Simulator development: Modeling (S & P)

System channel is usually represented in S-parameters. They can be extracted in frequency domain using a 3D field solver, and/or cascaded stage by stage using tool like SPISim’s SPro. With LTI (linear time invariant) assumption, it’s possible to synthesize eye or BER plot of millions of bits using statistically analysis… using single time domain pulse for these parameters. However, it’s still often desired to be able to simulate the s-parameter in time domain for defined bit patterns. Thus, a system simulator like our SSolve must be able to support such requirement. In addition, one may also want to know the frequency response when given a broadband spice converted spice elements, such as via, package or connector models. So the reversed process, i.e. extract S-parameters from spice elements, is also often required. In this post, we will briefly talk about how these may be developed in simulator like SSolver.

S-Element… S-Parameters:

There have been many conference and journal papers proposing different methods of simulating S-parameter in time domain. However, at the most basic level, S-parameter can be considered as a transfer function or filter block. Thus DSP techniques can apply: transfer function multiplying inputs in frequency domain can be converted into time domain using convolution:

Convolusion

The time domain at the right hand side can be further separated into two parts: history up to this time point (integrate from -infinity to t=n-1) and the value at this particular moment t=n due to input. The first part is a constant as it’s already happened in the past and can’t be changed, the second part is, however, input dependent and must be updated within the “solve” and “stamp” hot loop inside newton iteration. When putting together, they form a Norton circuit form of I = Y * V + J where Y is value affected at this moment and J, a constant, is due to past history. This Norton form can then be “stamped” accordingly for matrix solving.

Interested reader may refer to the paper published by HP linked below for detailed explanations and math:

Integration of Transient S-Parameter Simulation into HSpice

The equation [18] and [19] is the aforementioned Norton equivalent circuit form and can be used accordingly.

The convolution method needs to update history with the solved results of this time step for next time step to be used. In addition, the basic convolution requires that the dt to be constant, thus a variable time step simulation will be greatly hampered by this requirement in terms of performance. So the convolution modeling has rooms for improvement.

One of the possible approach is using vector fitting technique mentioned in previous post about “W-element” modeling. With the S-parameter data in frequency domain, one may construct a Pade approximation using several poles and zeros. Then basis functions can be created for each of the pole in time domain and simulate accordingly. A benefit of this process is that the constructed form is a rational function which is guaranteed to be causal. So if there are issue regarding causality of the provided s-parameter, it can be fixed during the modeling process. Lastly, due to exact fitting of multi-port s-parameter across the frequency spectrum are not likely, some sort of error minimization (in the MSE sense) is needed to have a balance between accuracy and number of poles.

 

P-Element… Port element:

Often times after a package, connector or via modeling engineer created a model, he or she will use tool like broadband spice to convert such 3D extracted s-parameters to spice equivalent circuit composed of various basic elements. When a system designer or SI engineer receive such converted models, the original S-parameter may not be available already. Rather than insert this model into the channel and simulate blindly, it’s often beneficial to be able to reconstruct and inspect the model’s frequency domain response first before actually using them. S-Parameter extraction via simulation is basically a form of AC simulation, thus with AC model of the system elements constructed, the S-Parameter extraction part becomes easy.

The context here is small signal S-parameter extraction, thus all the AC signal is done very close to the operating point. That is, a DC solution needs to be obtained first for each port’s respecitve bias condition, then the AC stimulus is applied and solve for each frequency point.

A “Port” or “P-element” has several properties: dc bias condition, reference impedance, port-name and port-order. For a multi-port s-parameter extraction, one port is excited at a time with specified dc bias value. AC sweep is then performed while the other ports are terminated to their reference impedance. The power wave of input and output, measured and processed using current injection and nodal voltage measured, can then obtained for this input to the other output ports. Using simple math described in the link below:

S-parameter measurements

one can obtain S-parameter of Sij (i is port with input stimulus, j are the other ports) content easily this way. Repeat the same process for the other ports one at a time (with their respective dc bias condition) and the full S-parameter can be obtained. Finally, the order of ports are arranged according to the port properties, their respective port name are written out at the top of the touch stone file and the process is complete. Should there be needs to convert to other formats such as Y, Z parameter (sometimes good for checking connectivity), one can do so easily with formula (assuming generalized 2-N ports) or simply use developed tool like our SPro.

 

Back to the top:

Back from these modeling physics to the computer science domain, one also need to consider the following topics when doing simulator development:

  • Memory pool management (allocation, expansion and clean-up)
  • Multi-threading consideration
  • Plug-in architecture for future devices
  • ….

While the list can go on and on and the tasks may be daunting, the end results are definitely worthy to the analysis flow and methodologies development. With developed simulator, there is no longer absolute need to form a close-loop formula or equation in order to solve circuit equation. The module or flow running on top can simply create netlist and have this simulator solved for you. Not to mentioned this also make maintenance and testing much easier. For an EDA company like us, I would say this is a journey worth taking.

Leave a Reply

Your email address will not be published.