Why are 4-layer boards (usually) made with 2 prepreg layers? - Page 1
Forum section: electronics / general

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: March 05, 2020, 03:18:08 pm
content: So, I always understood the following:A core layer is a rigid dielectric layer with cured resin/whatever. Usually, both sides are plated with metal, 17 um.A prepreg layer has uncured resin inside. This is stuffed inbetween layers of core as a kind of glue, to make multi-layer boards.So far so good. But from this understanding, I would think you make a 4-layer board by taking two core layers, and shoving a (number of) layer of prepreg in between and curing the two. But I understand that most 4-layer PCBs are actually made with one core layer, then two layers of prepreg on each side, and then a copper foil to make the outer metalization layers. I know this because in RF we often want core on the outside (=more predictable) and they call our stackups 'reverse stackups'.Why is this? Why is it easier/better/cheaper/more reliable (pick which fits)?

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: March 05, 2020, 03:51:52 pm
content: Quote from: blueskull on March 05, 2020, 03:27:16 pmSo it is not that the P+C+P is better from a manufacturing point, and it is driven by electronic performance for the majority of applications?

author: NorthGuy
author_rank: Super Contributor
timestamp: March 08, 2020, 03:02:13 pm
content: Usually 4-layer boards are used for high(er) frequency designs, where you want to get certain impedance of PCB traces, often 50 ohm. People do this by laying traces against the ground/power plan on the nearest layers (called microstrip) or by sandwiching the trace between two planes (called stripline). Striplines are better in every respect, but they are not practical for 4-layer PCB. Thus, you are likely to use microstrips on 4-layer board. Practically the only layout you may have on 4-layer board is signal-ground-power-signal. This way you get two signal layers and the microstrips will be formed by signal lines on the top/bottom layer laied against the plane on the nearest inner layer.The microstrip impedance depends on the thickness of the dielectric layer between the signal and the plane. It also depends on the width of your traces. Thus there are two ways to get the desired impedance - either make traces wider, or make the dielectric thinner. Wider traces waste lots of space, so thin dielectric it is. That's why the 4-layer board standard layout will have tick core between inner planes and thin prepreg between inner and outer layers. Of course, if your goals are different, you can always order any different stackup. But if you're not interested in controlling trace impedance, you're probably not concerned with the stackup anyway.

author: Koen
author_rank: Frequent Contributor
timestamp: March 08, 2020, 11:10:50 pm
content: Why does JLCPCB offer two stackup and when is one preferable over the other ? Thank youhttps://jlcpcb.com/quote/pcbOrderFaq/PCB%20Stackup

author: NorthGuy
author_rank: Super Contributor
timestamp: March 09, 2020, 12:13:46 am
content: Quote from: Koen on March 08, 2020, 11:10:50 pmGoogle "microstrip online impedance calculator". Then you can use it to see what kind of impedance you would get with different prepregs. 4 mil prepreg is aggressive and will let you achieve low impedance with very thin traces. If you need higher trace impedance, or want thicker traces to save money, then 8 mil prepreg will work better for you.

author: ANTALIFE
author_rank: Frequent Contributor
timestamp: March 10, 2020, 04:02:04 am
content: All of the above plus that way there are less things you have to stockFor example rather than stocking prepreg that can only do 2 layers boards, why not stock prepreg that can do 2/4/6... layer boards?

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: March 11, 2020, 10:43:26 am
content: Quote from: NorthGuy on March 08, 2020, 03:02:13 pmI was always told (and it makes a lot of sense if you ask me) that core is better than prepreg for RF. The thickness is more predictable (as it doesn't cure any further, so doesn't change) and often the losses are slightly lower. But I guess with FR4/low-cost/Lower-frequency this is less critical, so it makes sense.Thanks for clarifying this stuff!