Post-V8 New Features and Development News

[dsa-t]

Added support for importing Altium Schematic in ASCII format.

Backported to 8.0.2.

Previously only binary Schematic/PCB/Library Altium formats were supported.

[dsa-t]

Added PCB 3D image raytracing rendering from CLI, with transparent background support.

Usage string

Usage: render [--help] [--output OUTPUT_FILE] [--define-var KEY=VALUE] [--width WIDTH] [--height HEIGHT] [--side SIDE] [--background BG] [--quality QUALITY] [--preset PRESET] [--floor] [--perspective] [--zoom ZOOM] [--pan VECTOR] [--pivot PIVOT] [--rotate ANGLES] INPUT_FILE

Renders the PCB in 3D view to PNG or JPEG image

Positional arguments:
  INPUT_FILE        Input file

Optional arguments:
  -h, --help        Shows help message and exits
  -o, --output      Output file [nargs=0..1] [default: ""]
  -D, --define-var  Overrides or adds project variables, can be used multiple times to declare multiple variables.
                    Use in the format of '--define-var key=value' or '-D key=value' [nargs=0..1] [default: {}]
  -w, --width       Image width [nargs=0..1] [default: 1600]
  -h, --height      Image height [nargs=0..1] [default: 900]
  --side            Render from side. Options: top, bottom, left, right, front, back [nargs=0..1] [default: "top"]
  --background      Image background. Options: transparent, opaque. Default: transparent for PNG, opaque for JPEG [nargs=0..1] [default: ""]
  --quality         Render quality. Options: basic, high, user [nargs=0..1] [default: "basic"]
  --preset          Color preset. Options: follow_pcb_editor, follow_plot_settings, legacy_preset_flag, ... [nargs=0..1] [default: "follow_plot_settings"]
  --floor           Enables floor, shadows and post-processing, even if disabled in quality preset
  --perspective     Use perspective projection instead of orthogonal
  --zoom            Camera zoom [nargs=0..1] [default: 1]
  --pan             Pan camera, format 'X,Y,Z' e.g.: '3,0,0' [nargs=0..1] [default: ""]
  --pivot           Set pivot point relative to the board center in centimeters, format 'X,Y,Z' e.g.: '-10,2,0' [nargs=0..1] [default: ""]
  --rotate          Rotate board, format 'X,Y,Z' e.g.: '-45,0,45' for isometric view [nargs=0..1] [default: ""]

Isometric video render example:

kicad-cli pcb render --floor --zoom 1.4 --rotate '-45,0,45' -o render.png video.kicad_pcb

Previously it was not possible to use kicad-cli for rendering 3D images.

[craftyjon]

JamesJ has moved the Net Inspector to a docked panel (View > Show Net Inspector to show/hide)

This includes improved filtering and grouping UX, the ability to show/hide and reorder the columns, and save/restore of all the settings.

[stambaughw]

Jan Wichmann added tolerance calculations to the calculator regulator panel.

[stambaughw]

Miklós Márton added an option to change sheet names in the schematic hierarchy navigator.

[dsa-t]

Solid 3D model export improvements:

• Option to fuse copper geometry together
• Option to export copper on inner layers
• Options to exclude board body or components
• Net filter (can be used to export a single net)
• Zone geometry approximation with arcs for faster processing and smaller file sizes
• Export in BREP or XAO formats

XAO defines pad surfaces as face groups and can be imported into SALOME or newer versions of Gmsh for FEM simulations:

[JeffYoung]

Extended the physical_clearance rule to apply between copper fills & footprint courtyards.

(rule "No copper pours under Capacitors"
    (constraint physical_clearance (min 0.1mm))
    (condition "A.Type == 'Zone' && B.Reference == 'C*'")
)

will knock out the courtyard of any footprint whose reference starts with “C” from all copper fills.

[stambaughw]

@JamesJ added support for schematic rule areas that allow users to draw a shape to which net class directives can be attached.

[mf_ibfeew]

small tool added (by S.Hillbrand) to the context menu: Shape modification–> simplify polygon

[craftyjon]

Control over via tenting on top and bottom sides, at a board level and per-via overrides.

Note: this replaces the “tent vias” checkbox in the Plot dialog, which is now gone.

[JeffYoung]

Tables in Schematic Editor, Footprint Editor, and PCB Editor.

[JeffYoung]

Mark items excluded from simulation:

[JeffYoung]

DNP (and friends) at the sheet level:

[craftyjon]

@JeffYoung added a feature that lets you create ERC/DRC errors and warnings from textboxes and fields:

New text variables:

${ERC_WARNING <custom title>}
${ERC_ERROR <custom title>}
${DRC_WARNING <custom title>}
${DRC_ERROR <custom title>}

Variables must be at the start of a field, text item or textbox to be recognised by ERC/DRC.

They resolve to the empty string on the canvas.

[JeffYoung]

Allow editing unit in Edit Reference Field dialog:

[JeffYoung]

Plotting of pad outlines and numbers on fabrication layers:

[JeffYoung]

Right-click action to remove Ignored Tests from the ERC/DRC dialogs:

[Seth_h]

You can now embed various elements in your schematics, pcb layouts, footprints and symbols:

1. Worksheets
   

   

2. Datasheets:
   

   

3. 3d Models:
   

   

4. Fonts:
   

   

[dsa-t]

Export silkscreen and soldermask as flat faces to STEP / GLB (Binary glTF) / BREP / XAO
(since May)

[JamesJ]

New ERC check for local and global labels with the same name (from Wishlist: ERC local/global net name collisions (#9461) · Issues · KiCad / KiCad Source Code / kicad · GitLab)