1
\$\begingroup\$

Is the height of the substrate just the non conductive portion between copper layers ?

Using this calculator as an example

In a 4L board, if the top and bottom traces are of the same thickness and width with the same height for their respective substrates, would that imply that the impedance of the trace of the same since, they are both exposed to free air and a substrate ?

Are these calculators assuming that the adjacent layer is a ground plane ?

\$\endgroup\$
  • \$\begingroup\$ It is not a gnd plane, it is a reference plane. It could be gnd, vcc or some other arbitrarily assigned dc voltage. Otherwise yes what you are saying is correct assuming that the substrate material is the same. \$\endgroup\$ – Some Hardware Guy Apr 6 '15 at 13:25
  • \$\begingroup\$ The pictures on the page you link show you exactly what they are assuming. The 'H' parameter is the height between your trace and a ground plane. Whether that ground plane is on an adjacent layer or a lower layer is immaterial, as long as there's no other copper in between and the dielectric material is uniform (same Dk). \$\endgroup\$ – The Photon Apr 6 '15 at 14:36
3
\$\begingroup\$

1) Yes, H is the thickness of the prepreg between the top layer and the plane in layer 2. After pressing the board.

2) Yes, if you mirror the configuration from top to bottom the impedance will be the same.

3) Yes and No. The term is "plane" (not "ground plane"). The fields can't read... :-) Planes will work the same no matter what you name them.

Note 1: The impedance tolerance after manufacturing may be around +/-20% on outer layers and +/-10% on inner layers.

Note 2: This and other formula based impedance calculators may easily be way off if you have thin dialectric and skinny traces (which is what we often want in order to squeeze a lot of traces into a given area). If you want more accurate results in those cases, find a 2D field solver like the one in Hyperlynx og Cadence SigXplorer. There is a free one on the net called TNT as well.

\$\endgroup\$
1
\$\begingroup\$

Yes, the assumption is that these are ground planes, and these are required for the impedance to be correct.

The impedance of a coaxial cable is defined by the ratio of the core radius to the shield radius, and the permittivity of the dielectric. On a PCB, we approximate these as close as we can, replacing the shield with a ground plane, which can be on both sides (stripline) or just one (microstrip).

If there is only one ground plane, the impedance increases, but is still controlled by the ground plane. If I remove the ground plane, the controlling factor vanishes, and you get different values along the trace, depending on what other traces are nearby.

The height is indeed the non-conductive portion only.

\$\endgroup\$
1
\$\begingroup\$

Referring to your link H is the thickness of the dielectric between two copper layers. For a four layer board I guess it depends: if having an higher H can be good for you you can leave a copper layer "unpopulated" as in "with no copper", and make the plane in layer 3 or 4.

This calculator assumes that the bigger trace is a low impedance plane, ground, vcc or whatever, and that it's bigger than your microstrip, i.e. wider and longer. The last assumption is needed to neglect "edge effects" (is it correct?).

About your last sentence, if you make a microstrip on TL and one on BL for them to have the same characteristic resistance, apart w and t, you will need to provide a plane at the same H for each one. In a 4L board that can be achieved only with two planes in the intermediate layers, for a 5L board maybe one plane in L3 can do the job.

Keep in mind that you can bury a ustrip in an internal layer, here's another random calcolator, maybe that can suit your needs better.

\$\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.