Here’s a common scenario: You have an array of small components. Maybe some SOT23 transistors or a set of LEDs. On one side, you have wires and chips and stuff hooked up all over the place. On the other side, you have a ground plane.
The easy route would just plop the grounded pad of the part right on the ground plane. You would get better heatsinking if needed. You get a much more direct path to ground. It would be quicker to lay out.
But — and there’s almost always a “but” to such questions — you could get tombstoning. Especially if the parts are 0402s or smaller. You would also likely have soldering problems because the plane will act like a heatsink and may keep the solder paste from melting.
If you really need to, you could do the pad directly on plane thing, but you’d probably have to hand retouch each connection on the big pad and maybe rework tombstoned or crooked parts.
Much better would be to do something like the image on the right. You could also use thermal pads in the plane. With really small parts though, you might still be opening yourself up to soldering problems because of the heatsinking of the plane. The thermal pads would typically have three connections to the plane in a setup like this and that could still be an unequal amount of copper connecting on one side vs the other. You generally want the same amount of copper on both sides of the small parts.
You could also just run the eight traces straight to the plane. How would you approach this seemingly simple but surprisingly error-prone layout?
You’ll take the left road and I’ll take the right road
And I’ll be in reflow before you
How would I approach this? … as implied by you… it depends…
In your example…. It doesn’t appear there would be much heat sinking requirement.
The LEDs appear to be pretty small (don’t know value of resistors or voltage used).
so, thin (6-8 mil) traces on both sides of the components would be fine ( assuming modest ambient temp range for final product)..
Even if there was a short run (single trace, 50 mils long) into a ground plane… it would likely be fine.
On my CAD system… I generally don’t allow the pouring feature to automatically make thermal connections.. I like to control this on a component basis ( unless old large though hole technology is being used)… so I route a simple connection to each pad involved, then pour with the option of “disable thermal connections when pad connected”- enabled.
Another option: specify large thermal connection lengths with very narrow thermal connections. ( 50 mil thermal gap, 5 mil trace for thermal connection) when making a ground pour of the area.
However, If that were not the case….(higher power or temperature range)
Fatter traces both sides of the resistors and LEDs may be called for… to keep it balanced.
(as you noted, the need for a thermal balance on small parts)
Under no conditions would I pour the ground plane without any thermal connection considerations (top example) on one side of the components.
In some RF circuits… there may be a compelling reasons to “blow off” thermal and manufacturing issues (extreme sensitivity to extra inductance, etc..) .. but I would try to avoid this situation at all costs.
Saw some recent references to some new ICs that operate at over 700 gHz!
At these speeds… everything changes…