Playing with multisim I've noticed a strange behavior on a very, very basic circuit: a push button with a pull down resistor and an electrolytic generates more vcc than provided!? Of course this is not possible with this minimal circuit, so I think I'm missing something about the software or the simulation engine... Could you please suggest me where I'm wrong?
This is not a simulator fail. It is a very well known behavior of ANY simulator (SPICE based or otherwise) that uses the trapezoidal integration method. The trapezoidal rule may generate these "spikes" every time the Jacobian matrix of the system is abruptly changed; for example after flipping an ideal switch. That being said, the trapezoidal rule has many advantages: smaller truncation error, zero phase distortion, A-stability, and small number of history terms. For those reasons it is often set as the default in many simulators. If you want a "spike" free simulation use the Backward Differentiation Formulas (BDF) often referred as the Gear Integration methods.
To change the integration method in Multisim:
Simulate->Interactive Simulation Settings->Use custom settings->Customize->Transient
and change the "Integration method" from "Trapezoidal" to "Gear". The default order of the "Gear" method is set to two (max is 6). Gear order two is neither the fastest nor the most accurate, but it is the only one BDF that is A-stable. So you'll playing it safe by leaving the order at two.
p.s. A-stable in this context means that you simulation will not get numerically unstable with any eigenvalue with a negative real part.