You do not have to use "ports" for the intermodulation simulations. Just set up the simulation and make your own measurements plotting output versus input. Nearly any transient simulation setup will also work for PSS/PAC.

The direct plot functions are just scripts for making measurements, so don't let it limit your ability to make whatever measurements you want or need to make.

I suppose you could fake out the tool by creating a PORT to current converter.

1. Take a 50 ohm port and simply load it with a 50 ohm resistor.

2. Take a current controlled current source (CCCS) and put the input in series with the port/resistor network (this samples a current that is dependent on the port source).

3. Now use the output of the cccs to drive the input of your circuit.


If the approach works for you then you can, if you wish, set the gain of the cccs such that the dBm input power sweep is translated to some convenient level of input current. A convenient conversion might be 0dBm available RF input power delivered to the 50 ohm input load is equal to 0 dBi in current (I'll let you figure out the gain to do this conversion).

Good luck

I'll mention (again) that you can avoid all of this hassle of trying to fit your circuit in a RF 50 ohm input/output port simulation box by just thinking about what it is you need to simulate and then set up the simulation to do it.
You can do a lot of straightforward input/output sweeps by just using the parametric analysis tool rather than relying on the built in sweeps and direct plot functions.


You don't need to do impedance matching because you are sampling current in the fake input circuit to produce a proportional current in the real circuit.

0 dBm delivered to a 50 ohm load produces 0.316 V / 50 ohms = 6.32 mA or - 43.98 dBi.

I assume you would like 0 dBm to be some convenient relation to dBi. Maybe 0dBm = -40dBi ? In this case you need the cccs to have a current gain of  -40 - (-43.98) = 3.98 dB or 1.581 A/A.
Be sure to verify that I did the math correctly.

For the output you can use a similar trick as the input, but in reverse. You sample your output current (using a series 0V voltage source). Then use a cccs with a gain of 1 V/V and place the output across series a 50 ohm resistor. Ground one node and call the out node the output. I guess the values in the fake output don't really matter that much because you are trying to find the input referred linearity; although, you really do want to be able to probe the actual input/output currents and voltages in order to understand what is limiting the linearity in your circuit.

*** Be very careful not to change the loading of the output when sampling the output current. If you reduce the loading on the output then the output swing will not be correct and the output linearity will also be incorrect. So just make sure you voltage and current swings are all the same before and after using the added input/output circuits.

Ok, I guess we've got a slight communication breakdown here.

I have been assuming, from your previous posts, that you have a current mode input circuit and you are just trying to find a way to make the built in sweeps work with your circuit. But you are also saying, now, that you need to know the true IIP2 for your calibration routine.

Voltages and currents at any particular point in a system can always be related to the signal at a control impedance (i.e. 50 ohm or whatever) point in the system (LNA or amplifier input for a receiver). So what you need to know is where is the control impedance point of your system and how does it relate to the current that is driving the input of your current mode circuit. You really need to define this first to understand what to do to present the correct level signals to your circuit and interpret the linearity results.

dBi is 20log10(abs(I))

I may have a slight rounding error in the current.