Thank you for your interest in our webinar on transmission lines and controlled impedance. It will be presented by Amit Bahl and Brian Walker of Copper Mountain Technologies.
Missed the webinar? Watch the recording below!
You can ask your questions on this thread.
Are these PCB techniques applicable when using modulation frequencies in the range of 50-400 MHz?
Yes, these PCB techniques apply to modulation frequencies ranging from 50 to 400 MHz. Register for the webinar to learn more about designing transmission lines.
Thanks! I’m registered and ready for the event.
Watch the webinar recording here!
Here are the questions we got during the webinar:
| Question | Answer |
|---|---|
| Why does the calculator not include an option for a coplanar? | The Impedance Calculator does include an option for a coplanar waveguide. |
| Has the calculator’s result been correlated with measured data? How accurate are the calculator’s results? | Yes, the calculator’s results have been correlated with measured data. The results are usually within ±10% and often within ±5%. The accuracy is comparable to industry-leading characteristic impedance calculators such as Polar and HyperLynx. |
| How does conformal coating impact insertion loss? | Conformal coating increases insertion loss because all coating materials have a loss tangent, contributing to signal attenuation. |
| With ENIG finish, how does nickel loss compare with solder mask loss? | With an ENIG finish, solder mask loss is significantly higher than nickel loss. |
| What formulas have been used in those calculators? Most come from empirical equations; often, there are boundaries for w/h (width vs. dielectric to the reference plane). | Our impedance calculator does not rely on empirical formulas. Instead, it utilizes 2D numerical solutions derived from Maxwell’s equations, ensuring highly accurate results. These results are comparable to those from industry-standard impedance calculators |
| Once the characteristic impedance has been determined for a given transmission line profile, does the calculator provide effective Dk and attenuation (dB/length) as a function of frequency? | The calculator determines the effective dielectric constant (Dk) under the assumption of lossless impedance, so it is not frequency-dependent. However, attenuation (dB/length) is frequency-dependent and is calculated only at the specific frequency you input. Currently, the tool does not support plotting attenuation as a function of frequency. |
| We put a thermal pad on top of the PCB to maintain the board temperature. How does this affect the high-speed signal integrity? | The impact of a thermal pad on high-speed signal integrity depends on its placement relative to the signal lines. Since the thermal pad is a vertical structure, it typically does not affect signal integrity as long as there is a continuous ground plane beneath the signal traces, covering them adequately on both sides. In such cases, the thermal pad should have minimal impact. |
| Does the edge of a square wave signal change during transmission over an electrically long line? | Yes, the edge of a square wave signal does change during transmission over an electrically long line. This happens because a square wave consists of multiple high-frequency components, which can be affected by the transmission medium. As the signal propagates, the sharp transitions of the square wave can become smoothed out, leading to a rise time and fall time instead of the ideal sharp edges. In practice, achieving perfectly sharp edges in a high-frequency waveform is very difficult due to these effects, and some amount of ringing and other distortions can occur along the way. Therefore, high-frequency waveforms typically do not have perfectly sharp edges. |
| Which is preferable—a 50-ohm output and a 50-ohm line or a 25-ohm output and a 25-ohm line? | The preferred choice is usually a 50-ohm output and a 50-ohm line. 50 ohms is the industry standard, and most devices and communication protocols are designed to work with this impedance. Using a 50-ohm configuration ensures better compatibility and minimizes signal reflection or loss. A 25-ohm output and line are less standard and typically used in specific applications requiring different impedance matching. It would require more trace width compared to a 50-ohm output. |
| Should the via fence be spaced 1/4 of the wavelength? Since the idea is to stop the field and guide the wave, the via spacing depends on the frequency of operation. | The spacing of the via fence doesn’t necessarily need to be 1/4 of the wavelength, but it should be chosen based on the frequency of operation. A good general guideline would be to use a via spacing of around λ/8 or λ/10. |
| In the time-domain trace, why is the right-hand side impedance not 50 ohms? | The right-hand side impedance is not 50 ohms in the time-domain trace because one measurement shows the characteristic impedance while the other displays the return loss. In one case, you’re observing the return loss in dB, which reflects how much of the signal is reflected due to impedance mismatches. In the other case, you see the signal’s conversion to 50 ohms. These are different ways of representing similar information but focus on various aspects of the signal’s behavior. |
| When could we use the port extension to move the point of the reference plane to please when we will measure? | The port extension moves the reference plane to a desired point, correcting the phase and adjusting the delay so that the zero phase or zero time is at your desired location. It works by shifting the reference plane but does not address reflections between the original and new ones. For instance, if reflections are in a cable or pigtail, the port extension will not remove them, meaning the return loss could still be poor. Port extension assumes a constant delay across frequencies, which only works effectively for situations with uniform delay. If there’s any dispersion or variation in delay, such as over a wide frequency range, the results can become inaccurate, often leading to distorted or inconsistent readings. In contrast, de-embedding provides more accurate results by accounting for reflections and removing loss factors. It gives a more precise response without artifacts like arcs or squiggles. De-embedding is more reliable for precise measurements and calibration, especially when dealing with components that have non-uniform delay characteristics. |
| Have you used the TDR to check the impedances of vias? I am interested in (and concerned about) the change in dielectric constant in the Z direction from that for the X and Y directions and how this needs to be taken into account in computing via structures. | Yes, the TDR can be used to check the impedance of vias. You can check Sierra CircuitsVia Impedance Calculator that can help analyze via structures. The dielectric constant in the Z direction, which is the direction of the via, can indeed be different from the X and Y directions, and this needs to be considered when designing via structures. Ideally, the via impedance should be as close as possible to the line’s characteristic impedance, such as 50 ohms, to maintain signal integrity. While it may not be feasible to match the impedance exactly, the closer you can get, the better the performance will be. However, vias introduce impedance discontinuities at both the entry and exit points, which can cause signal reflections. The impact of these discontinuities depends on the signal’s frequency and data transfer rates. If the signal frequencies are not too high, these discontinuities might have a minimal effect on signal integrity and can be ignored. However, at higher frequencies (e.g., 20 GHz and above), these effects can become more significant, and careful attention should be paid to the design of the vias to minimize their impact. |
| Where can I find practical techniques for connecting VNA ports to traces designed with various impedances on a production PCB that needs troubleshooting? | Several resources offer practical techniques for connecting VNA ports to traces with various impedances. The Southwest Microwave website has excellent papers on in-launch connectors and related topics. Additionally, Copper Mountain Technologies offers fixture creation papers. You can find them on their website. |
| Is there any concern about reflection and EMI at frequencies below 300 Hz? | At frequencies below 300 Hz, reflection and electromagnetic interference (EMI) are generally minimal. This is because the wavelength at such low frequencies is extremely large. Practically, 300 Hz behaves almost like DC for most applications, which means issues like reflection and EMI are negligible. |
| For the time domain analysis, did you have to select the time amount manually, or does the VNA select it automatically based on the frequency sweep? | The VNA doesn’t automatically select the time range for time domain analysis based on the frequency sweep. Instead, I had to set it up manually. The VNA typically displays zero in the center of the time axis, with negative time on the left and positive time on the right. |
| Brian, was there any reason you used the trace calculator vs the fixture simulator during the diff pair measurement? | Yes, I used the trace calculator instead of the fixture simulator. This is because the fixture simulator is only available on our 4-port VNAs, which wasn’t an option since I was working with a 2-port VNA. Typically, a 4-port VNA is necessary for differential measurements because you need to analyze both sides of the differential pair, which the fixture simulator is designed to handle. |
| What cad PCB software design do you typically recommend? | For PCB design software, we typically recommend Allegro and Altium. These are two of the industry’s most popular and widely used tools, especially among professionals. Allegro is favored in many professional settings, while Altium is highly popular, especially in the United States. KiCad has also been gaining traction because it’s free and accessible, but for professional-grade work, Allegro and Altium remain the top choices. |
| I’m working on a CPW transmission line in the silicon substrate, with 3-layer Si, Sio2, and metal layers as trace lines. However, I cannot find the correct dimension of the trace with and gap and ground width. Pls suggest how I can find. | The challenge might stem from the fact that most impedance calculators rely on the wheeler formulas, which can break down when dealing with extreme or non-standard mechanical dimensions. For a complex structure like a CPW transmission line on a silicon substrate with multiple layers (Si, SiO₂, and metal), I recommend using a planar electromagnetic (EM) simulation tool such as CST or Ansys. These tools can more accurately handle the intricacies of your design. |
| For the time domain trick that was mentioned, I understand the Software mirrors the frequency domain for the negative frequencies. Do you just interpolate the DC and then perform the IFFT, or do you leave it out and use the actually measured and mirrored data in the IFFT? | The DC term is not interpolated or left out for the time domain. Instead, it must be explicitly defined. For example, if the measurement is an open circuit, the DC term is 1 + j0. If it’s a short circuit, it’s set to -1 + j0. You must determine the appropriate DC term for other cases based on the specific scenario. You can manually input this DC term or let the vector network analyzer (VNA) determine it automatically. This step is crucial for accurate time-domain analysis using the IFFT. |