2
\$\begingroup\$

I am thinking about a project that has need for various different complicated wiring connections. I would like to make a single board that would make it as easy as possible to make arbitrary connections between signals. My thought is something like this:

Matrix

By putting the signals in a configuration such that they all cross every signal from the opposite side at some point, then I can use the vias to make connections by soldering a thin piece of wire in the appropriate hole.

I made this image in Eagle to demonstrate my point, but vias will not work, because they will be always connected all of the time. What I want is the copper on top and bottom but not in the through hole part. Is this possible to do in Eagle? Can most fab houses deal with things like this (I generally use ITead)?

In my final design it will be much larger than this (64 in - 64 out).

\$\endgroup\$
  • \$\begingroup\$ That may not actually be a good idea: soldering to copper on both sides of a non-plated-through hole can at times be challenging as gas from fluxes or contaminants which have gotten in the hole can bubble out as the joint on the 2nd side is trying to cool, leading to a cold solder joint. In contrast, with a plated through hole the small space between the solder-wetted wire and solder-wetted hole plating should entirely fill with solder and then cool without being disturbed. \$\endgroup\$ – Chris Stratton Sep 4 '13 at 20:52
  • 2
    \$\begingroup\$ For one thing, I would lay this out as a grid (move JP2 and its wires to the left side of the PCB). Next, why not use solder jumpers? Only one side to solder, and with solder wick you can even remove a jumper. \$\endgroup\$ – Wouter van Ooijen Sep 4 '13 at 21:21
  • \$\begingroup\$ @wouter, that's not a bad idea. It is a difference between the headers being 90 degrees vs straight across (which I prefer), but I could deal with that. I'm having trouble envisioning the wire routing in that case. \$\endgroup\$ – captncraig Sep 4 '13 at 22:06
  • \$\begingroup\$ @CMP You could make an 16x8 grid of pads, each column connected to a pin on each header with the a very similar layout to the one you have now. Stagger the headers, and run a single trace away from each pin, put 8 pads along this trace. From here you can just use solder jumpers across columns to connect pins how you want. It's not very different from your current idea, but the routing should be very simple. \$\endgroup\$ – Shamtam Sep 4 '13 at 23:26
  • 2
    \$\begingroup\$ @cmp: While I understand that your plan for unplated holes may make the eventual assembly of your board easier, you should know that the "normal" PCB manufacturing process will plate all holes by default. Unplated holes will require an extra drilling step. You should (must, really) check with your board shop to ensure that they can build the board the way you want (and to determine how they want the unplated holes defined). \$\endgroup\$ – Peter Bennett Sep 5 '13 at 0:32
3
\$\begingroup\$

Yes, in eagle "help hole" (I'm a eagle CLI nerd)

HOLE

Function Add drill hole to a board or package.

Syntax

HOLE drill •..

See also VIA, PAD, CHANGE

This command is used to define e.g. mounting holes (has no electrical connection between the different layers) in a board or in a package. The parameter drill defines the diameter of the hole in the actual unit. It may be up to 0.51602 inch (13.1 mm).

Or if you like clicky buttons: Picture of EAGLE's hole tool

Will board houses be able to do this? Yes -- it is not uncommon. I can not speak for how they accomplish this in processing, since some boards are drilled before etching + through hole plating, but check with your board house before ordering.

\$\endgroup\$
  • \$\begingroup\$ Wow. Its that easy. Now how can I make pads on top and bottom to solder to? Do I need to add a part to my schematic to connect pads to the headers? I'd worry if I just put holes through the wires there won't be anything to solder to. \$\endgroup\$ – captncraig Sep 4 '13 at 20:27
  • 1
    \$\begingroup\$ Well that is mostly true (depending on your copper trace width). You should talk to your manufacturer since as far as I know when EAGLE spits out gerbers, vias are included as copper on all layers they hit. To be honest, I personally would just use wide copper next to the drill hit. \$\endgroup\$ – HL-SDK Sep 4 '13 at 20:34
  • \$\begingroup\$ It depends on the PCB vendor. For example, a few years ago Sunstone Circuits started to do non-plated holes in their cheap PCB service. Before that, they plated all holes. It's not uncommon for a PCB vendor to charge extra for non-plated holes, because that requires an addition drilling step in the process. \$\endgroup\$ – Nick Alexeev Sep 5 '13 at 0:39

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.