TO-71 PCB footprint

[Eamonn Harter]

Hello,

I am designing a PCB that will use a TO-71 package component, and am trying to decide on the correct footprint to use for the layout.  With pins in a 100mil diameter circle, there isn't much room to use for the pads and plated through-holes.  If I had more space, I would probably go with 25mil diameter holes in 40-50mil pads.  Should I not be afraid to spread the pins on the TO-71 component and use a wider hole/pad spacing for the PCB?  Does anyone know what the standard practice is in designing a PCB that uses TO-71 components?  The internet hasn't been much help on this question, and datasheets also avoid the topic.  (The specific component in question is an LSK389 dual N-channel JFET from Linear Systems.)

[T3sl4co1l]

Yes, normally the leads are formed to a larger circle, or to a DIP-6 or 8 pattern.

Tim

[floobydust]

It's a really small part for 6-pins in basically a TO-46 can.
You can splay out the pins to a larger circle but patience to install the leads. The part sits up anyhow.

See here at the tiny pads if you keep the leads straight (0.1" dia.) verses a bit increased circle to 4mm dia.rad (0.157")
This is what I came up with for a LSJ689/LSK489 pcb footprint. I haven't finished pcbs with it but the parts are here.
Shown is 1.1mm pad (43thou) with 0.7mm hole (28thou) on 2mm radius, gives about 18thou clearance between pads.

[Eamonn Harter]

Thank you both for your replies.  I like the idea of using a slightly larger circular pattern.  I searched on JEDEC for an officially sanctioned footprint, but came up empty handed.  I guess for some problems you just need to use common sense.

[David Hess]

Just like with a TO-92, there is no sanctioned footprint.

With a TO-92, the pins are on 0.05" centers so often the outer two holes are placed 0.1" apart and the center hole is offset 0.05" which is common for crimped TO-92 leads anyway.  With a TO-71, you could use this arrangement on each side or just make it up as you go along.