Prepare a manufacturing release

Before you start

• A PCB with DRC run and no errors
• A BOM with part numbers
• Your fabricator's or assembler's file requirements

Applies to: Resin web app

Follow the steps

1. 1

   Commit the source

   Run ERC and DRC one last time, then commit in Project > Version Control so the release can be traced to a version. The package is generated from the current working revision.

   Project > Version Control
   

   Expected result

   Changes is empty and History shows the commit.

2. 2

   Open Output & Export

   Open Project > Output & Export. The source strip shows the Version and the Variant the package will use; the active assembly variant is chosen in the schematic and PCB editors. If DRC has not been run on the current board, a readiness notice says so.

   Project > Output & Export
   

   Expected result

   The source strip shows the version and variant you intend to release.

3. 3

   Select the outputs

   Outputs are grouped as Fabrication (Gerbers, drill files, board outline DXF, ODB++, IPC-2581, IPC-D-356, fabrication drawing, stackup report, panelization), Assembly (pick-and-place, assembly drawing, BOM CSV, interactive BOM, test point report, stencil specification), Documentation (schematic PDF, PCB PDF, 3D PDF), Reports (DRC, ERC, board statistics), Netlists, Design & CAD exchange (Specctra DSN), and Other formats. Tick the ones your receiver asked for, or use Select recommended. Start from manufacturer preset applies a fabricator's settings, which you can still change. STEP, GLB, and IDF are exported from the 3D view's Export menu; the PCB editor's Export menu also offers an Altium Project (ZIP), and the schematic editor's Export menu offers KiCad Schematic and Altium Schematic files.

   Output & Export > Package outputs
   

   Expected result

   Every file the receiver asked for is ticked and nothing else.

4. 4

   Check the settings

   Select a row and press S, or open Output settings, to see its options: layers, units, origin, file naming, BOM columns, and so on. Settings changed here apply to this output only.

   Output & Export > Output settings
   

   Expected result

   Units, origin, and layer selection match the receiver's requirements.

5. 5

   Generate

   Choose Generate package (N). Progress is shown per output; a failed output is listed with its reason and the rest still complete. When it finishes, use Download package (.zip) or download single files. Generated files are held in the browser session; use Save package to keep them in the project.

   Output & Export > Generate package
   

   Expected result

   The ZIP downloads and every selected output is present.

6. 6

   Check the files

   Open the Gerber and drill files in a Gerber viewer and check the outline, layer count, drill holes, and that the layers align. Open the pick-and-place CSV and the BOM in a spreadsheet and check the reference count and board side. Open the STEP file in your mechanical tool if you exported one.

   Outside Resin
   

   Expected result

   Every file opens in its viewer and matches the board.

7. 7

   Save the configuration

   Use Save configuration or Save as... to keep the output selection and settings as a named package configuration, so the next release uses the same set.

   Output & Export > Save configuration
   

   Expected result

   The configuration is listed under saved configurations.

Check your result

• ERC and DRC clean
• Committed
• Version and variant confirmed
• Outputs selected
• Settings checked
• Package generated
• Files opened in viewers
• Configuration saved

Example files

Troubleshooting

Find the symptom, apply the fix, and repeat the affected check.