If you use Gear or trapezoidal for the Default Integration method, things will compute as expected. You'll find this under the SPICE tab of the control panel. You still need to use double precision math (numdgt=15 setting).
Since you asked about the differences in integration methods in LTspice, here is a posting in alt.sci.engineering by Mike Engelhardt (brains behind LTspice), 21 Feb 2004.
Integration Method Explained:
Gear, compared to trap, has the advantage that it is numerically more stable, but less accurate. In
principle, it's better defined because Steven Gear even specifies when
you change integration order and timestep size. PSpice is hard-wired
to use Gear(well, the docs say it a proprietary algorithm, but it acts
like Gear.) The inaccuracy of Gear comes from the fact it dampens the
circuit. The amount of dampening decreases with decreasing step size.
Trapezoidal is faster and usually much more accurate. Occasionally
it's not as numerically stable, especially when running non-physical
circuits described with macro-models. It has the disadvantage that it
can ring as a simulation artifact. This can be disconcerting to novice
SPICE users. Most SPICE programs have some form of Trapezoidal
integration as the default. There's fair bit of leeway in trap
implementations, so I call them all affectionately cowboy integration.
Modified-trap is a proprietary algorithm that has the speed and
accuracy of trap but precisely cancels traditional trap ringing. It is
the most accurate method I know of.
If you're using LTspice, use the default of modified trap. Use trap
and Gear only as diagnostics. Gear will let you duplicate some PSpice
simulations. For example, if LTspice says a circuit is unstable but
PSpice says it's stable, you can switch LTspice to use basically the
same integration method of PSpice to duplicate it's erroneous results
for diagnostic purposes. Switch to pure trap instead of Modified-trap
if you want to see if your circuit is trap ringing. If the trap
ringing that Modified- trap cancels is spread over several circuit
nodes, then the cancellation might not work well. Using pure trap lets
you investigate potential simulation artifacts.
There's yet another method called backward Euler. Where mod-trap,
trap, and Gear are all implemented as 2nd order methods in SPICE
programs, backward Euler is the 1st order method. 1st order mod-trap,
trap, and Gear are all identical and simply called backward Euler. You
can use this method by adding the SPICE directive ".options maxord=1"
to your simulation. Backward Euler is as stable if not more so than
Gear, but is the slowest and least accurate of all methods.
The alternate solver runs with about 1000x more internal accuracy in the sparse matrix package but at half the
simulation speed. The advantage of it is that is solves certain
convergence problems. Here's a simple deck that demonstrates that it's
more accurate then the normal solver:
V1 1 0 ac 1
R1 1 2 1T
C1 2 X 1
R2 X 3 1T
C2 3 0 1
.ac oct 10 1 1Meg
Node V(x) should be -6dB for all frequencies. However, the normal
solver(and other other SPICE program) makes errors solving this
matrix. If you switch to LTspice's alternate solver, you get close to
the correct answer. The alternate solver was released on June 13, 2003
and was discussed in message number 434 of this group.
On Gear vs. Trap, here's a circuit that will illustrate that Gear is
over-stable, that is, it incorrectly dampens the circuit in the
interest of avoiding convergence problems:
L1 1 0 10u Rser=0 Rpar=0
C1 1 0 100p
I1 1 0 PWL(0 0 .1u 1 .2u 0)
.tran 1m 1m
(Mod-)Trap will give the correct answer, that is, that the current
spike starts the tank ringing and the ringing then continues
indefinitely. If you run that circuit in PSpice, it will only ring a
few times. This over- stability of the Gear causes an error and is
what makes many circuits converge in PSpice but not LTspice. PSpice is
giving you the wrong answer.