Export Gerber files from Altium Designer

A PCB manufacturer does not need your project. It needs manufacturing data: one Gerber file per layer and drill files for the holes. This guide walks you through exporting them from Altium Designer so the board can go straight into production.

Buttons and menus appear as Altium Designer shows them, in English. The steps follow the unified Gerber X2 Setup window in current Altium Designer; older dialogs look different. The windows in the figures are redrawn after Altium Designer, so your version may differ in small details. We have verified exports from Altium Designer 21.3 and 26.3 with our automatic check, which we run after you upload ("our check" below).

What we need from you

We cannot take an Altium project. We do not read .PcbDoc, .PrjPcb, .SchDoc or .OutJob files, and a board cannot be made from them. Upload manufacturing data instead: Gerber files and NC Drill files in one ZIP. KiCad is the only project format we convert directly. We do not list ODB++ or IPC-2581 as accepted formats, so use Gerber and NC Drill.

The figure shows what a two-layer board needs and how Altium names the files. For boards from Altium we have checked both naming options: *.gbr and extensions such as .GTL. You need the paste layers (Paste) only if you order a stencil with the board.

1. Check the board

First set the Altium rules to our limits. Open Design » Rules (the PCB Rules and Constraints Editor window). The table shows which rule matches which value. The full list of limits is in our PCB manufacturing capabilities.

Limit	Altium rule
Track width: at least 0.2 mm	Width (Min Width)
Spacing between copper objects: at least 0.2 mm	Clearance
Annular ring (copper around a hole): at least 0.12 mm	Minimum Annular Ring
Plated holes (PTH): from 0.3 mm	Hole Size
Non-plated holes (NPTH): from 0.5 mm	a second Hole Size rule
Hole to hole: at least 0.2 mm	Hole To Hole Clearance
Hole to board edge: at least 0.2 mm	Board Outline Clearance
Board size: from 10 × 10 mm to 155 × 130 mm (either orientation)	no rule

Altium applies a new rule to all objects by default (scope All). So for non-plated holes, create their own Hole Size rule with a minimum of 0.5 mm. Under Where The Object Matches choose Custom Query and enter the query IsPad And PadIsPlated = 'False' And Hole > 0. A new rule gets the highest priority, so it is the one that applies to non-plated holes.

Then, in the PCB Editor, before you export:

1. Repour the copper polygons (Polygon Pours, the poured copper areas). Choose Tools » Polygon Pours » Repour All. The copper in the files then matches what you see on screen.
2. Run the design rules check (DRC): open Tools » Design Rule Check and click Run Design Rule Check. Fix the errors. Our check helps after you upload, but it does not replace your own DRC.
3. Check the board outline. The board shape (Board Shape) must be one closed shape. If you drew the outline with tracks and arcs, select them and choose Design » Board Shape » Define Board Shape from Selected Objects. An open or split outline is an error, and we cannot make a preview of the board from it.
4. Measure the distance from holes to the board edge. Reports » Measure Distance (shortcut Ctrl+M) measures between two points, for example the edge of a hole and the nearest point of the outline. Reports » Measure Primitives shows the smallest distance between two objects, such as a hole and an outline track. The value should be at least 0.2 mm.

2. Export the Gerber files

Open File » Fabrication Outputs » Gerber X2 Files. The Gerber X2 Setup window opens. Gerber X2 is an evolution of RS-274X: the files also carry layer stack data and pad and via attributes, and older software reads them as plain RS-274X. A correct X2 export can remove some warnings from our check.

Set up the window as in the picture. The numbers match the list below it.

1. Units: Millimeters.
2. Decimal: a high resolution works. Our check read the 4:5 export (0.00001 mm, Altium's usual X2 default) and the 4:3 export (0.001 mm). Keep the Gerber and drill formats matched, as Altium recommends.
3. Outputs: FileName.Extension: both options are fine, *.gbr and filename.* (gtl, gbl, gto,...). Our check reads files from either.
4. Layers to Plot: on the Layers to Plot tab open Plot Layers and choose Select Used. Then keep only Board Outline (the first row of the list), the copper layers including inner ones, the silkscreen and the solder mask ticked. Tick paste only for a stencil. We do not need the mechanical layers. We do not need the Drills group either, because the holes go into the NC Drill files (our check also accepts drills from the Drills layers). Altium takes Board Outline straight from the board shape, not from objects on a mechanical layer.
5. Advanced: keep File Subject: Autodetect, the board type Altium writes into the files (a single board is marked as Single). Keep Unsorted (raster) too, the normal mode for modern raster photoplotters. Sorting is only for old vector plotters.
6. Others: we do not need the options Generate Reports and Generate DRC Rules export file (.RUL). Our check skips what it does not recognise.
7. Click Apply. You find the files next to the project, in a folder whose name starts with Project Outputs for and continues with the project name. To use another path, set Output Path in Project » Project Options on the Options tab.

Each ticked layer becomes one file. If the board has inner layers, each one adds one more copper file.

3. Export the drill files

Open File » Fabrication Outputs » NC Drill Files. The NC Drill Setup window opens. The files are written as soon as you click OK.

1. Units, Format: Millimeters and the same format as the Gerbers (4:3 works).
2. Leading/Trailing Zeroes: Suppress trailing zeroes. Our check read Altium drill files made with this setting without an error.
3. Coordinate Positions: Reference to absolute origin. Ideally the drill files use the same origin as the Gerbers.
4. Other: turn on Generate separate NC Drill files for plated & non-plated holes. Plated and non-plated holes then go into two files.
5. Other: we do not need Generate Board Edge Rout Paths or Generate EIA Binary Drill File (.DRL). The outline is already in the Board Outline Gerber file, and the .TXT files are enough. Our check skips what it does not recognise.
6. Click OK. The folder now also holds the -Plated.TXT file. The -NonPlated.TXT file exists only if the board has non-plated holes. Slots or square holes can add more files, for example -RoundHoles- or -SlotHoles-, which is fine. Put all of them in the ZIP. The drill report (.DRR) is only for you.

Repeating the export: an Output Job

Altium can save both exports in an Output Job file and run them with one command. This helps when you export the board more than once. The settings in an Output Job are separate from the settings you use when exporting directly from the PCB Editor, so enter them again as in steps 2 and 3.

1. Create the file: File » New » Output Job File.
2. In Fabrication Outputs click Add New Fabrication Output, choose Gerber X2 Files and the board as the data source. Add NC Drill Files the same way. Set up each output by double-clicking its row, as in steps 2 and 3.
3. For both outputs, turn on the Enabled field for the Folder Structure container. You set the folder the files are saved to in the container's settings.
4. Select the container and run the export: Tools » Run or the F9 key.

4. Check the result and zip it

Open the files in the Altium CAM Editor or in any Gerber viewer. The CAM Editor opens them by itself if you turned on Open outputs after compile before the export (Project » Project Options, Options tab). The holes must sit on the pads and the outline must enclose the whole board.

1. Check that the folder holds one Gerber file per layer and the drill files: -Plated.TXT and, if the board has non-plated holes, -NonPlated.TXT.
2. Put the files in one ZIP. We also accept RAR, 7z and tar. If you zip the whole Project Outputs folder, we skip documents (PDF, HTML, XLSX, CSV) and Altium design files (.PcbDoc, .SchDoc, .PrjPcb, .OutJob).
3. Upload the ZIP to the quote calculator. We check the board, show you a preview and the price, and you finish the order in your account.

Common mistakes

• Missing drill files. The check reports missing drill data for plated holes. A missing file for non-plated holes is only a warning.
• A missing or open outline. Without Board Outline ticked, the check reports a missing outline. An open or split outline is an error, and we cannot make a preview of the board from it.
• Polygons that were not repoured. The copper in the files can then differ from what you see on screen. Tools » Polygon Pours » Repour All fixes it.
• A different origin or format for the drill files than for the Gerbers. The holes can shift off the pads.
• Two files with the same name. The check reports an error, even if the files sit in different folders or differ only in letter case.
• Missing silkscreen. This is only a warning: that side has no legend.

Done? Upload the ZIP to the quote calculator. Do you also design in KiCad? You can upload its project without exporting, see the KiCad guide.