What is meant by "DC operating point analysis" in SPICE programs?
In an answer to an old question I gave a run-down of the three main analysis types done by SPICE and SPICE-like simulators.


  As far as I know the traditional transient circuit analysis is done by Laplace transform which superpositions both transient solutions and steady state solutions.


This is incorrect. SPICE typically does transient analysis using a time domain integration method, such as Runge-Kutta or Gear's method.

Where a transient simulation is solving a system of ordinary differential equations, DC analysis is solving a system of nonlinear algebraic equations. A simple method for this Newton's method, although a good SPICE will generally use something more robust.

Some simulators (ADS, for example) will let you choose different solution methods in case one method is quicker or more robust for a certain circuit.

Edit

In comments you asked,


  My main question is SPICE dealing with DC operating point as a part of transient analysis? 


This is answered in the quote you posted:


  
    a transient analysis first performs a DC operating point analysis
  


This means that when you request a transient analysis (unless you use a .UIC directive, as pointed out in comments), the simulator first does a DC analysis, and uses the result of this as the starting state for the time domain analysis. 

Whether this is "part of a transient analysis" or a separate step that isn't "part of" the transient analysis is a semantic question and you could view it however you like. 

Note: If you request both DC analysis and TRAN analysis, most SPICE's are smart enough to not do the DC analysis twice. Does this mean the DC analysis is not "part of" the transient analysis? Again, it's really up to you how you want to look at it.