Hspice does not give correct energy consumption for a RC circuit connected to a DC supply
I think your simulation is flawed. When you run a transient analysis the simulator first calculates a dc operating point. As I recall the .IC statement provides a suggestion of possible initial conditions but is not a hard requirement. Since you have just one voltage source and it is a constant value of 1.0V, that is the voltage that the simulator will use to do the operating point analysis. So, when your simulation starts the capacitor is already charged regardless of resistor value. You may be able to get the initial condition to work the way you want it to by adding UIC at the end of your .tran statement. In general, I think it is better to use a source that changes after the simulation starts.

You have set the tstop condition for when the voltage on the capacitor is exactly 1V (if the syntax is correct, I'm not convinced that the value should be in single quotes). The simulator uses floating point arithmetic, and trying to compare two floating point numbers for exact equality is always a bad idea.

So, I would change your voltage source to a pulse or PWL source. Change your stop condition to something reasonable, such as >0.999V  Finally, if you are really going to simulate circuits with femtosecond or attosecond time constants then your minimum timestep may need to be much, much smaller in order to get reasonable results.