• Please review our updated Terms and Rules here
  • Exhibitor application for VCF West 2022 is now open! If you are interested in exhibiting, please fill out the form here.
  • If you attended VCF East, please take a moment and fill out the survey here. This will help us improve the event for next year.

A general purpose Flip Chip adapter board - Worth doing?

intabits

Experienced Member
Joined
Jan 22, 2019
Messages
145
Location
Melbourne, Australia
There's a bunch of projects out there for "after market" and DIY boards for DEC machines, targeted at Unibus, Omnibus, Qbus, and possibly others. These projects include: extender cards, prototyping cards, Unibone, QBone, MOS memory boards, Boostrap card emulators, etc.

What they all have in common are the 36 pin edge connectors that plug into DEC equipment. And that introduces some complexity due to the need for accurate mechanical design, and the need for a non rectangular PCB. Which then increases the cost of getting them manufactured, plus the extra cost imposed by the need for gold plated fingers (of varying possible qualities and cost).

That's OK for a proven design that serves one's purposes out of the box, especially if it is something that will be always needed in a given configuration. But I'd like to experiment with my own variations of the projects mentioned above, plus others yet to be identified. I'd also like, initially at least, to make my own prototypes for these projects using DIY PCBs, and probably mostly single sided ones, as that's easier.

So it would be nice to be able to do that, but the edge connector requirements almost make it mandatory to get them made professionally, with the attendant costs and time overheads. And if there's an error in the design, the costs and delays get repeated. Also, if the particular project is only needed occasionally (eg: extenders), the costs may be a little harder to justify.

So I've been thinking about making a universal FlipChip adapter board that is basically just the edge connectors plus some other cheapo connectors that make the finger signals available to some simple rectangular (even single sided) board that plugs onto the adapter. Of course, this would need to be professionally made, double sided, with gold plating, cutouts, registered name and all the details.

But the "mating" board that plugs onto it has no such restrictions. It can be crappy as one likes, and may be just single sided, made at home in an afternoon. Even a just a bit of perfboard! If the design has errors, just make another one, ready to try out in a few hours. Once the design is sorted, and the polish of a purpose built PCB is desired, only then spend the time and money on adding the edge connectors and getting it made properly.

My initial design for the adapter is shown below. A double height board seems a good compromise between single, double, quad and hex. Use 2 or 3 adapters for quad or hex, get out the hacksaw for singles. FLIPCHIPConn.png


These are the sort of cheap connectors I plan to use for connecting the adapter to the mating board.
Header&Plug.png


This shows how it would attach. For strength and rigidity, small straps, made of metal (or PCB or whatever) would bolt the two boards together.
FLIPCHIPConn-1.png


I think this is a good idea, do you?
Seeking your comments and suggestions...
 

thunter0512

Experienced Member
Joined
Sep 27, 2020
Messages
334
Location
Perth in Western Australia
I like the basic idea, but how would you extract the adapter boards? My OMNIBUS backplane sockets are very stiff and it is at times difficult to extract standard quad height boards even with handles.
I would also suggest to design all 4 variants (single, double, quad and hex) for mechanical stability and proper alignment.

Tom Hunter
 

Roland Huisman

Veteran Member
Joined
Mar 24, 2011
Messages
1,314
Location
The Netherlands
If it works for you then it is fine off course. But I'm afraid that you once will plug it in wrongly. One spot to the left or right or to the back or front... You could avoid that using 40 pin box headers that forces you to connect them in the right way. Malcom did a great job on designing a universal template btw. And Glitch made a prototype board. There are many projects out there which might be useful for you.

When you are making a prototype just finish it with HAL. And to be honest, gold plating isn't always necessary. My PDP8/L came with original tinned cables. This has worked for at least 15 years and I can still use the cables. My prototype of the boot loader was also tinned and I still use it without problems. I know gold is far better, but think about if it is really necessary.

I've made a little PCB for my PDP11/20 to be able to use a later model power controller (861B). No way that I'm going to use gold plating here. Just HAL with lead.

power control.jpg

Another reason to make your proto close to the end product is that it is easy to make a few modifications in your board design. You don't have to remove these kind of connector constructions out of your design. That is very error prone...

Well, everyone has its own way of working I guess...

Regards, Roland
 

Al Kossow

Documentation Wizard
Joined
Sep 1, 2006
Messages
2,728
Location
Silicon Valley
I had thought about an Omnibus expansion backplane with DIN connectors instead of edge connectors.
I'd also rotate it 90 degrees so all of the cables would come out towards the back of the chassis.
 

intabits

Experienced Member
Joined
Jan 22, 2019
Messages
145
Location
Melbourne, Australia
... but how would you extract the adapter boards?

One spot to the left or right or to the back or front... You could avoid that using 40 pin box headers that forces you to connect them in the right way.

That's what the small straps joining the boards are for.
The idea is not to have the adapter sitting in the ominbus, and then plug the project board into that. Rather, it is to plug the boards together, join them rigidly with the straps, and then plug the whole assembly into the backplane. It's just a way of leaving all the edge connector related issues out of the project.

There's nothing stopping the use of box headers, but they are not necessary if the straps are used.

I'm familiar with Malcolm's Ominbus designs. They prompted me to look at hex modules as well, and that led me to investigate the DEC drawings with their errors and inconsistencies (the numbers didn't quite add up). I ending up spending a few days working out how the horizontal spacing was actually organized, and writing a program that can generate the PCB file for any size FlipChip module. It generated my adapter design including the 40 pin headers and routing the traces to them, which I prefer to the simple diagonals in Malcolm's design. I haven't yet checked the power and ground pin assignments for Unibus to see if they are the same as Omnibus, but otherwise Malcolm' prototype board is for Ominbus only. I wanted to make something that could be used in any DEC system.

Your advice on HAL vs gold plating is good to know. When I get to making them, I'll keep that in mind if the cost of gold seems a bit much.

On removing the header constructions for a final design, I envisage no problems whatsoever.
I'll tell my program not to add them, then paste the design for the project board into it, and simply join short straight traces for those pins that are actually used.
 

vrs42

Veteran Member
Joined
Nov 24, 2009
Messages
603
Location
Beaverton, Oregon
First, let me say that the issues in the edge connector are indeed daunting. Unless you took the edge connector geometry from a known working source, your adapter board is probably a couple of revisions away from something that can be reliably inserted in the backplane, and also useful in your CAD software. The specs in the logic manuals vary and aren't "quite right" in a few different ways. There is also the issue of the size and placement of the SMD pads for the edge connectors, and their alignment with the routing and other grids in use in the CAD program.

What I do about it, and presumably others do too, is to componentize it. I use Eagle, so it's easy for me to include dimension lines, etc. in the component. I have suitable footprints for the single, double, quad and hex boards, as well as common board outlines, all in the component library. (I also use that library to describe various vintage chips that DEC used but no one designs with any more.)

I haven't had any issues with board vendors and non-rectangular boards being expensive. Gold is a little expensive -- I find it approximately doubles the cost of a quad height Omnibus card. So I've stopped using gold on my more experimental prototypes :).

I have had similar thoughts about switching to more modern and easier to find connectors, but so far haven't found it necessary to go there.

I have used simple zip ties to keep the handles on my new boards for years without problems, so you may not need fancy metal straps to tie your adapter boards on. OTOH, the mechanical stress of pushing the boards in may be a bit much for your headers and sockets to bear.

Vince
 

Dare

Experienced Member
Joined
Dec 28, 2015
Messages
65
I like the idea. However unless the mounting is very strong I expect you'll see considerable flex at the seam during insertion, especially near the center of wide boards. Old backplanes can require a lot of insertion force (well, all mine do, at least). To get the necessary rigidity I think you'd need metal straps on both sides of the boards to keep the insertion forces balanced top to bottom. This may cause issues with clearance on the solder side, however, as technically you only have .063" to play with. Maybe the answer is to use flat head screws on the solder side that are recessed into the straps.
 

intabits

Experienced Member
Joined
Jan 22, 2019
Messages
145
Location
Melbourne, Australia
Good to hear that non-rectangular boards don't cost much more. I've only ever ordered rectangular boards, so I was worried that it might significantly add to the cost. I've also never ordered boards with edge connectors, or gold plating, so I'm also concerned about specifying all that correctly (solder mask, end bevelling, etc)

That's a good idea about using zip ties. Maybe they are enough to keep the boards together and provide up-down tensile strength, with the 80 pins hopefully providing enough lateral rigidity. If not, the straps should be up to the job, especially if the center two are combined into a plate using all four holes.

(I hate Eagle, and KiCad, and Altium. I wrote my own PCB software long ago, and I hate that too :rolleyes:)

A bit of a rave:-

I'm 99.9% sure that I've got the important FlipChip dimensions correct. Of course there is some final checking to do, and the proof will be in the pudding.
But the biggest discrepancy between the output of my flipchip generator program, and the horizontal measurements in the DEC diagrams is 3 mil. That's for an 8 inch measurement where the tolerance is +/- 10 mil, so it's very close and well within spec, and I think I know where that difference comes from.

There's a 5 page PDF document floating around called "flipchip-dimensions", which is an extract from the 1975-76 Digital Logic Handbook. Malcolm's Omnibus prototype board documentation also links to the same dimensions diagram from that handbook, as the guiding reference that he used.
(BTW, The 1973-74 DLH from Bitsavers contains a better quality image of that diagram)

The earlier Digital Logic Handbooks up to 1972 used different diagrams, and separate ones for each board height. But I think that they must have had problems with accumulated errors in these earlier diagrams, where they used the gaps between edge connectors to determine the edge connector positioning.
These problems appear to have been addressed in the new format dimensions diagram introduced in the 1973-74 DLH. This is the "universal" diagram that covers single, double and quad heights. In that diagram, they explicitly specified the edge connector positions as measured from the board edge, thus eliminating errors accumulated by adding up edge connector gaps and widths.

In my research, the penny dropped for me when I realized that the gap widths are controlled by the connector pin pitch. The backplane connector blocks not only use the 0.125" pitch spacing between the pins, but the 18 way groups are also spaced apart at 0.125" multiples. So double, quad and hex boards can be thought of as one very wide edge connector of up to 124 pins, but with either 2 or 4 pins missing between each group of 18.

These images show the 0.125" spacings overlaid with the edge connector:-

Click image for larger version  Name:	FLIPCHIP Spacing.png Views:	0 Size:	51.0 KB ID:	1228673


Click image for larger version  Name:	FLIPCHIP Spacing-2.png Views:	0 Size:	69.7 KB ID:	1228674

Starting on the right at 0.033" outside of the nominal board width, and working leftwards in 0.125" increments, the precise position of each pin is determined. The edge connector positions, widths and gaps are then found by moving a fixed margin out from the first and last finger of each 18 pin group.
That margin appears to be 0.058" from the finger center to the edge connector edge ;).
The -0.033" base origin is the 0.125" spacing pitch, less the 0.058" finger margin, less the 0.1" indent specified by DEC.
 

intabits

Experienced Member
Joined
Jan 22, 2019
Messages
145
Location
Melbourne, Australia
I like the idea. However unless the mounting is very strong I expect you'll see considerable flex at the seam during insertion, especially near the center of wide boards. Old backplanes can require a lot of insertion force (well, all mine do, at least). To get the necessary rigidity I think you'd need metal straps on both sides of the boards to keep the insertion forces balanced top to bottom. This may cause issues with clearance on the solder side, however, as technically you only have .063" to play with. Maybe the answer is to use flat head screws on the solder side that are recessed into the straps.

Strength and rigidity does seem to be a concern. I think the strap modification mentioned above to make the center straps into a four hole plate will help a lot. And together with your idea of double sided straps, should put an end to rigidity problems. Though the clearance could be an issue, but as you suggest, countersunk holes should fix that.

I've decided that before ordering anything, I'll do a full dress rehearsal, making some DIY adapters and a quad project board to see how things hold up. (also to check accuracy).
 

1944GPW

Veteran Member
Joined
Apr 26, 2011
Messages
631
Location
Brisbane, Australia
I like the basic idea, but how would you extract the adapter boards? My OMNIBUS backplane sockets are very stiff and it is at times difficult to extract standard quad height boards even with handles.

A loop of tough cord through a hole close to each side would allow pulling it out readily enough, with two hands. I think there may be more of a problem putting it in, considering the short height. Boards each side might have to be temporarily removed to do so. Or maybe a piece of plywood cut to size and profile to push down on the outer edge from above.

Thin 10mm wide sides could be added to the adapter (giving clearance to the piggyback boards), these going up and having holes for those latching handles. Lots of things are possible.
 

Roland Huisman

Veteran Member
Joined
Mar 24, 2011
Messages
1,314
Location
The Netherlands
I still don't see any advantages of a split board. A split board only makes it wobbly. Boards are so cheap these days to produce at jlcpcb.com for example. An edge connector on a board doesn't cost anything extra unless you want to make it gold plated. If you have a PDP backplane it makes no sense at all to me to be honest... If you want to expand on a modern platform then Al's idea might be far more preferable. Make your own backplane with modern connectors. Then make your own boards for that. But it is your hobby off course, if you have fun doing things the way you like, then go for it :D
 

thunter0512

Experienced Member
Joined
Sep 27, 2020
Messages
334
Location
Perth in Western Australia
I had thought about an Omnibus expansion backplane with DIN connectors instead of edge connectors.
I'd also rotate it 90 degrees so all of the cables would come out towards the back of the chassis.

I have never seen a DIN connector with more than 8 pins, so I am confused about how that would be useful in this context.

Tom
 

vrs42

Veteran Member
Joined
Nov 24, 2009
Messages
603
Location
Beaverton, Oregon
Good to hear that non-rectangular boards don't cost much more. I've only ever ordered rectangular boards, so I was worried that it might significantly add to the cost. I've also never ordered boards with edge connectors, or gold plating, so I'm also concerned about specifying all that correctly (solder mask, end bevelling, etc)

Most sites quote engines ask about either the number of pins to be plated or the number of inches to be plated. The right answer for end bevelling is "yes". The exact angle isn't critical, so I usually just pick 30 degrees. The bevel helps the board self-center front-to-back in the slot, and helps spread the fingers inside the backplane connector instead of mashing them.

Another thing which helps is to shave a 16th off tjhe edge connector corners so that they'll also self-center left-to-right as they are inserted.

Vince
 

Dare

Experienced Member
Joined
Dec 28, 2015
Messages
65
In my research, the penny dropped for me when I realized that the gap widths are controlled by the connector pin pitch. The backplane connector blocks not only use the 0.125" pitch spacing between the pins, but the 18 way groups are also spaced apart at 0.125" multiples. So double, quad and hex boards can be thought of as one very wide edge connector of up to 124 pins, but with either 2 or 4 pins missing between each group of 18.

I just finished working through all of this for a set of KiCAD templates I made for the various sized flip chip boards (see here). You are absolutely right about the .125" pin spacing. However, I prefer to think of the AA pin as starting at .158" - half the pin width (.040") = .118". From there, the A pins for each successive connector are at alternating 2.75" / 2.5" distances (.125" * 22, .125" * 20), or +2.75", +5.25", +8", +10.5", +13.25". Alternatively, as you've shown, you could imagine a series of .125" wide pin "cells", with the pin pad centered in the cell, and the cell for pin AA starting at .158" - (.125" / 2) = 0.0955".

The positioning of the right edge of PCB tabs that form the connectors seems a little more arbitrary. I used the given dimensions for the quad-height and extrapolated for the hex-height.

If you wanted a more parametric placement of the tabs, you could imagine each 2.24"-wide tab being centered around the pins it contains. This would give you:

tab right edge = 0.0955" + X + (0.125" * 9) - (2.24" / 2)​

where X is the progression described above. This gives you 2.8505", 5.3505", 8.1005", 10.6005", 13.3505"--all within the tolerances given.
 

vrs42

Veteran Member
Joined
Nov 24, 2009
Messages
603
Location
Beaverton, Oregon
To give a perspective on this, the 5 M9042 clone boards I ordered were $28.95 US + $12.95 shipping. This included a $17 charge for ENIG-RoHS surface finish.

That brings up metallurgy. I think the only finish that can be expected to hold up for 50 years is good old tin/lead. The other stuff is good for consumer projects that get thrown away after a few years. (Before the cracking, whiskers, and other issues get noticed.)

The soft gold finish is also too thin and soft for repeated insertions. Either leave it off or spring for the hard gold.

There used to also be a question about who to trust with your metalurgy, with the USA generally getting it right, but at a cost several times more in both time and dollars than some of their lower priced overseas competitors. These days, there are reputable Chinese vendors who will deliver proper metallurgy quickly and cheaply. (A couple of the formerly "American made" vendors actually sub-contract to China now.)

I have one set of boards which a colleague ordered from eastern Europe over 20 years ago. I don't know if they left off the nickel or what, but the edge connector metal just slowly dissolved into the underlying copper over the first few years. The copper then promptly oxidized, leaving the edge connector basically worthless.

Vince
 

intabits

Experienced Member
Joined
Jan 22, 2019
Messages
145
Location
Melbourne, Australia
Wow, leave it for a couple of days, and there's quite a bit to catch up on.
Some responses:-

... considering the short height. Boards each side might have to be temporarily removed...
That's not my intention with this. Please see my response in message #5.


I still don't see any advantages of a split board.:D
And I don't understand why you don't understand!:? I thought I explained the motivation for this quite well in my post #1.

Clearly, you and I are viewing this from quite different perspectives.

It seems that you view this a rather crappy way to make a flipchip module, which is true. You have more experience with this than I, and obviously are quite confident in your designs, and therefore comfortable with taking them straight to the professional finish.

I'm just starting out with this, and have no clue what I'm doing, or what I want to do. At first I just want to do research and experiment with Omnibus (and later Unibus) interfacing. And do this in baby steps, with homemade PCBs, where an error or new insight will result in the next iteration. Initially my projects will do nothing useful, just some basic monitoring and controlling of signals with an Arduino or something.

With time, I may end up with a similar viewpoint to yours.
But meanwhile, my intent is to have something that provides a *reusable* and *temporary* means of connecting my crappy, home made, mostly single-sided PCBs to the Omnibus, while also insulating those projects from the physical aspects of the edge connectors. This avoids the expense and delays associated with having to get professionally made boards at each iteration.


Most sites quote engines ask about either the number of pins to be plated or the number of inches to be plated. The right answer for end beveling is "yes".
Another thing which helps is to shave a 16th off the edge connector corners so that they'll also self-center left-to-right as they are inserted.

Thanks. I expected the beveling to be fairly simple. (I assume it's obvious how to specify which edge, or the fab will know from looking at the design)
I was more concerned with how to keep the solder mask off the fingers. I'll be looking at existing designs for guidance.
And I may seek help here, asking if someone can take a look at my design (in KiCad format).


...I prefer to think of the AA pin as starting at .158"

Not that half a thou makes any difference, but your 0.0955 term should be 0.095.

Then both our formulae would give the identical (better) results:-
Board edge to Edge Connector A LHS: 0.1000
Board edge to Edge Connector B LHS: 2.8500
Board edge to Edge Connector C LHS: 5.3500
Board edge to Edge Connector D LHS: 8.1000
Board edge to Edge Connector E LHS: 10.6000
Board edge to Edge Connector F LHS: 13.3500

I used this formula in my program:-
0.1 + ( (N-1)*20 + Trunc(N/2)*2 ) * 0.125

Yours uses a lookup table:-
Table=(0, 2.75, 5.25, 8.0, 10.5, 13.25)
0.095 + Table[N] + (0.125*9) - 2.24/2

Much of a muchness. (The 0.1 & 0.095 terms are suspiciously close, not sure where the difference comes from)

The offsets we used 0.118 = 0.158 - 0.080/2 and -0.033 = 0.125 - 0.1 - 0.058 are both reasonable. I think I did it that way because it fitted better with what I already had in place for the board outline. But purely for interest sake, note that both of these are dependent on finger width, which was specified slightly narrower at 0.075" in the Logic handbooks of 1970 and earlier.

That's an important point you make on your template GitHub page (that I had not considered), about Unibus SPC quad board connectors being labeled C-F. I'll add that detail to my generator program.


To give a perspective on this, the 5 M9042 clone boards I ordered were $28.95 US + $12.95 shipping. This included a $17 charge for ENIG-RoHS surface finish.

Thanks. I've had JCLPCB (and a number of others) make boards for me over the years. But they have always just been simple 2 sided rectangular designs, so the additional considerations in this project are new to me.

As I've tried to explain all along, although reasonable, those costs are something that I can't justify for what I envision my initial forays will be.
Hence my aim to limit those costs to only what *has* to be done that way.
 
Last edited:

Dare

Experienced Member
Joined
Dec 28, 2015
Messages
65
Not that half a thou makes any difference, but your 0.0955 term should be 0.095.
I got 0.0955" by taking the offset to the middle of the first pin (0.158") minus half the cell width (0.125"), or 0.158 - (0.125/2) = 0.0955". This represents the right edge of the cell for the first pin.

Of course, you are completely right, half a thousandth is meaningless in this context. So 0.095" is the better value to use.
 
Top