5
\$\begingroup\$

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.

\$\endgroup\$
  • 2
    \$\begingroup\$ Just keep the traces short (less than 1 inch would be good) and none of this matters. \$\endgroup\$ – Olin Lathrop Nov 13 '12 at 18:05
4
\$\begingroup\$

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:

IMPEDANCE CONTROLLED TRACES:

  • 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

\$\endgroup\$
3
\$\begingroup\$

I you want realistic results, you cannot compute the impedance using simple formulas.

PCB manufacturers perform simulations that take into account:

  • the thicknesses of the substrates
  • the thicknesses of the copper
  • the Er of all parts
  • the nominal trace width
  • the resulting trapezoidal shapes of the etched traces
  • The thicknesses of the soldermask (different thickness on trace than on substrate)
  • temperature
  • etc...

This will give them the width and distances you have to put in the design to obtain the correct impedance. Thus the simple computation formula embedded into Altium designer is just a rough approximate that works more or less well.

And if the impedance is critical in you design, the PCB manufacturers usually add a test coupon on the PCB pannel. This coupon is a trace that has the geometry they suggest you to use to obtain your 100 Ohm diff, for example. Then, the PCB manufacturer will test every panel with a TDR in order to guaranty that the impedance is correct for every manufactured panel.

To answer your question, you can find online computation program that computes the track width for you. But this is a approximate (sometime too rough). You should use the values that are computed by your PCB manufacturer.

Ideally, you could do that simulation by yourself if you have the right tool. First I don't know if such a tool is available for free on the web and second, you don't have the numbers to feed the beast. Usually the PCB manufacturer do not communicate numbers such as the one required to know the trapezoidal shape of the etched coppers or the resulting thicknesses of the soldermask and its Er.

\$\endgroup\$
2
\$\begingroup\$

If you're laying out the board, just design the traces for the desired impedance. I use an online calculator and input the specifications of my board.

Edge Coupled Microstrip Impedance Calculator

You can usually get stackup information from the board house, like Sunstone, which will give you the spacing and dielectric information.

Sunstone Two Layer Stackup

I've never had impedance problems from the standard spec boards by doing it this way, but if it's particularly critical you can, as you have done, ask for impedance control. By the way, if you're using Altium, Sunstone and other board houses will often provide DRC files for Altium.

\$\endgroup\$
  • \$\begingroup\$ This is your best bet to specify the impedance on the stackup drawing and pay for the board shop to control the impedance and verify on board test. It doesn't add much to the cost of testing. They put an identical track on the peripheral for impedance verification and adjust the track width for etch-back factors and variation in dielectric constant and thickness variances, which can add up as much as 20% untested. Keep in mind impedance can vary with microwave frequency as dielectric value decreases. so compensate for this ( in future) \$\endgroup\$ – Sunnyskyguy EE75 Nov 13 '12 at 22:48
0
\$\begingroup\$

Here is a nice tool that I use often at work for quick calculations. The nicer layout tools will do it all for you but you still need to plan your stackup based on the manufacturer's capabilities like what Samuel is saying. This will give you constraints like minimum trace thickness and dielectric thickness to enter into the tool.

Olin is right too, of course. Designers try to put the transformer/receivers as close to the connector as possible.

Saturn PCB Toolkit

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.