Intro: Why do fabricators always ask, "Where should this hole be drilled?"

In the electronics supply chain, speed is everything. From consumer electronics to the latest AI servers, Hardware R&D and Layout Engineers rush to release Gerber files before DVT (Design Validation Test), thinking they can finally take a break and grab a bubble tea. But within half a day, the inbox is flooded with "EQ Bombardment" (Engineering Queries) from the fabricator's CAM engineers.

"The Drill layer doesn't align with the Top layer. Which one is correct?" "Is Layer 3 GND or Power?" "Are the units in the drill file Inches or Millimeters?"

Every EQ iteration is a waste of time. Statistics show that over 30% of PCB project delays are caused by communication loops due to "non-standard output data." For projects racing against Time-to-Market, this is suicide.

This blog won't discuss deep electromagnetics; we are strictly talking about "how to output files correctly." By mastering Gerber, ODB++, and coordinate settings, you can transform from an engineer "hunted by the fab" into their "favorite efficient partner."

Round 1: Gerber vs. ODB++ — Why You Should Consider Upgrading

The Traditional Ruler: Gerber (RS-274X)

The Gerber format has dominated the PCB industry for decades. Essentially, it is just a "2D image."

• RS-274D (Obsolete): This is the legacy format. Its fatal flaw is that the "Aperture List" (D-code definitions) is separated from the graphics file. Fabricators often receive the graphics without the aperture list, leaving them guessing about line widths and pad sizes. If your software still defaults to 274D, change it immediately—it is extremely error-prone.
• RS-274X (Current Standard): This solved the "D" version's problems by embedding aperture definitions within the file. However, it is still just an "image." It doesn't know which circle is a Via and which is a Component Pad; it doesn't know if a footprint is an 0402 resistor or a BGA.

The Smart Rising Star: ODB++

As AI servers and HDI (High-Density Interconnect) boards increase in layer count (often exceeding 20 layers), the fragmented file structure of traditional Gerber (dozens of .gbr files) becomes increasingly difficult to manage. This is where ODB++ enters the stage.

ODB++ is not just a pile of images; it is a database.

1. All-in-One: It packages the layer stackup, netlist, drill data, and coordinate files into a single .tgz or .zip file. You will never again face the tragedy of "forgetting to attach the drill file."
2. Attribute Preservation: It distinguishes between a Pad and a Via. This is crucial for CAM processing (e.g., Vias may need plugging/tenting, while Pads need opening).
3. Fool-proofing: Because it includes a Netlist, the fabricator can directly compare electrical connectivity upon import, detecting graphical errors immediately.

eCloud’s Advice for Engineers: If you are designing a board with 4 layers or more, or one that includes HDI or blind/buried vias, we strongly recommend prioritizing ODB++ output. It can reduce CAM processing time by over 50% and significantly lower the chance of misinterpretation. If the fabricator insists on Gerber, ensure you output RS-274X and verify that file versions are consistent.

Round 2: Coordinate Alignment — The "Mystery" of Drill Files

This is the classic "low-level error": The Gerber graphics look perfect, but the drill holes (NC Drill) are shifted miles away, or their scale is 10x too large or small. This is usually not a software bug, but a coordinate format mismatch.

1. Precision Format: 2:3 vs. 2:4

NC Drill files are typically text files. To save space, they often omit the decimal point.

• 2:3 Format: 2 integers, 3 decimals (Resolution: 1 mil).
• 2:4 Format: 2 integers, 4 decimals (Resolution: 0.1 mil).

The Disaster Scenario: Suppose you output a coordinate 12500.

• If set to 2:3, the fab reads it as 12.500.
• If set to 2:4, the fab reads it as 1.2500. If the settings don't match, the drill location is off by a factor of 10! With modern components shrinking (e.g., 0.3mm BGA pitch), the 1 mil error margin of the 2:3 format is no longer sufficient.

2. Zero Suppression: Leading vs. Trailing

• Leading Zero Suppression (LZ): 00.125 becomes .125.
• Trailing Zero Suppression (TZ): 12.500 becomes 12.5. If the fabricator selects the wrong mode during import, 125 could be misread as 0.125 or 12.5, causing holes to "fly" all over the board.

3. Origin: Absolute vs. Relative

Absolute Coordinates mean every point is referenced to the board origin (0,0). Relative Coordinates mean the next point is referenced to the previous point. Always choose Absolute Coordinates! With Relative coordinates, if one point is calculated incorrectly, every subsequent point will be wrong. The risk is too high.

eCloud’s Advice for Engineers:

1. Standardize: Ensure Gerber and NC Drill output settings use the same units (Inches recommended), same precision (2:4 or 2:5 recommended), and same Zero Suppression settings.
2. Explicit Decimal: If your software supports "Explicit Decimal Point," check it. 1.25 is always 1.25, leaving no room for ambiguity.
3. Self-Check: After outputting, use a free viewer like ViewMate or CAM350 to overlay the Gerber and Drill files. If they look aligned to the naked eye, they are generally safe to send.

Round 3: Layer Naming — Don't Make CAM Engineers Guess

When a fabricator opens your zip file and sees Layer1.pho, Layer2.pho... up to Layer10.pho, they despair. They have no way of knowing if Layer 2 is a GND plane or a Signal layer.

Why is this critical?

• Stackup Sequence: If filenames are unclear, the fabricator might stack inner layers in the wrong order, ruining impedance control and Signal Integrity (SI).
• Top/Bottom Confusion: Sometimes Layer1 is Top, but some designers define Layer1 as Bottom.

Recommended Naming Convention

Use "Self-Explanatory" filenames:

• Top_Elec.gbr / L1_Top.gbr (Top Copper)
• L2_GND.gbr (Inner Layer Ground)
• L3_PWR.gbr (Inner Layer Power)
• Bot_Elec.gbr (Bottom Copper)
• Top_Silk.gbr (Top Silkscreen/Legend)
• Top_Mask.gbr (Top Soldermask)
• Board_Outline.gbr (The most frequently forgotten file!)

Top Overlay vs. Silkscreen

In Altium Designer, the silkscreen layer is called Top Overlay. Many beginners ask, "What is this?" It is simply the Silkscreen.

• Note: Never mix Assembly drawing content into the Silkscreen output. The Assembly layer often contains component physical outlines (Courtyards). If these lines are printed on the PCB, they may cross over pads, leading to soldering defects.

eCloud’s Advice for Engineers: Build a habit of including a README.txt or File_List.txt in your output package. List the mapping: "L1_Top.gbr is Top Layer, L2_GND.gbr is Layer 2..." This takes 2 minutes but saves the fab 2 hours of confirmation time and serves as your liability disclaimer.

Round 4: Mainstream EDA Software Output Guide

Different EDA tools have different "traps" in their output settings. Here are the essentials for the three most common tools in Taiwan:

1. Altium Designer (AD)

AD is user-friendly but prone to "accidental clicks."

• Critical Settings:
  • Gerber: File -> Fabrication Outputs -> Gerber Files. In the Advanced tab, verify the precision (e.g., 2:4).
  • NC Drill: File -> Fabrication Outputs -> NC Drill Files. The Units and Format here must match the Gerber settings exactly!
• Pitfall: Do not check "Generate Board Edge Rout Paths" unless you specifically intend to. The board outline should be output via a dedicated Mechanical Layer.
• Pro Tip: Use Output Job File (.OutJob). Configure it once, save it, and for every future revision, just click one button to auto-generate all files. This guarantees consistency.

2. Cadence Allegro (OrCAD)

Allegro is the standard for large system houses (like Quanta, Wistron), but its settings are complex.

• Critical Settings:
  • Gerber: Manufacture -> Artwork. Ensure every "Film" contains the correct classes. For example, the TOP Film should not contain SILKSCREEN.
  • NC Drill: This is the boss level. You must go to NC Parameters and check "Enhanced Excellon Format". This option automatically adds a header defining the format to the drill file, allowing CAM software to auto-recognize it, solving 99% of scale errors.
• Pitfall: Check Undefined Line Width. If set to 0, lines with geometry but no width attribute (often used for outlines) may disappear. Set it to 5 mils.

3. Mentor PADS

PADS users often face "Drill and Copper misalignment" issues.

• Critical Settings:
  • CAM Documents: PADS output is based on CAM document definitions.
  • Offset: This is the biggest trap! Each CAM Document (Top, Bottom, Drill) has an independent Offset setting. Ensure all output Offsets are set to (0,0). If the Top layer has an offset but the Drill layer doesn't, they will be misaligned.
• Pitfall: Before clicking "Run," use the PADS CAM Preview function. Select both Top and Drill layers simultaneously to view them. If they align on screen, the output is correct.

eCloud’s Advice for Engineers: Regardless of the software, "Version Control" is paramount. Do not name files Final_v2_Modified_RealFinal.gbr. Use dates or formal revision numbers (e.g., Project_RevA_20231027). Furthermore, once sent, if any modification is required (even just a silkscreen change), re-output the entire file set. Do not just send a single replacement file; this inevitably leads to version chaos.

Round 5: DFM Checks — Kill the EQ Before It Happens

Beyond format errors, certain "hard" design flaws trigger EQs.

1. Acid Traps: Trace angles less than 90 degrees. These trap etching solution, causing open circuits or shorts. Always use 45-degree chamfers or arcs. In practice, avoid acute inner angles and T-junctions without fillets.
2. Solder Mask Bridge Too Thin: If IC pins are too close, the solder mask sliver between them may be narrower than 3-4 mils. The factory cannot print this, and it will peel off. If space is tight, use a "Gang Opening" (one large opening for multiple pins) in your design.
3. The Importance of Netlist: Many people are too lazy to send the IPC-D-356 Netlist. This is wrong! Gerber is just a "Drawing"; the Netlist is the "Logic." The fabricator uses the Netlist to verify if your Gerber has broken connections due to software bugs. Treat it as your final insurance policy.

Conclusion: High-Quality Output = Professionalism

PCB file output may seem like just the final "Save As" step in the design process, but it is the critical moment where a product transitions from "Digital" to "Physical." A clean, standardized, and unambiguous output package not only makes the fab's CAM engineers grateful (they might even prioritize your order), but it also directly helps your company save costs and shorten lead times.

For those just starting out or currently learning: Start building good Output habits now! The best EQ is No EQ.