Tektronix 7000 flexible extender project, need some advices regarding PCB design
The PCB prototypes are back from the fab (JLCPCB).
The 76 pins connector is actually available as both "eyelets" and PCB pins. I didn't know that originally, that's why I bought the eyelet version at first.
See the manufacturer's references on the photo (https://groups.io/g/TekScopes/album?id=248160).
The PCB pin version has many advantages, the main one being ease of assembly, and a backplate can be designed so each individual pins can be probed.
Unfortunately, I've not added enough tolerance and the EDAC connector cannot fit. Guess it's very useful to have a version 0.9 to double check everything.
The datasheet specifies 0.76 x 0.47 mm (0.03 x 0.018 inch), my design has solder pad drills at 0.8 x 0.5 mm.
Whereas my caliper measures 0.8 x 0.5 mm on the actual connector at end, but my caliper has only 0.05 mm precision.
I've added an about 5% (because it was closest round number) whereas it should have been 10% at least, probably 15%.
Do you guys have a rule thumb regarding tolerance that should be added whenever "mechanicals" are involved?
The other issue, a lesser one, is regarding solder pad specifications. If you look at the photo, they seems very tiny.
For that extender project, the solder pads for ribbon cable or individual wires are targeted for 24AWG, which is specified as 0.0201 inch in diameter.
However, as I later found out, that 0.0201' diameter is only correct for solid wire. The 7/32 wire (a wire made up of 7x32AWG stranded "sub" wires) is actually specified with a 0.024 diameter.
In fact, for a wire gauge, there are numerous possible diameters: https://www.calmont.com/wp-content/uploads/calmont-eng-wire-gauge.pdf
I've used a .022 drill size but hopefully, my 7/32 (1550 alpha wire) fits (it wasn't supposed to), albeit snuggly.
This part is probably a "non-problem", I can actually specifically target 7/32 24AWG with a .024 drill size and add 10% tolerance (for a grand total of 0.0264 inch).
In fact, I have the feeling that wire/cable manufacturers have much tighter tolerance and it may actually be easier for soldering to have snug wire that can hold by themselves.
Any suggestion on that idea?
My concern is rather about the ratio between the drill size and the solder pad size.
That is my drill size is a .022 inch diameter, the total size of the solder pad being .055 inch diameter, so a ratio of 2.5.
On the photo, it looks really tiny, not a lot of "meat" for the solder. Is there any general rule of thumb regarding the ratio to be used?
There are however a few good news.
1) The cutouts of the backplate appear correct.
2) Even if I should rework the solder pad dimensions, the PCB edge connector is usable, solder it with the eyelet 76 pins connector, and test it with an actual plug-in.
To end up, I have to find a way to recycle the 5 backplate prototype PCBs. Do you guys have any idea to do with them?
I was thinking about using them for putting my coffee cup on them :)
On 6/5/20 2:26 PM, Ke-Fong Lin wrote:
To end up, I have to find a way to recycle the 5 backplate prototype PCBs. Do you guys have any idea to do with them?Yeah, I was saving some early version pcbs of a project but tossed them out in a 5 lb pile last week.
The tolerance of the solder pads is not super critical. What is critical is the overall width of the card edge and its tolerance fit with the female opening of the connector. Too loose and you could have shorts to adjacent pads. Too tight and your product is not a speed tool convenience for buyers.
I did a sampling of all the plugins I could find laying around and they varied a lot, so I made mine as loose as would not short with about a 15% safety margin. (The width could go 15% of 0.10 inches narrower before shorts became possible with nominal parts.)
I always add 0.15mm (6mil) to the diameter of the pin (rectangular pins: diagonal) and round up to the next level of precision (0.1mm, or 4mil) for holes, never had anything that did not fit. For automated component placement this number may be a bit on the tight side: my assembler asked for the double number.
The minimum annular ring for the pad is specified by the PCB manufacturer, but never less than the minimum track width (usually 6 or 8mil).
When the pad has to absorb mechanical stress (like with connectors) I make the annular ring as wide as I can get away with, sometimes I even add copper traces for extra support...