Manufacturing Outputs

Overview#

A fabricator needs files, not your design document. A typical order contains:

• Gerber files, one per layer. Autodesk says the CAM Processor uses Gerber RS274X by default and also supports Gerber X2.
• Drill files in Excellon format.
• Optionally ODB++ (Export ODB++: .tgz, .zip or .tar).
• An IPC-D-356 netlist (ASCII, used by manufacturers for test fixtures), if requested.
• A BOM from the Electronics Bill of Materials.
• A Pick and Place (centroid) file with layer, XY location and rotation of SMDs.

Where to find it#

• In the 2D PCB, the Manufacturing toolbar holds CAM Preview, CAM Processor, CAM Export, PickAndPlace, Export ODB++ and IPC-D-356 Netlist.
• The CAM Processor runs CAM job templates; Fusion automatically selects a predefined template that fits the board's layer setup (for example a two-layer board), and you can Load job file and Set as Active CAM job.
• The Bill of Materials opens from the Common tab of a project, or from the Document tab of a schematic or 2D PCB; it updates automatically as the design changes.

Step by step#

1. Finish the design. Clear ERC and DRC with your fabricator's rules (Autodesk recommends running DRC before CAM Preview), and re-fill copper pours.
2. Check the stack in the Layer Stack Manager.
3. Run CAM Preview (Manufacturing toolbar): check the Preview (top, bottom, drills), Board and Drills tabs. PTH and NPTH holes and drill counts are listed; the Drills table exports as CSV or JSON, and the preview can export DXF or PNG/JPG.
4. Optionally open CAM Processor to review output files, load a fabricator's job file, and click Process Job. Output is a ZIP with subfolders for Assembly (TXT), Drill (XLN) and Gerber (GBR) files; Upload to Fusion is optional. The default folder is set in Preferences > Electronics > Directories.
5. Or use CAM Export for a one-click ZIP (review the file list and template, optionally Upload to Fusion, then Save).
6. Autodesk's ODB++ default prefix is CAMOutputs/ODBFiles and Gerber is CAMOutputs/GerberFiles.
7. Verify visually. Open the files in a Gerber viewer (the fabricator's online viewer works) and confirm outline, drill hits and silkscreen.
8. Export the BOM. Open Bill of Materials, use Column Settings to show attributes (including custom ones), then Export BOM and choose a format such as .csv. The list type switcher offers Group by Value (Device, Technology, Package, Value) or Components (flat list).
9. Generate pick-and-place, if ordering assembly, with PickAndPlace (writes an MNT file; the mountsmd ULP writes separate top and bottom SMD files). Confirm the origin and rotation conventions with the assembler.
10. Zip the Gerber and drill files and upload with the order.

Options reference#

Tips and pitfalls#

Warning: Always run DRC immediately before generating files. A late edit without re-checking is how clearance violations reach production.

Tip: If a fab supplies a CAM job file, load it in the CAM Processor (Load job file > Set as Active CAM job).

Warning: Fabricators and assemblers differ on rotation conventions in pick-and-place. Compare one polarized part (an IC or LED) in the viewer with its rotation in the file before ordering assembly.

Tip: Keep a "release" folder per revision, with the zip, BOM and a note of the design version.

Warning: Do not trust only the 3D view for verification. Gerbers can reveal missing outlines or wrong drill sizes that 3D hides.

Tip: Name nets and add the board name to silkscreen; it identifies the revision when you hold the physical board.

Practice exercise#

Generate Gerber and drill files for your practice board. Open them in a free online Gerber viewer. Verify the board dimensions against your outline, find the mounting holes in the drill layer, and confirm the silkscreen text is readable and not mirrored. Export a BOM CSV and check that every part has a value.

File set by board type#

File extensions per layer are not listed in Autodesk's pages, which only mention subfolders for Gerber (GBR), Drill (XLN) and Assembly (TXT). The common extensions .GTL, .GBL, .GTS, .GBS, .GTO, .GBO, .GTP, .GBP are general industry naming and may not match what your job produces. If your fab asks for a different naming scheme, load their CAM job instead of renaming files by hand.

Worked example: preparing an order for a 45 x 30 mm two-layer board#

1. Clear ERC and DRC against the fab's published rules (for example 0.15 mm trace and space, 0.3 mm drill).
2. Check the area: 45 x 30 mm is 13.5 cm2. Many prototype services price by area and quantity (general guidance); five boards total 67.5 cm2 of board.
3. Run CAM Export (or Process Job in the CAM Processor), saving to a folder named sensor_v1.2_gerber.
4. Open the zip in the fab's online viewer. Check: outline 45 x 30 mm (use the viewer's measure tool), four mounting holes at 3.2 mm, silkscreen readable, no text over pads.
5. Confirm the drill table: the number of distinct drill sizes (for example 0.4 mm vias, 0.8 mm header pins, 3.2 mm mounting holes) and total hole count against what you expect.
6. Choose finish and thickness: 1.6 mm FR-4, 1 oz copper, HASL lead-free for cost or ENIG for fine-pitch parts and flatter pads.
7. Order, and keep the exact zip you uploaded in a release folder.

BOM details#

The Electronics BOM groups parts by Device, Technology, Package and Value in the default list type, and supports assembly variants (3D PCB and Drawings show only the Base variant).

A BOM line for passives that are only distinguished by tolerance or voltage must carry those in the description (for example 100nF X7R 50V 0603), otherwise the assembler may substitute a 10 V part.

Pick-and-place details#

A centroid file lists, per part: designator, X, Y, rotation and side. Points to check with a physical or rendered sample:

• Origin. Autodesk's pages do not state the origin convention; many assemblers expect the lower left corner of the outline (general guidance), so check the file against a known part.
• Rotation. Rotation zero is defined per footprint. A SOT-23 drawn with pin 1 at top-left and a reference rotated 90 degrees can load incorrectly in the assembler's library. Spot-check at least one IC, one polarized capacitor and one LED against the assembler's preview.
• Bottom side parts. The X coordinate of a mirrored part may be reported flipped; compare with the assembler's documentation.

Choosing and verifying fab capabilities#

The fab values here are general guidance, not Autodesk data.

When a fab's value is tighter than your design rule, your design is still fine; when it is looser, DRC will pass while the order fails. Always enter the fab's real numbers, not what you hope they can do.

Failure modes and fixes#

Revision control for releases#

1. Increment the version on the silkscreen (V1.2) and in the file name.
2. Generate fresh DRC output and note "DRC clean" with the date in the release notes.
3. Store: Gerber zip, BOM CSV, pick-and-place file, PDF of the schematic, PDF of the board, and a copy of the rules file and CAM job used. Alternatively tick Upload to Fusion to publish the ZIP to your project, which creates a new version (v1, v2, ...) of one file per job; the design must be saved in a Fusion project.
4. Tag the Fusion design version with the same string.

Practice exercise#

Create a release package for your sensor board.

1. Run DRC with the fab's numbers.
2. Run CAM Export into sensor_v1.0_gerber.
3. Open them in a viewer and measure the outline (45 x 30 mm) and a mounting hole (3.2 mm). Write both numbers down.
4. Export the BOM and confirm the totals: count rows and quantities against the schematic.
5. Run PickAndPlace. Choose one polarized part and write down its rotation, then compare with the 3D view.
6. Zip the folder, name it with the version, and write release notes of three lines: what changed, DRC result, fab rules used.

Related#

• ERC, Design Rules and DRC
• Board Layout
• Electronics Limits in Personal Use