1
\$\begingroup\$

In my two-layer pcb design I have an LM317 with a TO220 package. I took the generic TO220 package from the default "linear" Eagle library which does not have a polygon copper pad under the body of the part. However, since the body is connected internally to pin 2 (middle pin) which is the regulator output, the current design would short output to ground (top layer, red).

But I am not really sure where to put the polygon under the part body. If I manually put it to the top layer of the board itself, this does not seem like a robust solution because on the next board I will have to remember again in order not to short supply voltage.

On the other hand, if I put the polygon on the pad layer (green) of the package of the part, it is going to be on the bottom pcb side as well where I probably want to place other traces (like for the design below, blue).

And finally if I put the polygon on the top layer of the package, I won't be able to place the part on the bottom side of the board, if I ever wanted to (or at least the polygon will be on the wrong side then). Edit: I was wrongly assuming that the top layer would stay the top layer when the part is mirrored (placed on the bottom of the board). On the contrary, it is going to become the bottom layer (quite logical...). So placing the pad on the top layer inside the package (like it is the default for SMD parts) is my solution.

So what is the right way of placing the poylgon under the regulator body?

enter image description here

\$\endgroup\$
2
\$\begingroup\$

So what is the right way of placing the polygon under the regulator body?

The right way would be to choose correct part package first.

If you want the part to be placed flat on the board, use SOT-223 or TO-263 package. The TO-220 is designed to be mounted vertically and bolted to the heatsink above the PCB. That's exactly the reason why Eagle library does not have a pad for it.

UPDATE:

The hole in the package is for mounting on heatsink. The manufacturers usually have guidelines for mounting their products, see for example the one from ST, or from Motorola.

FWIW, I think that footprint should not have been in the library to begin with. While bending TO-220 leads is possible, it is hard to do consistently in mass production without special fixture (the guidelines above call this fixture a "clamping tool"). Some companies offer customized lead bending, but it is for huge orders only.

One possible solution is to modify the footprint to make a hole in the PCB larger than necessary and use washers. Otherwise if you bend leads slightly off-place and force them into holes there will be a strain on the plastic body that can develop into crack overtime.

| improve this answer | |
\$\endgroup\$
  • \$\begingroup\$ Thanks for your answer. But the SOT-223 and TO-263 inside the "linear" package appear to be SMD's. On the other hand, why does the TO-220 package have a hole where the cooling fin is (see image in the OP), when it is supposed to be mounted vertically? \$\endgroup\$ – oliver Jan 18 at 8:50
  • \$\begingroup\$ @oliver see an update in the answer \$\endgroup\$ – Maple Jan 18 at 8:55
  • \$\begingroup\$ I see, but in my case (hobby electronics) I am not so worried about manually bending the pins. And, at least I think I remember from times when through-hole components were the norm, you could see the horizontal placement of TO220 pretty often. \$\endgroup\$ – oliver Jan 18 at 8:58
  • \$\begingroup\$ But I understand that this all limits the necessity of having such a package in the standard libs of Eagle. So from the SMD packages you have mentioned, it looks like placing the body pad on the top layer of the package is the usual way to go, isn't it? \$\endgroup\$ – oliver Jan 18 at 9:00
  • 1
    \$\begingroup\$ You can still see horizontal TO220 here and there. But you've asked for a "right way", and that is a wrong thing to ask in hobby electronics. You can pretty much do whatever is convenient for you and thermally/electrically sound. For the mass production you'd design (or find off shelf) a heatsink and make custom library footprint for it. Then you arrange for manufacturer to supply components pre-bent to your specification. \$\endgroup\$ – Maple Jan 18 at 9:05
1
\$\begingroup\$

If you are laying down a TO-220, you can add a pad under the tab as a separate pad on the symbol. What you do with it depends on your intent. On a 2-sided board you might want to use the top layer as a heatsink and make the pad relatively large. On a multilayer board you might want to pepper it with thermal vias to make contact with the ground plane. You might want to leave room on the sides for a U-shaped heatsink between the part and the board. If the dissipation is negligible you might just want a keepout on the top layer. There are even heatsinks that take up no extra board area (from here):

enter image description here

Basically, just make up a footprint for the particular situation as you need it- if you can re-use a previous one, all the better, but don't hesitate to make a new one if it makes the design better.

If you manually flip it to the other side of the board, you are going to have to have the face (plastic side) facing the board anyway to keep the pin order correct, so it's not going to short to the PCB.

| improve this answer | |
\$\endgroup\$
  • 1
    \$\begingroup\$ wow, that's a nice find. certainly beats cutting them myself from old CPU heatsinks :) \$\endgroup\$ – Maple Jan 18 at 9:33

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.