Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It only takes a minute to sign up.
Sign up to join this community
I am curious about what numerical methods are used in circuit simulation. Googling around, I did not find many technical descriptions of the actual numerical methods used for example by the variety of SPICE simulators.
I am not curious about using a simulator, or analyzing circuits, but understanding what the actual numerical methods used are, how they are implemented, etc. What are the key resources?
For an overview of numerical methods in circuit simulation, I'd suggest reading some of the published SPICE papers, and in particular Laurence Nagel's exemplary PhD thesis:
From the abstract:
The numerical methods that are employed in [versions 1 and 2] of SPICE are presented in detail. These methods are chosen according to guidelines that are presented in the introductory sections of this thesis. Different guidelines probably would result in the implementation of different methods. The widespread use of SPICE, however, indicates that the algorithms that are employed in SPICE are applicable to a wide range of practical circuit simulation problems.
Nagel was the "ad-hoc team leader" of the simulator CANCER, which was an MSc class project at the University of California Berkeley. This was renamed SPICE, released in 1971. It was written in Fortran; Nagel earned his PhD with SPICE v2. Then others took over the program. SPICE was rewritten in C and released as SPICE 3 in 1989. As it was open source, this was the basis of the other SPICE programs.
As a thesis, it is extremely well-written and covers the material clearly, covering the state of the field at that time. As the most influential simulator, it was the starting point for pretty much every subsequent project of this kind. Regarding numerical methods, the conclusions are especially clear about which work well and their performance issues in space, time and the need for stiffness-stability. About a third of the bibliography is about numerical methods.
The numerical methods covered are:
Because most interesting circuits are non-linear the nodal equations can't be solved directly by straightforward methods (eg. LU decomposition), so Newton-Raphson method is applied to converge to a solution within tolerance criteria. Nonlinear components are linearized about an operating point and a new operating point is calculated, repeating until convergence is achieved.
Once an operating point has been found, for transient analysis a numerical integration (using one of several possible methods) is used to calculate the effect of capacitors and inductors for the next time step and the process repeats. Time steps are dynamically chosen from tolerance criteria.
For AC analysis, the operating point is calculated and linear models are used.
You can refer to documents such as UC Berkeley memorandum ERL-M520 (424 pages) authored by one of the originators of SPICE. For example, he discusses Runge-Kutta and its drawbacks and modifications.
The book Inside SPICE by Ron Kielkowski has a lot of detailed information, concentrating on SPICE 2g.6. The information on the timestep control algorithm variations may be of interest.
From here is a flowchart of the program flow:
Of course you can download the source code for some versions of SPICE (Berkeley has some C code available) and examine it.
Most of them use either the plain trapezoidal approximation or Gear integration. LTspice specifically also has a proprietary modified trapezoidal method that they claim is less prone to spurious oscillation than standard trap but more accurate than Gear.
It would theoretically be possible to use other differential equation solvers, like the Runge-Kutta method or the Yoshida algorithm, but for one reason or another they don't tend to.
It might be enlightening, if you want to know more, to look at the code of open-source SPICE implementations, as well as non-SPICE simulators like QUCS. Or to just read some books on numerical integration and linear algebra.
