kicad-developers team mailing list archive

[Lorenzo Marcantonio <l.marcantonio@xxxxxxxxxxxx>]

Since Farnell bought Eagle, RS responded with their own package, design
spark PCB...

They call it 'The World’s Most Powerful Free Schematic and PCB Layout
Tool' (copy and paste from their web page :D). A little googling shown
that it could be probably a rebranded entry level cad from the pulsonix
people.

Anyway I've *a lot* of thing to disprove this :D:D from a cursory glance
(in mixed order):

- Zoom is still at the x2 /2 stage :P:P and you have to ctrl-wheel to do
  it with the mouse;

- Grid handling seems ok, even it you have to go thru a dialog each
  time. No grid offset. It also have different units... it even lists
  *both* mil and thou (which were the same things, last time
  I checked...)

- In schematic capture drag is the default (you have to 'unfix' the nets
  to move); kinda interesting. Also if you change the symbol wires
  remains attached :P

- Schematic editing is awful... you can't remove a single piece of wire,
  it seems do delete it all to the nearest junction!

- OTOH dragging seem reasonably smart (but still can produce overlapped
  wires, bad drag!)

  My ideal drag would be: try to keep ortho but make it free angles if
  it would overlap (so I see it and fix it manually)

- No bus support (OTOH Altium invented 'shrouds' :P)

- *No hierarchical sheets* at all, and only global labels allowed! (Booo
  hiss!) Also the flat multipage schematic system seems flaky, too...

- OTOH net classes right on the schematic editor.

- No 'labels' as graphical element, there are only text objects; net
  name is set using properties on the wire (but not shown on the
  drawing)

- Nice style support for text (and others things). I.e. no more perl
  script for changing component value sizes for me :D

- Drawing glitches a lot (V to redraw); we're not alone in this...

- Component/symbol/package handling fixed like in Eagle... mixed feeling
  about this, package assignment is only a really minor nuisance...
  It feels pretty complex to because you have a component, built of
  gates and packages and then there is a spreadsheet thing connecting
  all these. It was discussed a lot previously on this mailing list...

- But anyway there seem to be no pin/gate swap (there is a swap pin, but
  it isn't exactly what I meant)

- Funny thing: there is a 'triangle' primitive in the symbol editor :D
  Arc are done as modified line segments (like in autocad);

- Pins are *really* awful to define! You actually have to draw them with
  shapes (the line, the negation circle, clock triangle and so on), the
  pin primitive is actually only the connection point (with name and
  number attached); also no pin type (well, I agree that the DRC using
  pin type is mostly not useful, since there are a lot of programmable
  pin these days...)

- At least they have some kind of wizard to automatically create the
  most common component types

- But no 'disconnected pin' function either... so no DRC for forgotten
  pins (it seems that their schematic DRC only checks netlists against
  the PCB)

- I don't like their font but it's only my opinion (they *still* use
  a square format font...), the symbols and silks aren't that beautiful
  too (but, again, it's only my opinion and you could do your lib)

- The title block/cartridge is actually a component :P:P It seems you
  have to complete it using text objects, then; the only document
  properties it keeps seems to be the traditional OLE ones.

- ... most probably because the files are binary OLE containers at
  a first glance...

- No keyword search for components (but a little browser in the sidebar)

- Funny side bar for browsing/adding components, could be interesting
  for newbies (I personally always use component name or keywords). The
  'component bin' for removed/parked/unused stuff is an original idea
  (why not simply delete the stuff you don't want?).

- The PCB editor seems heavily biased for orthogonal routing (you
  specify the routing direction in the layer properties :D)

- Net classes seems to be only for track width;

- No high contrast for multilayer! also track crossing isn't highlight,
  the higher layer wins (by the way, why they do component side copper
  red and solder side copper cyan by default when usually it's the other
  way around?); no wait, there's an option for this. At least they have
  a layer bar to toggle visibility...

- No deleting a segment in a track, it rips all till a junction. Segment
  drag is more or less like our 'drag parallel'... also deleted tracks
  *don't* revert to ratnests?!?

- Track snap is only *after* the click; don't try this on a busy board
  :D:D

- It *actually* makes you merge nets (i.e. connecting them) in the pcb
  editor! At least it asks for confirmation... (/me shudders)

- During manual routing no ratnests to guide you :(((

- No netname on pads/tracks

- Plots are very customizable (something like the eagle postpro)

- They have truetype support for gerber... a raster fill implementation
  like that I suggested. Results are... well... questionable :P Most
  probably they didn't hinted during rasterizing.

- It can import DXFs for the board

- I don't get *why* technology files should keep color preferences
  too...

- Supports some esoteric pad style (triangle pad anyone?). I think the
  useful one that kicad misses are the rounded rectangle and the bullet
  (they are feasible with normal pads but it's a nuisance...)

- It supports courtyards (using assembly layers). Well, there is no
  'fixed' layer, they're customizable (but I don't know if it flips them
  correctly, then...)

Said that (about one hour of experimentation, so it's not an indepth
review) I can say that there is some idea to pick from them. But I'd
like to say their motto is dead wrong XD


--
Lorenzo Marcantonio
Logos Srl