I am using a Linear Technologies LT-1534 part an need to create a planar PCB surface inductor with the specific value of 28nH; i.e., the inductor will be a copper trace on the PC boards Top Surface to have a value equal to a discrete inductive component, that value to equal 28 nano Henries +/- 10%.

What formula should I use to calculate the Planar Inductor's geometry that will enable me to achieve this specific value?

The PCB's layer stack up is a 4-layer board with Top & Bottom Signal Layers, Components on Top only, with Ground Plane and Power(s) Plane on Layers 2 & 3 respectively.

The system is powered by a LiPo battery.

I have designed Printed wiring boards for many years (over 30) and have done Multi-layer Planar Transformers before, but have not had such a specific inductor value on a single layer come up as a requirement before and am a little stumped as to where to start.

The circuit goal is to design a local RCL filter for the LT1534, where the capacitive and resistive elements are comprised of discrete passive leaded components, but because of size constraints as well as the small value of inductance required, the design engineer feels that the goal would be better achieved using a Planar inductor, rather than a discrete, even surface-mount component element.

The target PCB material is [email protected]" thickness, one-ounce clad to between 1 1/2-2 oz finished, to be determined by other targeted trace impedances and controlled impedance transmission line requirements.

Please let me know if more specific information is required to make an educated reply, or if a schematic of the sub-circuit which contains the inductor in question is needed to make a proper assessment of the formulas required for the PCB inductance to be specified.

  • \$\begingroup\$ Sorry to get your hopes up by generating a notification, but do you have any information on how to design less accurate PCB inductors and transformers? \$\endgroup\$ Commented May 28, 2014 at 8:49
  • \$\begingroup\$ 28 nano henries for a 250kHz switcher? Are you absolutely sure you have calculated this correctly? Oh I see - it has nothing to do with the linear tech device (so why did you mention it?) - it's for a filter and presumably this is on the input or output? Methinks the design engineer you mention is not giving out the full story - get him to say why he believes a planar is required and while you are at it post a schematic please. \$\endgroup\$
    – Andy aka
    Commented May 28, 2014 at 8:51
  • \$\begingroup\$ You won't be able to get anywhere near 10% tolerance on a PCB trace inductor unless you make absolutely sure nothing ferromagnetic can come close (<1" in any direction). Otherwise you are just making an air core inductor, for which there are many online calculators: daycounter.com/Calculators/Air-Core-Inductor-Calculator.phtml \$\endgroup\$
    – user36129
    Commented May 28, 2014 at 9:30
  • \$\begingroup\$ (Especially) if it's air-core, not just ferromagnetic stuff in proximity, but anything that couples as a shorted turn (like nearby copper) will reduce the inductance. There may also be EMI issues as a result. Really small inductances (< 1nH) can be made with microstrip, but this is not that small. \$\endgroup\$ Commented May 28, 2014 at 13:02
  • 1
    \$\begingroup\$ PS, in my world, this would be a pretty inappropriate thing to drop on the layout guy/gal - go design a component with tolerances!. How wet behind the ears is this engineer? You can get very inaccurate results from online calculators (plus tolerances) and you should not take the fall if it doesn't work out. Suggest you get dimensions and tolerances that can be supported by the PCB fab from the designer. \$\endgroup\$ Commented May 28, 2014 at 13:19

1 Answer 1


I love to use the Saturn PCB toolkit for this kind of calculations nightmare. It does everything ! (except the coffee.)

Try it. For your inductor (28nH) I get roughly

  • 3 turns
  • 0.2mm conductor spacing
  • 0.2mm conductor width
  • 3.320mm outer diameter
  • 1.320mm inner diameter


I tried to play a little bit with conductors width and spacing value, and from what I see the inductor will not be that sensible to manufacturing defect. For example, reducing the trace width to 0.14mm and raising the spacing to 0.32mm still gives a 26.1nH impedance, which is 'in tolerance'.

But, these kind of components are like PCB antennas and should be tweaked. You can add additional 'feeding' traces to the "prototypes designs" around the first spires and cut them until you come close to the required value (best RLC Q), or scratch the soldermask and solder a wire, or...

Keep in mind planar inductors are cheap in the long run (for big series of cheap product) but cost a lot of time during design due to tuning nightmare and tolerances checking craziness.

But imho it's doable !


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.