Since I'm using Eagle to try to form a single-sided PCB and the autorouter completed my circuit by 99% (2 airwires to go), I thought of constructing my circuit so that I insert a flat jumper wire underneath the IC so that its nicely hidden.

Currently I'm using inductors as wires but the appearance looks like they will take up too much space in the IC. Same goes with resistors and capacitors.

What can I do to successfully add wires directly under the IC and still satisfy the ERC? Is there a specific library that allows this?

  • \$\begingroup\$ Delete the net and terminate both ends by a single-pin connector. But generally - do not use autoroute, it's awful in most cases. \$\endgroup\$ – Eugene Sh. Jul 15 '16 at 20:22
  • 1
    \$\begingroup\$ I would not recommend "hiding" the jumper under an IC, as it not only make maintenance and repair more difficult, but also introduces a possible assembly problem (oops - installed the IC before the jumper!). \$\endgroup\$ – Mark Jul 15 '16 at 22:24
  • \$\begingroup\$ @Mark Then the OP can still solder the jumper on the bottom side. But in general it is error prone to bring a dependency into the assembly order. \$\endgroup\$ – Ariser Jul 15 '16 at 22:57
  • \$\begingroup\$ Did you try an SMD resistor? \$\endgroup\$ – Passerby Jul 16 '16 at 2:23
  • \$\begingroup\$ I'm not ready to go surface-mount. I'm staying with DIP-based devices for now. \$\endgroup\$ – user116345 Jul 16 '16 at 3:22

With the newer versions of Eagle, there's a neat trick to build jumper-wires which belong to the same net and pass ERC and DRC.

You can insert such bridges in your schematic and place them in the layout. Correctly placed the autorouter won't try to draw traces between the two ends.


  • in schematic you won't see, where the wire is replaced by the bridge
  • you have to design the bridge for each jumperlength you want to use.

How it's done

  • Go to the library editor. I prefer to create a new library for all my strange and special devices.
  • create a symbol resembling a jumper but with one pin only.
  • create a package with the two pads for your jumper. I recommend to draw the jumperwire in Layer tplace and bplace. But this is only a suggestion
  • make a new device
  • load your symbol into the device
  • make a new package variant selecting your package
  • connect both pads to the single pin either by connecting one first and appending the other or by selecting both pads and connecting them at once.
  • On the list of connections on the right you see now a column contaning two small green symbols of two pads. If they are connected click on them once. Make sure that they are disconnected.
  • Save the library

How to use it

  • "Use" the library
  • Place that jumper into your schematic and connect its single pin to the net you want to jump.
  • in the layout position your jumper where you need it.
  • run "ratsnest". There shouldn't be any more yellow airwires left crossing the void between the two jumper pads.
  • now you can route (manually or auto) however you like.


I recommend making a bunch of different jumper packages and store them as package variant in your one and only jumper device, which eases exchange of jumper sizes. If you are fine with some standard lengths of jumpers, just use existing resistor packages in your library. Drawback is, your jumpers resemble resistor drawings in tPlace and tDocu layer.

SMD-jumpers can be easily formed by importing SMD-resistor packages from other libraries and putting them into your library.

This is especially useful with 0-Ohms SMDs, which are frequently needed when routing a MCPCB.

DRC errors may well arise from violation of keepout errors. Fortunately vias and pads should be allowed in keepout areas, if you put the package on the right side of the PCB which doesn't make any difference in routing.


If though the PCB is single-sided, pretend it is double-sided and route the trace just up to the conflicting trace, and add a via. Do the same for the other side, where the original trace starts up again. Then put a piece of wire between the two vias on the opposite side of the PCB.

If you are only using through parts, then use can put all of the traces on the bottom, and components on the top, in a traditional component side (top), solder side (bottom) scenario. In this case the jumpers I referred to will show up on top, along with the components.

Here's an example; note the red and green jumpers:

enter image description here


Your Answer

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