Gerber files are the fabrication artwork for each PCB manufacturing layer. In OrCAD PCB Editor and Cadence Allegro PCB Editor, they are generated as artwork films from the layout tool, not from OrCAD Capture.
Allegro-style output is more explicit than one-click tools: you define films, set artwork parameters, create Gerbers, then generate NC drill files separately. After zipping those outputs, open the viewer and verify that the board outline, films, and drill data agree before ordering boards.
This workflow is closest to other professional PCB tools where a release package is built from configured outputs. If you also use Altium, the Altium Gerber export guide covers the same Gerber-plus-drill handoff from a more dialog-driven interface.
Quick answer
In OrCAD or Allegro PCB Editor, use Manufacture → Artwork. In the Artwork Control Form, define films, set General Parameters to Gerber RS274X or X2 with the required numeric format, then click Create Artwork. Generate drills separately with Manufacture → NC → NC Drill, using the Parameters or NC Parameters button inside the NC Drill dialog to configure Excellon settings.
Step-by-step OrCAD / Allegro Gerber export
- Open the completed board in OrCAD PCB Editor or Allegro PCB Editor. Do not try to export Gerbers from OrCAD Capture; Capture can create schematic outputs and netlists, but Gerber artwork is a PCB layout output.
- Run the layout checks required by your process before artwork output. Resolve outline, constraint, and unrouted-net issues while you are still in the board database.
- Choose Manufacture → Artwork. This opens the Artwork Control Form. OrCAD PCB Designer uses the Allegro engine, so the same core artwork workflow applies across both products.
- In Film Control, define one film for each fabrication layer set. Typical names are TOP, BOTTOM, SOLDERMASK_TOP, SOLDERMASK_BOTTOM, SILKSCREEN_TOP, SILKSCREEN_BOTTOM, and an outline or route film for the board profile. Multilayer boards need additional films for inner signal or plane layers.
- For each film, confirm the subclasses included in that output. For example, a top copper film normally includes the top etch data and related pin, via, and shape information. A silkscreen film normally includes legend text and package geometry, not copper.
- Make sure the board outline is assigned to the proper film. In many Allegro databases, outline information is stored in board geometry or route-related subclasses. Your company or fabricator may have a standard film name for this output.
- Open the General Parameters tab. Set the device type to Gerber RS274X, or Gerber X2 if the manufacturer accepts and requests X2 attributes.
- Set the integer-decimal places, units, and zero suppression according to your CAM standard. The spec often uses leading-zero suppression, but the critical rule is consistency: the manufacturer must know the format, and the NC drill output must use compatible settings.
- Select the films you want to output and click Create Artwork. Allegro writes the Gerber artwork files for the selected films.
- Open Manufacture → NC → NC Drill, then use the Parameters or NC Parameters button inside the NC Drill dialog to configure Excellon drill format, units, precision, and zero suppression to match your fabrication requirements.
- Generate the actual drill output from the NC Drill dialog. Include plated and non-plated holes as required by your stackup and mechanical design.
- Collect the artwork files, NC drill file, and any drill reports or fabrication drawings requested by your manufacturer. Zip the release outputs from one board revision only.
Typical film and extension reference
| Typical film name | Typical extension | Purpose |
|---|---|---|
| TOP | .art, .gbr, or .GTL | Top copper artwork |
| BOTTOM | .art, .gbr, or .GBL | Bottom copper artwork |
| SOLDERMASK_TOP | .art, .gbr, or .GTS | Top solder mask opening |
| SOLDERMASK_BOTTOM | .art, .gbr, or .GBS | Bottom solder mask opening |
| SILKSCREEN_TOP | .art, .gbr, or .GTO | Top legend artwork |
| SILKSCREEN_BOTTOM | .art, .gbr, or .GBO | Bottom legend artwork |
| OUTLINE / ROUTE | .art, .gbr, or .GM1 | Board profile and routed features |
| NC Drill | .drl or .txt | Excellon drill locations and sizes |
Film and drill handoff details
Allegro and OrCAD PCB Editor do not depend on Protel-style extensions for the meaning of a layer. The film definition is the source of truth. A manufacturer may accept .art, .gbr, or conventional names such as .GTL, but each file must still contain the correct subclasses. Before release, open each film entry and confirm that etch, pins, vias, solder mask, legend, and route geometry are assigned deliberately rather than copied from an unrelated board.
Drill setup is a separate handoff. The NC Drill dialog creates the Excellon output after its internal parameters are set, so the drill file can be wrong even when artwork films look correct. Keep the artwork and NC settings aligned on units, integer-decimal format, zero suppression, and origin. For boards with slots, tooling holes, or mixed plated and non-plated holes, verify the drill report as well as the visible hole positions in a Gerber viewer.
Common mistakes to avoid
- Starting from OrCAD Capture by mistake. Capture can feed the layout database, but Gerber artwork is created from OrCAD or Allegro PCB Editor after placement and routing.
- Reusing film names without checking subclasses. A film called SILKSCREEN_TOP is only useful if the correct legend and package-geometry subclasses are actually included.
- Setting artwork format parameters and forgetting to open the NC Drill dialog's Parameters or NC Parameters control. Drill units and zero suppression must match the release requirement too.
- Creating artwork and assuming an Excellon file was generated at the same time. Manufacture → NC → NC Drill is a separate output step.
- Omitting route or outline subclasses for board-edge slots. Slots may need route artwork, drill data, or manufacturer-specific notes depending on how the design represents them.
- Archiving files from several artwork runs in one ZIP. Allegro projects often use custom file names, so stale outputs are harder to spot by extension alone.
Verify your Gerbers before ordering
Load the ZIP that contains your selected artwork films and NC drill file into the Gerber viewer and inspect by film purpose, not only by filename. Look for a visible board profile or route film, correct copper polarity, top and bottom solder mask openings, readable legend artwork, and drill hits centered in pads.
If a film is blank, first check whether its subclass list is empty or pointed at an unused class. If holes are offset, return to the NC Drill dialog and review the internal parameters before regenerating both the drill output and any affected artwork. Keeping the files synchronized from the board database is more reliable than patching a release ZIP manually.
FAQ
- Can I export Gerbers from OrCAD Capture?
- No. Capture is the schematic environment. Gerber artwork comes from OrCAD PCB Editor or Allegro PCB Editor after the board layout has been placed and routed.
- What is a film in Allegro artwork export?
- A film is a named output layer set in the Artwork Control Form. Each film usually becomes one Gerber file, such as TOP, BOTTOM, SOLDERMASK_TOP, or SILKSCREEN_TOP.
- Should I use RS274X or Gerber X2 in Allegro?
- Gerber RS274X is the broadly accepted baseline. Gerber X2 may be appropriate when your manufacturer supports the additional attributes. Use the format requested by the board house.
- Why do my Allegro drills not line up with Gerbers?
- The usual causes are mismatched units, integer-decimal format, origin, or zero suppression between Artwork and NC Drill settings. Regenerate both outputs from the same board revision with consistent parameters.