LtSpice computation limitation: Which conditions do affect it?
LTspice does not have a limit on the number of components or nodes.

Likely, not the number of components or the overall size of yor schematic is the problem, but you might be facing some no-nos that make your circuit hard to solve.

If you have capacitors, try adding a small ESR by editing the component properties. If you have inductors, adding a DC (copper) resistance is even more important.

Also, ideal diodes or ideal transistors won't solve well sometimes. Try using models of reals components (e.g. 1N4148 instead of the generic, unlabeled diode). Maybe your logic or opamp models interact in weird ways with their neighbourhood.

It is also possible that something in your schematic tries to oscillate at some very high frequency when, in reality, it wouldn't. (3 GHz around an audio frequency BJT? No way!) Such behavior is often caused by unwanted resonance of too-ideal parasitics or L/C tanks. Try locating the root cause for these possible oscillations and add some additional resistors here and there. Just as bad as severy oscillations are very, very steep spikes. Do you see some traces going up to the kA or kV range when all you have is a little, small-signal circuit?