16
\$\begingroup\$

My PCB design software comes with some libraries that include some common components, like chip resistors and capacitors. I have noticed, however, that the footprint land pattern for the 0805 resistor is not identical to the 0805 capacitor.

I then did some googling, and discovered multiple IPC standards that don't seem to quite agree with each other.

Is there a reason an 0805 resistor would have a different land pattern than an 0805 capacitor? Is there a "best standard"? IPC-7351, IPC-SM-782, or what?

| improve this question | |
\$\endgroup\$
  • 2
    \$\begingroup\$ what assembly process? (wave, reflow, hand, etc) \$\endgroup\$ – Mark Apr 15 '11 at 1:40
  • \$\begingroup\$ Lead free reflow \$\endgroup\$ – ajs410 Apr 15 '11 at 14:33
20
\$\begingroup\$

The current standard is IPC-7351B, which replaced IPC-7351A, IPC-7351 and IPC-SM-782 (in that order). Mentor Graphics have a free PCB land pattern viewer for Windows (old link; they rebranded to PADS) for all of the standard parts using this standard. Each part also includes a "courtyard" layer which defines how much space needs to be left around the component for manufacturing; useful when you are designing high density boards.

The standard itself consists of three versions but for most boards it is recommended that the "N" suffix (Nominal) footprints are used. Note that most parts do differ slightly from manufacturer recommended patterns but in my experience (and the experiences of my board loader these footprints do tend to meet manufacturing requirements very well.

As for you query about the 0805 resistor vs 0805 capacitor, I suspect that the footprints have been designed to best attach the parts; while they are fairly similar in the horizontal plane, capacitors do tend to be slightly higher so maybe the differences in the footprints take this into account.

| improve this answer | |
\$\endgroup\$
  • 3
    \$\begingroup\$ depending on the value of the cap the thickness can be a large issue. Your average 0805 resistor is 15-20mil thick, a 10uF MLCC is ~60mil tall which can be really tall for a stock 0805 land pattern. \$\endgroup\$ – Mark Apr 15 '11 at 1:39
  • 3
    \$\begingroup\$ I think I read something about how the solder should reflow to the top of the component. Considering that a cap is taller than a resistor, this would imply that the land pattern should be larger, to allow for more solder paste that can reflow properly. I think this was called the...toe fillet? \$\endgroup\$ – ajs410 Apr 15 '11 at 14:51
6
\$\begingroup\$

Taller SMT discrete packages require bigger pads tio get get a good fillet.

| improve this answer | |
\$\endgroup\$

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.