Section 3 – PCB Design: PCB Outlines (Boards and Panels)

John Burkhert

This is the third section in the back-to-school series for PCB Designers and those who may want to know more about it.

Contents

PCB Outlines: Boards and Panels
Getting Ahead of the Tolerance Problem
Assembly Sub-Panels - Making Room for Manufacturing
Graduate School Zone

PCB Outlines: Boards and Panels

Before you can place the virtual components on the board, you need a virtual board. In addition to describing the outer limits of a PCB, the outline drawing will cover several things. Expect connector placement, mounting holes, keep-outs for mechanical hardware like heat pipes and RF shields.

When you get a new outline drawing, it pays to do a thorough evaluation. There may be an area where the PCB is overly constrained. The longer you wait to express your concern the less likely it is that there will be wiggle room. Once the interconnections that feed the board are drawn up, it may be too late to rotate a connector or move a mounting hole.

Getting Ahead of the Tolerance Problem

If the outline drawing includes any high-precision positional tolerances, thickness, flatness, or unilateral tolerances, it would be necessary to run all of these past the fabrication vendor(s). A lot of component vendors put unrealistic tolerances on their datasheets. The mechanical engineer or librarian would be inclined to pass these tolerances right along.

As the expert, it’s up to you to confirm that the tight tolerances can be met in volume production. From my experience, the most common request that can’t be met is regarding PCB thickness. A two layer PCB made of ceramic material has a chance of holding a tight thickness tolerance. Multilayer boards made of glass, resin copper along with various plating and coating layers will generally be held to 10% of the nominal thickness.

Wishful thinking in product design would like to have a better handle on this variable. Control of the Z-stack would be nice but a PCB is not like a block of aluminum. The dielectric breathes in moisture like a sponge. It expands and contracts with temperature. Even if the vendor “inspected in” the thickness by discarding all of the panels that didn’t meet the tolerance, there’s no guarantee that it wouldn’t go into an altered state.

To some extent, this applies to warpage as well. While I’m confident in this statement, the mechanical engineer may not want to believe it. You may have gone down this road yourself. The thing to do is bring in the final arbitrator. The fab shop is just a phone call or an e-mail away. You still might get a “yes-man” answer from the sales team so ask the planner or the CAM engineer. If you don’t know them, ask for a tour of the factory and get to know them. If they’re too remote, you may wind up doing a little bit of networking to get the unvarnished truth.

Assembly Sub-Panels - Making Room for Manufacturing

While you’re contacting the vendors about the new outline criteria, it would be a good time to broach the subject of assembly sub-panels. Edge connectors have to be factored into the sub-panel so that they can be placed without depanelizing the individual boards. Break-off tabs that allow removal of the assembly may intrude into the board a little. Knowing where they will go allows you to accommodate them. The end-game is probably the worst time to negotiate details that could have been solved earlier. The fewer surprises, the better.

For the simplest board outlines, it may be possible to design the assembly sub-panel yourself. One such situation may be when the outline is a rectangle or a square. Those are often the ones where there was no outline drawing or other mechanical engineering support. Using V-score grooves eliminates the need to calculate how many break-off tabs would be sufficient.

Figure 1. Image Credit: Author - A rectangular PCB that is panelized with V-score grooves so it can be depanized by hand as the unneeded sections can be snapped right off.

To design the sub-panel in-house, you would need to know the upper and lower size limits of the assembly machines. There are a few popular sizes for tooling holes that you’d want to use. The rails that support the board have a minimum width. I hesitate to put actual numbers to these features because no two assembly houses are alike and they usually get better over time.

Depending on the format of the outline drawing, you may have to interpret some things. On day one, it’s rare to see a completed drawing. More likely the input is a file that you can import and maybe a screenshot of the PCB in its native habitat.

Graduate School Zone

The layers used for data transfer don’t always make sense. For instance, the component keep-out area is often used to indicate the location of a feature like a connector. No part goes there except for the part that goes there! That’s a loop you’ll want to close with the physical designer. Their software supports a particular set of layers that may not be optimal, particularly for flex circuits where there are additional layers to consider.

The distance from the edge of the PCB to the copper features is an important factor. A pull-back of 200 to 250 microns is typical. I took a walk around a PCB Design conference and asked every fab shop what the most aggressive board edge-to-copper clearance was possible. The common answer among the advanced vendors was 127 microns.

I needed something more extreme. There weren’t many fabricators who were willing to use lasers to form the edges of the PCBs. The ones who could insist on a maximum PCB thickness of 400 microns. There was a common issue with carbon deposits on the edges. Those were some hairy boards and a significant cost driver. Part of the reason for the $70,000 price tag on the flagship product was the number of boards that had to be cut out with lasers.

Figure 2. Image Credit: Author - The outline can be the most challenging aspect for the fabricator. Without the little grooves, this six-layer board would have been half the price.

The gap between the metal and the board edge can be reduced to zero in two ways. The most obvious is wrapping the plating around the edge. Another is so-called castellated vias. The castellation is going to be larger than a typical via and will be drilled right on the edge of the board before the board outline is routed. What is left is a half-via that can be used to connect inner layers as well as the outer layers.