I’m reaching out because I made a mistake in my latest PCB design. I accidentally connected a pad on a QFN package IC to ground, while it should have been left floating or connected to a different signal. Thankfully, I requested a few samples before having the PCB fab house assemble all of them.
Reordering the boards would be costly, and there are vias-in-pad connected to internal layers. My idea is to disconnecting the IC’s exposed pad from the PCB’s ground pad using additional solder mask. The pads are currently tinned with HASL.
Could you advise if my next steps are feasible?
- Ask the fab house to mask the pads and assemble the boards.
- For my received sample boards:
• Desolder all the affected QFN chips.
• Remove all the solder with a copper braid.
• Clean with isopropyl alcohol.
• Apply solder mask paint cured by UV light or cover the pad with
Kapton tape.
• Re-solder the parts using a heat gun.
Would this approach work?
Putting solder mask over the unwanted pad would be easy.
1 Like
The rework can be achieved, but your fab house would probably need more details.
- Thickness of the boards?
- How many components need to perform the rework?
- What the pitch of the component?
- Alloy Type? Etc…
1 Like
Usually, a QFN package has an exposed pad to draw heat from the internal die and dissipate it into internal plane layers. If your component requires this heat sinking feature, wrapping it in a nice warm blanket of solder mask or Kapton tape will shrink its Safe Operating Area and probably shorten its life.
If you care about your product’s reliability, re-spin the PCB and correct this flaw.
2 Likes
Would this extra mask on only one pad upset the flatness enough that there might be problems reseating the chip and/or it might poke through the solder mask?
1 Like
IC vendors are not good about pointing out when an exposed thermal pad is not being used as a thermal pad, but in reality is only a default feature of the package. Many datasheets will spell out when it should be grounded, but other datasheets say nothing which is when mistakes can creep in.
If you do go the path of masking over the existing pad with solder mask (or maybe even a mask+silkscreen), be sure to modify the paste stencil so paste does not get applied during assembly. As JimJJewett already commented on…flatness might be a risk depending on the package details.
2 Likes
Doubtful this would be problem.
1 Like
Thank you for your valuable insight. I understand that it’s important to address the issue with the exposed pad for heat dissipation. I will consider your advice and evaluate the best course of action to resolve this issue.
I appreciate your guidance on modifying the paste stencil to ensure no paste gets applied during assembly—it’s a crucial step that I hadn’t considered.
Consider lifting and scraping off the pad with a knife for your received boards. Another option is to manually drill out vias or traces connecting the pad to GND using a small twist drill.
You might want to explore the option of purchasing polyimide adhesive dots, which are typically available in 1mil thickness. However, once you apply silicone adhesive, they tend to increase to around 2.5mils in thickness.
As for assembly, it’s advisable to consult with your assembly house or assembly team. For small quantities, considering that the coplanarity specification for QFP is typically +/-4 mils, this approach should likely suffice, possibly requiring a bit of extra attention to the stencil printing parameters to ensure a sufficiently thick paste layer. However, it’s worth noting that this method may not be suitable for very small parts, such as 0201 components on the same side of the board, which typically require a relatively thin paste.
1 Like
The fabrication house is unlikely to be able to mask the exposed pad. You may inquire, but be prepared for a negative response.
For small production runs, consider having the boards assembled while leaving the QFN unpopulated (modify the Bill of Materials to mark it as DNI - Do Not Install). If the fabrication house is sourcing the parts for you, request that they ship the unassembled QFNs along with the board. Additionally, provide an updated Gerber file for the solder paste stencil to remove the openings for the QFN pads, preventing any reflowed solder from accumulating on them. This approach will save you from unnecessary desoldering and cleanup.
For manual assembly of the QFN, apply a heat-resistant lacquer to the exposed pad. The lacquer should be as thin as possible to avoid raising the QFN pads too high off the copper. Ideally, it should be as thin as the existing solder mask. While Kapton tape (polyimide) could be used, it might be too thick. However, 25-micron thick Kapton tape, including the adhesive, might be suitable.
Once the pad is covered, use low-temperature solder paste, which can be applied with a tiny stencil just the size of the QFN if there is enough space around it. You can then use a hot plate, hot air, IR heater, or reflow oven to solder the QFN. The lower temperature solder paste helps avoid the risk of desoldering existing joints.
For larger production runs, it is likely more economical to respin the boards. Requesting non-standard procedures, such as covering pads from the assembly house, might cost more than simply remaking the boards.
1 Like