kicad-developers team mailing list archive

[Nick Østergaard <oe.nick@xxxxxxxxx>]

Starting to get TL;DR near the end, but did you consider Jean-Pierre's
proposal he posed around the 12th of February 2016? See
[Kicad-developers] Custom shaped pads work. First test.

2016-03-31 0:29 GMT+02:00 Collin Anderson <metacollin@xxxxxxxxxxxx>:
> Hi, a friend of mine who is one of the engineers working on the HAWC
> Gamma-ray Observatory ( http://www.hawc-observatory.org ) is designing a
> fairly high voltage (~5kV) circuit board to drive photomultiplier tubes that
> will be in an addition of over 1000 additional Cherenkov radiation detector
> tanks. He asked me if there was a way to create rounded pads in KiCad.  Not
> oval pads, which always have a maximum possible rounding radius, but beveled
> pads, which you can specify the radius of the corner rounding of.  I of
> course told them just use oval pads, but he actually needs beveled pads.
> Rounded corners are vital for HV pcb layout, as any sharp angles will
> locally increase the electric field and an arc over is that much more
> likely.
>
> So what's the problem? Oval pads fit the bill perfectly.  There is a subtle
> problem, however: certain parts, such as 2225 size 6kV ceramic capacitors,
> require their entire termination be solidly soldered down, and these pads
> are very long and narrow.  Using oval pads that are the correct length will
> cause the corners of the termination to have no copper under them, which I
> guess isn't preferred.  Lengthening the oval pad enough to prevent this
> (which ultimately amounts to taking the length and width of a rectangular
> pad size you need, and making an oval pad with the same width, but
> width+length in length) creates significant over(under?)hang of the pad, and
> minimizing exposed bits of metal without solder mask slathered on top is
> highly desirable when those exposed bits of metal will have 5000V of
> potential on them.
>
> Here is a screenshot illustrating what I mean, with the yellow box
> representing the desired termination soldering area for one end of a
> capacitor:
> http://metacollin.com/screens/upshot_SGxPxMCJ.png
>
> Width could be increased to mitigate this in normal circumstances, but they
> need all the creepage they can get, so that really isn't an option.
>
> Also, for large circular copper pours, there are flat angles that are very
> visible.  If you have a perfectly circular edge cut, and fill a ground
> plane, you get a triacontadigon (32 sided regular polygon).  This is both in
> the rendering and the gerbers.  In fact, I have one of my own boards in hand
> that is circular that does, in fact, have visible angles around the edge in
> the ground pour, though to be frank I never noticed it until this was
> pointed out.
>
> With that in mind, I've mostly finished a minor and probably most-niche
> branch of KiCad that has the following changes:
>
> 1. Increases the segment count used for arcs, circles, curves, text,
> everything (as well as the output geometry of the various plotting engines)
> to 2 or 4 times what it currently is, as decided by setting either
> KICAD_SMOOTH_CURVES or KICAD_SMOOTHER_CURVES.  These default to off, but the
> option is there.  The nice thing is that this is all applied to how geometry
> is generated, so, for example, refilling a pour and saving the .kicad_pcb
> file, then opening it in a stock version of KiCad will yield the same
> smoother geometry for some situations.  I think the gerbers would not
> though.  Regardless, there aren't any interoperability problems.
>
> Also, I would argue that the last time it was appropriate to approximate a
> circle with 32 sides was around 1996, as my Nintendo 64 has several games
> for it (a soccer/football game, for example) that draw large circles (white
> paint on the field) and they are also 32 sides.  It's now 2016, I think we
> can manage maybe a *few* more sides than my 20 year old console with 4MB of
> ram and a 65MHz graphics coprocessor.
>
>
> 2. Add a new pad type, beveled rectangle.  I would have preferred to not
> make it an entire 5th pad type, but I could not alter anything about the
> rectangular pad type without breaking compatibility with older KiCad
> versions.  Geometrically, a beveled pad is two rectangles drawn in a cross
> "+" formation, each one narrower/shorter in one dimension (x for one, y for
> the other) by the bevel radius.  This creates 4 square cutouts at the
> corner.  Then the GetRoundCorners function which handily already exists in
> KiCad finds the correct locations to draw the rounded corners.  4 circles
> are drawn, one at each corner, with a radius equal to the bevel radius.
> This allows any desired amount of beveling to be applied to a pad.
>
> 3. The needed GUI modifications for the above are added.
>
> 4. I have only added this 5th pad geometry to the gerber plotter, and am not
> sure if it is possible to also output them to the kicad_pcb files in a
> non-backwards compatibility destroying way.
>
>
> I mainly wrote this for my friend (took an afternoon, nothing huge) and
> their need is fairly niche.  They're using my modified build for this one
> project, and that's all.  I have no plans of completing or polishing it
> further at present, but I thought I'd ask if there was any interest in my
> changes (or some set of them) being used in the main branch, or reworked
> somehow to be fit for the main branch.  If so, I can push the code to launch
> pad and develop it further.
>
> Given the compatibility-breaking nature of the changes that aren't just a
> bunch of #defines added in the right spots, I am guessing there is no
> interest :).  In fact, I am 95% sure there is no interest, mainly because
> even I, the author, have a hard time justifying the changes in light of such
> a small and niche benefit.  It seems to me that nearly all of the time, one
> can manage just fine with oval pads.  But I wrote the code, so I figured I'd
> mention it on the mailing list just in case.
>
> The main point was to start getting more familiar with KiCad's innards, as
> well as help out a friend, and that goal was achieved, so it's all good :).
>
>
> "Violence is the last refuge of the incompetent." - Isaac Asimov
>
>
> _______________________________________________
> Mailing list: https://launchpad.net/~kicad-developers
> Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
> Unsubscribe : https://launchpad.net/~kicad-developers
> More help   : https://help.launchpad.net/ListHelp
>