Avoid the crossover by re-ordering pins first. If the crossing cannot be removed, use the cheapest jumper that meets the circuit's current and reliability needs: normally a zero-ohm SMT link in a static, stiffened area. If that approach does not fit, add a second copper layer. Do not choose a jumper before checking connector orientation, contact side and the installed fold.
This flex PCB crossover jumper single-layer routing guide starts with that decision, then shows the crossing arithmetic, the construction options and the drawing details an engineer or buyer should settle before requesting a quote.
Judgment first: rank the options before routing
The following order is engineering judgment, not measured cost or reliability data. The middle options have narrow uses; they are not steps every production design should pass through before adding copper.
- Remove the crossover. Swap pin assignments, change connector orientation, correct a mirrored footprint or flip which side the connector contacts face. Check before layout. Cost: no extra part.
- Use a zero-ohm SMT link. Start here for an unavoidable crossing if the selected part meets current requirements and fits outside the bend.
- Use a hand-soldered wire or ribbon jumper only for prototypes and very low volume. Treat its repeatability and mechanical weakness as reasons to limit its use.
- Consider double-access single-layer flex when access from the back is needed. It changes where the copper can be reached; it does not create a crossover by itself.
- Consider a printed crossover only within a printed-circuit technology choice. A dielectric patch and silver ink bridge belong to a different technology family.
- Add a second copper layer when the jumper approach fails the electrical, mechanical or quoted-cost check. Cross on separate layers with plated through-hole connections, outside the bend zone.
For the broader construction comparison, use the single-sided versus double-sided flex PCB guide. Here, the question is narrower: how to resolve the crossing without adding unnecessary assembly or compromising the flexing region.
Count the crossings before choosing a component
Fully reversing the order of n parallel traces on one copper layer needs:
Crossings = n(n − 1) / 2
Each trace must exchange order with every other trace. Counting those pairs gives n(n − 1), then dividing by 2 removes the duplicate count of each pair. This is the crossing count for a full order reversal, not a claim that every connector mismatch reverses the whole strip.
| Parallel traces n | Arithmetic for full reversal | Crossings |
|---|---|---|
| 4 | 4 × (4 − 1) / 2 | 6 |
| 6 | 6 × (6 − 1) / 2 | 15 |
| 8 | 8 × (8 − 1) / 2 | 28 |
| 10 | 10 × (10 − 1) / 2 | 45 |
| 20 | 20 × (20 − 1) / 2 | 190 |
For example, the n = 8 row is 8 × (8 − 1) / 2 = 28. The table follows directly from the formula; it is not supplier production data.
This is why a flex strip that gets folded or flipped into a contact-side mismatch, or has mirrored connector pin numbering, is a layout problem, not a routing problem. Tightening trace spacing does not change the required order of the endpoints. Check both connectors as they will actually mate, including which contact faces the flex copper after installation.
Make a pin-to-pin map before routing. Review whether changing the assignment or connector orientation removes the reversal. A footprint mirror must agree with the intended contact arrangement; changing the drawing view alone does not change the connection. Count the crossings that remain after this review, then select the construction.
Zero-ohm links: the practical jumper starting point
A zero-ohm link is a resistor-format part used as a jumper. In the simple arrangement evaluated here, budget one SMT part per crossing, with a pad on each side of the crossed trace. The link bridges those pads while the other trace passes beneath its body without connecting to them. It is an assembled connection, so the bare flex drawing is only part of the release package.
A zero-ohm part is not zero resistance. It also has a rated current in the manufacturer's datasheet. Read the selected part's data; do not assume that the nominal value establishes suitability. The buying decision must identify a component that meets the circuit's current requirement, rather than leaving the assembler to choose anything described as a jumper.
Keep the part off the bend zone and support its component area with a stiffener. Each jumper introduces extra solder joints that can fail under flexing. A stiffener supports the intended static mounting area; it is not permission to place the assembly in a moving fold. Use the flex PCB stiffener guide when defining that support.
Check the footprint and crossed trace together. The jumper needs landing pads, the trace beneath needs clearance, and the coverlay openings need to match the pads. Agree these features as an assembly detail before release. The flex SMT component mounting guide provides related assembly guidance.
Wire, back access and printed bridges are different choices
These options should not be grouped together under a vague instruction to add a jumper. They change different parts of the design and require different supplier discussions.
| Option | What it provides | Decision boundary |
|---|---|---|
| Hand-soldered wire or ribbon | An added conductor across the required connection | Prototypes and very low volume only; poor repeatability and weakness under vibration or flex |
| Double-access, or back-bared, single-layer flex | Openings in the base polyimide expose the same copper from the back | Back access for a component or jumper; no crossover by itself |
| Printed dielectric patch and silver ink bridge | An insulating patch with a printed conductor crossing above it | Typical of printed or membrane PET circuits, a different technology family |
| Double-sided etched flex | Another copper layer and plated through-hole connections | Removes jumper parts, with added layer/PTH cost and stiffness |
Hand-soldered wire or ribbon can address a prototype connection, but it is not a repeatable production routing method. Its weakness under vibration and flex makes the mechanical setting part of the decision. Do not carry this choice into a production quote merely because it completed the prototype connection.
Double-access flex still has one copper layer. Openings in the base polyimide allow the same copper to be soldered from both sides. A component or jumper on the back can reach the traces through those openings, but the openings do not let copper traces cross. Ask the fab house whether it builds this construction and how it handles the openings. Specify the required access instead of assuming that single-layer flex includes it.
Printed crossovers use a dielectric insulating patch and a printed silver ink bridge. They are typical on printed or membrane PET circuits, not an etched-polyimide flex solution. Their conductivity and flex durability differ from copper, so ask for supplier data. Treat a proposal to use them as a technology choice requiring review, rather than a direct substitution for an etched copper crossing.
When to add the second copper layer
A second copper layer lets traces cross on different layers and connect through plated through-hole vias. It removes the jumper parts while adding layer/PTH cost and stiffness. Keep the vias outside the bend zone; the flex PCB via design guide covers that related design decision.
Use this quote comparison:
Total jumper cost = crossings × (part + placement + inspection)
Quoted layer difference = double-sided panel price − single-sided panel price
Put your supplier's quote numbers into both expressions. Compare on the same panel basis: the crossing count used in the jumper formula must cover the same panel represented by the board quotes. Confirm that part, placement and inspection costs are actually included before treating the result as a comparison of complete options.
The formula supports a purchasing decision; it does not establish electrical or mechanical suitability. A cheaper jumper arrangement still has to meet current requirements and keep its solder joints in a static area. Conversely, the layer price difference should come from the quoted construction, not a generic multiplier copied from another design.
As engineering judgment, a handful of crossings can justify jumpers; dozens usually justify a second layer. This is a rule of thumb, not a measured break-even point. Use the actual remaining crossings and the actual quote to decide.
If the design needs controlled impedance, differential pairs or a ground reference, pick the second layer and plan the return path. Jumper crossovers break the return path that these routes need; solving endpoint connectivity alone is insufficient. The ground-plane guide listed under References is related reading, not a prescription to hatch the reference under every signal.
Layout rules for a jumper design
Apply the following as design guidance to agree with the fabricator and assembler, not as quoted requirements from a standard.
| Drawing or layout feature | Guidance |
|---|---|
| Jumper location | Place jumpers in the static, flat, stiffened area |
| Bend routing | Keep traces perpendicular to the bend axis |
| Clearance under the body | Keep crossed-trace clearance at least the minimum spacing quoted by the fab house |
| Pad transitions | Use rounded or teardropped transitions |
| Coverlay | Keep the openings registered to the solder pads |
| Identification | Mark every jumper by designator and include it in fabrication drawing notes |
Start with the static area, then fit the jumper footprint and the crossing into it. Do not finish the copper routing first and leave the assembler to find a mounting position. If the only available location bends, revisit the pin map or layer choice. The dynamic bend life design guide is relevant when defining where movement occurs.
Use the fab house's quoted minimum spacing for the trace beneath the jumper and the adjacent pad features. Do not infer clearance from the component body outline. Review the crossing with the trace width and spacing DFM guide, then put the agreed geometry in the released layout.
The coverlay openings must register to the actual solder pads. Keep that review connected to the footprint choice and rounded or teardropped pad transitions. Refer to the coverlay opening and registration guide when communicating the pad openings to the supplier.
What to send for a comparable quote
Send a package that shows both the electrical crossing and its mechanical setting. Include the pin-to-pin map, copper layout, crossing count, jumper designators, selected part and datasheet, current requirement, bend locations, stiffener area and coverlay openings. If back access is proposed, identify the base-polyimide openings and request confirmation of the construction.
Mark every jumper on the drawing with its designator and tell the fab house in the fabrication drawing notes. Follow the flex PCB fabrication drawing guide to keep the connection, bend and coverlay information together. A note saying jumper required leaves too much of the construction undefined.
Request the single-sided and double-sided panel prices through the flex PCB service, and identify the jumper part, placement and inspection scope for flex assembly. Ask for a comparison covering the same panel and order, with the assembly content explicit. This gives the cost formula usable inputs while keeping the mechanical and current checks visible.
References
- Zero-ohm link — concept source for a resistor-format jumper connecting PCB traces.
- IPC-2223 and IPC-6013 — flex design and qualification of flex boards, respectively; check the current revision. The layout guidance above is not a quotation of their clauses.
- Related reading: Hatched ground plane design for flex PCB — reference-plane design context when electrical requirements lead to an additional copper layer.
FAQ
Can a single-sided flex have crossing traces?
Yes, with a jumper providing the crossing connection while the copper remains on one layer. Check pin assignments and connector orientation first. Double-access openings expose the same copper from the back; they do not create a crossover by themselves.
Is a 0 ohm resistor safe as a jumper on a flex PCB?
It can be suitable if its datasheet current rating meets the circuit requirement and it sits in a static, stiffened area. Its resistance is not literally zero. The extra solder joints can fail under flexing, so component selection and placement both matter.
How many crossovers before I should go double-sided?
There is no universal count. Compare crossings × (part + placement + inspection) with the quoted panel price difference. A handful can justify jumpers and dozens usually justify another layer, as engineering judgment. Controlled impedance, differential pairs or a ground reference favor the second layer regardless of that cost comparison.
Can I put a jumper in the bend area?
Keep it out of the bend area. Put the jumper in a static, flat, stiffened section, with traces perpendicular to the bend axis. If you add another copper layer instead, keep the plated through-hole vias out of the bend zone too.
What should I send the supplier to quote a jumper design?
Send the pin map, copper layout, crossing count, jumper designators, selected part and datasheet, current requirement, bend locations, stiffener area and coverlay openings. Identify any back-access openings. Request part, placement and inspection costs alongside comparable single-sided and double-sided panel quotes.