While they had their own custom made dry transfers for circuit symbols, they might have used Reber/Edding R41 dry transfers for some PCB pads:
Where can I download those footprints?
The image above is from a single generated test footprint (but you should be able to copy pads and resize with context menu Properties… → Custom Shape Primitives → Polygon → Transform Primitive → Scaling factor and adjust Size X and Hole size X in General):
octagons.kicad_mod (27.1 KB)
For more footprints, see also the 2nd part of this posting:
I’m in Italy, that remembers me the old times at school and by the way, by that time Elektor was published in Italian as well
Continuing the discussion from Elektuur Style Symbol Library.
Oktizer is an Action Plugin to create octagonal looking pads and vias in the PCB Editor. It works somewhat similar to how KiCad 6.99 is currently doing teardrops but it also modifies pads.
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:
Elektuur Style Symbol & Footprint Library
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
Note: In KiCad 6.99 there is now an alternative to unchecking
Automatically place symbol fields (but it will need modification of the Value/Rating/Indicator/IndicatorControl fields of the symbols).
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).
Version 0.0.9 now available in PCM:
Note: This version of the plugin doesn’t run in experimental KiCad 6.99 because of KiCad’s incompatible Python APIs (PCBs modified with the plugin in KiCad 5.1 or 6.0 should be OK in KiCad 6.99).
Example PCB based on E-CALL EIC-801 Solderless Breadboard (400 Tie-point), similar to Adafruit Perma-Proto Half-sized Breadboard PCB, SparkFun Solder-able Breadboard or YoMo EPB-M:
octaproto400.zip (29.7 KB)
Colors above are:
Preferences 3D Viewer General ☐ Show solder paste layers Colors ☑ Use colors: Silkcreen top: #F5F5F5FF (White) Silkcreen bottom: #F5F5F5FF (White) Solder mask top: #441A9600 (Opacity: 0) Solder mask bottom: #441A9600 (Opacity: 0) Copper/surface finish: #B29C00FF (Gold) Board body: #000000FF (Black)
More pictures of breadboards (mostly based on patents USD228136S or USD235554S).
Does this mean that octagonal pads will be available among existing “pad shape” in 6.0.6 as well? btw, what’s the chamfer size you are using in this plugin?
- Take a piece of paper and something to write.
- draw a square with inscribed circle.
- Make the square into an octagon.
- Draw an extra line from the center to a corner of the octagon.
- Apply some trigonometry: (1-sin(pi/8))/2 = 0.3086582838174551
- Draw a pad:
Yep, 30.8% seems about right.
Edit:, euhm, oops, “about”, but not quite.
It bothered me that the chamfers looked a tiny bit too big, and then I realized I should have taken the tangent instead of the sine: >>> (1-tan(pi/8))/2 = 0.2928932188134525
Or you can use some proportions. You get the same number with: 1/(2+sqrt(2)) = 0.2928932188134525
For EAGLE import (
*.brd, and for added EAGLE libraries
*.lbr as well), it’s a KiCad 6.0 standard chamfered rectangular pad shape with now 29.28932188% chamfer ratio (the plugin above uses custom pad shapes to be compatible with KiCad 5 and also support rounded corners; see the comments in the python script above). Altium import uses 25%.
The chamfer ratios used in the plugin are 1-√½ (≈ 29.29%) for squares and √½-½ (≈ 20.71%) for rectangles, which correspond to 1÷1 and 2÷1 side ratios, respectively.
With a pad size of 1+√2 (≈ 2.414) times the track width (or slightly smaller), it allows angles of 135° (instead of ≈ 90°) without using teardrops, as was used by Elektuur/Elektor in the late 1970s until the 1990s. EAGLE’s initial footprints and symbols looked very similar. Since tracks are nowadays much narrower, the plugin uses fillet teardrops to get a similar look, especially if the octagons or rectangles use rounded corners (by default the same as TI recommends for DIL, SOIC, TSSOP, TO-92, etc.).
completely legit. I’ve installed the symbols in my own library, The Elektor/Elektuur artwork was the best.
I appreciate your keeping it alive!
Habe das Büchlein nicht gelesen, aber ein Vorteil scheint zu sein, dass IEC 60617 Normsymbole verwendet werden:
I have no complaints with your posting in German?, but an accompanying English translation would be nice for we ignorant of the German? language. ( I hope it is German, it looks like it may be German).
Probably if you can’t read the post you can’t read the book?
I haven’t read this German book(let) but an advantage seems to be that standard IEC 60617 symbols have been used:
Thanks for the translation.
Your first threads ran out of time… no one posted for three months.
Don’t know what happened to the first post here. Maybe @hermit could shed some light on that.
The newer thread (your Mar2022) has been attached to the bottom of the old one and the opening post (a duplicate of the closed post) is now halfway up this thread.
Closing threads after 3 months of inaction, I believe, is to prevent people resurrecting ancient, no longer applicable threads.
You can always ask to have old thread reopened as long as it hasn’t drifted too far. Long threads have serious downsides. Like are the top posts still relevant? Is there lots of duplication and thread high jacking? Yuk - yuks? I think Level 4’s can help house clean those.
To keep the topic open: Did you recognize the Elektuur shadow of the IC symbols ?
Right and bottom line of any rectangular IC box have slightly increased line width for old schematics.
To allow symbol rotation, this would require some code to modify the line width if not available for all
rotations in the library.