Small SMD components like capacitors and resistors appear in most designs, even in basic prototypes or hobbyist designs. Once you get down to 0603 or 0402 SMD components, it’s still possible to solder these components by hand if needed, even without a professional soldering station. This means that you could assemble your own boards or do rework with these components.
There are two much more aggressive size codes that appear in much higher density designs: 0201 and 01005. These components are so small that they are very difficult to place and solder by hand, and they can easily fly off your lab bench if you’re not careful. There are other points to consider in your design software that can aid successful application of solder paste and printing prior to reflow. With some basic design rule settings, you can implement these successfully and achieve high yield.
In this article, it is assumed that all case referenced sizes are in Imperial units.
0201 and 01005 Assembly Starts in Design
At a high level, the assembly process used for 0201 and 01005 footprints is not much different than the standard process for larger case SMD components. 0201 components have become the new 0402 components as design densities scale to higher levels. The same applies to SiP and heterogeneously integrated processors, which may include some in-package/on-chip capacitance for power integrity purposes.
Although your assembler might have the SMT capabilities required to successfully assemble boards with 0201 and 01005 parts, this does not guarantee high yield assembly. Footprints also need to be designed correctly to enable successful assembly with high yield.
0201 and 01005 Land Patterns
The critical aspect of creating a footprint for a 0201 component is to place the correct pad size and spacing between the pads. This probably sounds obvious as all SMD components need the right pad size and spacing, but it’s much more important with 0201 and 01005 components. The reason for this is the possibility of two defects:
- Tombstoning or skewing due to poor wetting of one terminal, which can happen much more easily if the component is only slightly misaligned on the pads
- Head-in-pillow that can occur without skew due to weak wetting on one side of the component
The placement of pads with the right gap will ensure that the leads of the chip are making contact with each pad. There is less margin for error with 0201 components than with 0402 and larger case components, so high yield only results with a narrower range of spacing values between pads.
A 0201 imperial case code example is shown below. The values shown in the tables below are IPC-recommended values for 0201 land patterns.
The nominal value of 0.66 mm between pad centers gives an edge-to-edge spacing of 0.2 mm. Some manufacturers will note or allow for larger edge-to-edge spacings and smaller nominal pad sizes of 0.3 mm and 0.3 mm (A and B) respectively. If the edge-to-edge spacing gets much farther beyond this, you may have defects below one of the pads, and the defect will only be noticeable in automated optical inspection (AOI) of the solder joint.
01005 pads are much more aggressive and they leave smaller possible ranges for pad size and spacing. If your assembler can provide 01005 SMT assembly capabilities, ask them for a recommended pad size and spacing, and modify your 01005 footprints to match their requirement.
Solder Dam Between Pads
The above footprint is a good starting point from an assembly consideration as it allows sufficient space between pads and large enough land pads for application of solder paste. However, there is one other point to consider that relates to the solder mask.
It is a good idea to ensure there is some leftover solder mask between pads on 0201 and 01005 components. On the 0201 pad above, the solder mask expansion applied around pads could be so large that you end up creating a sliver, which would snap off the board during fabrication and assembly. In the 0.2 mm spacing above, we only have 8 mils between the pads; this limits the allowed solder mask expansion to no more than approximately 2 mils around the SMD pads.
When you get down to 01005, you may not have any room for solder mask between the pads. Make sure you understand this limitation and apply the appropriate solder mask expansion value in your design rules. Your fabrication house also needs to have very low misregistration tolerance when building the board to ensure that your pads have large enough land area for solder paste application. This is a balancing act that your assembler can assist with.
No matter what components you want to assemble on your PCB, you can create cutting-edge designs that push the limits of density with the complete set of design features in Allegro PCB Designer. Allegro is the industry’s best PCB design and analysis software from Cadence, offering a range of product design features with a complete set of management and version control capabilities. Allegro users can access a complete set of schematic capture features, mixed-signal simulations in PSpice, and powerful CAD features, and much more.