I have just started to move from Eagle 7 to KiCad 8. So far making schematics is fine, but layouting drives me crazy.
1.) When I move a routed area, only the footprints move, but not the tracks. I even can’t select them separately to move them to the corresponding pads.
I have not found a way to unrute a segment of a track or the entire track from pad to pad.
Neither the ‘Select item(s)’ tool nor the ‘Delete selected items’ tool works.
OK, if I select a footprint I can unrute all the tracks connected to it, which is silly if you have 20 or more correctly routed connections and only one needs to be rerouted.
I’m convinced I’m doing something wrong, otherwise not so many people would use KiCAD.
I didn’t used V8 yet.
But what you write (both 1. and 2.) suggest me that may be you have excluded tracks from being selectable (in V7 it is screen bottom-right).
On the other side if you don’t like connection you made don’t delete it but rather correct (using D and G hotkeys).
I think (but not sure) OP is speaking about subset of components positioned relative to each other (at some place outside PCB) and routed there with no routed track to anything else.
Then such routed subset needs to be moved inside PCB.
May be I understand it that way only because I frequently design that way.
When I move a routed area, only the footprints move, but not the tracks
You have discovered the main difference in behaviour between eagle ↔ kicad layout editor. Eagle always rubberbands all drawn tracks. Kicad normally separates footprint ↔ tracks and connects them more loosely.
If you select only footprints you can use the DRAG command.
Note that the current routing mode (set with menubar Route–>interactive router settings) influences the drag-behaviour (shove mode, walkaround mode, allow drc-violations mode).
unroute a track:
select one track, expand selection with context menu–>Select -->Expand connection (normally hotkey “U”) , then “Delete”
Use command “Delete Full track”. This command is only available as hotkey. So look into your Preferences–>hotkey settings for the assigned hotkey
To me it also sounds like unfamiliarity with the selection filter in the lower right corner of the PCB editor.
Aso, a few years ago Rene Poscchl wrote a FAQ article on this forum about:
It has not been revised after 2021 (which is quite old for KiCad) but it will probably still be usable to point out the main differences between eagle and KiCad. I have never (seriously) used eagle myself, so I can’t help much in this regard.
Coming back to my second sentence (about using D and G hotkeys).
For many years I was using Protel 3 (program from 1997). There the only practical way to correct track was to delete it and route once more. From what you write I suppose that may be in Eagle it is also such (never tried Eagle).
When moved to KiCad (in 2017) at first I did it as I was used to. But now I prefer just to shift track segments using D (-rag) hotkey (other tracks are pushed). If you are used to delete and route once more I simply suggest to try to change this habit.
I am still not used to route tracks by pointing only start and end pads and allowing KiCad to find the way for the whole track and eventually correct it a little but all ahead of me.
My thinking (from Protel) that routing a track (to not have to delete it in future) I have to preserve the space for other tracks I know I will route here slowly changes. I need not to preserve the space. When I will be routing these future tracks the tracks already routed will simply be pushed.
Even reading a hotkey list I noticed F-finish I always had in mind that it is to be used when my track is 90% routed by me manually. Newer thought of using it that way.
I have just checked.
After pressing X once I can route many connections by:
