3
\$\begingroup\$

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.

\$\endgroup\$
9
  • \$\begingroup\$ Just to be sure, are you saying there is a total of 80 connections? Have you considered using mezzanine connectors with a cable between? \$\endgroup\$ Feb 10 at 16:43
  • \$\begingroup\$ "with a cable beween". 80 cables sounds complex and expensive. If you mean a single cable, then there's no longer an issue of alignment. \$\endgroup\$ Feb 10 at 17:14
  • \$\begingroup\$ Why is the only option on one of the PCBs SMD headers? \$\endgroup\$
    – Andy aka
    Feb 10 at 17:15
  • \$\begingroup\$ @Andyaka , I meant the only option is smd , since IMS cannot have TH components . \$\endgroup\$
    – Eng Sam
    Feb 10 at 17:33
  • 1
    \$\begingroup\$ @AndrewMorton , I am trying currently to make them 3 connectors and use ribbon cables as this sounds the easiest solution \$\endgroup\$
    – Eng Sam
    Feb 12 at 10:17

5 Answers 5

3
\$\begingroup\$

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.

\$\endgroup\$
4
  • \$\begingroup\$ thanks for the heads up , i didnot think of that , you are right . I could use epoxy potting for the base of the smd connector , but CTE mismatch could be an issue since the conenctor can no longer move. :( \$\endgroup\$
    – Eng Sam
    Feb 12 at 10:11
  • \$\begingroup\$ what kind of connector do you suggest " I would have used different connectors and I suggest you do the same" ??? \$\endgroup\$
    – Eng Sam
    Feb 12 at 10:11
  • \$\begingroup\$ @EngSam I like hermaphroditic but it mainly comes down to something with less engagement length and force. Yours is a little weird since you need low pin counts so you'd kind of have to look around since most B2B connectors have many more pins. You might get away with very short (<4mm) square post headers \$\endgroup\$
    – DKNguyen
    Feb 12 at 15:26
  • 1
    \$\begingroup\$ @EngSam And if you can you might be able to find SMD headers with positioning pegs. They tend to be shallow enough to not go through the board \$\endgroup\$
    – DKNguyen
    Feb 13 at 15:54
3
\$\begingroup\$

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.

\$\endgroup\$
1
  • \$\begingroup\$ can you give examples of connectors that are free to move in the plane of pcb ? . Bergquist company in an app note talk about headers that have " S " shape that act as spring to absorb movement but they donot look to be readily available anywhere !! \$\endgroup\$
    – Eng Sam
    Feb 12 at 7:58
3
\$\begingroup\$

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

\$\endgroup\$
2
  • \$\begingroup\$ this is what i am looking for in an answer . can you please tell how to know if " SMD headers have some kind of spring in them" ? are these custom made or normally available headers , \$\endgroup\$
    – Eng Sam
    Feb 12 at 10:09
  • \$\begingroup\$ The ones with springs in them are wide and will usually have some indication in the product page that they can tolerate misalignment. This one is not: digikey.com/en/products/detail/hirose-electric-co-ltd/… The best way to know is to ask a few manufacturers if they have anything like that or if you can parallel connectors. \$\endgroup\$
    – Voltage Spike
    Feb 12 at 16:27
3
\$\begingroup\$

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

\$\endgroup\$
4
  • 1
    \$\begingroup\$ I thought i explained the reason for having 20 separate connectors , the reason is that these are gate source signals for transistors , I could decrease the number to like 6 connectors (more pins off course) at minimum but the routing will cause coupling and bad effects on these weak signals . your forth suggestion of blind mate and genderless self mate is quite nice i will search more on these , thanks \$\endgroup\$
    – Eng Sam
    Feb 10 at 17:40
  • 1
    \$\begingroup\$ However the question still stands , does using standard board to board work ? is the problem i am stating real ? or the tolerance is not an issue ? \$\endgroup\$
    – Eng Sam
    Feb 10 at 17:45
  • \$\begingroup\$ "is the problem i am stating real ?" Yes. "the tolerance is not an issue ?" It is. \$\endgroup\$ Feb 10 at 21:09
  • 1
    \$\begingroup\$ @EngSam - why do you think they are "weak signals" aren't they coming from logic outputs? What speed are the signals? \$\endgroup\$ Feb 11 at 1:55
1
\$\begingroup\$

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.

\$\endgroup\$
2
  • \$\begingroup\$ i think you didnot understood the problem. "their should be no matching issue, no matter the type of connector." I have a problem with this sentence. for example a standard 2.54mm header with square pins has hole diameter of 0.9mm ( in most pcb libraries) when you place the connector in real life you can jiggle the connector , this is intentional to allow the component to be inserted (unlike fit and press type of connectors). Now this play / tolerance will make each board slightly different from other board . and this is the issue i am talking about , not placing in pcb software. regards \$\endgroup\$
    – Eng Sam
    Feb 12 at 10:15
  • \$\begingroup\$ Yes, holes diameters are always a little bit larger to be able to insert the THT component easily. If it's too tight it may become too difficult. I believe hole diameter given in the datasheets (and hopefully in the libraries) take tolerance in account. The "standard" 2.54 header can tolerate quite a good margin. If you have a lot of headers, bigger problem than tolerance is to insert all the pin into all the sockets at once. Standard 2.54 headers are not sturdy enough and some pins can miss their mating as they are pushed aside. Connector with a box to guide the pins will help. \$\endgroup\$
    – Fredled
    Feb 12 at 15:36

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.