HDI Board CAM: Pads, Non-Functional Pads and Laser Vias

High density interconnect exists to serve highly integrated devices and dense assembly requirements, and it pushed board fabrication onto a new level of difficulty. Among all the CAM work a shop undertakes, an HDI board for a phone platform is considered the hardest: complex outlines, high routing density, and a requirement to be finished quickly and accurately at the same time. The techniques below are the ones that make that practical.

Defining Pads Correctly

Imaging, etching and the rest of the process all change the final geometry, so CAM work applies compensation to both conductors and pads according to the customer’s acceptance criteria. If the pads are not defined correctly, the finished board can have pads that are undersized.

The difficulty is concentrated in small packages. A phone board may use a 0.5 millimetre CSP with 0.3 millimetre pads, and some of those pads also carry blind vias whose corresponding lands are also 0.3 millimetres — so the package pad and the via land coincide or overlap. In that situation the work has to be done carefully rather than quickly.

One reliable approach proceeds in a fixed sequence. First, switch off the drill layers belonging to blind and buried vias, so that they do not interfere with the pad data. Second, define the pads. Third, use feature filtering and reference selection to locate those pads that include a blind via, and move them onto a separate working layer.

Fourth, work on the layer where the CSP pads sit: select the 0.3 millimetre pads that touch a blind via and delete them, and delete the corresponding 0.3 millimetre pads in the CSP region on the outer layer as well. Then rebuild the CSP land pattern from the customer’s design — its pad size, positions and count — define it as a pad set, copy it onto the outer layer and add the lands corresponding to the blind vias. The other side is treated the same way.

Finally, compare the result against the customer’s stencil or paste file to identify any pads that were left undefined or defined twice. The value of this method is that each step has a clear purpose and there are fewer operations, which removes opportunities for misoperation.

Removing Non-Functional Pads

On an HDI board, non-functional pads are a routine removal, but the removal has to be done in the right order and only for the right holes.

Take an eight-layer HDI board as the example. Through vias must have their non-functional pads removed on layers two through seven, and the buried vias spanning layers two to seven must then have theirs removed on layers three through six.

The sequence that keeps this clear is straightforward. Start by removing the pads corresponding to non-plated holes on the outer layers. Then switch off every drill layer except the through holes, and run the removal with the “remove undrilled pads” option set to off, which strips the non-functional pads from layers two to seven. Finally, switch off every layer except the two-to-seven buried vias, keep the same option setting, and strip the pads from layers three to six.

The reasoning is easy to follow, which matters when the work is handed to someone new to HDI CAM: the option that prevents undrilled pads from being removed is what stops the tool from stripping pads that belong to a via that does not physically reach that layer yet.

Laser Via Formation

Blind vias on phone boards are typically around 0.1 millimetre microvias, produced with a carbon dioxide laser. Organic material absorbs infrared energy strongly and is ablated thermally, but copper absorbs very little of it and also has a high melting point, so the laser cannot ablate copper foil.

The industry answer is the conformal mask process. The copper at each laser via position is etched away first, and the CAM department produces the exposure film that defines it. This is also why the microvia positions are fixed during data preparation rather than adjusted during drilling.

There is a geometry consequence that has to be checked. The sub-outer layer must have copper at the bottom of the laser via, which imposes a minimum spacing between blind and buried vias — four thousandths of an inch or more. Drill checks against the fabrication rules are used to find every location that violates the limit, because the requirement cannot be judged by eye across a dense board. The general structural rules that apply are covered in this review of HDI layout and microvia rules.

Via Plugging and Solder Mask

In an HDI stack the sub-outer layer is often resin-coated copper, which has thin dielectric and a low resin content. Process experience shows that two separate plugging files are needed — that is, the vias are plugged twice — when any one of three conditions applies: the finished board thickness exceeds 0.8 millimetres, a metallised slot is 0.8 by 2.0 millimetres or larger, or a metallised hole is 1.2 millimetres or larger. In that case the inner vias are filled with resin and planarised, and the outer vias are then filled with solder mask ink before the mask is applied.

Mask production brings a related problem. Vias frequently fall on or immediately adjacent to pads, and customers typically require all vias to be plugged, so a via that is exposed — or half exposed — at mask exposure bleeds ink.

CAM prefers to move the via clear of the pad. Where that is impossible, the workaround is applied at the mask layer: for a via whose position is opened in the mask, add a clear feature three thousandths of an inch smaller per side than the finished hole; for a via that touches a mask opening, add a clear feature three thousandths of an inch larger per side, on the basis that the customer accepts a small amount of ink on the pad. The design rules that create these situations in the first place are described in this discussion of via design rules.

Outline and Panel Geometry

Phone boards are normally delivered as an array, and the outline is complex. The customer supplies a CAD drawing of the array, and redrawing it from the dimensions is unrewarding work.

A faster route is to convert the CAD file into a DXF interchange file and read it exactly as a Gerber file would be read. The outline comes in along with the mouse-bite positions, the locating holes and the optical alignment targets, with their sizes and positions — quickly and without transcription errors.

Routing the Board Edge

Unless the customer specifically requires exposed copper at the edge, the fabrication specification calls for a small amount of copper to be trimmed back from the routed border, so that copper does not burr or lift during routing. That trimming can leave a narrow neck of copper near the edge, and if its two ends belong to different nets and the remaining width is under three thousandths of an inch, the result can be an open circuit — or a feature too narrow to produce reliably.

The problem does not appear in a standard manufacturing analysis report, so it needs a separate check. Perform the net comparison a second time with the border copper trimmed an additional three thousandths of an inch deeper into the board. If the comparison shows no open circuit, then either the two ends are on the same net or the copper is wider than the minimum. If it does show an open, the copper has to be widened before release.

The pattern across all of this is that HDI data preparation is a chain of small, specific operations where the risk lies in the geometry rather than in the process, and where the checks that catch those risks are not always the ones the tool reports by default. The same reasoning applies to the finished panel, which is verified as described in this overview of PCB inspection after fabrication.

FAQ

Why is pad definition harder on an HDI board? Because package pads and via lands are often the same size and occupy the same position. Defining one incorrectly changes the other, and the error only becomes visible as an undersized pad on the finished board.

Why can a carbon dioxide laser not drill through the copper foil? Because copper absorbs very little infrared energy and has a high melting point. The copper is therefore etched away at each via position first, using a conformal mask, and the laser then removes the dielectric beneath it.

When does an HDI board need two plugging passes? When the finished board is thicker than 0.8 millimetres, or when a metallised slot or hole exceeds the size limits. The inner vias are then resin-filled and planarised, and the outer vias are filled with mask ink before the mask is applied.