Hi Evan, > On 8 Jul 2019, at 17:04, Evan Shultz <[email protected]> wrote: > > Apologies in advance for what will probably be a long message... > > Would 8-way spokes be possible to implement "quickly" (in the algorithmic > sense, not the time to implement sense)? (I don't know if the shortcut you've > (Jeff) devised works for a paired set of 4 thermal spokes.) 8-way thermals > can be quite useful where there is a tough balance between connection > "strength" for current but also a requirement for thermal relief during > soldering.
8 cannot be done “fast”, although both “+” and “x” can (we do that by rotating for the calculations and then rotating back). > > Because of varying pad shapes, sometimes "+" spokes are best and other times > "x" may be preferred. So having a choice of those options, even though both > have the same number of thermal spokes, may be desirable. I believe this is > captured in the "initial angle" concept, but IMO having the choice of "+", > "x", "8 way", and "solid" is more obvious that picking an initial angle. But > perhaps I misunderstood. Right now we do “x” on circular pads and “+” on everything else. > > What about if some spokes can't be connected because the pad is near a zone > edge? Would a "+" connection lop off the rightmost spoke, for example, > leaving the other three? Is there a way to set a minimum number of spokes? Or > to force the fourth spoke to move to another location around the pad so that > the specified number of spokes are always present? Currently spokes never move, but they are lopped off if they don’t reach the zone. > > Over the years I've made good use of a hierarchy of thermal spoke properties: > - Board (default for new zones on the board) > - Per-zone properties > - Per-pad properties > > As Seth said, SMD, THT, and vias all may need different connection types. The > "relief for PTHs only" option is usually OK, but having discrete options for > all pad types that can be connected to the zone does have some benefit at > times. Not often, as mentioned, so somewhat burying these options is probably > OK. I usually find these options powerful when I have one large zone touching > many parts; a patchwork of many zones might also work but is usually a bigger > hassle in the long run. > > In addition, sometimes I want to manually control the zone connection so > having a per-pin option for "none", that creates a ratsnest until I manually > add a track for connection, is a valuable choice as well. > > Each layer (or at least top, inner, and bottom) may benefit from a unique > connection type. For example, for large leads or parts that absorb heat (like > a THT power inductor) I can often use solid zone connection on the bottom as > that layer will touch the solder wave. But on other layers, I need thermal > relief to allow for acceptable barrel fill. > > Those three pad types above may also benefit from unique clearance settings > instead of only a single per-zone clearance. If I can set additional > clearance for a single pad, and better still if I can adjust that clearance > per-layer, I can often improve solderability. > > That's a huge matrix of options but they are all valid and valuable in some > circumstances (whether the user knows how to drive the tool or not). I see no > other way than to make all of this possible in other to best balance > electrical and thermal/manufacturing desires. I know it can be beneficial. > Surely there's a reasonable cadence of implementation and release, should all > of this be eventually added to KiCad. He he. I had trouble parsing that last sentence; I kept reading “Cadence” as the company. Cheers, Jeff > > On Mon, Jul 8, 2019 at 5:59 AM Seth Hillbrand <[email protected] > <mailto:[email protected]>> wrote: > On 2019-07-08 08:15, Jeff Young wrote: > > To support it we’d need to add count (and probably initial angle) to > > the zone properties dialog, the footprint’s local clearance and > > spacing seciton and the pad’s local clearance and spacing section. So > > it would complicate the GUI (although the second and third of those > > are at least on a seldom-used tab). > > If we decide to implement this, I'd like to also have an optional > "suppress instances" list so that if for some reason the auto placement > of spokes on a custom shape didn't work, I could remove the unwanted > spokes. > > But I think that these properties should not go in the zones, only in > the footprint and pads as it is sufficiently outre that it is unlikely > to find much use in the general setting. > > The properties that may be useful in the zones settings would be spoke > defaults for SMD, through-hole and vias. These might be addressable by > placing an ellipsis button after the Pad Connections drop down that > brings up an advanced dialog setting. > > This is pure spitballing however. > > -S > > _______________________________________________ > Mailing list: https://launchpad.net/~kicad-developers > <https://launchpad.net/~kicad-developers> > Post to : [email protected] > <mailto:[email protected]> > Unsubscribe : https://launchpad.net/~kicad-developers > <https://launchpad.net/~kicad-developers> > More help : https://help.launchpad.net/ListHelp > <https://help.launchpad.net/ListHelp>
_______________________________________________ Mailing list: https://launchpad.net/~kicad-developers Post to : [email protected] Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
