PCB Trace Inductance and Width: How Wide is Too Wide?

Zachariah Peterson
|  Created: April 5, 2020  |  Updated: January 3, 2023
PCB Trace Inductance and Width: How Wide is Too Wide?

Not all design rules are applicable in every situation, and they are often communicated without context. One particular rule for sizing traces is to always opt for wider traces when possible. Unlike many rules of thumb I’ve seen thrown about, this particular trace rule has some merit. However, when you need to control trace impedance and simultaneously reduce ringing, you need to carefully control the trace width to ensure transmission lines have desired impedance within some particular tolerance. Let’s take a look at the basic formulas for sizing traces and how to keep impedance within your tolerance range.

Impedance vs. Trace Width Formulas

I’ve brought up this point in previous articles specifically for surface microstrips and symmetric stripline traces. or microstrip traces, the IPC-2141 formulas are only highly accurate within a particular impedance range. You should use the more accurate Waddell's equations for determining the impedance of microstrip traces:

Microstrip trace geometry


PCB trace inductance and impedance from Hartley’s equations
Microstrip trace geometry, Waddell’s equations for microstrip impedance, and effective dielectric constant of microstrip traces


Similar equations have been developed for symmetric striplines, embedded microstrips, coplanar waveguides, and offset/asymmetric striplines. For now, I’ll confine the discussion to microstrips, but you can follow the process I’ll outline here for other trace geometries. Note that the above equation applies for single-ended surface microstrips that are isolated from all other signal traces.

What I’ll do now is use the above equations to determine the correct w value that provides minimum trace inductance per unit length for a specified trace impedance value. This need to minimize per-unit-length inductance is quite important, as the damping constant for any transient ringing signal (note that we’re not talking about reflections here) is inversely proportional to the PCB trace inductance. 

Controlling PCB Trace Inductance and Impedance

If you look at the above equations, you’ll find that there are three important geometric parameters to consider when sizing traces and PCB trace inductance. In a real board, you’ll have some constraints on the value of h, which will depend on the board and layer thicknesses. You’ll also be limited in terms of trace thickness, which is proportional to the copper weight you use for your board. This means you can use the above equations in an optimization problem while taking the layer thickness and copper weight in your board as constraints.

Here, the important parameter to determine is (w/h) for a given value of (t/h), substrate dielectric constant, and desired impedance value. There is an infinite number of pairs of these values that will solve the characteristic impedance equation. If you want to provide the greatest level of damping for transient ringing, then you need to determine the value of (w/h) that minimizes the inductance per unit length. This can be reframed as a problem of minimizing the effective dielectric constant for a given (t/h) value, substrate dielectric constant, and desired impedance value. The inductance per unit length, capacitance per unit length, substrate dielectric constant, and impedance are related as follows:

PCB trace inductance and capacitance
Trace inductance and capacitance per unit length in terms of impedance and signal velocity.


You could certainly attempt to do this graphically or through successive manual calculations. If you try to do this by calculating critical points from derivatives, you’ll end up with a set of products of transcendental equations (one piecewise and one continuous!) that must be solved numerically for various values of (t/h) and Dk. While this is a solvable problem in principle, it is clearly intractable due to the nonlinear piecewise nature of the effective dielectric constant and the fact that there are three relevant geometric parameters.

The best option to solve this type of problem is to use an iterative optimization algorithm to determine the values of (w/h) and (t/h) that minimize the PCB trace inductance per unit length. This type of problem can be easily solved with a gradient descent algorithm, an evolutionary algorithm, the Kuhn-Tucker method, or another nonlinear optimization algorithm. This allows you to define practical upper and lower limits on the value of (w/h). You can also set limits on the value of (t/h) and use this ratio as an optimization variable if you like.

Thankfully, this problem is simple enough to solve with the Solver tool in Excel. I’ve created a simple spreadsheet that solves the following minimization problem with Waddell’s equations and the inductance equation. In the following equation, a and b are constants that define practical maximum values of (w/h) and (t/h), respectively; these can be chosen by the designer:

PCB trace inductance optimization problem
Optimization problem for determining the maximum trace width for a given impedance, trace thickness, and distance from the ground plane.


Here, the goal is to determine the values of (w/h) and (t/h) that minimize L (defined above) while holding the trace impedance constant. If you like, you can set a specific value of t from the copper weight, and the value of h can be chosen by the designer for a given t value (layer thickness).

Example 1: Varying Copper Weight and Layer Thickness

In this first example, I’m going to allow the copper weight and layer thickness (i.e., the value of the ratio (t/h)) to be an optimization variable. The substrate dielectric constant is Dk = 4. For the constraints listed above, I’ve chosen a = 5 and b = 2. For my results, I find that the minimum inductance is 290 nH per meter when (w/h) = 1.572332 and (t/h) = 1.213156.

PCB trace inductance optimization results in example 1

Optimization results for example 1.

In interpreting the results, it should be obvious that the trace width cannot be increased forever without changing the trace impedance; there is clearly some optimum trace width that optimizes the transmission line. The designer has one remaining parameter that needs to be chosen: the layer thickness h. Once this is chosen by the designer, the values of w and t can be easily determined from the calculated ratios listed above.

Example 2: 1 oz/sq. ft. Copper Weight, 4 Layer Board

This example shows a more practical situation. I’ve run the above optimization problem for a board with 1 oz/sq. ft. copper weight (trace thickness t = 0.035 mm) and a standard 4 layer board with equal-sized layers (h = 0.393 mm) with real dielectric constant Dk = 4. Because I’ve chosen the values of t and h, the ratio (t/h) is no longer an optimization variable as (t/h) = 0.089172. For the constraint on (w/h), I’ve chosen a = 5. For my results, I find that the minimum inductance is 292 nH per meter when (w/h) = 1.92445. Since my layer thickness is 0.393 mm, the required trace width for this particular inductance value is w = 0.7563 mm (~30 mils).

PCB trace inductance optimization results in example 2
Optimization results for example 2.


Just as a sanity check, we can quickly calculate the total inductance of a trace determined with this method and compare it with typical values. The inductance of a ~1 in. trace is typically quoted as being 5 to 10 nH. For the optimized trace I’ve designed with this model, the total inductance for a length of 1 in. is 7.4168 nH, which is within the range normally measured for small PCB traces. In addition, if you look at the IPC 2152 nomograph, you can immediately use these results to determine the temperature rise for a given current in this trace.

If you’re interested in getting a copy of this spreadsheet, send a request to contact@nwengineeringllc.com. The built-in evolutionary optimization algorithm in Excel takes a significant amount of time to converge, although it will give slightly more accurate results than the built-in GRG nonlinear algorithm. One can easily adapt this method for other trace geometries and obtain similar results.

Does it Need to Be Exact?

The simple answer is "no," your width does not have to be exact. The level of accuracy you need depends on the allowed characteristic impedance deviation in your particular signaling standard or interconnect design. Turning this around, it also depends on the Dk excursion you can accept from your manufacturer. The above methodology assumes a Dk value and does not apply a tolerance on impedance, but if your manufacturer does not have a specific Dk value material available, you may have to accept a different Dk value in your layer stack.

To deal with this issue, you can take two possible approaches:

  1. Cycle through a possible range of Dk values, and determine a minimum and maximum width for your Dk range.
  2. Set upper and lower values for acceptable impedance, and run the optimizer for each to get an acceptable trace width range.

This analysis is important to ensure that you can produce your board with a sufficiently wide range of materials and at a broad range of fabricators. If you know your width and Dk tolerances ahead of fabrication, you will be able to quickly evaluate fabrication suggestions from fabricators should they try to change your stackup.

The routing and impedance calculation tools in Altium Designer® can help you maintain the right PCB trace inductance and widths you need, thanks to the built-in field solver in the Layer Stack Manager. This set of tools interfaces directly with your routing features and design rules, ensuring you can maintain consistent impedance while satisfying trace width constraints throughout your board. You’ll also have access to a variety of length/delay tuning features for high speed designs.

Now you can download a free trial of Altium Designer and learn more about the industry’s best layout, simulation, and production planning tools. Talk to an Altium expert today to learn more.

About Author

About Author

Zachariah Peterson has an extensive technical background in academia and industry. He currently provides research, design, and marketing services to companies in the electronics industry. Prior to working in the PCB industry, he taught at Portland State University and conducted research on random laser theory, materials, and stability. His background in scientific research spans topics in nanoparticle lasers, electronic and optoelectronic semiconductor devices, environmental sensors, and stochastics. His work has been published in over a dozen peer-reviewed journals and conference proceedings, and he has written 2500+ technical articles on PCB design for a number of companies. He is a member of IEEE Photonics Society, IEEE Electronics Packaging Society, American Physical Society, and the Printed Circuit Engineering Association (PCEA). He previously served as a voting member on the INCITS Quantum Computing Technical Advisory Committee working on technical standards for quantum electronics, and he currently serves on the IEEE P3186 Working Group focused on Port Interface Representing Photonic Signals Using SPICE-class Circuit Simulators.

Related Resources

Related Technical Documentation

Back to Home
Thank you, you are now subscribed to updates.