← Back to team overview

kicad-developers team mailing list archive

Re: Polygon work


jean-pierre.charras@... wrote:
Rok Markovic a écrit :


There are still some problems with thermals. One, that I encounter in my
boards is when in close pitch components (VQFP, ... ) two neighbouring
pads are on zone. When drawing thermal holes in such a situation, each
neighbouring pad draws around itself a hole. This hole cuts the thermal
connection to other pad. Please see atached pictures, I understand if my
explanation is unclear.

The only option I see is to add thermal connections after removing all
pads from zones. I understand that this concept has problems (DRC), but
I would like to ask if it CAN be done.

Removal all pads in zone is NOT the problem.
The problem is you have set parameters that cannot allow stubs.
You cannot want a minimun thickness copper zone bigger than max stubs width and expect to have subs. You cannot want an antipad size bigger than pads gap and have copper between pads.

You cannot solve this by code modification, because this is not really a code problem.

One can want to specify specific thermal parameters for a givn footprint ( or a given pad). A possible approach is to allow to define parameters (when are not set to default) on a footprint and/or pad basis. But obviously, minimun thickness copper zone must be bigger than max stubs width.

Advantage: handle very small pads ans special cases.
Drawback: more and more complex way to handle zones parameters, and in many cases not very easy to understand.
But this can be a solution in some cases and must be considered.

Many kicad users could be unable to set/choose good parameters.

the answer to your question is:
this can be done.
But this will creates some ugly code and problems:
- stubs must are tracks, not zone fill segments, because they will be outside filled areas, and must be considered in connection and DRC calculations As a consequence, they are obstacle to create new tracks. Existing zones are never obstacles, because copper in areas is removed when calculating new filled ares in zones.
- stubs *must* be removed when a zone (or its filled areas) is removed.

So i am not well-disposed to this approach because this problem is only the result of an other problem, mainly a bad parameters choice.

On my boards most all components are SMT with a handful of through hole components. I asked my board manufacturer if they thought I needed thermal reliefs and they said no. I guess thermal reliefs are only for hand soldered components? If so, aren't hand soldered components typically fairly large pads with fairly large pad to pad distances?

A wave machine or an SMT reflow process does not need thermal reliefs according to my board manufacturer. Does this information help, contradict, or confuse?


Follow ups