4
\$\begingroup\$

I've pulled datasheets for a dozen compatible NPNs from Toshiba, Diodes, Onsemi and Nexperia. They all had different recommended layouts for SOT89 package. More than that, Nexperia has different footprints for wave and reflow, KiCAD has yet another layout, and simple picture search on web produces a dozen more variants. It is like nobody knows what to do with this particular package.

I have no problems creating custom footprint for the part I will actually order, but I don't want to be stuck with it. Any recommendations?

EDIT: I would like to know if it is important to use recommended layouts from datasheet for each particular part even though they all are specified as SOT89 package. In addition, if one footprint can be used for all of them then I would like a recommendation on which one is better.

BTW, I've used this package before, did not pay any attention to recommended layout and simply used KiCAD footprint. Seems to work just fine, even though the recommended layout had 3 separate paste shapes for central pad, while KiCAD used pad outline for paste.

UPDATE: Just to illustrate what I am talking about, here are suggested footprints from TI, ROHM, Infineon and Diodes Inc datasheets. Note, how central pad comes very close to sides on ROHM and especially on Diodes layouts. Also note trapezoidal shape of TI pad for better paste release, as discussed here:

SOT89 footprint image adapted from Texas Instruments TL431 datasheet
Adapted from Texas Instruments TL431 datasheet

SOT89 footprint image adapted from ROHM BDxxFA1 Series Application Information application note
Adapted from ROHM BDxxFA1 Series Application Information application note

SOT89 footprint image adapted from Infineon PG-SOT89-4-2 footprint
Adapted from Infineon PG-SOT89-4-2 footprint document

SOT89 footprint image adapted from Diodes Inc. AP7370 datasheet
Adapted from Diodes Inc. AP7370 datasheet

\$\endgroup\$
0

4 Answers 4

2
\$\begingroup\$

There are three issues in play here:

  1. Not all packages are identical. SOT-89 is the JEDEC reference; SC-62 is the EIAJ reference; and most manufacturers have their own internal numbers which need not match an industry standard (for example, having their dimensions and tolerances a subset of the industry standards). There may also be lookalikes, with similar shape but outside the tolerances of such a standard. (I don't think there's any SOT-89-alikes, or that I recall offhand, but there are some quirky SOT-23-alikes that are just different enough you might want to update their footprint.)

  2. Not all footprints are created equal. There are two sub-issues in turn:

    (a) Manufacturers may specify their part is some e.g. JEDEC standard, but realize this includes gross-dimensioned parts like TO-220 (the non-AB version I mean!), DO-214 series, etc., and compliant footprints for these can be quite awkward. Real parts never (in my experience) use the full dimensional range of these old standards. But manufacturers rarely show what dimensions (tolerances included) they're actually making them to -- they give the JEDEC file, not their internal one.

    Assuming this is the case -- you can, perhaps, infer their package dimensions from the footprint, when a minimal footprint is provided. There are, for example, SMA diodes where the datasheet gives a footprint that won't even fit a LMC/MMC part per their own drawing (which again, isn't the internal drawing but the JEDEC one). And by "fit", I mean, the leads either won't both align with the pads, or one or both leads are resting on soldermask rather than pad face.

    (b) Footprints are dimensioned differently, for different purposes. IPC-7351B is the basic starting point, and also a good introduction for terminology, solder joint types, and measurement. They give three basic calculations: minimal / high-density, normal, and maximal / low-density. The manufacturer may choose any of these, or use their own bespoke calculations. And again, they may calculate them from their internal drawings, rather than what they show the customer.

  3. Different footprint dimensions serve different purposes. You might choose among the IPC options where component placement density is a primary concern (as the names suggest), or you might choose larger pad dimensions for easier hand soldering. Still other dimensions apply for wave soldering (which may include asymmetrical pads and different footprints for different orientations on the board!).

    Ultimately, footprint dimensions are driven by production: they determine soldering quality and consistency. And then it's worth getting into esoterica like home-plate or dogbone paste patterns, shaving pads or soldermask to optimize fab and assy yield, etc.

    If you aren't making thousands of boards per year, just stick with IPC calculations or manufacturer recommended dimensions. They won't be particularly good, but they're most likely to work at any CM (contract manufacturer), without incurring huge hand rework trouble.

\$\endgroup\$
8
  • \$\begingroup\$ This is nice overview of the common challenges with footprints. My usual approach is to see what KiCAD has available and if the differences with datasheet are under 0.1 mm just go with it. However there is a reason I've asked specifically about SOT89. Unlike other footprints, there are huge differences not only in dimensions but also in shape of the middle pad. Some of them are T-shaped, some hexagonal, and some have multiple paste openings. I've never seen such discrepancy with other packages, that is why I asked the question \$\endgroup\$
    – Maple
    Jan 5 at 23:20
  • \$\begingroup\$ Also, the differences between wave and reflow are usually smaller, one is mask-defined, another is pad-defined. I understand the point about the manufacturing factor, it has been pointed out in other answers too. Though I suspect very few small companies really go that deep into manufacturing process, most being content with whatever Chinese factories churn out because price drops with volume faster than with optimization. \$\endgroup\$
    – Maple
    Jan 5 at 23:32
  • \$\begingroup\$ You can view the shapes as variations on side/heel/toe fillet dimensions around the perimeter. The shapes don't in general have to match, though one would certainly prefer symmetry at least, so surface tension draws it on center. Multiple paste openings are a different matter, used to optimize the amount of solder deposited, or avoid excessively large openings that wouldn't screed a level dose otherwise. You see the same thing on QFN pads for example, if not in the footprint then the CM will do it automatically. \$\endgroup\$ Jan 6 at 4:55
  • \$\begingroup\$ "symmetry at least, so surface tension draws it on center" I think you have something important here. While these parts are symmetrical in one dimension, they are not in the other. I've looked over footprints options again and I believe that all T-shaped layouts have centroid quite offset from that of a middle pad on a package. Which means surface tension may put the component into position with up to 0.5 mm offset from what the courtyard is suggesting. That is a huge difference. \$\endgroup\$
    – Maple
    Jan 6 at 17:12
  • 1
    \$\begingroup\$ Personally I use something like the TI one as well, though with rounded corners. (But that doesn't mean much as it's not had many hundreds of units produced and checked. It's passed an automated DFM at least... I think?) Even if square outline pads best match part geometry, a tip is to use radiused corners, as most EDA tools will calculate square expansion/clearance around the square pad -- which isn't how distance works, but it's drawn correctly when a nonzero radius is used. \$\endgroup\$ Jan 7 at 3:12
4
\$\begingroup\$

The criticality depends on the manufacturing process, so it's really not even that much about the footprint itself.

If in doubt, best ask the place where you intend to assemble the boards with components what they suggest for the pads and stencil.

At least for smaller components, the pad shape versus stencil opening for paste is important, as then it is about the stencil thickness how much paste gets applied in total.

So to get the right amount, be sure to know what is the intended stencil thickness.

And then there are a lot of factors how well the paste is applied, and will there be air pockets or will some portion get stuck with the stencil when lifting the stencil up from the board. And some of these factors are dependent on paste viscosity and the size of solder beads it had. And the viscosity of the paste changes over time after the jar is opened, and temperature it is being used at.

Correct stencil design also prevents loose solder balls forming.

Assuming this is even meant for reflow or wave soldering.

\$\endgroup\$
3
  • 1
    \$\begingroup\$ First answer to mention paste openings. For me it seems most important part, along with the distance between central pad and two sides. KiCAD has diamond-shaped central pad with large clearance. In recommended footprints it is rectangular and comes pretty close to the sides, so with excess of paste there is a risk of hard to see bridges under the body... I think \$\endgroup\$
    – Maple
    Jan 4 at 19:54
  • \$\begingroup\$ @Maple I would also be concerned with the solder mask shape, especially for the large pad. \$\endgroup\$
    – qrk
    Jan 6 at 19:44
  • 1
    \$\begingroup\$ @qrk yes, all those sharp-cornered layouts are not exactly paste-friendly and it is my understanding that solder mask also holds better with round corners (IPC-7351C) \$\endgroup\$
    – Maple
    Jan 6 at 19:47
2
\$\begingroup\$

Most likely, all of the footprints you found will work. If in doubt, take one that seems to be the average of the ones you found.

The footprints are optimised for different manufacturers and different applications. In fact, your footprint has an influence on yield during manufacturing and soldering. If special considerations are taken while designing the footprint, you can even reduce thermal stress related failures when the PCB is deployed (this is why space-grade PCB footprints have rounded corners).

\$\endgroup\$
0
\$\begingroup\$

They will all work. The differences are subtle and affect yields depending on production facilities. Dense boards are harder for some manufacturers, others will easily do whatever you need. Also IPC610, the production standard, may require certain properties (normally slightly larger pads and certain amount of solder) for higher tiers, such as aerospace. For consumer - just do whatever doesn't fall apart when you breath near it.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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