Rules on editing schematics (was Re: [Milkymist-devel] reviews (was Re: [KiCad M1R4] First KiCad version for Milkymist One Schematics.))
werner at almesberger.net
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. :)
> 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):
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
run eeschema and plot to A4. exit eeschema.
The pages are a bit shifted in the printing case but not a lot is
> I picked nRESET style for KiCad m1r4 sch now. :)
> 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
- 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
- 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
- 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.
More information about the discussion