Considering PCI-32 edge connectors for a project.

[paulca]

I want to modularise a computer build.  So I need a large amount of interconnects.  It seemed to be a problem already solved many times over if I just  pick one of them.

I mean the 5V 32bit PCI slot.  104 contacts.  Not PCIe etc.

The foot print in KiCAD for this appears to only be "one sided" labelled "B" but does not appear to have the mirror "A" side anywhere to be found.  Am I supposed to use two footprints and flip one onto the backside myself?

The slots themselves seem to come in "gull wing SMD with board anchor through holes" or "4 lane staggered THT" with the later being the more popular. However the former looks easier to solder and route.  The full THT though provides a lot of mechanical support.

Are there any major gotchas?  I have no need to match the PCI spec for what pins actually are.  It will be custom.  However I was considering just placing signals as "SIG-SIG-SIG-GND-SIG-SIG-SIG-GND-"  and for special signals, like a clock say, GND-SIG-GND.    The alternative is to make one side "mostly signal" and one side "mostly ground".  Which might make routing it easier if the lower layer is ground plane, stop layer signal.  Thinking... THT would be easier to route on a 4 layer board.  4 layers to escape the foot print crowd without needing vias like on the SMD version.

In terms of fabrication.  I assume it's up to me to define the edge cuts for the connector AND specifiy I want "bevelling" as well as state which surface finish I want.

[paulca]

A different question, related.

If I had a PCB with 4 of these slots and routed them straight through, daisy chain, literally just a trace....   It places the issues of "pull up or down" onto the cards themselves.  As these will all be my design and despoke I do not need to be concerned with "rouges" not obeying the spec.

A chat with an AI was pushing me towards a full thevian? bus with pullups and downs to mid float the "transission" line which is the backplane.

I can see this being great in TTL days when filling a rack with A3 sided Manhattan style logic cards, but is it really necessary for a back plane maybe at best 150mm long?  Running at a bus speed not exceeding about 2Mhz.  (8Mhz CPU, but the bus speed is a division of that).  MCU DMA bursts might change that, but I have no need for speed. 

I was going to consider making it such that all cards have bus transcievers.   Either "just drive" or both ways, depending.  Without a bus arbitrator or surogate bus master the cards control their own "Drive enables" and just behave in spec with the CPU as if the transceivers were not there.  Later though, those drive signals could be controlled by a bus master.

The point is card outbound will be:  "Buffer->33R->Interconnect" the 33R open to calculation for a better value.  Just to limit the edge rate and limit current entering the backplane traces which may be "open ended" stubs.

I think its that later point which brings the argument for a pulled/terminated transmission line backplane.  Otherwise with 2 cards out of 5 (say) installed there are 3 stub connectors and a dozen cm of traces just hanging around on the end of the bus.

[fchk]

I suggest DIN 41612. Used to be common for backplanes.

Backplane: Female straight
https://b2b.harting.com/files/download/PRD/PDF_TS/0903296X825_100173852DRW156H.pdf

Card: Male Right Angle
https://b2b.harting.com/files/download/PRD/PDF_TS/0903196X921_100072506DRW318D.pdf

There are also perfboards suitable for this connector.

And you can also connect ribbon cables if you only use rows A and C (the outer ones).
https://b2b.harting.com/files/download/PRD/PDF_TS/0903264X828_100177370DRW003E.pdf

And there are bus boards - you don't even need to design your own
https://www.elpro.org/de/rademacher-computerplatinen/30333-vk940.html

[Ice-Tea]

There are a number of caveats with cardedge connectors. If you want to do it right, you will be ticking off a lot of checkboxes when ordering your plugin cards: selective hardplate gold, beveling, routing,.. You can get away with a straigth edge and ENIG or even HASL for prototypes but if you want it reliable you'll be spending money on that..

Connectors like fchk suggested don't have that problem. And needless to say there are many, many options that are much more dense than those older connectors.

[paulca]

I suggest DIN 41612. Used to be common for backplanes.

Thank you.  This work out quite nicely.  Fits the 100mmx100mm PCBWay board size for minimum price too.

They are not cheap.  Circa $5 a piece with gold plating and non-gold versions are rare.  From AliExpress they are still $2 each... and that brings me to my puzzle.

I was wondering why there were about 3 different copies of the same connector on Digikey.  So I picked a straight female and a right angled male.  Dropped them into KiCAD and... At first I was baffled, then I noticed.  The pin out orientation is different.  I had already been puzzling over geometry of having 2 "flat" end cards with 3/4 vertical expansion cards.  CPU><EXP1><EXP2<>EXP3<>DEBUGCARD.  For that to work with a "straight through" pin map, the last card (DEBUG) either needs to be upside down or I need to mirror the foot prints.

Then I noticed that the rightangled female and male have different pin mappings.  The rows are mirrored.

The thing is... they are bit of bent metal, the don't care what you solder them to.  Personally I don't care if the square pin 1 is in the right place or not. 

KiCAD however... does care.

So... Do I spent another 30 minutes trying to check foot print pin orientation and down load the correct footprints and actually buy those specific connectors and not chance fate... or do I just open the footprint, select the pins and mirror them?

I suppose the more important quesetion is.... are the actual connectors mechanically keyed to force the matching pin oritentation.  That could get messy and mirror imaging a foot print leads to tears and a dead board.  Been there.  "Bottom view" or "Boards view" footprints should be banned and their authors shot.

This is what I mean.

[Roehrenonkel]

Hi paulca,

I suggest DIN 41612. Used to be common for backplanes.

I was wondering why there were about 3 different copies of the same connector on Digikey. 

There are inverted/mirrored versions of the connectors (for use on the back of backplanes).
Also different length of pins, wire-wrap and solderless press-fit.

Best

[Doctorandus_P]

There are inverted/mirrored versions of the connectors (for use on the back of backplanes).

No that is not the reason.

Footprints of Male and Female connectors always "appear" to be mirrored to each other. Suppose you have a male header on your PCB, with pin A1 in the right top corner. Then take a female connector and mate it. (I.e it also has pin A1 in the upper right corner). Then take off the female connector and put it on the PCB next to the male connector. A1 of the female connector is now in the lower right corner.
(Or in the upper left corner, depending in which direction you rotated the connector).

DIN41612 also comes in different quality classes, and the connectors rated for more insertions are (a bit) more expensive.

For small (expected) production runs, I don't like edge connectors. Having to order gold plating and the chamfering offsets most of the cost savings of using "normal" connectors.