Post-V8 New Features and Development News

[johnbeard]

There is a new tool in the PCB editor called “Position Interactively”. It allows you to position an item by drawing a line and then redefining what that line should be.

The obvious use is a more direct way to manipulate objects than first getting it into a known position and then using Move Exact. However, it can also be used to set alignment in one axis or the other:

And the vector doesn’t have to be on either object, so it allows to directly use a dimension of something else and use it as a movement for the selection:

[Drinausaur]

KiCad now has a creepage DRC rule.

It can be set via a user rule like this one:

(version 1)

(rule HV_HV
   (constraint creepage (min 20mm))
   (condition "A.hasNetclass('A') && B.hasNetclass('B')")
)

[dsa-t]

It is now possible to export the board 3D model in STL and PLY formats

[twl]

KiCad now has a Multichannel Design tool (aka Repeat Layout, for more info, see Multi channel tool)

[craftyjon]

KiCad now supports vias with different diameters on different copper layers. This can be used for situations such as increasing annular ring size on one side of the board to use a via as a testpoint, or decreasing annular ring size on inner layers.

[mikebwilliams]

Schematic design blocks have been implemented. You can get to them from View->Panels->

Uploading: 2024-11-07_13-31-32_recompressed.avi…

[craftyjon]

Eric from HQ NextPCB contributed ODB++ export support to KiCad. This feature has been in the nightlies for a while, but it recently got moved out from behind a feature flag. You can find it in the Fabrication Outputs menu.

[twl]

KiCad (nightly and V9) can now drag multiple tracks:

[marekr]

Jobsets have now been added.

The What

This allows predefining sets of “jobs” (largely export) operations for kicad data from schematic and pcb.

The purpose is to allow automating final deliverables/packages which can involve different combinations of outputs. The purpose of independent jobset file is to be reusable as users may want to create output pipelines that they can apply across their projects for consistency. Pretty useful in corporate environments and similar to at least one competing commercial CAD software.

Jobset file

The jobset file itself is in a json format though there are no promises over the format structure, future KiCad versions should remain compatible with older jobset files:

Each job and outputs uses a key-value store for settings which can be expanded or shrunk in future versions.

Output Types

Currently two main “output” types are supported.

• Folders - Basic folder
• Archives - Only zip format for now but this is probably the most important one

Outputs can be made to contain all jobs, or contain a subset of jobs,

Multiple outputs can share the same jobs.

Jobs
Jobs themselves are what you already find as separate Plot/export options in KiCad and the CLI interface.

You may add them from a selectable list in the jobset editor

Each job, even if its the same type as another, has its own settings store, allowing you for example to export multiple SVGs with different settings.

Existing KiCad dialogs were leveraged for the configuration of each job to keep the experience similar.

CLI

The command line interface has also been extended to support running jobset files

kicad-cli jobset run --file <jobset_file_path> [--output <output_key>] <kicad_pro path>

And of course, you can start creating a jobset by accessing a new menu option in the KiCad launcher menubar

Due to late fixes, this is not functional in the “9.0.0-rc1” singular build but is in the nightlies.

[marekr]

You can now plot all PCB layers to a single PDF document with separate pages instead of to separate PDFs per layer.

[johnbeard]

These have been in the nightlies for a while, but there were some changes to editing libraries:

• You can now save a derived symbol into a different library and it will also save the parent symbols into that library as well.
• You can now “Save As” as well as “Save Copy As” in the symbol editor
• You will be warned when trying to edit a read-only library (e.g. a system library that you don’t have write permissions for) and there’s a button to make an editable copy:

• If you edit a footprint from a board, or a symbol from a schematic, there is a button to switch to editing the library version:

• The “D” hotkey in the footprint editor will open the first URL in the description, which is usually a datasheet link.

[johnbeard]

Another couple of minor changes made a while ago:

Grid arrays can now be centred on the original item, which is useful for, say, BGAs:

Circular array options are simpler to define and you can select the centre point interactively:

[dsa-t]

Total 2D length of selected track segments and shapes is now shown in the message panel:

[Seth_h]

This has been in KiCad for about a year now but we enabled the feature by default for v9:

Git-based project management. See project state for git-managed projects, commit/push/pull projects or individual files.