Why do we need sheet entries and sheet symbol in Altium
Indeed, nets are already connected to each other by their ID from
  sheet to sheets as I understand or via Port.


This depends on the Net Identifier Scope you choose for your project.


Global (Net labels and ports global)


This is the scope you refer to. Ports and net labels connect across all sheets throughout the design. This is similar to what you may know from "Eagle" layout editor and other "simple" design tools. It is not suited for a clean modular design.


Flat (Only ports global) – ports connect globally across all sheets throughout the design. 


This gives better control of the sheet inter-connections since you have to specify ports for signals that should go "off-sheet".


Hierarchical (Sheet entry &lt;-> port connections, power ports global) 


This requires manual inter-sheet connection and usually uses a "top sheet" with only sheet symbols on it as a base. Note that power ports (12V, GND etc) are global for convenience.


Strict Hierarchical (Sheet entry &lt;-> port connections, power ports local) 


This one requires you to also connect power ports between sheets. There may be two different 5V voltages in one design for example, which could be connected by accident when using the normal hierarchical design. "Strict" has the advantage that you would manually check every single connection.