Rules on Editing Schematics

Be noticed that here most of contents came from Werner Almesberger's great feedback on mail thread. And rules that guide to how to edit a good quality of schematics here.

Understandability

Understandability comes from simplicity and systematization.

Naming Values and Units

• For example, values would change as follows:

resistor: 1 MOhm -> 1M, 4.7 kOhm -> 4k7, 49.9 Ohm -> 49R9, 220 Ohm -> 220R, 20 mOhm -> 0R02
capacitor: 10 uF -> 10u, 3.3 uF -> 3u3, 100 nF -> 100n, 4.7 nF -> 4n7
inductor: 
bead: current rating
varistor: Vdc or Vac

• error percentage

Power Symbols

• 

  Used by POWERED flag

Directions of Global/Local Labels

• 

  Right use case: global lable

• 

  Wrong use case: global lable

Style of Junctions

Use the right-side variant of 3a of http://en.wikipedia.org/wiki/File:Schematic_junctions.svg

Better Looking

http://downloads.qi-hardware.com/people/werner/tmp/style-0.pdf

1. remove redundant of useless pins

• 

  No need Pin1

• 

  the wire coming from pin 14 (CE1) shouldn't have a junction marker (fat dot)

2. compared to 50-60 mil for most of the other text, make sure the name text had better not to smaller than 50-60 mil.

• 

  No need Pin1

3. avoid overlaps

• 

  the ground symbol on pin 32 (A0) overlaps the text "FLASH_A0".

4. avoid having positive rails point downward or ground point upward/leftward/rightward.

• 
• 
• 

5. as alignment as possible

• 

  global lable FLASH_D15 is not aligned with FLASH_D0 through _D14

Properties of Components/Symbols

Field Reference

1. set text size as 0.050-0.060"

Component Name

1. set text size as 0.050-0.060"

Pin Properties

1. Pin name and Pin number, set 0.050" for them. Meanwhile we should follow whatever the data sheets use, unless the data sheets are obviously wrong or misleading. (I've seen pins named "ON" that turn something off ...) what to do with pin names that aren't valid C identifiers ? (*) Particularly inverted signals often have a lot of presentations that are a pain to use in a program: e.g.,

nRESET, RESET_N, RESET#, /RESET, or RESET with a line on top.

Of these, only nRESET and RESET_N can be directly used in a program.(*) Picking C here as an example for an identifier syntax shared by most programming languages. Names that aren't identifiers could still be transcribed but this easily results in confusion. Possible remedies:

- always use C-friendly names in components,
- define transcription rules and hope for the best,
- a mix of both, e.g., use a C-friendly convention for inverted signals, leave the rest (FOO+, etc.) to transcription.

Note that this doesn't affect alternate pin names. E.g., if we have a pin calles, say, GPIO1/TX/MOSI, then one would normally pick the name corresponding to the respective function or the most generic one, depending on context. So the / aren't part of any identifier.

2. Electrical Type, KiCad has "No connection" (NC) and "Unspecified" (Unspec). NC produces an ERC complaint if anything is connected to it at all. Unspec doesn't care what is connected. When a data sheet says "NC", this can mean "no internal connection" or it can mean "do not connect anything here". Sometimes, a data sheet clarifies that, many don't. So we should use "NC" for anything says "do not connect" or that lacks clarification while we should use "Unspec" only if the data sheet says it's okay to connect something. Why make the distinction ? Because it can sometimes be convenient for the layout to be able to route a signal through an NC pin. But that only works if the pin truly isn't connected to anything on the inside of the package.

3. Graphic Style,

Checklists of Symbols

1. is the symbol understandable ?
2. are all pins present ?
3. do they have the correct name ?
4. do they have the correct number ?
5. does the pin type correspond to what the data sheet says ?
6. is text large enough ? (0.050-0.060" for component reference and value(s), 0.050" for pins and other text)
7. more ?

Checklists of Schematics

1. are the styles of values the same ?
2. are things free from overlaps ?
3. is text readable ? (When adding a symbol from the component library to schematics, a copy is made of the fields. So if the text size is/was later changed in the library, this isn't automatically reflected in the schematics and the two may diverge.)
4. can text be unambiguously associated with components ?
5. are component references on top or the left of values and/or part numbers ?
6. are comments/explanations understandable ?
7. when wires join in a T, is there a junction mark ?
8. are there no junction marks anywhere else ? In particular, do we only have crossings of the types 2b, 3b, and the right side of 3a, but never 1a or 2a ?
9. are connections straight and clear ? Here are some style
  suggestions:
  http://downloads.qi-hardware.com/people/werner/tmp/style-0.pdf
10. do positive rails point up, ground (and negative rails, but we don't have that in M1) down wherever reasonable ?
11. do labels point in the direction of the signal ? (This is all wrong in the original M1 schematics.)
12. more ?

Links

• International System of Units
• the beginning of the discussion thread of Values and units in schematics
• the conclusion of the discussion thread of Values and units in schematics
• the results of Values and units in schematics
• Schematic Junctions