`It moves some of my connectors (which properties was not changed at PCB level) out of the active area` This is probably because the footprints have an origin that is poorly defined and is some way away from the pin 1 or the centroid of the footprint. You may not have noticed it when the parts were first placed outside the board outline after first passing the schematic into PCB. You may be able to fix this by checking and if necessary, correcting the footprint origin. `it also changes the pin spacing of the components I did edit at PCB level.` Not sure I understand what you mean here. Is this because you have changed the pin spacing in the PCB but when you update the PCB from the schematic, the pin spacing reverts to what is in the footprint you have assigned in the schematic? If yes then you need to update the footprint (edit the PCB Lib and save it as a new version) to the modified pin spacing you have in the PCB and then update the footprint assignment in the schematic. If you then update the PCB the footprint pulled in to the PCB should then have the right pin spacing. `Is there a way I can move a NET in PCB level?` Easy. Just edit (i.e. swap) the net names of the pads you want to change. Suppose you have two resistors joined R1 pin 1 to R2 pin 1 by net A and R1 pin 2 to R2 pin 2 by net B. If you look at the net names of the resistor pins you see that R1 pin 1 and R2 pin 1 are labelled as net A and R1 pin 2 and R2 pin 2 are labelled as net B. If you relabel R1 pin 1 netname from A to B and relabel R1 pin 2 netname from B to A this will swap the resistor connectivity so that R1 pin 2 is joined to R2 pin 1 by net A and R1 pin 1 is joined to R2 pin 2 by net B. In other words you have swapped them. Try it out in a test project: just make a simple schematic, convert it to PCB and then play with the net names applied to the component pins.

@andyfierman thank you very much for your assistance. I believe your assessment on all issues are correct. I made changes at PCB level and did not adjust the footprints etc. Again I took the shortcut you proposed and manually relabeled the netnames on the components and then rerouted. This seems to have resolved my issues. I did change the schematic as well - for future reference only since I did not update my PCB from here due to time constraints.