBm. Now 1 dB remained same but IIP3 point shifted to +3 dBm.

Am I doing wrong in any of above steps?

Thanks a lot for your response Fabiano.