Altium to Gerber: step-by-step export settings for PCB fabrication

Export RS‑274X Gerbers and Excellon NC drills from Altium Designer, verify them in a CAM viewer, then zip and send to your PCB manufacturer.

Which layers do fabs need?

• Top/Bottom Copper: .GTL / .GBL

• Top/Bottom Solder Mask: .GTS / .GBS

• Top/Bottom Silkscreen (Legend): .GTO / .GBO

• Board Outline (profile only, single closed line): .GKO or .GM1/.GML

• Plated and Non‑Plated Drill files (Excellon): .TXT (or .DRL) plus .DRR drill report

• Solder Paste (for assembly): .GTP / .GBP

Step‑by‑step in Altium Designer

1) Prepare the PCB. Finalize the board shape in the PCB editor and place a single, closed outline on a Mechanical layer named clearly (e.g., “Board Outline”). Avoid multiple overlapping outlines and keep the outline at zero width.

2) Generate Gerbers. In the PCB document: File > Fabrication Outputs > Gerber Files…

• Units: Metric (mm); Coordinate format: 2:5

• Format: Embedded apertures (RS‑274X). RS‑274X is universally accepted; X2 is also fine if your fab supports it.

• Plot Layers: select Top/Bottom Copper, Solder Mask, Silkscreen, and the Mechanical layer that carries the board outline. Do not mirror bottom layers.

• Solder mask expansions: From rules (check your Clearance/Mask rules before plotting).

• Rebuild polygons before plotting so pours are current.

• Generate to a clean output folder.

3) Generate NC drills. File > Fabrication Outputs > NC Drill Files…

• Units: Metric (mm); Format: 2:5; Zeros: Suppress leading zeros (common choice and widely readable).

• Separate files for Plated (PTH) and Non‑Plated (NPTH) holes.

• Also generate a Drill Map and a Drill Report (.DRR) listing tool sizes.

4) Verify in a CAM viewer. Use Altium’s CAM editor (CAMtastic) or any independent viewer: import Gerbers and drills, confirm that drill hits are centered in pads, the outline is a single closed contour on its own layer, bottom layers are not mirrored, text is readable, and reference designators are not clipped. Typical manufacturable minimums to eyeball: legend line width ≥ 0.12 mm (5 mil), solder mask web ≥ 0.10 mm (4 mil), annular ring ≥ 0.10 mm (4 mil) for standard Class 2 work.

NC drills and board outline specifics

Keep PTH and NPTH drills in separate Excellon files; this avoids ambiguity around plating. If you use slots, generate them in the drill file as routed slots (oval/slot definitions) rather than drawing them in copper. The board outline should appear once only; do not place it on copper/silkscreen/mask layers. Include cutouts as closed shapes on the same outline/mechanical layer.

Naming, units, and coordinate format

Stick to mm and 2:5 coordinates for both Gerber and drill. Use a consistent file naming convention per layer (e.g., <job>_GTL, <job>_GBL, etc.). Set the PCB origin to a board corner for human‑readable coordinates; keep scale = 1.000. Zip only the fabrication set (Gerbers, drills, outline, drill report, and an optional README with stackup and notes).

What to double‑check before sending?

Open copper pours are up to date; no orphaned thermals. Silkscreen does not overlap exposed pads. Solder mask openings exist for all components that need them; testpoint mask tenting is per your intent. Impedance‑controlled traces are clearly called out in your README or fabrication notes with target values and reference layers. Vias tenting/plugging requirements are documented. If your design uses embedded copper coins, backdrilling, or edge plating, call these out explicitly—Gerbers alone don’t carry process intent.

Do you support IPC Class 3 and RoHS?

Yes. Boards can be built and inspected to IPC Class 2 or Class 3 acceptance criteria, and RoHS/REACH compliance is supported. HyperPCB operates an ISO 9001:2015 certified quality management system (SGS CN‑2023‑Q1156, valid to June 2027). Quotes are returned within 24 hours and DFM feedback within 1 business day, so if something in your export looks risky, you’ll hear from us fast.