Before generating any file
- Tools > Database Check — checks database integrity (enable DRC and shape updates).
- Display > Status — review DRCs, unrouted connections and out-of-date shapes. Everything should be zero or justified.
- Review the silkscreen: nothing on pads, readable references, pin-1 and polarity marks.
Gerber (RS-274X)
In Manufacture > Artwork you create one “film” per layer, choosing which subclasses go into each:
| Film | Typical content |
|---|---|
| TOP / BOTTOM | Etch, pins and vias of the outer layer |
| L2…Ln | Inner signal layers and planes |
| SOLDERMASK_TOP/BOT | Mask openings (pins, untented vias) |
| PASTEMASK_TOP/BOT | Stencil apertures (SMD only) |
| SILKSCREEN_TOP/BOT | Component legend |
| FAB / DRILL | Outline, dimensions, drill table and symbols |
Drilling
- Manufacture > NC > NC Parameters — format and units (agree with the fabricator).
- Manufacture > NC > NC Drill — generates Excellon files; separate plated and non-plated holes, and layer pairs for blind/buried vias.
- Manufacture > NC > Drill Legend — drill table for the fabrication drawing.
Intelligent formats: IPC-2581
IPC-2581 packs layers, drilling, stackup, netlist and BOM into a single file, eliminating the interpretation of dozens of loose files. In Allegro X, export via File > Export > IPC 2581. Ask your fabricator whether they accept it — more and more do.
Test netlist: IPC-D-356
The fabricator uses the IPC-D-356 netlist for electrical test (flying probe or bed of nails) and to compare the Gerber with your design intent. Export via File > Export > IPC 356.
Fabrication notes (must-haves)
- IPC-6012 performance class (2 or 3) and IPC-A-600 acceptance criteria.
- Material (IPC-4101 specification), Tg, finished thickness and tolerance.
- Stackup, copper per layer and impedances with tolerance.
- Finish (e.g., ENIG per IPC-4552), mask and legend colors.
- Via treatment per IPC-4761 (plugged, filled, capped).
- For assembly: BOM, pick-and-place, assembly drawing and IPC-A-610 / J-STD-001 class.
References and further reading
- IPC-2581 Consortium — open manufacturing data format
- Sierra Circuits — technical blog (DFM and fabrication files)
Original text for educational purposes. Menus and commands may vary between Allegro X versions; check the Cadence documentation for your version.