Continuing the discussion from Elektuur Style Symbol Library.
Currently, there is no GUI (edit the python file to change corner rounding [radius 0.05 mm ≈ 2 mil] or chamfer ratios [29.29% and 20.71%]) and it needs to be copied to the
plugins folder of
KiCad 5.1 or
KiCad 6.0 (it doesn’t need its own folder, though), or it can be installed using PCM on
KiCad 6.0. Thermal reliefs may not work correctly with the generated custom pads and may need explicit tracks (for
KiCad 6, chamfered rectangles could be enabled instead by uncommenting some code).
Before running it, the PCB needs to be prepared first with either:
- Tools → Cleanup Tracks & Vias… → ☒ Merge co-linear tracks
- Edit → Cleanup Tracks and Vias… → ☒ Merge overlapping segments
and after selecting the desired pads and vias (or else it modifies all round/circular/oval/rectangular/square PTH pads and vias):
- Tools → External Plugins… → Oktizer
or use its tool button. Undo/Redo should work. If only board graphics shapes are selected, the circles and rectangles/squares are changed to (filled) octagons (also useful for creating silkscreen to be copied to the Footprint Editor in
KiCad 6, beside pads themselves). For (explicitly selected) NPTH pads (mounting holes), it could be necessary to (temporarily) set their pad clearance to the surrounding zone clearance or the copper-to-hole clearance of the board.
oktizer.py (21.7 KB)
Example of NPTH rule area (keepout zone):
Example of manually created T-junction (i.e. set grid size to smallest track width):
Example of manually created thermal relief on chamfered rectangle pad:
The symbols (only) can also be installed on KiCad 6 with Tools → Plugin and Content Manager (PCM). To add the library after installing, use Preferences → Manage Symbol Libraries… followed by Add empty row to table (the
+ icon) with the Library Path given in the content description.
The libraries and demos are as well in the repository for local installation using Tools → Plugin and Content Manager → Install from File…. The zip files with demo in their name are example projects (use File → Unarchive Project… instead of PCM). Version 0.5.4 are KiCad 5 libraries (that can also be used and migrated in KiCad 6), version 0.6.4 are KiCad 6 libraries. Currently, the symbols are identical except for some arc adjustments and a few added chamfered footprints (and corresponding config files).
Elektuur (now Elektor) style symbols as introduced in the later 1970s (until the early 1990s when they became more angular). The symbol size has been increased by 1.6% (2 mm grid to 80 mil grid) and the pins realigned to a 100 mil grid.
It’s a generic symbol library (UJT, BJT, JFET, MOSFET, C, D, LED, LDR, Schottky D, Zener D, varicap D, L, P, R, NTC/PTC R, VDR, Re, S, La, LS, Mic, GND, Xtal, F, battery, meter, terminal, jumper, heatsink, opamp, inverter, AND/NAND/OR/NOR/XOR/XNOR, NOT, SCR, triac, plug/socket, TP, arrow) and some single-pad prototype footprints (generated with
oktizer.py above) optimized for some specific track widths. Most symbols have alternat(iv)e/multiple shapes (also KiCad-historically referred to as De Morgan conversion).
kicad-elektuur-symbols-demo-0.5.4.zip (50.9 KB)
Recommended settings for KiCad 6.0 (on Windows) [or copy and modify file
*.kicad_pro from demo]:
Preferences Preferences… Common Antialiasing Accelerated graphics: High Quality Antialiasing Fallback graphics: High Quality Antialiasing Schematic Editor Display Options ☑ Fallback graphics Editing Options ☐ Automatically place symbol fields Symbol Editor Display Options ☑ Fallback graphics Editing Options Default line width: 0 mm 0 mil (broken) File Schematic Setup… General Formatting Default line width: 0.254 mm 10 mil Pin symbol size: 0 mm 0 mil Junction dot size: Small Project NetClasses Default Wire thickness: 0.254 mm 10 mil View [or right mouse button] Grid Properties… Grid: 2.54 mm 100 mil Grid 1: 0.635 mm 25 mil [text or wires of gate/diagonal alt. shape] Grid 2: 0.254 mm 10 mil [transformer] Inspect Simulator Simulation Settings… ☑ Adjust passive symbol values (e.g. M → Meg; 100 nF → 100n) Compatibility mode: PSpice and LTspice
Recommended settings for KiCad 5.1 (on Windows):
Preferences Modern Toolset (Fallback) [✓ select this] Preferences… Common Graphics (Fallback): High Quality Antialiasing Eeschema ☐ Automatically place symbol fields Display Options Wire thickness: 10 mil Junction size: 40 mil Symbol Editor Default line width: 10 mil View [or right mouse button] Grid Settings… Grid size: 100 mil [50 mil for diagonal alt. shape] [25 mil for text or wires of gate alt. shape] [10 mil for transformer] Eeschema Tools Simulator Simulation Settings… ☑ Adjust passive symbol values (e.g. M → Meg; 100 nF → 100n)
SVG file was created using File → Plotting… with Default line width of
0.254 mm or
10 mil, Black and White and
Inkscape saved as
See also Elektuur Retro Lettering (oktuur.zip for Inkscape/SVG).
See also Getting Started with KiCad EDA - Eeschema Schematic Capture (Elektor TV video).