Something I use all the time in Altium that KiCad can’t do is editing multiple objects at once.
I don't understand. Can you explain that, svp?
Schematic:
Suppose the boss has said to change all the resistors from 0805 to 0603. I can do a Find to find and select all the 0805 resistors, then use the Properties to assign the 0603 footprint to all of them, all the while all their other properties remain unchanged.
Or maybe I need to change an IC from one type to another, for example the old 7805 to a more modern LM1117-style LDO. I can prepare a schematic symbol with the same layout, then select all my 7805’s and replace the symbol with the LM1117.
Or suppose the current limiting resistors for LEDs were first specified at 330 ohm, but user feedback says “the LEDs are way too bright” and we decide they need to be changed to 1Kohm. In KiCad, you’d have to change the value on each resistor one at a time. o_O
PCB layout:
Real world example I did this week: taking someone else’s board design (done by a novice in KiCad) and converting it to Altium, then tidying it up to prepare it for pick and place assembly. With 8 identical amplifier stages (4 channels x 2 stages), many changes needed to be made 8 times. (Had it been a from-scratch layout I would have used rooms to just replicate the layout, but it was already done…) I could select all 4 instances of a part in one column that need to be moved to a particular X coordinate, enter it, and all of them move there, even if they were at inconsistent X coordinates before. Their Y coordinates remain unchanged.
Or let’s say that we want to change to a cheaper PCB manufacturing process, and thus need to adhere to a larger minimum via size. I can use the Find feature to find the ones that aren’t compliant and then assign them all a compliant size, even if there were multiple noncompliant sizes. (For example, suppose we now need 0.5mm minimum, and before we had both 0.3mm and 0.4mm. I can search for all vias under 0.5mm, select them, and then apply a 0.5mm via template.)
PCB footprints:
Often, manufacturer-supplied footprints have a “hard coded” paste mask reduction of 0, so for the general paste mask reduction rule to apply, the pads need to be changed from “manual” to “rule”. I can set the selection filter to just pads, Ctrl-A to select them all, then change the paste mask setting. No big deal to do one at a time on a 3-pin device, but a proper pain in the ass on a 32-pin part, and an RSI nightmare on a 144-pin part.
You might remark that many of these things could be avoided by planning correctly from the start, and you’d be correct. But one doesn’t always have the luxury of starting a project from scratch, with the experience that comes with being a seasoned professional. One’s early designs have all sorts of sins, but also you’ll inherit designs from others, who used different defaults and had different preferences. So being able to clean things up easily is a big plus. (And I think it’s fair to say that a LOT of KiCad users are non-professionals who have neither the training nor experience to know how to do things correctly right from the start, nor have dedicated parts management people who will draw consistent footprints for them. So KiCad really should have this, because their users will need it!)