[hales]

> Pack & Move Footprint Tool

This is the biggest usability improvement on the list. Computers are good at menial sorting, humans hate it.

For those not in the know: your nice, organised schematic gets turned into a randomly assorted pile of parts when you first open the PCB editor. Now imagine your board has over a hundred parts, including lots of duplicated copy+pasted bits.

My workarounds have been to:

1. Number the parts with special codes/prefixes to make manual untangling and grouping faster. 2. Import parts into the PCB editor as a draw the schematic. It's annoying extra work (the schematic undergoes lots of changes) and requires you to assign valid footprints from the start (so your work is constantly interrupted by having to draw missing ones OR your assign invalid ones and forget to fix them later).

[sleepytimetea]

They listed it at the very end of the Release Notes but its a killer feature - I have been struggling with the random packing of components onto the PCB when the first export to PCB is done. It almost made me delete most of the schematic and then incrementally add to schematic and then make it add to PCB but its such a pain.

This new Pack and Move feature seems like a life-saver, since we can use it anytime to add components to a selection with Shift-select and then that will pull it into the other desired grouping area on the PCB.

[eternauta3k]

I made a simple script which lays out the components in the layout like in the schematic, so it's not so confusing when starting out.

https://github.com/ignamv/kicad_scripts#place_footprintspy

[aix1]

When choosing how to lay out footprints during packing, does KiCad take into account electrical connections between them?

(This does sound like an extremely useful feature either way, but I'm curious.)

[junon]

It appears to now, yes. It didn't before. One of the bigger headaches (for me, as a beginner) was when you had bypass capacitors that need to be physically as close to an IC as possible. However, the two pins go to a voltage source and ground. According to Kicad, those could be placed anywhere on the board, and have no direct relation to the IC itself. This meant you had to carefully find each capacitor by its reference and move it to where it needed to be - often it was packed somewhere completely irrelevant. Now it appears to be much simpler since you can select the components from the schematic and pack them together in the PCB editor, saving a lot of time.

[unxdfa]

Trick is to print the schematic out, draw red circle around each "decoupling environment" and then group them on the board like that. Then place the connectors where the mechanical design demands them and move the groups where they need to go. Then do the signal paths, then the power routing, then the ground fill.

Kicad doesn't make that particularly easy but one of the big errors people make is at schematic capture stage where people chuck all the decoupling capacitors in their own sheet or separate net all across the power bus. They belong next to the devices you are decoupling on the schematic.

Canonical good example from the HP 3478A service manual: https://imgur.com/LQiAKtI

[bombela]

I am a total amateur here. But I found it natural to keep a relative spacial coherence in the schematic, and have it somewhat similar on the PCB side.

Though kicad would just dump everything randomly when moving to thr PCB view. As I understand, "packing" should help keeping this spacial grouping.

There is a plugin though[1] that does place the components on the PCB similar as they are placed on the schematic (and this does work with sub-sheet too). This is tremendously helpful starting point.

[1] https://github.com/ian-ross/kicad-plugins

[aaronmdjones]

Isn't C312 the wrong way around?

[kps]

The curve doesn't imply polarization; see C306 on the right.

(I miss resistors that go -v^v^v^-. Why would you use a box? Boxes are for black-box ICs.)

[aaronmdjones]

Ah, right. I'm used to caps being 2 flat lines for unpolarised.

[ororroro]

In 6 you can select the bypass cap in the schematic editor and that will highlight it in the PCB editor but only one at a time. Still better than searching for C18 though.

[ilyt]

> This meant you had to carefully find each capacitor by its reference and move it to where it needed to be - often it was packed somewhere completely irrelevant.

1. Draw bypass caps for every IC as its separate space on schematic (also declutters the schematics that way)

2. Group them together on PCB then just... drag one (or two if you have say 100n + 1n) each to each IC.

Alternative is 0 ohm resistor (net tie footprint) before every power line so the cap and IC are on separate netlit

[the__alchemist]

I concur. This is a limitation of the net model. I've found the net model works well for most cases, with this as a notable exception.

Maybe the play would be a special BP cap setting on the schematic, that binds to a specific part + pin.

[aylons]

Long time since I last used it for complex board (life is weird), but the way I do it is to crossselect the part from the schematic. I remember earlier versions used a local socket between the layout and schematic tools to allow for that.

Really indispensable. Not sure how the current feature works, but for things like power supply capacitors that are electrically connected to tons of ICs and pins but logically belong to one specific pin, I can't think of a better approach.

[amelius]

I'm still on version 5 due to apt/snap issues, but what I miss the most is a way to place footprints of a group of components (as opposed to placing them all at once).

[contingencies]

I'm still on version 5 due to apt/snap issues

I'm still on 5.1.x as snapping is broken. Not apt/snap, but proximity snap. In 5.1.x the best way to place a group is to use https://github.com/MitjaNemec/Kicad_action_plugins 'replicate layout' (components and traces). See also, right click and Select ... Same schematic sheet (components only).

[duped]

I believe GP is referring to the `snap` package manager on Linux, not snapping in the UI.

[contingencies]

Yes, hence the clarification ("Aww, snap.") Incidentally, Ubuntu forced people to move to buggy 6.x at some point circa mid last year - another reason to avoid such distributions.

[duped]

Ubuntu didn't force people to move at all, at least any more than the normal apt-update.

Last I checked though, to install Kicad with apt you needed to manually add a PPA - it wasn't available from the distro at all.

[contingencies]

My point precisely, for them a 'normal' update includes precluding the ongoing use of a working package and replacing it with a novel and buggy one. No idea on the current state, I've largely stopped using Ubuntu.

[chuchana]

Version 7 doesn't seem to have made it to either of those yet, but have you considered installing a newer version through an additional package manager like Guix or Nix?

[the__alchemist]

From a skim of the website, I'm surprised they don't have a Linux binary to download, but there is a PPA avail. Or, you could compile from source if the dependencies aren't too messy.

[varispeed]

I wish they made migration easier. I'll probably use KiCad 7.0 for new projects, but for old I think I need to stick with 5.1.

When I import most projects to 6.0, I get so many errors, violations and whatnot that make no sense when taking a closer look so I just don't trust it.

[Pet_Ant]

Did you report those? Even try to make a minimal reproducible file that triggers the error? Might be a simple thing they can fix if pointed in the right direction.

[mastax]

IIRC in V5 I used to use subsheets simply because each sheet would cluster its components together.