Tolerance of board-to-board headers

Question

I am designing two boards. The bottom one is the power board that contains power switches on IMS (metal-clad board), while the top board is the logic board (4-layer FR4). Board to board height is about 0.5".

The connection of signals from top to bottom is through a 2.0 mm dual row pin header.

• the number of headers is about 20 pcs of 2x2 arranged in a 16 mm x 20 mm grid.
• On the bottom board the only option is an SMD male pin header.
• On the logic board I have multiple options: TH on the bottom layer, or SMD on bottom layer or SMD on the top layer with holes (the female header is made for variable board heights).

Since there is a high number of connections I am worried about soldering tolerance which might cause the two boards to mate incorrectly.

Question 1: which of the three options for female headers would be more suitable (I am thinking SMD is better since it has less play during soldering).

Question 2: If no solution would give the required tolerance for all the headers to mate, should I consider reducing the number of headers (knowing that the layout and performance will be worse)?

Any reference or guidance to where such information can be learned is highly appreciated.

Answer 1

Even if you overcome your alignment issues (and they are issues), you are going to rip your SMD headers off the board the first time you try to unmate so many pins at the same time with them being separated by such vast distances across the board. Without a separation jig that can separate the boards directly in line with each other, the first time you try to unmate them it's going to tilt, jam, and then tear off some SMD headers.

My experience was with boards that had a single 2x20 0.100", standard force, through-hole header. The force on all those pins adds up and the jamming gets worse the farther apart the pins are. If they were SMD square post headers, they would have torn off, and you have more pins and they are spaced farther apart. Going back, I would have used different connectors and I suggest you do the same.

Answer 2

Insulated Metal Base (IMS) PCBs are quite sensitive to shear strain on the connections, since the insulator tends to be brittle compared to FR4. Even if the static strain may be acceptable, it is a preload, so if you add vibration on top, you may well fatigue and crack the insulator around the connector's footprint pads.

It is best to use a couple of alignment pins to line up the top and bottom boards, and then use shear-less connectors, i.e. connectors that are free to move in the plane of the PCB.

Pogo pins would do this job well. I don't recommend zebra strips if longevity is desired - they are OK in limited lifespan consumer gear, but a bad idea otherwise.

Answer 3

the number of headers is about 20 pcs of 2x2 arranged in a 16 mm x 20 mm grid.

Make sure the SMD headers have some kind of spring in them, many of them can have misalignment. I had an issue with 2x40pin hirose connectors that were 0.5mm pitch. Even just a few mils of misalignment can cause dissconnects if there is no self alignment or 'give' in the form of spring contacts.

I think throughole pin headers would not have this problem with paralleling them because they are somewhat stiff and can tolerate ~10-30 mils of misalignment

Answer 4

You didn't mention the obvious solution: a single connector for all the circuits. For example, a genderless array connector*.

Or, for flexibility, consider one or more FFC (Flat Flex Cable) jumpers and FFC sockets* on each PCB.

Assuming that there is a reason why you must have 20 separate connectors, then consider board-to-board mezzanine connectors with a high degree of compliance to accommodate misalignment. For example, blind-mate board-to-board connectors* or genderless self-mate mezzanine connectors*.

Or, consider compression components: pogo pin headers* or spring leaf headers* on one board and matching targets* on the other board.

(*) My site

Answer 5

Everything depends on how the connectors are modelized in the library of your PCB design software. The "origin", should be in the middle of a pin. The "origin" define the placement in the PCB software project. Don't mix "origin" with "centroid" which is the reference point for the pick and place machine. They are two different things but sometimes they are superposed. (In your software, these names may differ or be inverted.)

Then place the various components separated by distances which are multiples of the pin pitch. If the pin pitch is 2mm, all the connectors should be separated by a multiple of 2, in the X and in the Y directions. If the pitch is 2.54mm, then they should separated by multiple of 2.54. And so on.

If all connector have their origin at the same place as one of their pin, and use pitch multiple for their placement, their should be no matching issue, no matter the type of connector.

If all the connectors on one board are identical, the origin doesn't have to be at the same place as of a pin, but it's more convenient. It's necessary when connectors are different to make sure they match a placement grid.

SMD connectors are less precise than THT, because they can drift or slightly rotate or be displaced during wave soldering. Respect routing rules for SMD components to avoid that.