Absolutely spot-on! 
The only caveat is that some tracks may need to be thicker as they are carrying power.
I’ll check the specs.
Later…
It’s complicated, but here goes:
The main frame power supply is shared between 5 edge connectors, so I guess absolute max drain from one would be about 1/3 of total (assuming some modules draw more than others.)
There’s + & - 33.5VDC fused at source at 2.5A each. And each rail is delivered via two connector contacts.
There’s +11.5V DC fused at source at 7.5A. And that is also delivered via two connector contacts.
There’s 17.5V AC not fused at source at all. (Delivered via a single connector contact.)
There’s 24.5V AC not fused at source at all and stated to be 500mA. (Delivered via a single connector contact.)
The Oscilloscope plugin has two fuses, one at 0.3A, and one at 0.75 A
The 550MHz Counter plugin (with LED numeric display) has a fuse at 2A.
I don’t think any contact is intended to carry more than 2A. That’s my guesstimation!
Putting fuses and test points on your PCB makes testing more reliable (fuses) and easier (test points). The PCB is a rigid structure and that feels like a good place to add these things. Hacking those parts in elsewhere is easier for the PCB design, but makes it less universal.
If your fixture looks anything like jmk is guessing, then adding a single or dual row male header is a good option. Then you have test points on all wires and you can easily make temporary connections with “dupont” wires.
A second connector footprint will allow pins for test points on up to all tracks, or just place the odd pad where needed.
Extend the board and fit a plastic or metal bar (pink bar) to clamp all the wires to the board, otherwise, after a few uses, wires will break off the board where soldered.
A few more comments:
The through hole connectors are 100 mil (1/10 inch) spacing between pads and between rows. How good is your soldering, especially with the pads connected to the back layer? Would you prefer larger pads more widely spaced?
Tracks shown are 30 mil wide.
The “finger pads” are “edge connector” type pads but I have no idea of the size and distance between pad centres you require. Same goes for where and width of key way.
Both the edge connector footprint and through hole connector footprint are created by making a single pad and then using the Array tool. The back layer “finger pads” are formed using the Duplicate tool, changing the layer in Properties then placing that row under the front row.
I haven’t yet read Paul’s FAQ, however it is my bed time.
Will check in tomorrow.
Excellent! I’ll see if I can reproduce that, many thanks.
Currently reading and absorbing info.
Much appreciated.
John
I agree about placing the fuses and TPs. Let’s see how I get on with the basics!
Yes, I think JMK has read my mind!
Are Dupont wires like sockets on the end of a wire - like ferrules?
Thanks
“Dupont wire” is just a historical name that stuck for some reason. I guess everybody know these things, but not all recognize the name. the black plastic is a 2.54 by 2.54mm square, and you can use them to make arbitrary connections between pins on 2.54mm headers or breadboards.
Note: the cheap ones do not even have copper wire (I guess it’s aluminimum), and they have a higher resistance then you would expect from a wire, so you can not use them for higher currents. But they are low cost and easy to replace while fiddling or when worn out and this makes them convenient to use anyway. They are available in all 3 combinations of Male / Female and you can buy them in different lengths.
Thanks! 
Same format perhaps as pc motherboard jumpers.
Yes, they fit on there too.
I once had a PC that refused to boot without the (non existing) fan. So I used a dupont wire to tap of the tacho signal from another fan and plugged it into that otherwise empty fan connector. (I just forced in a male pin of the dupont connector in between the plastic and the metal of the other female fan connector. It was a 2 minute fix and it lasted for years until I bought a new PC and scrapped the old one.
A tip:
Don’t make inside corners like this:
Use “dog bone” corners or draw rounded corners after making certain that the mating connector will accept those.
Otherwise a lot of unnecessary communication with the manufacturer occurs.
Thanks! What’s a dog-bone corner? I thought a dog-bone was like a cylinder with two lumps at each end!
I’ve tried adn tried but can’t form a rectangle of copper on the pcb layout.
Which tool should I use, and can you make any rectgangel adn then edit the dimensions (to 2.5mm x 8.0 mm)?
Can you set the grid to be spaced at 3.96mm?
I’vre used all sorts of software packages for decades, but this has me stumped!
Time for bed.
Thanks
Well, you have to think of the machine the manufacturer is using:
it’s a vertical drill/mill/engraver, meaning a vertically rotating cutting tool. So how should a rotating tool make a sharp inside corner? Answer: it can’t. A laser cutter can, but that’ll add considereable cost to your PCB.
The solution is called “Designing for Manufacturability” (meaning you’re responsible).
That is where “dog bones” come in: make inside corners like this:
In practice, expect a mill diameter of 2 mm, so give the cutouts a radius of 1 mm (contact the manufacturer for exact preferences).
This will save you lots of back-and-forth when sending design files.
And even if a rounded inside corner is OK for your design, then draw it that way.
BTW: this would be a really cool feature when working on the Edge Cut layer: a DRC warning on inside corners with associated help text. I haven’t checked the plugins, perhaps it already exists?
Are you sure your spacing between centres is 3.96mm (0.156")?
This is an old hand laid out board. It is probably laid out in Imperial. To get a more accurate result, measure from beginning of pad 1 to beginning of pad 28 and divide by 27. Try both Imperial and Metric. See the cyan arrow and purple information. Looking at your photo, I’d suspect the pads to be 100 mil wide with 150 mil between centres.
To change Grids:
Green arrows give Metric or Imperial
Left click the rectangle displaying your grid (where magenta is pointing) and a list will be displayed.
At the bottom is “Edit Grids” (red arrow). Click on this. A new window will open. See the below screen grab.
At the bottom of the list of grids in this new window is a + sign, two arrows and a bin. Click on the + and another new window titled “Grid Settings” will open.
You can have different grids for horizontal and vertical, but for this project, different grids are not needed, so tick the box “Linked” and type in the new grid you require into “X”. NOTE: The unit type being displayed and entered depends on the green arrow selection in the above screen grab. (I have mils selected, see above, so any grid I currently enter is in mils.)
Additions and removals of grids can also be accomplished by opening Preferences and selecting Grids in each of the four Editors. Grids are independent for each Editor.
After a:
paul@cezanne:~$ git clone https://github.com/anotherlin/tek_tm_ext.git
and then extracting the KiCad project, and opening / converting it in KiCad V8 I do indeed see a pitch of 156mils. [3.9624mm]
Now, that’s weird:
25.4 * 5 / 32 = 3.96875
I guess those 5um don’t matter much over the total width It accumulates to:
27 * (3.96875 - 3.9624) = 0.1714499999999961
The project itself is an extender board / cable for the TM500 It’s mostly connectors:
It also has some voltage detection / monitoring circuit:
I’m not sure what that is for.
Another website also confirms this pitch:
https://w140.com/tekwiki/wiki/TM500_Series_plug-in_interface
Mechanically, the interface is a direct card-edge connector with 28 contacts on either side, at 5/32" (~0.156" or 3.96 mm) spacing. The connector can be keyed in several places, the plug-in boards have matching cuts between contacts (see below).
Thanks Paul.
So the connector is based on 32nds of an inch and not 10ths as I originally suspected.
32 parts to an inch and 12 inches to a foot and 3 feet to a yard and 22 yards to a chain.
Ahhh!!! The Banana System of measurements is so uncomplicated. 
Anyway, @JohnBB should be able so set up a suitable grid now.
Or he just uses the connector from the project linked above.
Or takes the whole project and just modifies it a bit…
The EEVblog link below also has links to ready made extender cables.
Seems like a great idea to me! 
So he will be able to create grids in his next project.
Oh wow! That board [above] is intended for exactly what I have! (slightly different objective, but no matter. )
(I did mention Tektronix 500 series, and the weird-looking pitch right at the beginning, but I know how everyone dives into the detail without reading the title, I do it myself. )
At GitHub - anotherlin/tek_tm_ext: Tektronix TM500/TM5000 extender
the maker of this board mentions this:-
" The complete Kicad project is available at [[removed so I can post this replly]] . You will need pointhi/kicad-footprint-generator for running the Python footprint generation script (code is a bit ugly, I’m a Python noob, sorry). "
I have no idea, but I thought I’d flag up the footprint generator in case it is useful to anyone here.
If you’re interested:-
The edge connectors (that receive boards such as this, with the 3.96mm pitch) are readily available, and must (I think) have been quite a common standard a while ago. This Tektronix gear dates from the '70s and '80s.
Also used in the gaming industry:
JAMMA stands for Japan Amusement Machine and Marketing Association who in 1985 created the JAMMA wiring standard. This allowed all Arcade Cabinets that were wired in the JAMMA standard to run any game built to this standard. Since Japan designed most of the newer games in the 90’s the JAMMA became the standard by default.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.