2
\$\begingroup\$

What is the actual purpose of using the oval/oblong pads that are commonly used for ICs? Everywhere I read the answer is the possibility to allow a track between the pins, but as long as the pad diameters of a round and oval pad are the same I don't see the difference. I would prefer to avoid those when space is limited, does the elongation of the pad give any real benefit?

Thank you in advance!

\$\endgroup\$
  • \$\begingroup\$ Through-hole or SMD pads? \$\endgroup\$ – pjc50 Jun 1 '15 at 10:25
  • 1
    \$\begingroup\$ @pjc50: looking at the question title should answer that question. \$\endgroup\$ – PlasmaHH Jun 1 '15 at 10:35
6
\$\begingroup\$

The pad area is important, more so on single-sided boards, since on such boards the adhesion of the tiny annular area is all that is holding the component lead in place. On boards with plated-through holes, the pad area affects the solder fillet-a somewhat larger than minimum pad area makes the joint stronger and easier to inspect.

\$\endgroup\$
  • \$\begingroup\$ Alright, that makes sense. However in the case of plated through holes, if other components use round holes, I assume there is no purpose in making the holes oval for the ICs exclusively? \$\endgroup\$ – I have no idea what I'm doing Jun 1 '15 at 11:54
  • 1
    \$\begingroup\$ No I don't think there is any need to single out DIP leads exclusively, but usually they're the closest-spaced through-hole parts on a PTH board, so using oblong pads may in fact be consistent. Back ca, 1990 +/- I sometimes used oblong pads for close-spaced through-hole passives. \$\endgroup\$ – Spehro Pefhany Jun 1 '15 at 12:14
  • 1
    \$\begingroup\$ @IhavenoideawhatI'mdoing my answer mentions a possible reason, but if you're using a standard pitch DIP (0.1") it probably won't make much of a difference \$\endgroup\$ – DerStrom8 Jun 1 '15 at 12:33
5
\$\begingroup\$

Spehro Pefhany is absolutely right, oval pads allow for better adhesion. I would like to add to that answer and mention that oval pads also allow for easier hand-soldering in tight areas. I recently designed a board with a connector (50-mil pitch) and had to narrow the pads down significantly from what was in the library. This was to allow the traces to pass between them. In order to balance it out, however (to help ensure that the pads/component leads wouldn't rip up), I lengthened the pads and offset the hole. This also allows the assembler to have easier access to the pads for soldering, even though it has such a fine pitch (and narrow pads):

Oval Pads

\$\endgroup\$
  • \$\begingroup\$ Personaly I would probably have made the tracks thinner rather than going for such a crazy thin annular ring. \$\endgroup\$ – Peter Green Jun 11 '17 at 9:41
  • 1
    \$\begingroup\$ @PeterGreen You are right about the annular ring, I eventually adjusted it to meet the minimum requirements from my manufacturer. However, making the traces narrower was not an option because they were already at the minimum width allowed by my manufacturer. \$\endgroup\$ – DerStrom8 Jun 11 '17 at 11:44
  • \$\begingroup\$ Not to mention that the point of oblong pads in this case was not even for routing reasons (read my answer). \$\endgroup\$ – DerStrom8 Jun 11 '17 at 11:45

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.