Post-V8 New Features and Development News

[craftyjon]

In KiCad 9, plated through-hole pads and vias will be displayed differently than in previous versions. Now, the copper annular rings for these items will be shown in the same color as other copper items on the same layer.

Blind/buried vias and microvias now are drawn with the colors of their start and end layer in the drill hole:

These changes were made to make dense and complex boards easier to understand, and as part of preparing to add support for complex padstacks (where vias and pads may have different sizes and shapes on different copper layers) to KiCad

[craftyjon]

KiCad now supports PTH pads with different copper shapes on different layers. This is one type of custom padstack; other padstack features will be added over time.

[craftyjon]

Andrzej Wolski added the ability for copper tracks on outer layers to have soldermask removed:

[johnbeard]

There are now optional indicators (toggled in the view menu and schematic editor settings) to indicate when pins have alternate modes available, as this was otherwise only visible by noticing the appearance of an entry in the context menu:

[johnbeard]

In the PCB editor, you can toggle the session locked item prompt from settings:

Now you don’t need to keep the lock prompt on when you don’t really want to to avoid of having to restart if you want them back.

[johnbeard]

Zone corners can now be chamfered during editing in pcbnew:

[Seth_h]

@dtreffenstaedt Added a new DRC check for acute angles. You can now write rules like:

(rule test_track_angle (constraint track_angle (min 135)) (severity error) )

[johnbeard]

Some copy-paste updates:

• You can now paste images from the clipboard as reference images in Schematic and PCB Editors (and page layout)
• There is a ‘Copy as Text’ action which allows you to copy the text content of text items, fields, labels, tables/tablecells, and dimensions. This can be useful when you want to copy the text out of KiCad, but not as s-expression.
• PCB Editor now allows pasting text directly as text items in the same way as in schematics.

[Drinausaur]

When clicking a clearance DRC error, KiCad now displays it in the editor.

[johnbeard]

There is a scroll-action feature in PCB, Schematic, Footprint and Symbol editors. Shift-Alt-Scroll is a primary function and Ctrl-Alt-Scroll is a secondary function.

The current bindings are to use this to increment text, with the rightmost “part” being primary and the next rightmost part being secondary. For example, Shift-Alt-Scroll on “B2” goes to “B1” or “B3”, Ctrl-Alt-Scroll goes to “A2” or “C2”. This is a bit heuristic, but seems to work well for the obvious cases.

• Footprint editor: pad numbers and text
• PCB editor: text
• Symbol editor: pin numbers or names (depending on mouse position) and text
• Schematic editor: labels and text

As a side effect of being able to detect the mouse being over name or number, the symbol editor “Edit Pin” dialog now puts the initial focus on the number field if the mouse was over it when double-clicked or on ‘E’.

[johnbeard]

Hasan Jaafar contributed an implementation of inward-facing dimension arrows.

Amongst other things, it will greatly help making dimensioned footprint drawings.

[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.