Flex PCBs

Pricing

$15 per square inch, which includes three copies of your design. For example, a 2 square inch board would cost $30 and you’d get three copies of your board. You can order as many copies as you want, as long as they’re in multiples of three.

Turn Times

Orders will be sent to fabrication weekly, and ship within 21 calendar days of ordering.

You can get a quote, approve a design, and pay for an order at OSH Park.

Fabrication Specs

Flex PCB Specs

Quick Specs

  • 6 mil (0.1524mm) minimum trace width
  • 6 mil (0.1524mm) minimum trace spacing
  • 10 mil (0.2540mm) minimum drill
  • 20 mil (0.508mm) minimum drill slot
  • 5 mil (0.127mm) annular ring
  • Flexible core of 3mil (0.0762mm) polyimide.
  • 1oz copper on both sides (1.4mil, 35um)

Detailed Specs

  • ENIG (gold) finish for superior soldering and environmental resistance.
  • Solder resist and silkscreen on both sides.
  • Minimum 15 mil (0.3810mm) keepout distance from traces to the board edge.
  • PCB substrate is compatible with a lead-free process.
  • The boards themselves are also lead free and RoHS compliant.
  • Polyimide Substrate dielectric constant of 3.4 at 1 MHz.
  • Minimum 4 mil (0.1016mm) soldermask web.
  • Maximum soldermask expansion, retraction, or shift is 3mil (0.0762mm).
  • Manufactured in the United States.
  • Drill slots are supported from most tools, when used in typical ways. See our Slots page for detailed information.
  • Board edges and cutouts are laser-milled with a 1 mil (0.0254mm) kerf, and 5 mil (0.127mm) positional tolerance.
  • 15 mil (0.381mm) recommended copper to board edges and cutouts. Copper violating this spec may be damaged during fabrication or shipping.
  • 6 mil (0.1524mm) required copper to board edges and cutouts. Copper violating this spec will be removed prior to fabrication.
  • Minimum 68 mil (1.7272mm) width on internal cutouts. See our [Outline][outline] page for detailed information.
  • Castellations are not supported, and will be removed or fabricated with extremely high failure rates.

2 Layer Stackup

Layer Thickness Tolerance
Silkscreen    
Soldermask 1mil (0.0254mm) +/-0.2mil (0.00508mm)
Top Copper 1oz (1.4mil, 35um)  
Polyimide Flexible Substrate 3mil (0.0762mm) +-0.3mil (0.0076mm
Bottom Copper 1oz (1.4mil, 35um)  
Soldermask 1mil (0.0254mm) +/-0.2mil (0.00508mm)
Silkscreen    

2 layer Drill Specs

  • Minimum 10 mil (0.2540mm) drills with 5 mil (0.1270mm) annular rings.
  • Minimum 20 mil (0.508mm) drill slot slot size
  • Maximum plated hole size is 265 mils (6.7310mm). Unplated holes do not have a maximum size.

FAQ

Why isn’t it purple?

We tried! Coloring the mask results in it being too brittle, and it would crack when bent. Since this negatively impacts the performance and longevity of the boards, we opted for clear mask.

Why aren’t you using coverlay?

Cost, precision, and overall process robustness.

Mask can be used as-submitted, without any additional considerations. This is ideal for customers used to typical pcb processes, and doesn’t require design or library changes to switch to a Flex pcb.

Coverlay requires a number of additional design considerations to avoid manufacturing issues. Since most of our customers do not have design tools that can check for coverlay-specific issues, it would generate a lot of surprising fabrication issues and/or silent changes. We’d prefer to avoid both of these.

What’s the minimum width of a flex strip?

Pending.

What’s the minimum bend radius?

This is design and application specific: We recommend reading flex design guidelines before planning any sharp bends, and accounting for each bend individually.

These table should help as a rough guideline to check your calculations. Due to the application specific nature of actual bending, we can make no warranty about correctness.

The bend radius depends on the board thickness of all layers passing through the bend. Multiplying the total thickness by the appropriate “bend ratio” then generates the expected bend radius. See our stackup for details on layer thicknesses. For simplicity, the following calculations include mask on both sides, and the number of copper layers listed.

A “static” bend is intended to be bent into shape and mounted, and is not intended to be bent from that point onward.

Copper Layers in bend Conservative static bend Agressive static bend
1 10:1 ratio, 64mil (1.6256) 6:1 ratio, 38mil (0.9652mm)
2 20:1 ratio, 150mil (3.81mm) 12:1 ratio, 93mil (2.3622mm)

A “dynamic” bend will have a bend/straighten cycle during normal operation. Estimating the “dynamic” bend radius is more complicated, and rough guidelines are harder to define. We recommend simply making dynamic bends as large as your application will allow to minimize wear. Sharper dynamic bends will result in decreasing the number of bends a PCB can survive prior to failure.

Copper Layers in bend Aggressive dynamic bend
1 10:1 ratio, 64mil (1.6256)
2 20:1 ratio, 150mil (3.81mm)

Note, due to the use of soldermask instead of coverlay, our Flex PCBs are not well suited for use in applications where dynamic bends are used for operationally critical systems, such as medical and industrial.

What about stiffener layers?

Currently, stiffener layers are not available due to the complexity of our panels making it nearly impossible to properly fab them.

We’re investigating ways to handle this, so it may be an option later.

Will it fit <part number here> connector?

Probably! Check our stackup, and compare it to the datasheet for your component. There’s several common thicknesses connectors expect, and this is one of them.

If we’re missing information needed to verify your component, please email us at [email protected].

Seriously though? No purple?

We know. It pains us too.

Questions? Feedback? Suggestions?

Please send them to [email protected]