designer’s notebook
Component Placement is a Game of Compromises
Getting all the parts and processes aimed in the same direction.
Printed circuit board technology never sleeps. At this very moment, engineering teams are working out ways to increase circuit density with finer-pitch devices. When it comes to placing these components on a PCB, the margin of error shrinks along with the pin pitch. Let’s look at how we can enable these parts on the assembly line.

The first step in mass production of a PCB assembly is preparing the board to take components. The boards may be baked in an oven prior to starting the assembly process. Although they are packed in sealed containers with a little bag of desiccant, the sponge-like dielectric materials still absorb water one molecule at a time. Prebaking releases the steam that could interfere with reflow soldering.

Ideally, all parts on a board will use the same type of technology and will be roughly the same class of components in terms of pin-pitch and other physical aspects (FIGURE 1). Tall and heavy components plus small and light ones are not a good mix. Tall ones create so-called shadows where the surrounding area doesn’t get as hot during soldering.

Figure 1. Board outlines determine how much of the material is lost for processing. Sticking with SMD components helps narrow the number of steps required.
Most component datasheets include instructions for soldering. There could be a suggested paste type specified down to the granularity of the particles. There will likely be a graph that shows the thermal profile that gives the best results. It starts with a preheat ramp-up to near-reflow temperature, then a spike into the soldering temperature, followed by a cooldown period. Overlaying all the thermal curves for the components on a particular board will show similar but not exact matches for the recommended process window.

Your assembly house has a sweet spot for yields. A perfect board for them has all components in the same orientation. They would all be surface mount and on the same side of the board. Components with hidden leads would be avoided or given extra space as a “courtyard” for a rework nozzle to make full contact with the board surface. It’s more efficient if the assembler does not have to desolder a bunch of passive components, but some of them really want to be near a specific pin.

Fine-pitch components. Fine-pitch devices, if used, have a pair of local fiducial marks to permit the pick-and-place head to register its exact location for more accurate placement. These fiducials are in addition to board-level fiducials and could be shared among devices if there is symmetry among them. Ideally, every component faces the same cardinal direction with distinct and uniform polarity marks. The real world doesn’t work that way, but it is a goal. In 30 years of PCB layouts, I have never once had all the caps and resistors in the same orientation, let alone all the polarized components. The idea is to get a feel for how the components want to be placed for the best performance and settle on one general direction that uses that angle whenever possible.

Now you have your nearly perfect layout with the board ready for assembly. The next step is solder paste application. Depositing solder paste on the PCB must be precise and repeatable. Smaller boards or those with intricate outlines will require an assembly subpanel.

Meanwhile, larger boards usually incorporate component-free zones along the edges for placement and soldering processes. Typically, we’re looking at a 5mm-wide strip of component-free real estate along the longer edges of the board for the machines to grip. Tooling holes facilitate repeatable and unmistakable orientation for fabrication, stencil, pick-and-place, and test fixturing. Three alignment holes provide that kind of assurance.

Let’s circle back to the boards, with an assembly subpanel in addition to the larger fabrication panel. Consider the orientation of the components before choosing which edges require assembly rails. Surface mount and through-hole components both have a preferred direction of travel through the soldering station. The main point is to prevent solder bridges and other defects, as we will cover next.

Passive components prefer to go through the oven broadside (sideways) to the process flow. This way, both pads see the same temperature profile at the same time. If one side reflows and solidifies before the other, there is a greater likelihood of defects like cold solder and disturbed solder. Cold solder has a dull finish and lacks the fillet that indicates proper wetting. Disturbed solder has irregular contours that suggest some movement of the component during the critical transition when solder changes from a liquid to a solid. Those are two defect classes that lead to latent defects, the worst kind of defect.

Figure 2. Even if the board is big enough to process alone, a pair of long, straight edges aren’t always possible, so material must be added for a one-up panel. Note the break-off area is used to show the direction of travel on the conveyor belt.
Improperly placed components could also lift from one of the pads like a drawbridge, which we call “tombstoning.” I’ve had cases where ceramic and wire-wound components actually broke due to the stress of different thermal profiles. These defects occurred because one end of the capacitor/inductor was close to the edge of the board, while the other pin was inboard. The edges get much hotter, with the temperature rising and falling faster, while the board is in the reflow oven.

The key element to a reliable placement is the space between components. We want the shortest possible RF paths, so that is the first consideration. Wide busses also demand close proximity between drivers and receivers. Almost all decoupling caps will benefit from being near the associated power pin. Crystals should be kept on a short leash. It seems every little component would like a spot right next to the main chip.

Even so, the more breathing room a component has, the longer its expected time until degradation and failure. Close but not crowded? How about selectively separated as required for coexistence and thermal management. So many factors pull us in different directions. Smart placement makes all the participants equally nervous and none of them overly so.

Figure 3. Populated and depanelized version of Figure 1. Note the connectors are secured with adhesive because of the expected environment.
Sharing your work along the way is more important than ever. Arriving at the end of the design cycle with a product that everyone can buy into is the main goal. The last thing we want is for the board design to become the giant ship that gets stuck in the canal. That’s what it’s like when various factions are still working out their differences.

Getting buy-in on placement is harder than getting it for the complete design. I usually submit the first placement with the receive and transmit chains hooked up. All the components are colorized by their schematic pages. The reference designators are neatened up, even though there will be some churn for sure. At least some of it survives until tape-out.

The more you can do to grease the skids for that day, the better. Successful designers juggle a lot of data to deliver something that goes through the assembly line with a minimum of manual operations. Understanding the end-use and how it all goes together helps us improve our products while staying in the sweet spot.

John Burkhert Jr. headshot
John Burkhert Jr.
is a career PCB designer experienced in military, telecom, consumer hardware and, lately, the automotive industry. Originally, he was an RF specialist but is compelled to flip the bit now and then to fill the need for high-speed digital design. He enjoys playing bass and racing bikes when he’s not writing about or performing PCB layout. His column is produced by Cadence Design Systems and runs monthly.