Is There a PCB Trace Inductance Rule of Thumb?
PCB traces have inductance and capacitance, which collectively help determine the impedance of a trace.
Sometimes, it’s helpful to understand the inductance of a trace so that you can get an estimate of coupling due to crosstalk.
While there is no set value of trace inductance you should use, it can be a helpful tool for understanding signal behavior in some systems.
Do you know the inductance of these traces?
All PCB traces have some inductance, but do you know how the inductance in a PCB trace affects electrical behavior? Different conductor systems in a PCB need to have particular trace widths, which will determine the inductance of the trace. However, there is no specific PCB trace inductance rule of thumb, there are only formulas related to the trace impedance that can be used to determine the trace inductance. In addition, there is no specific rule about what trace inductance you need to use as a design goal for your board.
With an understanding of the important factors determining the input impedance of a trace, it’s much easier to understand when it’s appropriate to violate impedance goals and opt for a higher or lower trace impedance in your circuit board.
A PCB Trace Inductance Rule of Thumb
Trace width calculations in transmission line design always start from the perspective of stackup design and selecting a transmission line geometry. Other systems, like power converters, may not need controlled impedance along a trace, so they will typically use much larger copper with low inductance. The way to calculate the inductance is to first calculate impedance, and then use the impedance to calculate the trace inductance.
The bare minimum impedance model used in the PCB industry is the formulas in the IPC-2141 standard. The IPC-2141 impedance equations shown below for microstrips and striplines are based on experimental observations and are reasonably accurate below ~1 GHz.
IPC-2141 trace impedance equations for microstrips and striplines
One can show that the above equations are not perfectly accurate, as they include some assumptions that aren’t always true. In particular, the above equations are deficient in the following ways:
- Loss tangent is omitted: All PCB laminates have some attenuation, which is quantified using the loss tangent. The loss tangent always modifies the trace impedance slightly by adding some reactance.
- Copper roughness: The skin effect and copper roughness are lumped into the above equations and cannot be separated without a more sophisticated method (see this IEEE model for an example), so the above equations are not accurate for every fabrication process and material system.
Although the above equations aren’t perfect, they give a decent starting point for calculating trace impedance that covers many possible cases in PCB design.
Calculating the Inductance From Impedance
After designing the trace width to hit an impedance goal, the trace will have a specific inductance. The design process generally does not proceed in reverse except in cases involving low-speed digital signals, low-frequency analog signals, or switching power converters that have a specific low inductance requirement. If the trace is electrically short, then you can violate the typical 50 Ohm impedance goal and design with lower trace inductance.
All this means that there is no PCB trace inductance rule of thumb. In other words, there is no specific trace inductance you should use, and there is no simple formula that gives you a PCB trace inductance for every PCB.
To see how this arises, we can again turn to the IPC-2141 equations and the constitutive impedance relation for a lossless transmission line. The IPC-2141 equations provide a capacitance per unit length equation that can be used to calculate the PCB trace inductance.
Microstrip and stripline capacitance
The trace capacitance is defined with respect to the nearest ground plane in the particular configuration presented above. Finally, we have two equations for the inductance of microstrip and stripline traces.
Microstrip and stripline inductance
From this result, we see that the trace inductance depends on:
- Trace thickness (or copper weight)
- Layer thickness
- Trace geometry
These factors all have to be considered together to ensure the design meets impedance goals while also determining the inductance. Generally, when calculating the inductance, we have a fixed layer thickness (H or B) and copper weight (T), and the trace width is determined in order to meet impedance and/or routing density goals. If you design a trace on one stackup with a specific laminate material, it will not have the same inductance or impedance if the same trace is placed in a different PCB stackup with different dielectric materials. If you like, you can compare inductance vs. width curves for various layer stacks.
Where the PCB Trace Inductance Rule Breaks Down
Since the above equations are logarithmic, they are only valid above a certain range of values for the geometric parameters. Whenever the argument in the above logarithms is less than 1, the result will be negative inductance. By rewriting the argument in the logarithm in terms of the ratios (W/H) or (W/B), and (T/H) or (T/B), we arrive at the following inequality that restricts the allowed trace geometry in the above formulas:
Microstrip and stripline geometry limits in order for the IPC-2141 inductance to be non-negative
Just as an example, we can look at a simple PCB stackup with impedance control to see the microstrip inductance. For a 0.5 oz./sq. ft. copper trace on a 4-layer board with 8 mil thick dielectric and Dk = 4.2, the resulting trace width required for 50 Ohm impedance would be 15.15 mil, and the inductance would be 6.679 nH/inch. Other models will give wildly different results, which should illustrate the inadequacy of IPC-2141.
Instead of using outdated IPC-2141 formulas, there are better approaches for determining the impedance and inductance of your traces. The best PCB stackup and trace calculators will include a method of moments field solver or boundary element method field solver. These tools can be used to quickly calculate the PCB trace inductance in your board for a given stackup and impedance target. This value can then be used to determine some rough crosstalk results. Some very sensitive precision measurement designs or power converters require very low inductance routing, and these calculations can be used as a check against.
Cadence’s PCB design and analysis software can be used to validate any PCB trace inductance rule of thumb as you evaluate advanced electronics designs. Designers can use a powerful field solver and circuit modeling tools to simulate electrical behavior and calculate many important signal integrity metrics. When you use Cadence’s software suite, you’ll also have access to a range of simulation features you can use in signal integrity analysis, giving you everything you need to evaluate your system’s functionality.
Subscribe to our newsletter for the latest updates. If you’re looking to learn more about how Cadence has the solution for you, talk to us and our team of experts.