Massimo,
Please can you report some additional information about the alternate
solver? Which are the main differences between the two solvers?
Is it possible to understand why you have added this new solver? Are
there some limitations in the old one? Which are the circuits in which
the new solvers is more accurate?
The alternate solver uses a sparse matrix package that
accumulates much less internal round-off error. The new
sparse solver uses (what I call) a vertical solution method.
It runs at about half the simulation speed but 1000x more
accurately as far as the matrix solution goes in the test
cases that caused the investigation.
For practical circuits, there's no need for it. But some
opamp macro models use unphysical components that lead to a
difficult-to-solve linearized circuit matrix. I found three
ways to solve the problem, but only released the method to
use a more accurate sparse matrix solver that has less round-
off error because (i) it was of the most general use and (ii)
it's the hardest for other SPICE programs to duplicate. This
also gives a nice diagnostic that allows one to check if
numerical round-off is an issue by switching between solvers.
I think it's an interesting, very high-power means to solve
the problem and I don't know of any other SPICE in academia
or commerce that uses this vertical solution technology.
Intellectual property concerns don't allow me to feel
comfortable revealing the theory behind the implementation,
but you should find the operation to be exactly as I describe.
Besides the sparse matrix solver, there is no other intended
difference between the two SPICE solvers in the current
release. There's basically two copies of LTspice in the
executable because the new matrix solver is not compatible
with the old one so a copy of LTspice had to be modified to
work with it.
Anyway, I recommend only using the normal solver unless you
run into singular matrix issues. The normal solver usually
will be just as accurate as the alternate solver since round-
off error in the sparse matrix is rarely the limiting factor
to the accuracy of your circuit's solution. If you develop
macro models for others to use in possibly other simulators,
I definately recommend that you use the normal solver, or
could end up with a model that only LTspice can solve.
But of course I appreciate people testing both solvers and
reporting any un-intended differences between them. It was
a huge reorganization of the code to have two versions of
LTspice in the same executable. I find the feedback I
get from this, other groups, and individually extremely
valuable to the quality of the program.
--Mike
__________________________________
Do you Yahoo!?
SBC Yahoo! DSL - Now only $29.95 per month!
Mike Engelhardt