44
\$\begingroup\$

Some PCBs, like the PCI card specification have gold fingers which start very narrow near the bottom edge, and gain their usual width much higher, where the actual contact is expected to be made.

What is the advantage of having the narrow part?

PCB with gold fingers narrow at bottom, widening progressively.

Why not make the pad fully wide all the way to bottom, like ISA cards, DDR, etc.? Or simply make the finger shorter, only in the area of contact? What is better in gradually increasing the width?

My speculation:

  • To connect ground pins first - All the pins have this shape.
  • Resistance against peeling the pad off - The smaller trace seems much more susceptible to damage
  • Insertion force - I expect the narrow part to be made of equally thick gold, which would require the same amount of force.
  • Insertion force - Can it be that some number of the connector contacts (in motherboard) get pushed sideways in each stage as the card goes in, lessening the amount of force needed to insert the board?

Can't seem to find any evidence or description why this is designed this way. Some high frequency high pin count stuff (DDR modules) use rectangular pads.

Note: See page 196 of the linked PCI card specification document.

\$\endgroup\$
  • 3
    \$\begingroup\$ my guess is less of a blunt edge on the insertion vector to prevent the copper from eventually peeling up from the FR-4 \$\endgroup\$ – justing Aug 14 at 17:20
  • 2
    \$\begingroup\$ Another guess, copper that extends out to the board edge sometimes has a risk of damage during the profile cutout, and increasing the gaps between adjacent copper regions at the edge may reduce risk of short from any damage incurred during fabrication. \$\endgroup\$ – a sandwhich Aug 14 at 17:49
60
\$\begingroup\$

To electroplate the fingers with gold they must all be joined together electrically. This is done with a "plating bar" trace outside the final board area, which is cut off afterwards.

enter image description here

Usually the board edge will be chamfered for easier insertion in the socket. Since chamfering removes the lower part of the fingers they only have to be wide enough to carry the electroplating current. Making them narrower saves gold, which makes the board cheaper. If the board is not intended to be plugged in often then chamfering may not be applied, and then the narrow parts remain.

Gold plating for edge connectors

\$\endgroup\$
  • \$\begingroup\$ One point that could help make the answer clearer is whether or not the 'stepped' pattern as shown in the OP photo is part of card functionality, or left over artifact of plating. [I'm kind of surprised they wouldn't shave more of the leads off for gold recovery if they're not actively part of the end-use connection. That small bit of gold has to add up over a few hundred thousand boards...] \$\endgroup\$ – TheLuckless Aug 16 at 17:27
  • \$\begingroup\$ But there must be something different then about the board edge connector pads compared to all the other gold pads on the PCB. Maybe a thick nickel plating under the gold to make them more durable? Or if the board edge pads are not different from all the other gold pads, then how do the other pads get gold plated? Surely there is not a plating bar trace connecting every pad on the board. \$\endgroup\$ – mkeith Aug 17 at 1:58
  • 1
    \$\begingroup\$ 'Gold' pads are usually ENIG (Electroless Nickel Immersion Gold) which doesn't require bonding electrically. Where electroplated 'hard' gold pads are are required in the middle of the board (eg. on keypads) any plating bar traces required can be severed by punching or drilling holes through them. \$\endgroup\$ – Bruce Abbott Aug 17 at 2:42
  • \$\begingroup\$ Thanks! Yes, most boards I have designed were specified as ENIG. Thanks for clarifying. \$\endgroup\$ – mkeith Aug 17 at 2:47
6
\$\begingroup\$

Some PCB manufacturers mention some specific design requirements for gold finger edge connectors:

  1. No plated through holes are allowed in the plated area
  2. No solder mask or silkscreening can be present in the plated area
  3. For panelization, always place gold fingers facing outward from the panel center
  4. Connect all gold fingers with a 0.008” conductor trace at the edge to allow for manufacturing
  5. Features can be placed on one or both sides to a depth of 25mm from the outside edge

I am not sure about 4, but maybe they are referring to narrowing down the pads like on the picture you embedded?

\$\endgroup\$
2
\$\begingroup\$

Bruce is probably right that cost is the major reason for that end of the contact to be narrow, but I believe this also makes cross-contact between neighboring pins less likely if the the board is not completely straight during insertion. I remember this was a major problem with inserting boards into the Apple II.

\$\endgroup\$
-2
\$\begingroup\$

My guess is that it has to do with the characteristic impedance of the connections. Which depends on (among other things) the width of the traces. Looking at the gold fingers on the picture it looks like they increase in size in two steps, this is a very common technique when "matching" for instance a 75ohm trace to a 50ohm trace. It doesn't give a very good match, but it does better than if you didn't pay attention to it at all.

\$\endgroup\$
  • 7
    \$\begingroup\$ but the contacting happens from atop of the wide area, so this is probably not the reason. \$\endgroup\$ – Marcus Müller Aug 14 at 17:14

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.