2
\$\begingroup\$

I am working on a PCB for which I need external soldered wires. I made the whole PCB with al the traces on the front layer. Then, with 3 vias, I got to the back layer. Here I need to solder 3 wires to the traces (green traces on picture). I used a "Test point" for that. Does this work: Does placing a pad on a trace make it a connection?

enter image description here

And one more question: I am new to PCB designing. In this design I did not made a ground plane. I am planning to do this in the future, but how can I then solder a wire to this ground plane? Also through a pad placed random on the board where it is filled with copper?

Thanks!

\$\endgroup\$
  • \$\begingroup\$ I don't know about KiCAD, but if you placed a test point in the schematic with a footprint it should. In OrCAD you can also add it on the fly in the PCB layout to ensure it connects to the net. You could just plop it on as a mechanical symbol on top of the trace you want but that's bad practice since it messes up bookkeeping. If you want to solder a wire to a ground plane you must open up the solder mask by placing a footprint that does though (or remove the solder mask in that area with a shape) \$\endgroup\$ – DKNguyen Apr 11 at 17:56
  • \$\begingroup\$ Thanks for your reply. Thus, everywhere where I place a pad, the soldermask gets removed and there is connection between the pad and the trace underneath it? \$\endgroup\$ – jan Apr 11 at 18:41
  • \$\begingroup\$ Go download "DFM Now". It is a free Gerber viewer. Use the "Open Folder (Gerber/NC)" option and look at the gerbers to see how things end up. Do NOT rely on placing random things all over the PCB even if it works out okay. It is very easy to lose track of things when modifications start happening. If you need something connected to a net, make a schematic symbol, give it a footprint and position that in the PCB layout. Don't place random pads with no nets assigned onto traces that you want them connected to. Adding a negative shape in the solder mask layer that cuts some of it out is ok \$\endgroup\$ – DKNguyen Apr 11 at 18:50
  • \$\begingroup\$ You helped me a lot. Thanks for the advice. I will soon follow a course on KiCad so I get a much better understanding on all of this. \$\endgroup\$ – jan Apr 11 at 19:16
  • \$\begingroup\$ For anybody interested here the link to a related question on the forum: forum.kicad.info/t/ws2812b-neopixels/16262 \$\endgroup\$ – Rene Pöschl Apr 11 at 22:50
3
\$\begingroup\$

I would do it like this: in the schematic, place a Conn_01x01_Male component and connect it to the signal you need. Then in "Assign Footprints" search for the test point you want to use, e.g. TestPoint_Pad_D2.0mm. After updating the board (in KiCad 5.1 there is a new button for this, in older version you have to do it with the usual process with the netlist), you can place the testpoint on the back with "flip" and then connect it just as all other components. The DRC test would verify that it is connected.

To be 100% sure, and to check if your method works, you can use the gerber viewer which is integrated in KiCad (the "GBR" symbol in the main window) and enable only the top and bottom copper planes.

PS: If you don't mind that there is a hole, I would use Connector_PinSocket_2.54mm for the test points. You can solder wires to it, too. Looks like you have plenty of room on your board for it.

\$\endgroup\$
  • \$\begingroup\$ Thanks. I eventually used a testpoint in the schematic, and associated it with a footprint. I completely forgot to add the testpoint in the schematic at first. I only added it on the PCB. Now I know how it works. Beginners mistake hahah thanks \$\endgroup\$ – jan Apr 12 at 15:39
  • \$\begingroup\$ Glad to hear that it works now. Maybe accept my answer as the answer which solved the problem, in case other people are searching for the same problem. \$\endgroup\$ – Frank Buss Apr 12 at 19:12
1
\$\begingroup\$

A wire may have significant pull and the standard test for any wire connection is 5lbs or ~ 2kg.

You can imagine your pad getting ripped off. (!)

So drill a hole for suitable wire size maybe two holes but plan on some design of strain relief. then pad on last side. and feed the wire thru. Two holes gives strain relief. in 1 side and out the other.

The popular alternative is a screw terminal block. or PCB connectors and Plug

But I am glad to see you are adding Test Points to your design. We call these design for testability DFT (points) which must be included in your thought process in DFM.

Try to interface where it makes sense for cable routing, such as near an edge.

\$\endgroup\$
  • 1
    \$\begingroup\$ There will actually be no pull on the cables, but I understand your point. The idea of screw terminal blocks is very good. Thank you. \$\endgroup\$ – jan Apr 11 at 19:10
  • 1
    \$\begingroup\$ The other factor is Vibration tends to break wires at the point of connection from fatigue, but you will probably say "there won't be any vibration" but I had to ask \$\endgroup\$ – Tony Stewart Sunnyskyguy EE75 Apr 11 at 19:11
  • \$\begingroup\$ hahaha thanks for your advice. I am making a wordclock which will just hang on the wall somewhere. But I could consider these options because of the risk of dropping the clock. \$\endgroup\$ – jan Apr 11 at 19:15
  • \$\begingroup\$ yes everyone should consider if their design is drop proof or have shock grommets \$\endgroup\$ – Tony Stewart Sunnyskyguy EE75 Apr 11 at 19:16

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.