Is it enough to use s-parameters model for transistent and hb simulation?

for example, in qucs simulator. is it necessary to have schematic device model, or it can be replaced by s-parameters for certain bias and operating point conditions?

S-parameters are small signal parameters but HB and Transient simulations need large signal nonlinear models.I mean, even if you change bias/supply or driven voltage etc. the ouput will be same and erroneous because they are linear and independent from your simulation conditions.Using s-parameters in HB or Transient simulations doesn't make sense.
In additional to this, discontinouty between sampled s-parameters will create some convergence problems.

thank for the reply. But also some small question to make things more clear. What if i use biasing for certain s parameters, so real value of current through biasing resistor is exact, it is still will be not useful to use S-parameter?

Also i want to ask this: there is device model schematic in some datasheets. There some capacitors, inductances, etc. with parameters. Is there any hope that using such schematic in free simulator like qucs i can get results that are not too far from reality? I tried to download spice models made for ads, mwo, spice etc. all paid programs and import that data into qucs, but it is not worked. file format is different, and qucs internal conversion utility gives syntax errors. So i want to draw this schematic by myself and do simulation, as i understand spice model and that schematic in datasheet is the same thing, right?

The measurement conditions of measured s-parameters are mentioned in s-parameter datafile ( Touchstone or MDIF etc)
I repeat again here. S-parameters "AC Small Signal Parameters" and they are not defined at DC ! Because the frequency is Zero at DC, that's why s-parameters can not be used at DC.Even if you use s-parameters of a resistor which a current flows through it, the simulation will be false.The simulator will make an extrapolation down to DC while HB or Transisent simulation is used and therefore simulator will not either converge or will be completely erroneous.
Instead, use a RLC model of this resistor by using s-parameters ( Broadband or Narrowband Model SPICE Model Generator of ADS or the others) and use it as model.It's more accurate and troublefree..
A simple resistor will have an ideal resistor with a parallel capacitor and there will-may be-a series inductor if you work at very high frequencies.It's very simple to modelize a resistor..

Yes, you should draw your own schematic by placing intrinsic model ( of active device ) and peripheral parasitic end environmental elements around it.

Using S-Parameter models give the results for the device at the current the S-Parameters were measured. Most S-Parameter sets are available for several bias currents.

The capabilities of qucs are listed here. -->http://qucs.sourceforge.net/tech/technical.html
I have not used it much, but for what I did do, the results are the same as when using MWO.

qucs has most of the fast equation models for FET and Bipolar devices, so that you enter the math model parameters.
The hoops one has to jump through in getting proprietary models going in commercial simulators is often similar to the effort to attach a model, with parameters maybe adapted from other formats, to use in qucs. Most simulators try to be incompatible.

You can make subcircuit models from model equivalent circuits, but it will cause a significant slowdown when using Spice-type simulation and time domain transients to simulate. That is why specialist companies like Modelithics sell fast equation type models.

Use S-parameters on the assumption the bias circuits are figured out, and go for the matching etc.

Use a few cycles of signal simulated in Spice option to check for distortion and suchlike if the levels are large enough to threaten non-linearity. I regret I cannot help more on using qucs, because I am still trying it out. For a free thing, it does a surprising amount, and what you are unhappy with, you have the opportunity to modify, or ask the user community to help. The code is open source.

Thanks for the replies. Also i want to ask what is usual startup time of 2.4ghz and 5ghz oscillators? how much ns startup time is good, how much we need to simulate to see steady state?



What if harmonic balance gives no result, but transistent simulation works. What can it be? Wrong setup of hb schematic?

For the osc startup time, you can use ADISimPLL to simulate it, there are many factors can impact it. Usually about us level.

In order to start-up an oscillator, sometimes a temporary excitation signal ( a short pulse or step response etc) is neccessary to wake-up the circuit.This connection point depends on circuit topolgy and other factors.But nobody knows how long it should take, you must define it by trying.
In ADS, there is an option in HB simulation controller. Transient Assisted Harmonic Balance.This can help you to excite the oscillator and find the its' HB outputs.
With this option, HB simulate the circuit with a transient simulation in a short period then once it has found " Steady State Response" then it stops and arrange resting HB simulation.
I use this option with hard to start oscillators and it's really perfect option for them..