How to Avoid Pitfalls in PCB Design
6 min
- Hole Size in Via Design
- Slot Holes in Via Design
- Hole Attributes in Via Design
- Trace Width and Spacing in Trace Design
- Hatched Copper Filling in Large Area Traces
- Uneven Copper Pour Distribution
- Copper Pour Design
- Conclusion
Designing a printed circuit board (PCB) requires careful attention to various factors to ensure a smooth manufacturing process and avoid potential pitfalls. From hole size and slot design to tra ce width and copper pour considerations, understanding these aspects is crucial for creating reliable and functional PCBs. In this article, we will explore some common pitfalls in PCB design and provide recommendations to overcome them.
Hole Size in Via Design
In PCB manufacturing, a 0.3 mm hole is considered standard, while holes smaller than 0.3 mm are classified as small holes.
Small holes can have several negative impacts on production:
Difficulty in Plating: Smaller holes are more likely to result in unplated or poorly plated holes. For small holes, JLCPCB uses a four-line low resistance process to ensure reliability.
Lower Processing Efficiency: Smaller holes require slower drilling speeds and shorter drill bits. Subsequently fewer boards are drilled at a time. Therefore, when designing, it's advisable to use holes larger than 0.3 mm, considering the use of small holes only when space is limited.
JLCPCB's minimum process capabilities:
Single/double-sided boards: 0.3 mm (inner diameter) / 0.45 mm (outer diameter)
Multilayer boards: 0.15 mm (inner diameter) / 0.25 mm (outer diameter)
Outer diameters should be 0.1 mm larger than the inner diameters, with a recommended difference of 0.15 mm or more.
Slot Holes in Via Design
Short Slots in PCB Drilling: Slots with a length less than twice their width are termed short slots. The optimal length-to-width ratio for short slots is length/width ≥ 2.5 (with a limit of ≥ 2).
Using Hot Air Solder Leveling for Long Slots: For slots selected for hot air solder leveling, it's recommended that one side of the slot hole has a minimum width of 0.4 mm (with an absolute minimum of 0.3 mm) or consider using gold immersion technology.
Hot air solder leveling involves high-pressure and high-temperature processing. Small slot widths can lead to plating peel-off.
Slots with copper plating on one side but no copper ring on the other side, particularly single-sided copper ring slot holes, are more prone to peel-off due to high-temperature stress.
For densely arranged slots, it's advised to use gold immersion technology.
Hole Attributes in Via Design
During design, hole sizes are categorized as VIA holes or PAD component holes, and it's crucial not to mix them.
VIA Holes: These typically serve the purpose of providing electrical connections between circuitry on both sides. During manufacturing, VIA holes are usually treated with soldermask, and JLCPCB does not specify VIA hole size tolerances during production.
PAD Component Holes: These are generally designed as component holes for soldering components.
Mixing them can lead to:
Mistakenly treating VIA holes as PAD component holes and selecting solder mask treatment can result in solder mask covering or clogging component holes, making it unsuitable for soldering. This also makes it difficult to control their size effectively.
Using PAD component holes as VIA holes will prevent the software from giving them soldermask, resulting in vias requiring soldermask treatment remaining uncovered.
Trace Width and Spacing in Trace Design
Thinner traces are not necessarily better; wider traces are preferable whenever conditions allow. Thinner traces have lower conductivity, a higher likelihood of breakage, and lowered yield rates.
Standard trace width and spacing: 4 mils for both. Anything narrower than 4 mils is considered thin.
JLCPCB's minimum trace width/spacing capabilities:
| 1 oz | Single/double-sided: 0.10/0.10 mm (4/4 mil) Multilayer: 0.09/0.09 mm (3.5/3.5 mil); 3 mil allowed in BGA fan-outs PCB coils: 0.254 mm |
| 2 oz | Double-sided: 0.16/0.16 mm (6.5/6.5 mil) Multilayer: 0.16/0.20 mm (6.5/8 mil) |
| 2.5 oz | Double-sided: 0.2/0.2 mm (8/8 mil) |
| 3.5 oz | Double-sided: 0.25/0.25 mm (10/10 mil) |
| 4.5 oz | Double-sided: 0.3/0.3 mm (12/12 mil) |
Hatched Copper Filling in Large Area Traces
When filling large areas with copper, avoid using small hatched grids as this can severely impact production. Choose solid copper fill or large grids instead of small ones. Small grids can lead to several issues:
Inadequate solder mask coverage, as illustrated.
AOI (Automated Optical Inspection) may not detect small grids and may result in errors.
Small grids can cause solder mask peeling, affecting conductivity.
If you must use grid copper filling or need to separate networks, ensure:
Grid line width/spacing is at least 0.254 mm.
There is at least 0.254 mm spacing between traces from the same net.
Uneven Copper Pour Distribution
Uneven Outer Layer Copper Pour: Uneven outer layer copper pouring affects plating current balance and may lead to excessive copper thickness or short circuits due to resin gathering.
Uneven Inner Layer Copper Pour:
In cases where the void area is too large, the resin glue on the PP accumulates and flows toward the copper-free area. This results in thinner boards, copper wrinkling, missing resin causing white spots, and delamination issues.
For products with strict thickness requirements in key areas like gold fingers, if the corresponding inner layer area is too spacious, it can lead to thinning in the gold finger region, poor contact with connector slots, and other problems.
Inconsistent copper coverage area ratios on different layers can also risk board warping.
Copper Pour Design
Avoid Leaving Void Areas: Try to fill copper in void areas whenever possible.
Keep Copper Away from Normal Trace Pads: Ensure that when routing traces, the distance between traces, copper areas, and drill holes is at least 0.5 mm or more. Use solid copper fill rather than small grid copper fill.
Copper pours must be present on all layers where gold finger connectors are located to ensure the thickness of the final board. Care should also be taken to avoid laminate structures with insufficient thickness.
Copper Under Antennas: Follow product design guidelines for copper placement in antenna areas to prevent interference.
Consistent Copper Pour on Both Sides: Ensure that copper is consistently poured on both sides and not left empty on one side.
These design considerations are essential for a smooth PCB manufacturing process and to avoid common pitfalls.
Also Read: Top 6 Custom PCBA Defects Engineers Must Avoid
Conclusion
A well-designed PCB will not only function reliably but also contribute to the overall success of your electronic product. So, take the time to familiarize yourself with these design considerations, incorporate them into your workflow, and enjoy the benefits of a smooth and efficient PCB manufacturing experience.
Keep Learning
Custom PCB Layout Services in Modern Electronics
Custom PCB services are an important part of making electronics today because they make sure that exact design and performance needs are met. Custom PCBs are different from generic PCBs because they are made to fit the exact technical and functional needs of a wide range of businesses. These services cover everything from making prototypes to mass production, which lets companies make electronic products that are small, efficient, and very reliable. This article covers the importance of custom PCB ser......
5 Common PCB Design Mistakes to Avoid as a Beginner
PCB design is both an art and a science. Every electronics engineer wants to turn their circuit into a reliable printed circuit board. However, beginners often make the same mistakes that lead to noisy signals, overheating, failed prototypes, or costly redesigns. In this guide, we’ll examine the 5 most common PCB design mistakes and how to avoid them — with practical explanations and simple rules you can apply right away. 1. Poor Planning and Component Placement In mixed-signal systems (analog + digit......
PCB Layout Services and Impact in Electronics Design
The electronics design process depends heavily on professional PCB layout services. These services transform a schematic into a manufacturable printed circuit board by optimizing component placement, routing, layer stack-up, and thermal performance. In today’s competitive market, from consumer gadgets to automotive and industrial systems, expert PCB layout directly determines product reliability, size, and cost. JLCPCB offers integrated layout services through EasyEDA with automatic DFM checks, making......
How to Create Your Own PCB Trace Width Calculator with Python
PCB traces are critical for current carrying, signal integrity, and thermal performance in any design. While IPC-2152 provides the standard formulas, manual calculations are time-consuming. In this tutorial, we’ll create a lightweight Python trace width calculator based on IPC-2152. You can run it in any online compiler and cross-verify results with JLCPCB’s free online impedance calculator for real-world manufacturing accuracy. Let's start with an example: if I am designing a power PCB and my trace i......
Unraveling PCB Traces Magic Enhancing Electronics through Smart Design
Introduction Printed Circuit Boards (PCBs) are the foundation of modern electronics. At their core are conductive copper pathways known as PCB traces, which transmit signals between components. Proper trace design directly affects signal integrity, power delivery, EMI, and manufacturability. This article covers the fundamentals of PCB traces, key design considerations, optimization techniques, and how JLCPCB’s capabilities (including its free impedance calculator) help designers achieve reliable resul......
Annular Rings in PCB Design: Mastering Reliable Via Connections and Precision Fabrication
In fact, I have a question, which is worth considering: when did you last actually compute the worst-case annular ring size of your PCB, including all fabrication tolerances? When you say, or not recently, you are certainly not the only ones. We simply scale pad sizes to the EDA defaults or what we have already used without further checking whether this number measures up to the actual drill wander, layer mis-registration, and etch compensation. The only mechanical and electrical connection between th......