The PCB manufacturer I work with mentioned that the cost remains the same for board thickness between 0.4mm and 1.6mm (for a 2-layer design). What are the advantages of opting for thinner or thicker FR-4 board thickness? My assumption is that thinner boards are lighter but could pose challenges for pick-and-place machines due to bending, while thicker boards might help with signal isolation. Are there other factors to consider?
Depends on the design but for a regular double sided – 2 layer – pretty much industry standard is .059”-.063” thick material. It’s cost effective due to the high volume and is easy to process. Thinner isn’t a problem but it’s best to keep it at least .030” thick to avoid any handling/process issues. Good example is no one makes a de-burr machine that can reliably process panels below .030”and this isn’t something you want to do by hand for no good reason. A 2 layer is built on a standard core so probably the biggest factor is glass style with thicker cores typically being made with heavier cloth. Usually not a problem unless the board has special requirements like 6mil holes and laser rout making thinner material a better choice.
2 Likes
Thanks a bunch! It’s great to get a practical perspective. So, sticking to the .059"-.063" thickness range for a 2-layer design makes sense for cost-effectiveness and ease of processing. I hadn’t considered the challenges with handling and processing thinner boards below .030". And the point about glass style and its impact on special requirements like hole size is quite interesting. Anything else you think is crucial when deciding on board thickness for a 2-layer design?
1 Like
Absolutely, glad the info was helpful. When considering board thickness, thermal considerations can be crucial too. Thicker boards might handle heat dissipation better, but thin ones could offer more efficient thermal performance in certain cases. Also, if your design involves tight space constraints, a thinner board could be advantageous. It’s a bit of a balancing act, and it’s fascinating how these factors play into the decision-making process.
1 Like
Finding the right balance is key here. For instance, if a thinner board offers advantages like improved flexibility to mitigate vibrations, that’s great. However, opting for a thicker board would be wiser if the board undergoes stress or strain.
In reality, the differences between these options are usually minimal. Follow your board manufacturer’s or supplier’s recommendations, as they have the expertise to suggest the most suitable option based on your specific requirements.
1 Like
In most cases, unless there are specific space or design constraints, opting for the thickest available board (such as 1.6mm) is a reliable choice. Many manufacturers offer this thickness at the same cost as thinner options. However, the optimal board thickness can depend on several factors, which should be considered based on your design needs:
-
Thinner boards can be flexible, which may create challenges for assembly machines if the board is too large or panelized incorrectly. V-grooves are not recommended for very thin boards, and smaller panels are preferable to larger ones. The maximum size for thin boards is determined by the fabrication house. Additionally, flexible boards can lead to broken connections with components, particularly BGAs, so proper support from the casing is crucial to prevent this issue.
-
In multilayer boards, the thickness of the PCB determines the thickness of the dielectric between layers, which affects the capacitance and can influence signal integrity. For high-frequency signals where impedance matching is critical, choosing the right board thickness is essential for optimal performance.
-
Certain PCB edge connectors or PCB-based USB connectors require the board to match the thickness of the mating connector for a proper fit.
-
Thinner boards take up less space in the enclosure, which can be critical for compact devices like USB dongles or Bluetooth headsets, where every millimeter counts.
-
Thinner boards are lighter, which can reduce shipping costs and result in a lighter end product, making them a better choice in applications where weight is a critical factor.
-
Some through-hole components are designed to work with specific board thicknesses. For example, press-fit connectors might require a certain thickness to ensure proper mechanical fit and reliability.
While the standard PCB thickness 2-layer option (around 1.6mm) is commonly used for ease of processing and general reliability, thinner boards can be beneficial in certain design scenarios, such as space-saving or specific mechanical requirements. It’s always a good idea to balance these factors with your design needs.
1 Like
One notable advantage of opting for thinner boards, which hasn’t been highlighted yet, is the ability to drill smaller vias. This is due to the maximum aspect ratio (the ratio of drill depth to drill diameter) that mechanical drills can achieve. A thinner board allows for smaller vias, which can result in lower capacitance, assuming all other factors remain equal. This can be particularly beneficial in high-frequency designs where minimizing parasitic capacitance is crucial for maintaining signal integrity.
1 Like
One of the primary issues with thinner boards is their tendency to flex during assembly. When running them through a pick-and-place machine, the pressure applied to seat components can cause the board to bend or “bounce,” potentially dislodging components that were previously placed. This can be a significant challenge, particularly with larger boards. Over time, thinner boards might also be more prone to warping, though this depends on factors like the environment and how the board is supported in its final application.
1 Like