Rules on editing schematics (was Re: [Milkymist-devel] reviews (was Re: [KiCad M1R4] First KiCad version for Milkymist One Schematics.))

Werner Almesberger werner at
Thu May 3 23:12:23 EDT 2012

Adam Wang wrote:
> Here's one wiki page:

Looks very nice ! I like the illustrations.

> Good idea ! Yeah, I moved few applicative power symbols locally. :)

Excellent !

> Liked you pointed an A3 size for still be probably readable, the four banks
> for fpga chip are split. :)

And the FPGA is no longer a crowded mess :-) A3 prints fine.
There are only a few trouble spots now. (Below.)

> For Milkymist One schematic, only on Dram.sch I quite didn't realize how to
> make a better outlook way to arrange vertical crowed resistors which is a
> little against rules I edited in wiki. :)

There's not much you can do :-) And your solution looks good.

> yeah,do you have good idea to generate a good quality pdf  instead of using
> KiCad's print ? So this way seems good for reviews without installing KiCad.

Plotting all the sheets and then combining them into a PDF should
do the trick. For color (set the path to schhist according to the
directory structure on your system):

  cd board-m1/r4
  rm *.ps
  eeschema --plot=ps --plot-sheetref m1.sch
  for n in *.ps; do normalizeschps $n _$n; done
  ../../eda-tools/schhist/schps2pdf -o m1r4.pdf -t _m1-_ _*.ps

I've uploaded the result to

For printing, you get acceptable results with

  rm *.ps
  run eeschema and plot to A4. exit eeschema.
  lpr *.ps

The pages are a bit shifted in the printing case but not a lot is

> I picked nRESET style for KiCad m1r4 sch now. :)

Excellent !

> With C-friendly names did really save me suffer from some troubles while I
> edited m1r4. Like I used it for url link.

Hah, instant gratification ! ;-)

> Not sure if schhist can apply for m1r4 now.

It's up and running again but it doesn't cover M1r4 yet. Need
to nag Wolfgang a bit more ;-)

> yes, if one discovers new problems or comments given.

Yes ! :-)

I had a quick glance. I found the isses below. Some are just
questions of preference so you'll have to choose whether you
want to do something about them or if you like things how they
currently are:

- DVH-ISingle.sch (D5), MiscControl.sch (D6-D13): including the
  package in the drawing makes the diodes look quite strange.
  Particularly the DMX diode circuit takes a while to decipher.

  Perhaps we could use a diode symbol with the pin numbers set
  to match the package, like it's done for Q1 or Q2.

- a few fonts are a bit small:
  J17 on DVI-ISingle.sch (unreadable),
  U3 on Misc.sch (borderline, not sure if we want to change that

- text very close to other things:

  - Audio.sch: 4V4 power symbol. The text touches the circle. In
    the other power symbols (3V3, etc.), there is a little gap.

  - Audio.sch: similarly, AUDIO_AGND overlaps slightly with the

  - Audio.sch: the AUDIO_AGND at the bottom, slighly right of
    the middle, is even off-center.

  - Audio.sch: the component reference of C4, etc., sits right
    on the "X".

  - USB*.sch: R136, R137, ... are very crowded. It would be
    better to move the resistor value above the symbols (like
    for DRAM)

  - USB*.sch: the text below the GND symbol on V1 is very close
    and looks as if it was part of the GND symbol.

  - MiscControl.sch (U4, U5), USB*.sch (U16, U26, ...) have the
    pin names touch the side of the symbol. There should be a
    small gap. Like, e.g., in U8.

- some of the ground wires look a bit awkward

  - Audio.sch: J23 etc., perhaps just make the GND wire drop
    and cross the other signals, instead of making a loop.
    Similar to J1.

  - Audio.sch: J26 there, you could even just flip the component
    along the X axis, and then have ground point down and 3V3
    point up.

  - Ethernet.sch: R174 would look better if you dragged nETH_RESET
    up and put the resistor (and GND) under it.

- Audio.sch: TP5 is rotated without need.

- EXPANSION_RESET.sch: the text above J21 would sound better as
  "Users [...] their [...]" instead of "User ... your ..."

- FPGA_BANK3.sch: perhaps we should add a table for the revision
  codes, similar to what I've done in the lower left corner of

I like look of the new schematics a lot. They're so much cleaner
than what we had before. Thanks and congratulations !

Once the style is done, the next step should then be a component
by component comparison between the AD version and the KiCad
version, to see if anything has changed by accident.

- Werner

More information about the discussion mailing list