DFM Analysis and Improvements

Before continuing, you can watch the companion videos where I demonstrate the full DFM analysis and improvement workflow for the LattePanda Mu Carrier board. In the videos, I show how to export the Gerber files, run the HQ-DFM tool, and systematically correct each identified issue to ensure the board is ready for fabrication.

Introduction

Design for Manufacturability (DFM) analysis is a critical step that ensures a PCB design is not only electrically functional but also manufacturable and reliable. Even when a design passes all of KiCad’s built-in Design Rule Checks (DRC), manufacturing tools like NextPCB HQ-DFM can reveal hidden risks related to hole sizes, copper spacing, or annular rings.

This process is especially important for a dense, high-speed design like the LattePanda Mu Carrier, where tight tolerances and multiple high-speed interfaces demand precise clearances. Running a DFM analysis before sending the design to the manufacturer can prevent expensive fabrication errors and save weeks of development time.

Exporting Files and Running the DFM Analysis

The process begins by exporting Gerber and drill files from KiCad.
Use File → Fabrication Outputs → Gerber to generate the necessary files, ensuring that all copper, mask, and drill layers are included. Once exported, the files can be loaded into the NextPCB HQ-DFM tool, available for Windows.

An offer from our sponsor

The tool displays a layer-by-layer visualization of the board and automatically checks for manufacturability issues, including clearance violations, unconnected features, drill-to-copper spacing, and annular ring dimensions. When the analysis completes, the tool categorizes findings as Errors, Warnings, or Checks, each pointing to specific design regions that need attention.

Reviewing and Fixing Common Issues

The HQ-DFM tool flagged several issues in the initial analysis. Each was systematically reviewed and addressed.

1. Sharp 90° Corner in a Differential Pair

A 90-degree turn in an HDMI differential pair was detected. Sharp corners introduce impedance discontinuities and reflections, which can degrade signal integrity.
The solution was to re-route the trace with a gentle arc or 45-degree bend to maintain controlled impedance without altering pair skew.

2. Pad-to-Pad and Via-to-Via Spacing

Multiple areas showed spacing violations between vias and pads. Some measured 0.1 mm, below the manufacturer’s minimum of 0.2 mm. I compared these areas with the LattePanda reference design and contacted NextPCB engineers for confirmation before adjusting the layout. In most cases, I increased the spacing slightly to meet the specification.

3. Annular Ring and Drill-to-Copper Checks

Several vias had smaller-than-recommended annular rings. My vias used 3.94 mil rings, and the manufacturer’s minimum allowed 3.5 mil, which was acceptable.
However, some drill-to-copper clearances were borderline. I repositioned critical vias—especially those part of differential pairs—to ensure a minimum 8 mil (0.2 mm) spacing between copper and drills.

4. Copper-to-Edge and SMD-to-Edge Clearance

The copper pours near internal cutouts were too close to the board edge. This was corrected by rounding internal corners using arcs, which maintained consistent copper-to-edge clearance and improved manufacturability.
Additionally, the coin-cell battery pad was moved further from the edge to reduce mechanical stress.

5. Drill Spacing

In dense areas near high-speed interfaces, several vias were too close together. These were spaced apart slightly to meet hole-to-hole clearance requirements.

6. Silkscreen Overlaps

Some silkscreen text overlapped with pads, which could interfere with solder mask printing. I edited the affected footprints in KiCad, repositioning the text for better separation.

7. Ground Connectivity Improvements

Several ground pads were connected with short traces and stitched to the internal ground plane using vias. I replaced these short traces with solid copper fills, improving current capacity and reducing impedance on the ground network.

Repairing Drill-to-Copper Violations

The most significant set of issues involved drill-to-copper clearances, where vias were positioned too close to adjacent copper features. Out of 17 flagged cases, most affected high-speed differential pairs.

Each via was adjusted slightly to restore proper spacing while maintaining:

• Differential pair length matching to preserve signal skew.
• Symmetry between paired vias.
• Compliance with impedance and net class constraints.

After making the corrections, I re-ran the DFM analysis. All major errors were cleared, leaving only minor warnings that did not affect manufacturability or performance.

Final Verification

To conclude the process, I visually inspected the board using KiCad’s 3D Viewer. This final check confirmed that all copper pours, rounded edges, and via placements were clean and well-aligned.

After verifying every fix and confirming clearance compliance, I re-exported the Gerber and drill files. Once the last clarifications from NextPCB engineers were received, the design was ready for manufacturing.

Key DFM Checks and Their Purpose

The table below summarizes the most critical DFM checks performed and their corresponding objectives.

Ready for the next tutorial in this series? Here's the next one, or choose an alternative from the list of articles in the side bar. There's also lots of interesting article in our Blog. where you can read about off-grid communication technologies, electronics test equipment, course updates, and much more.