smallest header pin pads

[Simon]

I am looking to do a design where some PCB's plug into a main PCB. Being right angle connectors it makes sense to have TH both sides. So if i use a 1mm pitch connector (2 rows) with a 0.3mm post that leave precious little for traces to go between the pins. The hole needs to be 0.5mm (the post is 0.425mm diagonal). I need 0.1mm spacing and a 0.25mm trace seems to be the smallest sensible but maybe 0.15mm. so 0.5-2x0.1-0.15 = 0.15mm that has to be shared between two pads so 0.075mm copper around the hole. Is that practical?

[langwadt]

I am looking to do a design where some PCB's plug into a main PCB. Being right angle connectors it makes sense to have TH both sides. So if i use a 1mm pitch connector (2 rows) with a 0.3mm post that leave precious little for traces to go between the pins. The hole needs to be 0.5mm (the post is 0.425mm diagonal). I need 0.1mm spacing and a 0.25mm trace seems to be the smallest sensible but maybe 0.15mm. so 0.5-2x0.1-0.15 = 0.15mm that has to be shared between two pads so 0.075mm copper around the hole. Is that practical?

jlcpcb says >3mil annular ring so just barely, you could make the pads oblong to get a bit more pad

[Simon]

Yea, I think I will go back to 1.27mm idea, there is more support, I can get ribbon cable too which I am not sure exists in 0.5mm pitch and 1mm pin pitch seems to have very few products.

[Simon]

even 1.27mm is near impossible!!!! pin is 0.4 so 0.57mm diagonal. What is the smallest sensible hole? 0.7mm.

so 1.27-0.7 = 0.57

assume spacing of 0.1mm leaves 0.37mm, out of that I need to have my trace width and the annular.

For 0.25mm that leaves 0.12 which is 0.06mm or 2.4mil

So I still have to use 0.15mm traces to get it to 0.11 or 4.3mils.

I suppose i can neck traces

[Gribo]

How many positions do you need? Can you separate the mechanical part (mating boards at 90 degrees) from the electrical part and use an FFC?

[Simon]

what is an FFC?

[apurvdate]

https://en.wikipedia.org/wiki/Flexible_flat_cable

typically used for LCD panel to PCB connections

[T3sl4co1l]

Yeah, don't try and get traces between THT pins in fine pitch.  Internal layers maybe.  Use SMT.

Tim

[Simon]

This has been something going round and round in my head for a while. I have concluded that I may as well use a ribbon cable for my backbone connection. SMT does not solve it. As soon as you have two rows you have to squeeze traces between pads. The recommended footprint for the same TH part in SMD has even less space for traces to pass through. I suppose I could thin the pads out but I don't like going against manufacturers recommendations.

I think last time I came to a conclusion it was 2.54mm pitch on 3 rows, that gets me slightly less density at 0.847mm pitch rather than 0.635mm but I can get 3 0.25mm traces through with 0.1mm spacing. It also makes the mechanical connection really robust whereas with 1.27mm i need to support my PCB's by other means but i was always concerned about the extra cost/material of 2.54mm pitch stuff just to carry signals.

The only way I can find of getting 0.25mm traces between 2 row 1.27mm pitch is to use samtecs "mixed technology" headers that have one row TH and one row SMD. This means that I can forgo any pad on the SMD layer leaving maximum space for a trace to pass through and its just straight lines almost through the pads top and bottom. But this is really weak mechanically.

I could of course look at 4 row 2.54mm pitch, that get my density back to 0.635mm

[Simon]

Right. So the search is on. I need right angled 4 row 2mm or 2.54mm pitch headers. Anyone?

[coppercone2]

you might wanna consider a PCB that is a mixture of flat flex and ridged substrate for this application to minimize interconnects and solder junctions, then just bend it around a mechanical frame

[Simon]

Well i want one or the other, it has to be commercially viable and easily assembled. It's jut that at the moment i could make one massive board to suit 3 different applications that are similar or modular it which makes sense as a large single PCB will have packaging issues. Several stacked modules will be much more compact and easy to make different systems from the same module set. It will have to be 1.27mm double row with ribbon cable or 3 or 4 row 2mm or 2.54mm pitch.

Of course for MCU signals 0.15mm will be enough but how far can I reasonably run that at up to what frequency? With a PCB interconnect I can have ground planes. with ribbon cable there will be more copper there.

[Larry80]

With ribbon cables or FFC beware, that the voltage drop of quite small currents will throw the ground planes off. So any interconnection is best to be separated grounding or you can find spurious difficulties.

Ie. if you have sensor on the other board, you should make a connection island from it. Analog components could be bundled (2 sensors or whatever shared) island, but signals need to have their own paths for EMC reasons and be next to each other on the cable.

Though hole connection (pinheader to board) is much better in this regard (although high frequency signals will become more problematic).

[Simon]

Well i can dot ground pins anywhere that will link to ground planes in the module PCB's and the backbone PCB so tight return paths are easy and universally available where as i could need to put a ground wire with every wire in a cable nearly doubling my pin count unless I designate specific pins for the high speed stuff.

[Larry80]

If both boards have dedicated ground layer (4 layer board or more), i guess just multiplying the interconnections is enough.

[langwadt]

This has been something going round and round in my head for a while. I have concluded that I may as well use a ribbon cable for my backbone connection. SMT does not solve it. As soon as you have two rows you have to squeeze traces between pads. The recommended footprint for the same TH part in SMD has even less space for traces to pass through. I suppose I could thin the pads out but I don't like going against manufacturers recommendations.

with SMD just use a via to get to another layer

[Simon]

with SMD just use a via to get to another layer

Yes but with TH pins you have to get through the deader and the pads if you have one header after another.

[Simon]

I'm wondering about PCIe, the advantage is that the connectors are readily available from multiple sources, standard and the mating half is the PCB itself. The pin pitch is 2mm or 1mm staggered. The effective pitch is 0.5mm as i wanted and I think given the staggering of the pins it makes it easier.

The hole is 0.7mm with 6 mils each side that is 1mm leaving 1mm between pins.

BUT! how rugged is PCIe? I need this is mobile applications, not military vibration profiles but still moving vehicles. the DIMM sockets starts to come to mind as well.

[Simon]

Except DIMM's are a single size, the varying lengths of PCIe are ideal.

[coppercone2]

I mean the PCI slot is meant to have a connection to chassis along the exit strip on most cards. In this case its durable I tipped my computer tower over a few times and the only thing that ever suffered is the shitty ram slot and hard drive.

I imagine if there is a top reinforcement with 2 (or more) points of contact the socket is very good. You can make crosses on top of the PCB that bond to all four sides of the chassis above the slot that overlay (imagine a redical moving around leaving its previous location behind), not sure how much strength it would give though. and the cards would not be swappable along the bus anymore, it would be location specific (grid) , unless you can reposition the cross support with rivets/bolts

a rugged spectrum analyzer is built this way, but they rely on back planes then cross elements. you can make top strips that bond the cards together while totally assembled

make extension cards so you can work on it like a sane person

[Simon]

Well PCIe does not have any mechanical support of it's own baring the 16 lane having a clip on one end. the main of the mechanical strength is in the fixing to the case. but this means lots of brackets with complicated folds. I suppose i can use right angle brackets that rivet to the module PCB's and screw to the backbone PCB's

[T3sl4co1l]

This has been something going round and round in my head for a while. I have concluded that I may as well use a ribbon cable for my backbone connection. SMT does not solve it.

Why, how?  You have a free layer to route on.

You shouldn't be routing anything to the back row anyway, that probably all needs to be grounds.  Is this digital signals?

Well PCIe does not have any mechanical support of it's own baring the 16 lane having a clip on one end. the main of the mechanical strength is in the fixing to the case. but this means lots of brackets with complicated folds. I suppose i can use right angle brackets that rivet to the module PCB's and screw to the backbone PCB's

How about single lane and mobile (laptop) PCIe connectors, they're right angle edge connectors and the board mounts with standoffs and screws?

PCIe is capable of transmitting over a short distance but it is not recommended.  The CM range is tiny.  Shielded cables are required (SATA like?).

Can we interest you in a 1G Ethernet router instead...

Tim

[coppercone2]

Well PCIe does not have any mechanical support of it's own baring the 16 lane having a clip on one end. the main of the mechanical strength is in the fixing to the case. but this means lots of brackets with complicated folds. I suppose i can use right angle brackets that rivet to the module PCB's and screw to the backbone PCB's

if you make things thick there is no need to fold

[Simon]

This has been something going round and round in my head for a while. I have concluded that I may as well use a ribbon cable for my backbone connection. SMT does not solve it.

Why, how?  You have a free layer to route on.

You shouldn't be routing anything to the back row anyway, that probably all needs to be grounds.  Is this digital signals?

Well PCIe does not have any mechanical support of it's own baring the 16 lane having a clip on one end. the main of the mechanical strength is in the fixing to the case. but this means lots of brackets with complicated folds. I suppose i can use right angle brackets that rivet to the module PCB's and screw to the backbone PCB's

How about single lane and mobile (laptop) PCIe connectors, they're right angle edge connectors and the board mounts with standoffs and screws?

PCIe is capable of transmitting over a short distance but it is not recommended.  The CM range is tiny.  Shielded cables are required (SATA like?).

Can we interest you in a 1G Ethernet router instead...

Tim

I'm not looking at terribly high frequencies. The highest is likely to be a 16MHz clock and i would prioritise module placement based on signal speeds. Most signals would be up to something like 1MHz SPI or kHz of PWM.

Yes with SMD I can take all signals down to the lower layer but i am trying to find something mechanically rugged. So far the cheapest option is literally 4 row 2.54mm pitch right angle headers if i could find any but can settle on 3 rows. I would have a few ground pins say one ever 8 to 32 but not matched pairs.

[Simon]

These look really nice: http://suddendocs.samtec.com/catalog_english/hsec8-pv.pdf