SOT223-6 compact footprint

[Paroidia]

The lands on the default SOT223-6 footprint seemed excessively large, especially compared to those for a similarly sized SOIC so I made some adjustments. Will this be ok or is there a good reason for the "standard" lands being so large that I'm not aware of? Original footprint is on the left and the modified version is on the right.

[tszaboo]

Footprints usually come in 3 sizes. M N L. Minimum, nominal, large (I think).
So you might want to find the minimum recommended sizes for that footprint.

[thm_w]

As tszaboo says, there should already be a standard footprint that matches your right side image. Probably N or L.
Least, Nominal, Most (https://electronics.stackexchange.com/questions/378766/altium-what-stands-for-n-m-and-l-as-a-suffix-for-soic-packages)

The reasons for the larger pads that extend out would be hand-solderability. If you are not hand soldering there is no need.
The tab copper area can be enlarged int the design itself if more heatsinking is wanted.

[wraper]

Footprint on the right is garbage as it does not allow space for proper solder fillet to be formed (if 3D package represents real terminal dimensions) and minor component misplacement will result terminals to be at least partially out of the pad. Also larger pads provide more mechanical strength. Making too small pads for no reason (like increasing PCB density) is pointless.

[PCB.Wiz]

The lands on the default SOT223-6 footprint seemed excessively large, especially compared to those for a similarly sized SOIC so I made some adjustments.
Will this be ok or is there a good reason for the "standard" lands being so large that I'm not aware of?

Packages like SOT223 are usually expected to dissipate some power, so larger copper is common. Most PCB designs add a lot more copper to that tab.

If you are tight in one direction, you could shrink from the generic footprint, but you should leave some overhang to allow a solder fillet and inspection.
Check against the exact part you will be using.

There are also SOT89 packages for medium power devices.

[Paroidia]

The lands on the default SOT223-6 footprint seemed excessively large, especially compared to those for a similarly sized SOIC so I made some adjustments.
Will this be ok or is there a good reason for the "standard" lands being so large that I'm not aware of?

Packages like SOT223 are usually expected to dissipate some power, so larger copper is common. Most PCB designs add a lot more copper to that tab.

If you are tight in one direction, you could shrink from the generic footprint, but you should leave some overhang to allow a solder fillet and inspection.
Check against the exact part you will be using.

There are also SOT89 packages for medium power devices.

 I added some additional overhang to the leads and tab. The tab is soldered to a copper area with multiple vias connecting it to the ground plane on the back of the PCB. Heat dissipation isn't super critical as this will be outputting 5V from a 2S li-ion pack so the voltage difference will at most be 3.4v and usually more like 2.4v or lower. It's also not likely go over 1A unless someone were to connect two ELSR receivers to it and then configure the telemetry for 250mw (which would already be dumb anyway) and then connected it to a controller with an H7 processor on it.

[T3sl4co1l]

Footprint on the right is garbage as it does not allow space for proper solder fillet to be formed (if 3D package represents real terminal dimensions) and minor component misplacement will result terminals to be at least partially out of the pad. Also larger pads provide more mechanical strength. Making too small pads for no reason (like increasing PCB density) is pointless.

I wouldn't be so dismissive; rule I heard is, as long as there is one fillet, and no pins resting on soldermask (gross fit / alignment error), it's okay.

Relying on toe fillets (under the part) may make headaches for assembly and inspection, though.

Toe fillets are generally preferred as they are easy to inspect, and 2nd preference for side when possible (so, the tab can do here, maybe not so much the leads, but the leads of a SOT-223-4 certainly can get some).

Mind, I'm not involved in assembly, so this may be in-house specific, out of date, etc.

Packages like SOT223 are usually expected to dissipate some power, so larger copper is common. Most PCB designs add a lot more copper to that tab.

If you are tight in one direction, you could shrink from the generic footprint, but you should leave some overhang to allow a solder fillet and inspection.
Check against the exact part you will be using.

There are also SOT89 packages for medium power devices.

Not to mention DFNs -- the SO-8 style (variously PDSO-, PDFN-5x6, etc.), and 3x3mm packages, are very common and perform quite well.

Tim

[Paroidia]

Ok how's this?

 Because everyone always asks D1 is an OR-ing diode necessary because the controller can be connected to USB for setup and the 5V from USB will power the device, (it has an OR-ing diode on the USB port already). Disconnecting the battery isn't an option because then the servos wouldn't be powered. Also the battery and ground is connected to the servo power buss on both sides of the PCB which is why I have those big pads with all the vias connecting to the + and - on the pin header.

[PCB.Wiz]

Heat dissipation isn't super critical as this will be outputting 5V from a 2S li-ion pack so the voltage difference will at most be 3.4v and usually more like 2.4v or lower.
It's also not likely go over 1A unless someone were to connect two ELSR receivers to it and then configure the telemetry for 250mw (which would already be dumb anyway) and then connected it to a controller with an H7 processor on it.

So that means it could be ~0.5A at 2.4V ?
That's still a reasonable 1.2W, so I'd do maximal copper for the tab. ie use all the free board for cooling/spreading copper.

[tszaboo]

As tszaboo says, there should already be a standard footprint that matches your right side image. Probably N or L.
Least, Nominal, Most (https://electronics.stackexchange.com/questions/378766/altium-what-stands-for-n-m-and-l-as-a-suffix-for-soic-packages)

The reasons for the larger pads that extend out would be hand-solderability. If you are not hand soldering there is no need.
The tab copper area can be enlarged int the design itself if more heatsinking is wanted.

Thanks for correcting me, I get these wrong all the time.

[Paroidia]

Heat dissipation isn't super critical as this will be outputting 5V from a 2S li-ion pack so the voltage difference will at most be 3.4v and usually more like 2.4v or lower.
It's also not likely go over 1A unless someone were to connect two ELSR receivers to it and then configure the telemetry for 250mw (which would already be dumb anyway) and then connected it to a controller with an H7 processor on it.

So that means it could be ~0.5A at 2.4V ?
That's still a reasonable 1.2W, so I'd do maximal copper for the tab. ie use all the free board for cooling/spreading copper.

 No it'll always be 5v output and 5.5V~8.4V input depending on if using HV servos or 6V servos (HV servos are made to use 2S li-ion) I'd expect an F7 based FC to pull around 400mv which leaves plenty of headroom for any 5V devices connected to the 5V side of the pin header.  I connected the copper area around the regulator to the large ground plane on the other side by many vias.

 EDIT: Took your advice and poured a maximized copper area on the top side as well to help with heat dissipation.