Control PCB Fabrication Costs by Thinking About Panel Sizes
Getting the most for your money in custom printed circuit board manufacturing requires a little up-front knowledge of how they are made. Unfortunately, your manufacturing partner may not talk completely straight about their processes and pricing model (kudos to those that have live pricing on the websites). If you're new to the industry, or just looking for hints on how to lower your PCB costs, keep reading and perhaps you'll learn something new. Nothing in this article is rocket-science, it's really a matter of some common-sense math.
While designed-in features are the predominant driver of PCB manufacturing costs, the more subtle factor of panelization efficiency can also have a dramatic impact. One of the key things to understand about your PCB order is that the manufacturer (some would say "fabricator") probably doesn't build individual boards. For the sake of automation and repeatability, their machinery and processes are setup to handle uniformly-sized "panels" of material. Unless your board is large, or requires special processing, it's likely it will flow through the manufacturing process on panels with other designs.
The second key thing to understand is that the cost of manufacturing panels is basically fixed for a given set of technology. This obviously doesn't include non-reoccurring charges (i.e. the "one time" setup required for a new design) but it is the case for the actual fabrication processes. Other than the price of materials and labor, not much varies from panel to panel.
Working from a fixed panel cost, you can quickly see that more boards packed into a set of panels means more efficient (less costly) manufacturing. And, generally speaking, the more boards that fit on a panel the lower the per-board price. This works out well for both customers and fabricators. However, it's one of those things that seems to be missed during PCB layout. Costs can skyrocket when your design differs from "what everyone else is doing" because your boards will need to be on panels all by themselves. Boards that are done using "common" technology are easily aggregated; meaning the cost of manufacturing the panel can be spread among multiple customers. This can be a huge cost saver. But if you're boards are going to be on panels by themselves, you have to take a close look at panelization efficiency.
To make the best use of the available space on a panel (and thus lower your cost), carefully choose the size of your board. Ask you manufacturer for the details of the panel sizes they prefer, and if possible pick board dimensions that are an integer divisors of the length and/or width of the panel size. Don't forget to account for the margin around the edge of the panel and spacing between the boards. Your manufacturer should be able to provide specific instructions for sizing your board for maximal efficiency -- if they can't (or won't), you may want to consider a more cooperative manufacturer.
The math behind finding the best board size isn't complex, but it's tedious. So to save you a little time in a spreadsheet, we've added a little calculator at the bottom of this page. Before we get to that, however, I want to volunteer a couple examples of PCB panelization scenarios:
The point of the above examples is that size really does matter when it comes to effectively using the space on panels. Assuming panels have fixed cost (and they should, when they are identically built), then size choices can also impact your price. The difference between getting 2 boards per panel and 4 boards per panel may be a tiny fraction of an inch. The designer of the board in the third example above could cut their per-board price by as much as 50% by shaving a tiny bit off each dimension. Here are another couple examples, this time with the exact same size board and panel, but with the board rotated 90 degrees:
What a difference! Getting 60% more boards per panel seems like a win-win-win situation to me. Is your fabricator quoting your order based on only one rotation? You'll never know if you don't ask.
And, finally, keep the spacing between boards in mind. You might be temped to think that smaller boards would always lead to better panelization, but that isn't the case. As the board size gets closer to the inter-board spacing, efficiency drops like a rock. Consider these three cases:
above is from http://circuitpeople.com
Array Design Tips
The primary reason for having your boards delivered in an array is to make automated assembly faster and less expensive. Running an array of boards through a pick-and-place machine is far more efficient than sending them through one at a time. Arrays are also desirable because they allow the addition of tooling rails, tooling holes, and fiducials, all of which help your assembler.
Tooling Rails are the ‘frame’ for the array. They provide stability and make it easier to handle the arrays throughout the assembly process. Tooling holes and fiducials are usually added to the tooling rails.
Tooling Holes are non-plated holes added to the rails so the array can be pinned down to prevent unwanted shifting during assembly. They are typically 3.0mm diameter, but can be drilled to your required specification.
Fiducials are copper spots on the rails, which aid automated pick-and-place assembly equipment by providing a uniform reference point. The copper fiducial is typically .040" in diameter and will not be covered with mask to make it easier for assembly equipment to see.
At PCB Universe, Inc., many of our customers are contract electronics manufacturers (CEM’s - EMS's). Elmatica have a lot of experience in setting up arrays for automated assembly, and can follow your array specifications or we can set one up for you.
We will score where possible and tab-rout (rout and retain) where it isn’t. Many assemblers have guidelines as to how they prefer arrays to be constructed. Check with your assembler if they have size limitations or preferences regarding rail placement, tooling holes, or fiducials. Here are some guidelines and standards that will work for most contract assemblers.
Which array is best for you?
There are three types of arrays: Scored, Tab Routed, and a mixture of both. So how do you decide which one is right for your design?
Scoring can be the preferred choice for two reasons.
Scoring has the advantage of a more consistently smooth board edge, and it wastes less material, which can mean cost savings especially
for larger quantities or high layer count printed circuit boards where every square inch counts.
Consider tab routing, breaking nabs, when your design has an irregular shape or if you need space between your boards to allow for
A mix of scoring and tab routing can be used when some board sides are straight, which can be scored, while irregular sides must be tab routed.
In the absence of other instructions, below can be a standard array handling:
We will place .25" (6-10mm) tooling rails along the two longest sides and there will be no space between the boards. The score will be made along the shared board outline. Scoring is performed only parallel to the x- and y-axes, not diagonally. Because scoring runs all the way across the array in a straight line, the board outline should be straight for scored arrays.
Click here to see tips on how to setup scoring for irregular shapes.
The score depth is approximately 1/3 of the total material thickness. Score lines will be made on the top and bottom sides of the PCB. This will leave a remaining web of material equal to approximately 1/3 of the total thickness of the board. If your board is 1.6mm thick, the remaining material will be ~0.53mm.
Standard PCB material is essentially fiberglass. Even though your board is scored, it will still be sturdy so be careful when separating the boards. Expect some amount of flexing before the score line will give. Some fiberglass strands are common along a scored edge. A quick bump with a belt sander will take care of any rough areas.
It is possible to stop a score from continuing all the way across an array; this is referred to as jump scoring. However, this is not a recommended array solution due to the limitations and expense of this process. We strongly encourage the use of tab routing rather than jump scoring.
Scoring cannot be stopped precisely enough to end a score line like a CNC rout. To make a complete score, the scoring blade must travel past the end point and come to a stop. We require a minimum of a 12.7mm gap between the stop score location and anything that is not intended to be scored.
Tab Routed Arrays
If your design has an irregular shape, then tab routing may be required. Our default is to add a 2.4mm gap between the boards to allow the router bit to pass between them. Small tabs of material will remain to hold the boards in place. To make separation easier, we can add small non-plated holes to the tabs called ‘mouse bites’ to perforate the tab. If you desire a smooth edge on your PCB’s, these areas will need to be sanded after the boards are removed from the array.
Because tab routed arrays are inherently less sturdy than scored arrays, we will add a 10mm tooling rail to all 4 sides of the array. This will give your array more support during handling and assembly processes. (In the above photo there are rails on only 2 sides per this customer’s request.) After the 2.4mm router bit passes between the board and the rail, the resulting rail width will be 7.6mm.
Article is from PCB Universe, Inc