direct connect vs relief connnect in GND plane

[sakura_irw]

relief connect

is there any good reason why the GND plane should be used direct connect @ relief connect in pouring the GND plane?

 

[Rame]

direct connect与relief connect

Hi,

A wagon wheel-shaped relief pad etched in the copper of a ground plain around a through hole. It connects to the plane through one or more narrow track across an opening in the plane, rather than connecting directly to the plane, so that heat transfer to the plane is minimized during soldering.


Regards,

Ramesh

 

[cyberrat]

is thermal relief required for smd pads

A more direct connection will obviously give you a much better path to ground as there is more copper contacting the pad.

However there is a drawback to this during assembly, as Ramesh says.

(thats if your making a board commercially)

What that means is that the pad connecting to ground, if completely covered in ground plane will heat slower and cool faster then the opposite pad on a 2 terminal component I.E. resistor.

This can cause a SMT component to stand on end (tombstone) or rotate if more than 2 terminals.

For PTH components I.E. terminal blocks etc it will make the soldering very poor.

As current requirements are for lead free solder which requires a greater heat & wicks less it seems even more important to add "thermal relief" to pads.

Thats the reasoning for "not" having a full connection to a plane, the reasons for are "technical" & likely to cause assembly problems.

However if you are making an RF board then you may have to do this, in which case you would ensure that you balance the copper distribution on the opposite pads & have an enhanced inspection & rework stage.

If the board is just a home project, low volume/hand assembly then go for it.

 

[FvM]

how to add thermal relief on power pins

with usual SMT solder technologies, PCB board material is warmed up almost even, thus thermal relief isn't generally needed here to my opinion. With any fast circuit, I disable it for vias and use it for throughplated pins only. With high current pins, you should consider, that thermal relief could act as an unwanted "fuse" with melting integral lower than intended circuit protection means.

 

[touringmike]

thermal relief connecting to power plane pcb

with usual SMT solder technologies, PCB board material is warmed up almost even, thus thermal relief isn't generally needed here to my opinion. With any fast circuit, I disable it for vias and use it for throughplated pins only. With high current pins, you should consider, that thermal relief could act as an unwanted "fuse" with melting integral lower than intended circuit protection means.

I agree. The majority of board fabricators will now balance the copper coverage
percentage to be equal on all layers of the board. Certain high-end design programs will report copper coverage, so that the designer can create the balance themselves. This helps to eleviate any thermal separation possibilities, which I have experienced a few years ago.

Also remember, if using high pin count BGAs with an enormous amounts of power/ground connections with small via hole diameter =<.010 inch, it's best to use direct connect over thermal relief pads which could cause island effects (floating/unconnected pins)