3
\$\begingroup\$

I'm new to impedance control PCB design, and I got following information from a PCB manufacturer. This is their standard stack, and I'm planing to control the impedance of my design according to their specification, because it's cheaper. Is it possible to do that? When designing impedance control PCBs, should pre-pegs and core both be FR-4?

Pre-preg thickness - 1080 = 3.04 mil - 2116 = 4.67 mil - 7628 = 7.68 mil

Four-layer top layer - 18 µm copper foil (plated to 35 µm+) pre-preg - 1 x 1080 + 1 x 7628 Layer 2 & 3 - 1.0 mm FR-4 core with 35 µm/35 µm copper pre-preg - 1 x 1080 + 1 x 7628 bottom layer - 18 µm copper foil (plated to 35 µm+) 1.6 mm +/- 10%

How do I calculate εr between the top layer and the second layer using the above information?

\$\endgroup\$
  • 2
    \$\begingroup\$ A stackup diagram (even in ASCII art) would be much easier to read than your text description of the stackup. You can use the "code" formatting to get a fixed-width font. \$\endgroup\$ – The Photon Mar 26 '13 at 4:21
3
\$\begingroup\$

You can get approximate known-impedance transmission lines by simply defining the correct trace width and dielectric height. For many designs, this approach will be perfectly fine.

But if you do that, it's not called impedance controlled. An impedance-controlled design means rather than controlling the trace width according to your gerbers, your fab shop controls for the impedance and lets the trace width vary as needed. Another way to look at it is, you give the fab vendor freedom to adjust the trace width and dielectric thickness as needed, and they take responsibility for obtaining the correct impedance.

| improve this answer | |
\$\endgroup\$
  • \$\begingroup\$ Hi Photon, Thanks for your information.So when I do impedance control design I have to do rough calculations about impedance of transmission lines and Do I have to inform to PCB fab, which lines have to maintain impedance and value? and what exact material use for?Thanks Dan \$\endgroup\$ – Dan Mar 26 '13 at 16:09
  • \$\begingroup\$ If you want them to be responsible for getting the right impedance, you need to include it in the fab drawing. I usually add a note something like, "traces drawn as 8.1 mil on layer 1 are 50-Ohm +/- 5 Ohm controlled impedance". It is also a good idea to specify the exact laminate material if you want controlled impedance. \$\endgroup\$ – The Photon Mar 26 '13 at 16:22
5
\$\begingroup\$

Physics/Materials

You need to specify the maximum operating frequency and/or fastest edge-rate. Impedance is a function of frequency.

You should also think carefully about the size of your design/length of traces. You may actually be worrying about something that isn't a problem.

Er is an intrinsic material property. It isn't effected by the dimensions (to the first order). FR-4 is a composite material consisting of glass fibers and resin Er about 2 and 6, with a typical weighted average of 4.6 or so.

Your Case

The maximum operating frequency of my circuit is 1.5GHz. I need to maintain impedance in 100ohm differential pairs and 75ohm lines about 30mm maximum lenght each

In your case, you are at the low end of the "gray" zone. In general, you can ignore reflections (the consequence of mismatched impedances) when the propagation distance is less than an order-of-magnitude of the wavelength. This works because any reflecting waves would have time to decay (die out) before the next clock edge. They'd have to bounce off the ends more than five times and still have enough energy to distort the signal beyond your trigger threshold.

In copper-over-FR-4, the speed of light is approximately half that of free-space (1.5e8 m/s). There the corresponding wavelength at 1.5GHz is 10cm. Your tracks are 3cm. If you can reduce the track length to 1cm (or less) you can easily ignore impedance control.

That said, don't take it as license to do something silly. You should still route cleanly, hold spacing and track width constant, neck smoothly, etc -- but you don't have to pay for "impedance control" services from the fabricator).

What I Would Do

There is no magic to "impedance control". The fabricator uses a model for the material (which they will happily share with you -- since it ties you in to their factory) to determine a track width/spacing and uses it. When you pay for impedance control services they simply add an extra step to the fab process where they will verify that they got it right.

  1. Ask the fabricator for the target track widths and spacing.

  2. Use it ;-)

I wouldn't pay for impedance control in this case at these frequencies given your route length. Remember the energy of the reflection is in proportion to the ratio of the impedance mismatch. If you are off only a little, and your distances are small, and your material is close to spec... you'll be fine.

If this is an expensive low-volume product where you can't afford respin or 5% performance degradation (et. al. r.) then by all means ignore this advice.

| improve this answer | |
\$\endgroup\$
  • \$\begingroup\$ Thanks a lot for ur help.The maximum operating frequency of my circuit is 1.5GHz. I need to maintain impedance in 100ohm differential pairs and 75ohm lines about 30mm maximum lenght each.As I understand the spec from PCB fab, they using 1x1080+1x7268 fiber layers in between top layer and 2nd layer.So my signal layer is top layer and GND layer is 2nd layer.I'm trying to use PCB fab's standard stack with out using Impedance control fabrication. Is it possible to do with the running frequency and track lengths? Thanks. Dan \$\endgroup\$ – Dan Mar 26 '13 at 16:01
  • \$\begingroup\$ @Dan -- Expanded answer to address. \$\endgroup\$ – DrFriedParts Mar 26 '13 at 22:09

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.