Mechanical construction of PCB. What is between the layers?

Question

I came across an answer about the construction of a multilayer board. It included an image showing the mechanical construction of a board (see image 1.)

This prompted me to think of the actual construction a bit more.

Image 1: Construction of multilayer board

The image shows the through hole and via pouring in between the layers. Is pouring into a gap really what happens or is it just some artistic freedom on part of the image creator? Is the shape of the hole really ribbed? I mean it would make sense to make construction more connected, but it also makes sense for the author to emphasize the effect. Equally plausible would be that some manufacturers do this some don't. Is there any practical stack design where there would be internal ribs?

What I'm asking is the last copper buildup like:

The image seems to suggest A because there is a line between the copper layer and hole.

Also something that the image does not show is what is filling the gap between the layers where there is no copper.

Answer 1

You've got several parts to your question.

Those parts are represented by the red, blue, and green arrows I've added to the drawing:

The blue part references what's between the layers where there's no copper.

PCBs are manuafactured from sheets of fiberglass matts and epoxy. Each layer is a premade sheet of fiberglass and epoxy with a sheet of (thin) copper on the top and bottom of the sheet.

The copper is etched to make the traces on the top and bottom of the layer.

When a multilayer PCB is assembled, the fabricator stacks up several of those sheets and lines them up carefully so that all the traces and other details line up.

There is a thin coat of epoxy between the layers. The whole stack is put under pressure (clamped flat together) until the epoxy is cured (hardens) so that the stack will stay together.

Between the layers is (at most) a very thin layer of epoxy. The fiberglass is "mashed" into the open areas around the copper by the pressure. Any open areas where the fiberglass can't reach (closest around the traces) will be filled with epoxy.

The red arrows indicate the "ribs" where the vias go through each layer.

Vias are made by drilling holes through the finished stack after the epoxy has set. The vias are then plated with copper. The copper plating in the holes joins all the copper layers together.

The PCB design software will include "rings" of copper on each layer to make the noted "ribs." The assembly process doesn't leave little gaps for the copper plating to spread out and make the "ribs." The "ribs" must be in the etched copper layer. When the through holes are plated, the rings specified by the design software are joined to the plated hole to make the "ribs."

The line indicated by the green arrow is somewhat misleading. That line appears to mark the boundary between the plating that make the through hole and the copper plating on the surface of a layer of fiberglass. The line would more properly be in the place marked in purple (just to the left of the green arrow.)

---

Speculation about the "ribs."

I don't know that any manufacturer requires adding the ribs. As far as I can tell, they are added by the PCB design software when placing the vias.

The Eurocircuits guidelines for making PCBs specificall says to remove the pads on any inner layer that you don't want connected to the through hole plating. That means the "ribs" aren't a required part of the manufacturing process.

---

Eurocircuits has a nice series on the construction of PCBs, describing the individual manufacturing steps. Each section in the series has a description with pictures and a video of the process.

---

To answer the additional question posted in the comments, the plating looks like "B" in the image below:

The "rings" in "A" are on the fiberglass layers. The plating goes inside the hole and over the surface of the top and bottom layers of the stack.

Answer 2

The copper sections should all be connected -- the lines in the original diagram are not meaningful in terms of the resulting structure. Here's an updated diagram with fewer lines:

Answer 3

The distinction between the via, its annular ring, and the copper trace or layer is somewhat arbitrary. It's all continuous copper.

The graphics are showing the vias using the abstraction with which you'll work with them in your PCB software. The ribs or rings are defined by the annular ring diameter property, the presence of connecting copper is defined by the trace or plane structures that you may or may not connect to the via. Often, the trace or plane extends all the way to the center of the via where it gets drilled away, and it's purely for eye candy that you don't see this in your PCB editor; you can see it in some generated Gerber layers.

However, mechanically, the assembly order is:

1. Fiberglass sheets are covered with copper foil to form the inner layers
2. Some copper is etched away where you don't want a trace or plane; eg. a circular void is added to the foil where a via that you don't want to connect passes through.
3. Fiberglass sheets and the inner etched copper sheets are stacked and epoxied together
4. Vias and plated slots or through-holes are physically drilled through the stackup. The hole edges are deburred at the surface and desmeared to ensure no epoxy resin is left on the exposed inner layer copper.
5. Copper plating is added to the entire exposed surface of the board, which now includes the walls of the holes and the 25 micron thick visible rings from the inner layer connections. The deposited copper makes the finished hole slightly smaller in diameter than the hole that was drilled in the fiberglass
6. The surface copper is etched away as the inner layers were etched in step 2
7. Non-plated through holes, soldermask, silkscreen, V-groves, board edge milling, and so on are later added.

The copper layers are built up and removed by chemical deposition, chemical etching, and physical drilling into a continuous 3D shape of copper. In the end, there should be no seam. If you were going to draw one you might make a distinction between the plated hole walls and the surface of the layers where you might have a failed deposition if contaminants get inside the hole before it's plated.