FEDEVEL
Platform forum

Karan paliwal , 05-31-2026, 05:52 AM

Subject: Query on Differential Pair Impedance Profiles

Hi @Robert Feranec

I was reviewing the iMX6 Rex PCB and noticed that separate differential pair routing rule have been created for 90Ω and 100Ω impedance.

I was trying to understand why the impedance profile was not defined using Altium's built-in impedance profile functionality. My understanding is that the differential pair width and spacing values were probably calculated using an external impedance calculator.

I have also seen several other PCB projects where designers prefer external impedance calculators instead of Altium's impedance profile feature.

Could you please explain why the Altium impedance profile option was not used in these designs and what advantages the external calculation method provides?

Thanks.


Thanks.

, 05-31-2026, 05:53 AM

🤖 In the meantime, here’s a response from the [FEDEVEL AI HW Assistant]().
It helps to find relevant resources for your question, but it may make mistakes as it’s still in early development.

This is the response from the AI Assistant:
The preference for external impedance calculators over Altium's built-in impedance profiles comes down to three key factors: manufacturer collaboration, practical accuracy, and workflow efficiency. Here's the detailed breakdown:

1. **Manufacturer-Specific Requirements**
PCB manufacturers often provide exact impedance parameters based on their production capabilities and material stock. As shown in the iMX6 Rex example, designers typically use values calculated by the fab house using their preferred tools ([Example calculation with JLCPCB's stackup](https://www.youtube.com/watch?v=KWIzhbQaZZk&t=19510)). This avoids mismatches between Altium's theoretical models and the manufacturer's actual process.

2. **Simplified Rule Setup**
External calculators (like Saturn PCB or manufacturer tools) give direct width/gap numbers that designers input as fixed rules. This avoids Altium's layer-by-layer impedance profile configuration, which requires detailed knowledge of dielectric constants and stackup behavior. For example, USB 2.0's 90Ω pairs are often implemented with fixed 6mil/8mil rules rather than dynamic profiles ([USB impedance rule setup](https://www.youtube.com/watch?v=KWIzhbQaZZk&t=19695)).

3. **Tolerance Handling**
Real-world impedance varies ±10% due to manufacturing tolerances. External calculations account for this upfront by providing conservative width/gap values, while Altium's profiles might give a false sense of precision.

, 05-31-2026, 05:53 AM

As noted in a PCIe example, even 108Ω measured impedance still works fine despite being "out of spec" ([Impedance tolerance discussion](https://www.youtube.com/watch?v=fJCRrEf_IH8&t=1900)).

**When Altium's Profiles Shine**
The built-in tool becomes useful when:
- Prototyping with unknown manufacturers
- Exploring stackup tradeoffs early in design
- Working with tightly coupled pairs requiring EM-field-aware calculations

Most experienced designers reserve Altium's impedance profiles for initial exploration, then switch to manufacturer-validated external numbers for production ([Impedance strategy comparison](https://www.youtube.com/watch?v=nshfdrw9lbc&t=3457)).

You can continue chatting with the AI Assistant here:
https://fedevel.com/hw-assistant

QDrives , 05-31-2026, 01:11 PM

Probably at the time when it was designed, Altium did not have the impedance profiles.
You cannot use what does not exists.

Robert Feranec , 05-31-2026, 01:30 PM

@QDrives is correct that feature did not exists. But I don't use them anyway - simple reason: if you thigh up your PCB layout to a specific stackup it is hard to move production between different PCB manufacturers. For example if different PCB manufacturer needs to use different materials and if that would mean that to achieve specific impedance manufacturer would have to make your tracks a little bit wider - often that is not possible. Hover it is easy to make your tracks narrower ... so I always route my PCB with wider tracks as needed and then when you finish your design you select all the tracks and make them narrower based on requirements from specific PCB manufacturer. This way I can easily move my PCB between different PCB manufacturers.

Karan paliwal , 06-03-2026, 03:41 AM

@QDrives @Robert Feranec Thanks for the explanation.

However, I have one doubt. Altium provides impedance calculation and impedance profile features, so there must be some practical way to manage this situation.

For example, if I design a PCB based on one manufacturer's stackup and later decide to switch to another manufacturer due to cost or availability, wouldn't the impedance values change? Also, different manufacturers may recommend different trace widths, spacing, and dielectric parameters for the same target impedance.

In practice, how do experienced PCB designers handle this? Do they redesign the impedance-controlled traces for each manufacturer, or is there a standard approach to make the design more portable across different PCB fabricators?

Robert Feranec , 06-03-2026, 10:32 AM

i explained it in my previous post

Karan paliwal , 06-03-2026, 05:54 PM

Sorry for asking about the same topic again, but I have one more doubt.

Would the same concept apply to vias as well? For example, if I calculate via impedance using Altium's impedance tools or any other field solver/calculator, and later move the design to a different PCB manufacturer, could the manufacturer arrive at slightly different via impedance values because of differences in drill tolerances, plating thickness, stackup, or fabrication process?

In practice, how is via impedance handled across different PCB fabricators? Is it generally considered fixed by the designer, or is it also adjusted/validated similarly to controlled-impedance traces?

QDrives , 06-03-2026, 07:13 PM

Solution is to not switch fabricator (often).

As for vias: the drill size is what matters there. Plating thickness is irrelevant.
You may want to state in documentation that the hole sizes for vias are drill size, while all others are finished hole sizes.
A via will have a impedance discontinuity anyhow, so a bit more or less may not give that much problems.

Robert Feranec , 06-04-2026, 06:38 AM

via impedance is mostly important only for a very high speed projects ... not sure what you are designing but it may not be that relevant for most projects.

Karan paliwal , 06-04-2026, 07:30 AM

Thanks,

I am currently working on a Radar PCB that includes USB, LVDS, and QSPI interfaces.

For trace impedance, I think I can follow the approach you described and work with the PCB manufacturer to achieve the target impedance.

My main concern now is about vias. If I need to route a USB differential pair from the Top layer to the Bottom layer using vias, is that generally acceptable? If yes, how do designers ensure that the impedance remains controlled through the layer transition?

Also, if I design the PCB and later send the same PCB design to a different manufacturer, how can I be confident that the via transition will still behave as expected?

In that case, how do designers typically validate or gain confidence that the USB differential pair remains within specification when it passes through vias?

This is my first time routing a USB differential pair through a layer transition, so I am trying to understand the practical approach used in real projects.

Robert Feranec , 06-05-2026, 05:48 AM

here are some videos where we covered vias and when it is important to consider them - it may help you understand if you need to think about them or not: https://youtu.be/yQIBS5xwvVQ https://youtu.be/bzDheVwJZDM https://youtu.be/A_VRMU3yFTU https://youtu.be/U60y4JC0Wxs
https://youtu.be/fJCRrEf_IH8

Robert Feranec , 06-05-2026, 05:49 AM

you can use our HW AI assistant, it will even tell you where exactly we talk about it so you dont have to watch the whole video: https://www.fedevel.com/hw-assistant

Karan paliwal , 06-05-2026, 06:46 AM

Thanku