11
\$\begingroup\$

I was looking at the footprints in Altium's Atmel library, and I noticed that many (most?) of the pads had rounded rectangles. However, if you use Altium's own "IPC compliant footprint generator", by default the footprints are rectangular (not rounded).

Is there a specific reason to use one of these over the other? It would seem that rounded pads would be easier to manufacture, and would make a more natural shape during reflow, but that's just complete speculation on my part.

(On a related note, would rounded pads have to be made slightly larger than strictly rectangular pads?)

\$\endgroup\$
  • \$\begingroup\$ Rounded pads also help with tolerances when routing 45º traces near components. \$\endgroup\$ – Wesley Lee Feb 5 '17 at 6:47
  • \$\begingroup\$ I think this has been asked before. Rounded PCB traces are better because the sharp turns act as antennas. \$\endgroup\$ – Bradman175 Feb 5 '17 at 11:20
  • 1
    \$\begingroup\$ I'm not asking about traces, rather the edges of SMD pads themselves. (I think the answer to the question about sharp bends in traces was that it only really mattered in high-frequency designs, anyway) \$\endgroup\$ – Ernest3.14 Feb 5 '17 at 11:25
16
\$\begingroup\$

Yes, SMD footprints should have rounded corners as per IPC-7351A

Corner radius is 25% of the shorter side of the pad but not more than 0.25mm (10mil which is not exactly the same but close enough here)

Why? The corners do not add anything useful (no additional adhesion, no additional stability or conductivity). But on reflow soldering the solder does not always flow into every corner possibly leaving copper exposed. Additionally: it's better to have stencils with rounded corners.

The only reason for pads with edges was that some tools did not support rounded edges.

Addition: no, pads with reasonably rounded corners do not have to be bigger because the corners didn't add anything useful to begin with.

| improve this answer | |
\$\endgroup\$
1
\$\begingroup\$

per IPC-7351B standard:

Also, the usage of oblong, or rounded, land pattern pads is considered advantageous for lead free soldering processes in comparison with rectangular pads, as the oblong shape provides for a pull of the solder on the pad. An exception to this rule occurs when the heel portion of the land pattern has to be trimmed due to the component body standoff being less than the paste mask stencil thickness or the heel having to be trimmed due to “Thermal Pad” interference. In these two cases, the rectangular pad shape is preferred to compensate for the reduction in copper area of the land pattern pad length.

| improve this answer | |
\$\endgroup\$
0
\$\begingroup\$

You can use rectangle pads and have rounded corners on your paste stencil, there can be issues with Gerber sizes due to pads being drawn not flashed. Most use std. rectangular pads.

Bradman175, you are incorrect 90 degree corners have no real effect untill the signals reach the GHz...

| 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.