2
\$\begingroup\$

I am planning to use a PCB-mount triaxial connector, CBBJR79TL, in a design for a laboratory prototype. Making reference to the "recommended mtg hole pattern" section from the CBBJR79TL drawing, I have attempted to make a footprint in KiCAD. I am new to PCB design generally, as well as KiCAD specifically.

There are 6 pads. The pads are located at (-79,0), (21,0), (129,129), (-129,129), (129,-129), and (-129,-129). Pad Number 1 corresponds to the center conductor, Pad Number 2 corresponds to the inner shield, and Pad Number 3 (technically 4 contacts) corresponds to the outer shield. All units are in mils.

How to interpret the dimensions provided on the drawing?

The pins themselves appear to be 50x40 mil (+-5mil in each dimension), and yet the recommended hole diameter is 62.5 mil. Suppose I add 22.5 mil of pad diameter to account for the annular ring -- that leaves a total pad size of 85 mil. The closest of the two pads (Pad 1 and Pad 2) are 100 mil apart (center to center). With a total pad size of 85 mil, this means that there will be only 15 mil of solder mask between (edge to edge) of Pad 1 and Pad 2. This distance is lower than recommended pad separation distances (50 mil) for through-hole parts that I have come across online.

That being said, I am unsure what Pad Size and Hole Size I should be using. I have a feeling I am missing something – perhaps something related to the pre-tinning note (note 7) on the drawing?

Drawing, Footprint Editor, and Pad Parameters

\$\endgroup\$
  • \$\begingroup\$ Could you get a 45 degree thickness of the pins perhaps? \$\endgroup\$ – rdtsc Nov 26 '19 at 20:26
0
\$\begingroup\$

I'll try to answer your questions:

How to interpret the dimensions provided on the drawing?

I believe you have correctly identified the x-y coordinates of each hole. The hole diameter of 62.5 mils is also correctly identified. As far as I can tell, you have transferred the useful information from the mechanical drawing for an electrical connection. You may consider adding additional silkscreen for indicating the body of the connector, but it's not mandatory.

The pins themselves appear to be 50x40 mil (+-5mil in each dimension), and yet the recommended hole diameter is 62.5 mil.

The diagonal of a 50x40 mil rectangle is 64 mil. However, if they're recommending a 62.5 mil drill hole, I suspect the corners are rounded. I would go with the recommendation and not worry about it too much. The paranoid might order the connector and get it in hand to verify this with calipers before fabbing the board.

With a total pad size of 85 mil, this means that there will be only 15 mil of solder mask between (edge to edge) of Pad 1 and Pad 2. This distance is lower than recommended pad separation distances (50 mil) for through-hole parts that I have come across online.

I'll note first that by virtue of the hole diameter, there will be less than 50 mils separating pads. However, what you're used to seeing in 100 mil pitch boards are typically 32 mil drills. If this is a hand-made prototype, I'd probably be fine with those holes for signal and guard. I would make the pad diameter for the ground pins much larger, maybe >100 mils, to help with ground plane soldering as well as heating up the big metal chunk of that connector.

... perhaps something related to the pre-tinning note (note 7) on the drawing?

I think this is a red herring. Less than 2 mils isn't going to change much.

| improve this answer | |
\$\endgroup\$
0
\$\begingroup\$

You can import the footprint into freecad using stepup and then check the dimensions in a powerful CAD environment (if you have access to freecad 0.17 then drawing dimensions workbench otherwise techdraw or export to dxf and then use librecad.)

More details: https://forum.kicad.info/t/how-to-check-footprint-correctness/9279

The tutorial https://forum.kicad.info/t/tutorial-how-to-make-a-footprint-from-scratch/11092/4 has a section about how one can select the correct hole size if it is not given in the datasheet (or if you do not trust the datasheet)

| improve this answer | |
\$\endgroup\$
0
\$\begingroup\$

The footprint I proposed in my original question worked without issue. The part fit well in the PCB and soldered without shorting. I had some trouble heating the connector body pins well enough for the solder to flow well, but I found that the trick was just to let the connector body heat up longer before soldering.

| improve this answer | |
\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.