QFN Package Stencil Design for Thermal Pad

 To effectively remove heat from the package and maximize electrical performance, it is crucial to solder the die paddle to the PCB thermal pad with minimal voids. Despite potential challenges due to thermal vias and the large size of the thermal pad for larger packages, striving for minimal voids is essential. Furthermore, careful consideration must be given to the reflow process, as out-gassing can lead to defects if the solder paste coverage is too extensive. Therefore, using smaller multiple openings in the stencil for solder paste printing is recommended, as this can result in 50% to 80% coverage, as illustrated in the figure below. While improved coverage generally enhances thermal contact, it's important to be mindful of potential voiding and floating issues in QFN packages.

Thermal Pad Stencil Design for 7mm x 7mm (Left side) and 10 x 10 QFN Packages with 4.9mm and 7.4sq Pads

Depanelization Tab Routing

Board assemblies can be de-tabbed using perforated breakaway tabs, v-grooves breakaway tabs, or hand-cutting with a de-tabbing tool. For Tab and V-Score (i.e. PCBs that must be sheared along an edge):

1. Traces and via should be a minimum distance of 0.050"(1.27 mm) from the routed/scored edge.
2. Components should be a minimum of 0.100"(2.54 mm) away from routed/scored edge.

The rules are set to prevent components or board damage during the depanelization process and prevent flooding during the wave soldering process.

For 0.062" (1.6 mm thickness) Printed Circuit Boards:

1. Perforation holes should be typically spaced at 1 mm intervals.
2. Tab routed with a 1 mm radius.
3. Routed slot should be 2 mm minimum, for single image panels. Use 3 mm routed slots when two or more boards are in a panel. This allows for more accurate edge dimensions.
4. 75 mm typical distance between tabs, not to exceed 100 mm.
5. Place tabs approximately 25 mm from corners to reduce sagging during reflow or wave soldering.
6. Desirable to have at least one tab per side.
7. A slight inset of perforation is preferred; it provides an edge that requires little or no additional labor to clean up.

NOTE: Two parallel edges are required for a PCB to be processed in the SMT line. This is to prevent skewing through the conveyor system. All odd-shaped PCBs MUST have edge rails incorporated to meet this requirement. Custom reflow fixtures will be made if this requirement is not met.

Design for manufacturing or DFM

Design for Manufacturability rules and guidelines are a collection of PCB design best practices to help our design be as easily manufacturable as possible. The easier it is to manufacture a PCB, the more likely it will be to reduce both manufacturing errors and costs. DFM rules have been developed by PCB manufacturing experts and the rules will vary depending on the board design, and the manufacturer's capabilities.

It is highly recommended to check with the PCB manufacturer for their precision and limit on the width of the solder mask Dam. Solder mask dam between surface mount pads will prevent solder bridging during assembly. Below is one of the PCB suppliers' capabilities.

In summary, the width of the solder mask dam depends on the copper thickness and solder mask color. Generally, 3 mils of solder mask dam can be achieved using 1oz of copper but that will be 6 mils for 2 oz of copper. Similarly, the minimum solder mask dam for the Green solder mask is 3 mil and others will be 5 mil.

To get a solder mask dam between pads (if individual relief is required) spacing between copper should be 8 mils or more. Otherwise, the finished PCB will get block relief without a solder mask dam.

PCB under microscope with and without solder mask dam can be seen in the photo below.

PCB Know How

Generic Standard on PCB Design (IPC2221A)

PCB

Rigid Laminate material (FR4, typically) consisting of a glass epoxy substrate clad with copper on two sides for double sides (0.062” typically)

PCB fabrication Gerber data requirement

1   1) Top Electric (Artwork)

2   2)    Bottom Electric (Artwork)

3   3)    Top Silk (Artwork)

4   4)    Top Resist (Artwork)

5   5)    Plated Through Hole (N.C Drill)

6   6)    Non-Plated Through Hole (N.C Drill)

7   7)    Board Outline (Artwork)

8   8)    Drill Table

    Electrical Clearance

    AC and pulsed voltage > 200V must consider the dielectric and capacitive effect of the substrate in addition to spacing.

     

     Minimum spacing requirements according to withstand voltage are as below

Withstand Voltage (V)	Minimum Spacing (mil)
0 ~ 30	3.9
31 ~ 150	24.0
151 ~ 300	49.2
301 ~ 500	98.4

Electrical Isolation (Creepage Vs Clearance)

     Creepage is the shortest path between two conductive parts measured along the surface of the insulation. Clearance is the shortest distance between two conductive parts measured through air.

     Copper Weight

     1 oz of copper will cover one square foot area when rolled out to a thickness of 0.0014 inch or 1.4 mil.

Copper Weight (oz)	Thickness (inch)
½	0.0007
1	0.0012 ~ 0.0014
2	0.0028

     PCB Surface Finishing

     Different types of PCB finishing are as below

     1)    Hot Air Solder Level (HAL or HASL)

     2)    Hard Gold-Electro plated gold

     3)    Electro Less Nickel Emersion gold

     4)    White Tin

     5)    Organic Solderable Preservative (OSP)

     

     The most common surface finishing we can see is Hot Air Solder Leveling. In this process, Panels are processed through a bath of molten solder, conversing all exposed metal surfaces. High-pressure hot air, directed at both sides of the panel simultaneously, removes excess solder from the holes and surfaces.

     PCB Trace Width vs. Current Table

       A PCB trace width vs. current table helps you understand the relationship between PCB trace width and current carrying capacity so you can determine the required trace width for your printed circuit board design.

IPC Recommended Track Width for 1 oz copper PCB with 10°C temperature rise.