sch-rnd-aux knowledge pool

Size conventions

sizes by Tibor 'Igor2' Palinkas on 2022-01-21	Tags: convention, size, mm, inch, mil, pitch, print
node source

Abstract: The cschem specification states that coordinates are integer, but leaves details on the interpretation of actual coordinate values up to the implementation. The user is free to follow whatever convention. This pool node describes the default conventions sch-rnd choose for sizes and explains the research behind these values.

sch-rnd size conventions

Librnd uses nanometer as coordinate units when drawing to screen, so sch-rnd needs to convert every coord to nanometer. Since sch-rnd is not naturally tied to the physical world, this conversion could be anything, e.g a cschem integer unit could be 1 nanometer or 1 mm or 1 cm. To keep things simple and code fast, I decided ^rationale to use the following conversion:





    1 cschem unit  = 1024 nm = 1.024 um
 1000 cschem units = 1.024mm

Note: mm and mil values below assume the matching drawing area size was and print page size is used. (Sch-rnd scales automatically.) Sch-rnd UI and user always uses the integer cschem unit, never mm or mil or inch; mm and mil values in the table below is only to predict approximate size of objects on typical printouts.

name size in cschem coord expected approx. size in print
pin distance ^rationale 4000 4.096 mm (~161 mil)
font height: pin label ^rationale 3000 3.072 mm (~121 mil)
font height: name ("refdes") label ^rationale 4000 4.096 mm (~161 mil)
wire line thickness 250 0.256 mm (~6.5 mil)
wire junction thickness 1000 1.024 mm (~40 mil)
terminal line thickness 250 0.256 mm (~6.5 mil)
decoration line thickness 125 0.128 mm (~3.25 mil)
lib: resistor body/zigzag box 12000 * 4000 12.228 mm * 4.096 mm (~481 mil * 161 mil)
lib: resistor/capacitor/coil total length (pin ends) 20000 20.480 mm (~806 mil)
lib: diode triangle base:height 8000:4000 8.192 mm : 4.096mm (~322 mil : 161 mil)
lib: opamp triangle base:height 16000:16000 16.384 mm : 16.384 mm (~645 mil : 645 mil)
lib: transistor circle diameter 11000 11.264 mm (~443 mil)

name	size in cschem coord	expected approx. size in print
pin distance ^rationale	4000	4.096 mm (~161 mil)
font height: pin label ^rationale	3000	3.072 mm (~121 mil)
font height: name ("refdes") label ^rationale	4000	4.096 mm (~161 mil)
wire line thickness	250	0.256 mm (~6.5 mil)
wire junction thickness	1000	1.024 mm (~40 mil)
terminal line thickness	250	0.256 mm (~6.5 mil)
decoration line thickness	125	0.128 mm (~3.25 mil)
lib: resistor body/zigzag box	12000 * 4000	12.228 mm * 4.096 mm (~481 mil * 161 mil)
lib: resistor/capacitor/coil total length (pin ends)	20000	20.480 mm (~806 mil)
lib: diode triangle base:height	8000:4000	8.192 mm : 4.096mm (~322 mil : 161 mil)
lib: opamp triangle base:height	16000:16000	16.384 mm : 16.384 mm (~645 mil : 645 mil)
lib: transistor circle diameter	11000	11.264 mm (~443 mil)

Rationale

1024 multiplier

We need to choose a base grid size first. A good reference for starting that is looking at "default pin pitch". The considerations:

the smallest integer coord we want to specify, typically line widths, is about 100 times smaller than pin pitch
to avoid rounding errors, line widths should be in the magnitude of at least a few dozen coords
for translation to physical world, look at existing printed schematics

Considerations for the physical world conversion:

our print will auto-scale, so we are not drawing anything on screen thinking in millimeters or inches; autoscale means: you can print the same drawing to A/4 or A/3; the A/3 print will be twice as big (assuming you used portrait for one and landscape for the other).
sch-rnd size conventions should be picked to suit the most common case automatically: make a dense schematics printed on A/4 just readable

I took printed schematics in a local HAM radio magazine as reference. The target audience of such magazines include veteran users, which often means not perfect eye sight; the size that works in this context is probably the smallest safe size. I found ^research that their pin pitch is about 4mm. Thus the choice of approx. 4mm pin pitch in sch-rnd.

This led to defining default pin pitch convention to 4000 grid units, which results in:

about 4mm in default print
about 40..100 units for smallest line thickness
convenient for halving grid density twice on the GUI for precision placement of labels, still having 1000 as grid unit

1024 vs. 1000: it's a conflict of interest between screen-only and print usage. On screen, the multiplier doesn't matter at all, since the user can zoom in and out arbitrarily; 1024 is faster for the computer. On paper this value matters because it determines the final sizes in mm, which will not be round: for 1000 units, we will have 1.024mm (assuming the right border is set up). This means sch-rnd can not be used easily for accurate 1:1 mm drawing.

My decision as to prefer screen over paper. Rationale: devices such as tablets and portable computers are very accessible so as years pass the total number of hours spent on looking at printed schematics decreases in favor of looking at the screen. Accurate mm scale drawing is not in the scope of sch-rnd (use a mechanical CAD or pcb-rnd for that).

Values in mil/inch system is even less round: this design has a preference of metric over imperial units. This is because the metric system is simpler in general and is used in a smaller part of the world.

font height is the total height from the lowest to highest pixel in the tallest glyph and the lowest pixel in the most ascender glyph.
I use pt only as an approximation so readers with word processor experience can estimate font size; when you see a pt value in this document, always take it with an error margin of +-1.
for whatever reason, different font at the same pt size results in different height meusured in mm. So I took a shortcut and said 72 pt = 1 inch, which means 1 pt is 0.3528 mm

I've measured different text labels ^research in (HAM magazine) printed schematics to get an approximate font height. I concluded smallest font, typically used for pin labels, is about 3mm high. So I choose 3000 for sch-rnd default pin font height.

Then looked at gschem's ratio ^research between pin and refdes font and found their refdes font is 25% larger than pin font. To keep things round, I decided to go for 33% larger and use 4000 for names.

Research

Print: HAM magazine

From a 2005 issue of Radiotechnika :

pin pitch: ~4 mm
font height (pin label): height=3mm ~9pt (capital part: ~ 2mm)
resistor body: 5mm*2mm, pin-to-pin len: 10mm
diode: triangle 2.5mm:2.5mm
transistor dia: 8mm
opamp triangle: 9mm:9mm
line thickness (normal; wire, deco): 0.25mm
thin line thickness (deco): 0.15mm
junction dia: 1mm

gschem

With A/4 titleblock.

default grid: 100
A4 titleblock is 116*82 grid; 11600*8200; 1mm = 39 grid; 1mil = 1 grid
pin pitch: 200 = 5.1mm
font height
- pin label: cap100+desc30 = 2.56+0.76 = ~3.3mm (9.5pt)
- refdes label: cap125+desc39 = 3.2+1 = ~4.2mm (12pt)
resistor body: 600*200 = 15.4mm*5.1mm, pin-to-pin len: 900 = 23mm
diode: trinagle 400:300 = 10.25mm:7.7mm
transitor dia: 640 = 16mm
opamp triangle: 800:600 = 20.5mm : 15.4mm
line thickness
- deco: 5 = 0.128mm
- wire: 10 = 0.256mm
- pin: 10 = 0.256mm
- junction dia: 40 = 1.02mm