I’m dabbling in synth modules, largely influenced by Eurorack design principles but not keeping to their form factor. Where I am right now is PCB-mount pots and jacks on boards fit into 3-D printed cases with 2mm-pitch 4-conductor power connectors (sliding all over my testbench).
In order to make the synth workbench more space-efficient (and to save on crimping my own power cables) I am considering a simple backplane model where the modules would have card-edge connections and get mounted vertically, with side-adjust/right-angle “UI” parts. A slotted enclosure would provide physical stability.
For most modules, the only connections are for power (+/- 12V, +5, GND, the signals are routed over user-facing patch cables) but others might make use of esge-connected bus lines (for example a vocoder has multiple channels sharing carrier and modulation lines). Capacity for 20 connections would probably be overkill but better to leave room for future ideas, so 2/2.54mm pitch would be fine. Since it’s analog synth, high-speed and RF issues don’t enter into consideration for the large part.
Let’s assume I’m good enough to lay out the Edge.Cuts so my fab house can implement what I intend.
Two questions: How do I pick the connector? A first pass at DigiKey show up a couple of reasonable-looking choices like this: https://s3.amazonaws.com/catalogspreads-pdf/PAGE50-51%20.100%20LP%20DS%20EYE%20RA.pdf. Do I pick a few that look close and evaluate some prototypes? (I can budget for throwing some away.) Is this enough of a solved problem that I can get most of the way to done by following some simple design principles?
Secondly, are there any pitfalls I should look out for when designing the connectors? Do I want a special finish?
If you are ok with slightly narrower pitch PCIE x1 card edge connector sounds like a perfect fit for you. It’s cheap and manufactured in massive quantities.
I’d suggest using DIN41612 or DIN41617 backplane connectors instead. Cheap and plentiful.
Edge connectors need gold plating and special edge milling. Drives up PCB cost.
I did make PCB <-> USB (A) adapters in the past which simply used ENIG (not hard gold as normally is being employed for edge connectors, higher price) and no special edge milling.
My expectation for those was 20-30 mating cycles and it did work well.
No idea how this would fare for a consumer product though - for ‘prototyping’ it definitely works.
You naturally need to make sure the PCB thickness matches the connector of your choosing.
I was Engineering Director for one of the largest connector companies, Proj/Design Engr for another and have patents on connectors. We did plating of Tin, Gold, Ber/Cu, other…
Naturally, a bazillion tests were conducted to gain knowledge…
No, you Don’t need Gold plating - you can earn a Phd on this subject.
Aside from Materials, What’s important are:
Normal force on contacts
Number of mating cycles
Plating thickness
PCB Entry lead-in (chamfer)
The book below was useful for some of the engr’s that worked for me - you may find useful if you can find a copy (perhaps available if Brush Wellman is still around…)
I’ve seen plain old home etched PCBs used without any plating (bare copper) and with tin plated (actually solder coated by hand) edge connectors. That was for 2.54 mm pitch connectors (something similar as in OP’s link). Although these coarse connectors didn’t even need a chamfer (you could stick a piece of blank material in there without any problems), they were made by hand with a file. And it worked fine in a low mating cycle application.
I wouldn’t be confident enough that you could get away with something similar for PCIe connectors though.
Connector mfg’s always use plated contacts. Plating ranges from Tin to Gold and, naturally several other conductive materials (including bare Cu, but for very specific applications).
I’ve worked with nearly All connectors brands and handfuls of companies that buy/use them - all connectors go through a significant regime of testing to qualify for ISO/Mil/etc…
Thus, you can be sure that whatever brand you use, as long as it’s suitable for the Application/Usage/Environment…etc, they will work.
For a PCB that mates with, say, an Edge-Card connector, aside from the Geometrical aspects of insertion (meaning, PCB thickness, chamfer, pad width, length and thickness), you need only consider the size/attachment/hook-up… And, the Pad geometry & plating.
Regarding the Pad plating on a PCB:
I make my own PCB (on CNC Mill) and dip them in Homemade Tin solution. You can buy the Tinning solution or make it (Here’s the link I posted at Fritzing a few years ago)
So, look for a connector (assuming Edge-Card) that meets your needs and look at it’s requirements for the mating PCB.
I like this. It is way more connections than I think I need but I can double up on them or just use every other one until I’m more confident about the physical alignment. Lots of supplier choices. Cardedge footprint already in KiCad. JLC will do “gold fingers” For a Few Dollars More and the push of a button.
Just ordered a copy of the handbook mentioned below so I can do a bit of bedtime reading before setting out on the design.
Snagged from a bookseller hawking a single used copy.
When I started down this road a couple years ago I thought I’d end up working on transistor theory and active filter design but the big surprise was how much I was thinking about interconnects. This was undoubtedly because I wanted to explore things from first principles so didn’t adopt any existing conventions (except for the EuroRack power standard because I already had a couple of modules that needed it, but eventually I got fed up with using a ribbon cable for power and rolled my own).
So, having backed into this topic it will be interesting to absorb some actual design principles.
No doubt you’ll glean good info from the Guide. I mentioned it only in response to the subject of Gold (hence, contact materials) - the Contacts are the ‘Meat’ of a connector.
It’s a guide focusing on “contact’s” and does not include Connector housings, PCB,… etc.
A housing design is centered around containing the contacts, Male/Female interfaces…etc.
Thus, my apology if it doesn’t fully satisfy your needs (and hope you didn’t pay more than a couple of bucks) but, again, it appears to me you’re simply going determine the Contact Pad needs as it relates to an Off-The-Shelf connector. Which, to me suggests looking at the PCB requirements of the Connectors you’re interested in.
EDIT: You may be interested in this totally non-essential aspect - making a connector/cable footprint… The Connector details are up to user to take care of but, once having the dimensions in hand (or a downloaded Step file of it from a source such as Digikey or Mouser), the task is nearly finished…
I posted These Vid’s awhile back… You can slow the video play using youtube’s player controls…
Also (forgive me) For nostalgia, I was motivated to dig into the dust-bin and pull out some connectors I designed for the Medical field (catheters, ophthalmology, endoscope, bone cutter/shaver, includes two edge-card conc’s…)
Although I like the Idea of using pci-e connectors (because of their price and ubiquity), for your application I’d tend to go for a connector with a 2.54mm pitch.
-That way you would have the option to use PCB-mount connectors as well as IDC-ribbon cable card edge connectors. (You could even use a pinout so maintain eurorack-compatibility with the use of a custom idc cable)
I have built some synthesizer modules too and personally i don’t care for a the cv/gate signals on the power connector and i think there’s a good reason that there are almost no modules out there using them. Also I think if you don’t have ICs running on 5V on every module It makes more sense to have a small regulator on every board than having a 3rd power rail.
That said, I don’t know your plans and I’m sure there are innovative things that could be done with a powerfull backplane connector for specific applications (modular semi-modular synth, SPI on the backplane?, 3.3v line?, direct output to audio mixing bus…)
I hear ya, but I’m sitting here looking at the nice BUS_PCIexpress_x1 footprint already in the library and it looks pretty workable to me, especially if I start out prototyping by leaving every other line unconnected so I can work out the basic problems first without worrying too much about the 1mm pitch.
And yes, you’re echoing the same ideas I have about how to use more of the lines. My approach is to crank out a lot of “atomic” or “elemental” modules rather than try to cram a lot of features into a few complex designs, so the prospect of using the backplane to tie them together (patch cables are pretty but I’m just getting started and already a bit swamped) is an intriguing challenge.
Although the concept of card-edge connectors is simple and straight forward, it is not so well suited for small production volumes and experimentation.
Instead I personally prefer to use bog standard dual row 0.1" pitch IDC connectors, and solder them to the edge of the PCB.
For the PCB’s it’s easier because you do not need gold plating and chamfering, and you can put the money you save from that into the connectors. 0.1" IDC headers are also excellent for ad-hoc modifications and tinkering. You can even connect them with “dupont wires” if such need arises, or replace the whole “backplane” with just a flat cable and some pressed -on connectors.
Connectors soldered to the side of a PCB are less fit for mass production though. An alternative for that is to use the standard angled connectors, but those need more room on the PCB.
Is there even a way to specify a chamfer in pcbnew? Do I have to go to a premium fab house to get it done?
I’m willing to pay for extra features at jlcpcb (and I’m not sure they even do chamfering–just asked) but the cost of moving to a “full service” shop could be a deal-killer.
I just did a bit of clicking.
“Gold fingers” requires ENIG
ENIG is USD17 extra (for the default settings).
If you click “Gold Fingers” then an option for 45 degree chamfering appears: https://cart.jlcpcb.com/quote?orderType=1&stencilLayer=2
Toggling the chamfer does not result in a price change.
As far as I know there is no built-in option for chamfering in Gerber files and it has to be communicated in some other way. Sometimes manufacturers have a guide on their website how they want it communicated (Often in a Gerber layer with notes, or just the lines where the chamfering should be.
For most Edge connectors it is a quite easy guess though.
But do you want to depend on them guessing right?
For me, exploring possibilities is as much of an objective as getting the device built. I have a design that’s an initial prototype and I’m likely going to outfit it with an edge connector plus my current power header so I’ll still have something to work on even if the edge connector isn’t a feature.
Without all the critiques here I wouldn’t have a shot, so thanks again all.
