Author Topic: Ideal 0402 footprints  (Read 352 times)

0 Members and 1 Guest are viewing this topic.

Offline Rachie5272

  • Regular Contributor
  • *
  • Posts: 159
Ideal 0402 footprints
« on: April 11, 2021, 04:22:09 pm »
I've been designing a lot of boards with 0402 resistors and capacitors lately, and I feel like the footprints are off.  I do prototype assembly and rework myself using hot air, and I've noticed the components tend to wander a bit on their pads.  They don't snap cleanly into place like they do in Louis Rossmann's videos (yes, I'm using copious amounts of flux).

I generated the footprints using Altium's IPC footprint wizard, with level B density.  Curiously, resistors and capacitors have different sizes.  And of course, different manufacturers have different footprints for the same size components in their datasheets, when they bother to list them at all.

What would people recommend for ideal footprint dimensions, for machine assembly?  Should resistors and capacitors be the same?  Rounded corners, even though most datasheets are rectangular?

For reference, my current 0402 resistors have 0.5mm x 0.6mm pads, with a 1mm on center spacing, 50% rounded corners.  The 0402 capacitors have 0.4mm x 0.5mm pads, with a 0.8mm on center spacing, 50% rounded corners.

Offline T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 16973
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: Ideal 0402 footprints
« Reply #1 on: April 11, 2021, 04:59:10 pm »
IPC is just a starting point -- it's not just okay, but highly recommended, to tune things for the particular assembly process you're using.  IPC should get pretty close, and no one should have trouble using it, given basic (but adequate) tools for the process required (e.g., reflow).

I have two footprints in my library, long and short.  (I have R and C variants, but the dimensions happen to be the same right now.)  The long one has enough meat to get a soldering iron tip in there (tip radius < 0.5mm say).  Pads are a bit wider than the component body (0.7mm).  I use it when I expect to change parts a lot, say for prototypes.

The short one has minimal pads (possibly less than IPC minimal, I forget), it's almost an LGA style footprint -- which is arguably quite fair, as most of the metallization is on the bottom face, and you can make toe fillets if you like*.  It has nearly net size pads, 0.55mm wide.  I find it has better "grab" (centering) with hot air, and I normally use it for production designs.  It is, as expected, almost impossible to fix by iron; your best bet is a fat blob of solder to sort of manually wave-solder it.  Either method is... kind of a PITA sometimes; last board I used a lot of them on, had heavy internal layers, it took five solid minutes of hot air to change a few chips...

The exact dimensions are:
Overall length (pad to pad ends, 'Z'): 2.2mm
Width ('X'): 0.7mm
Centers ('C'): 1.3mm
Pad gap ('G'): 0.4mm
Pad length ('Y'): 0.9mm

Overall length (pad to pad ends, 'Z'): 1.275mm
Width ('X'): 0.55mm
Centers ('C'): 0.85mm
Pad gap ('G'): 0.425mm
Pad length ('Y'): 0.425mm

(Symbols are from IPC-SM-782A)

All of them have 20% corner radius.

*Toe fillets are preferred for inspection purposes, if nothing else!  If you have one good fillet, you're probably alright.  For most parts, the toe fillet takes priority (or heel for J-leads), since it's external and inspectable.  Side fillets aren't even possible, much of the time (IPC specs most DIL side fillets at +/- something small -- yes, they can even be negative!).  Heel fillets are probably more important for strength, say on gull wing leads, so don't ignore them, but they are hard to inspect and confirm that they're doing what you want them to do.

YMMV, I haven't had too many through high production (10k's?), or at least haven't heard anything back from assembly.  Can't be too bad, but not necessarily great?

Mind that turn-key assemblers may modify geometry to suit their process; simple square (or rounded) pads are generic enough, and may do as-is, or with just a paste mod (sometimes a "home plate" or other shape is used to optimize release and placement of solder).  Don't worry about it, whatever they do is for their process, after all.

So if you're tuning for your own process, try things and see what works. If for someone else's, don't worry about it, IPC should be pretty close.

Seven Transistor Labs, LLC
Electronic design, from concept to prototype.
Bringing a project to life?  Send me a message!

Offline Mecanix

  • Regular Contributor
  • *
  • Posts: 218
  • Country: cc
Re: Ideal 0402 footprints
« Reply #2 on: April 12, 2021, 03:56:59 pm »
Measured mine for you and yours seems quite in line with what I have already. Less the wobbling thing.
I do however need to use a Sn63Pb37 (Type 5: 15~20uM) paste for the 0402 though.
How about yours?

Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo