Polygon pad connections and thermal reliefs

[MarioBlunk]

I’m playing with the polygon setting “Pad connections” where the user sets the kind of thermal reliefs.
What is the idea of the setting “Reliefs for PTH only” ? If selected, this setting results in ALL SMT-pads to be solidly embedded into the polygon with out any thermal spokes. I presume it is because of some RF considerations regarding SMT pads ?

[DavidR]

For reflow oven soldering of SMT parts there is not much need for thermal reliefs.

[ronsimpson]

I do not use thermals.

1. not needed because of how we solder the boards.
2. many of my parts are hot and I need to get the heat out into copper and away from the part. (heat sink)

[MarioBlunk]

Yes, I agree, there are parts which need a low thermal impedance between pad and surrounding copper polygon. But this requirement can/shall not be generalized for all parts connected with the polygon. Manual rework of such SMT pads is close to impossible. This applies to PTH pads likewise.
Shouldn’t there be a special option for a pad like “no thermal relief” in the footprint model instead ? This enables the user to set up special footprints that require a solid connection.

[Naib]

You can do that already.
The footprint editor permits you to choose the pad connection so you can force a part to default to thermal or solid or inherit from the zone.

This can either be done with the footprint (best way) or actually on individual pads in PCBnew. The downside of specific pads is IF you do a refresh from library those custom settings are lost.

I always set the connection to copper zone as SOLID for parts where high current (inductors, resistors, FETS…) is needed

It does mean rework is bordering on impossible but the need of the circuit outweighs the need of modification unfortunately. I have an IMS card and the 0603 resistors have thermal relief but I am unable to rework them as the IMS sucks the heat away so it does beg the question… why did I add them for such cards