Electronic – How to specify 100 ohm impedance on a pcb gerber


I've been using Altium for several years when I've needed to designed boards. However it's all been for simple analog designs and never anything too technical. I'm now trying to take a jump into a board requiring 100Base-TX ethernet.

I'm using a Microchip ENCX24J600 and it seems I need to use run 100 ohm impedance Differential Pairs for the TPOUT+/- and TPIN+/-.

I found a pretty good example video that has explained how to set up Altium here I thought I'd just need to call the manufacture and get the numbers as explained around 4:00 in the video. However I called the PCB shop and they said all I needed to do was provide a sample trace on the side and they'd make it work.

I'm sure this would work but I was wondering if there was a nice standard way that one should specify 100 ohm or 50 ohm for traces (as this seems complete different from in the tutorial I found).

Perhaps I'm making a mountain out of a molehill but I'd rather get things figure out once and then be consistent rather then get a few bad habbits that I'd have to relearn later on.

Best Answer

First a clarification: For 100Base-T if you keep the lengths short (<1") between ENCX24J600/magnetics/connector, the impedance doesn't really need to be controlled, just be in the ballpark. A high speed digital design book will explain why.

Secondly, this question needs to be answered because later on you'll want to use a faster interface, such as 1000Base-T or 10 GbE, or any other fast digital signal like 3G-SDI, or your lengths may need to be a bit longer, or you may need to route a high speed memory bus like DDR3, so what are you to do? repeat this question?

Finally, to address the issue at hand:

  • Calculate (by hand, with software, etc.) what the trace dimensions should be based on a typical stackup that the manufacturer offers. If the results are plausible use that.
  • If the resulting traces are not practical (too wide or too narrow), you need to specify a stackup that will work. It can become an iterative process. Start with a trace thickness that is practical for routing, spacing, manufacturability, etc. Then calculate the dielectric thickness (given a material with a specific dielectric constant) for the impedance you need. Then from real options of core thicknesses and prepreg sheets and materials, choose the closest one. Then recalculate the trace dimensions you need.
  • If your software allows for it, simulate your critical lines and make sure your signal integrity is ok (this requires driver model, trace dimensions, stackup specification (distance to reference plane(s) and dielectric value), and any vias you may be using (and their dimensions). Correct as needed.
  • Now you have your stackup and trace dimensions for the impedance you need, but you need to convey this information to the pcb manufacturer (which is the gist of your question).
  • To specify the stackup, draw on the gerber a representation of it, specifying thicknesses. Add some notes specifying desired dielectric constant and material.
  • To specify controlled impedance, since the value of the trace widths of specific impedance will be special, you can refer to them in the notes by width. Their tools will help them identify the traces easily. You can say for example:


  • 5 mil traces on top layer should be 100 ohms (+/- 20%) impedance with respect to the plane in layer 2.

In reality, the pcb manufacturer will adjust the widths to match the desired impedance, according to their internal data of the exact dielectric contants and widths that they will use to manufacture your pcb. But thanks to your calculations, it will be close to what you specified (so that things like spacing between traces, minimum widths and overall routability are not significantly affected when they make the adjustments).

A google image search yielded the following example:

enter image description here