Online Gerber viewer

How to use the Gerber viewer

1. Export Gerbers and drill files from your PCB tool, then drop the zip, the folder or the files on the viewer. Not ready? Click Try a sample board.
2. Look at the Top and Bottom renders. The bottom is mirrored, as you would see it holding the board upside down.
3. Switch to Layers to see each file in its own colour. Tick layers on and off, pan by dragging, zoom with the buttons, a pinch or Ctrl + scroll, and click Measure to measure between two points.
4. Check the layer list. Each file shows how it was identified (X2 attribute, job file or file name). If one is wrong, pick the right type from its menu and the render and checks update.
5. Read the checks. Fix anything marked as a problem before you upload the zip to a fab.

The files are read and drawn in your browser. There is no upload step, no account and no file size quota beyond a sanity limit of 300 MB unzipped.

What is a Gerber file?

A Gerber file is a plain-text, vector description of one layer of a printed circuit board. The format, RS-274X, is maintained by Ucamco and is what every PCB tool exports for manufacturing. A board is a set of them: one per copper layer, the solder mask and silkscreen for each side, paste layers for the stencil, and the board outline. Holes usually come in a separate Excellon drill file, and newer tools add a Gerber job file (.gbrjob) that lists the whole set.

Inside, a Gerber file declares its units and number format, defines apertures (round, rectangular and custom shapes), and then moves, draws and flashes them at coordinates. This is the start of the sample board’s top copper, exported by KiCad:

%TF.GenerationSoftware,KiCad,Pcbnew,10.0.3*%
%TF.FileFunction,Copper,L1,Top*%
%TF.FilePolarity,Positive*%
%FSLAX46Y46*%
%MOMM*%
%ADD10R,1.700000X1.700000*%
D10*
X137500000Y-110460000D03*

The %TF lines are Gerber X2 attributes: the file says it is copper layer 1, the top. Files without them (often called X1) depend on their file names, which is why naming conventions still matter. The attributes never change the image, so readers that ignore them draw the same board.

Gerber, Excellon, ODB++ and IPC-2581

Gerber plus Excellon is the format every fab accepts. ODB++ and IPC-2581 carry layers, drills, netlist and stackup in one structured package and are used mostly in volume production. This viewer reads Gerber (RS-274X and X2) layers, drill files in Excellon or Gerber form, and Gerber job files.

How the viewer reads a Gerber set

Each file is sniffed by content first: an M48 header means Excellon, a %FS format statement means Gerber, and reports, PDFs and readmes are set aside. Each layer is then identified from, in order, its own X2 TF.FileFunction attribute, the job file, the naming conventions in the table below, and finally layer names that EasyEDA and ProtoFlow write into comments. Of several outline candidates (Altium sets often have GKO and many GM layers) it picks one, preferring a closed shape. The board is then drawn with pcb-stackup, the open-source renderer from the tracespace project, using these layer types rather than guesses from file names.

Worked example 1: decoding a KiCad coordinate

%FSLAX46Y46*% means leading zeros are omitted and there are 4 integer and 6 decimal digits, in the units set by %MOMM*%. So the last line of the excerpt flashes a pad at X = 137500000 ÷ 10⁶ = 137.5 mm and Y = -110.46 mm. That pad is on the sample board, whose outline runs from 100 to 142 mm in X.

Worked example 2: an Altium drill hit in inches

An Altium drill file with INCH,LZ and ;FILE_FORMAT=2:5 keeps leading zeros and drops trailing ones, so digits are read from the left with 2 before the decimal point. X00255 is padded to 0025500, which is 0.255 in or 6.477 mm. Read with the opposite rule, as if leading zeros had been dropped, the same digits would be 0.00255 in, a hundred times closer to the origin.

Worked example 3: board size from the outline

The sample board’s Edge.Cuts outline is drawn with a 0.1 mm line. Measured on the line’s centre, the board is 42 × 26 mm. KiCad’s job file reports 42.1 × 26.1 mm because it adds the line width (0.1 mm). The viewer reports the centre-line size, which is the shape the outline describes. Its drill files hold 16 holes in 3 sizes, from 0.3 to 3.2 mm, all inside that outline.

What to check before ordering from JLCPCB or PCBWay

Fab uploaders mostly identify layers by file name and run their own review, but a minute in a Gerber viewer catches the mistakes that hold orders up. JLCPCB’s KiCad guide asks you to confirm the outline exists and is watertight, that cutouts and slots appear on the outline layer, and that holes line up with the other layers. The viewer’s checks cover those, plus:

• One file per layer. Every copper layer present, including inner layers on a four or six layer board, and no second copy of a layer from an older export.
• Mask for every copper side. A missing solder mask file means a bare side or a question from the fab.
• Drill files in the zip and in the same units. The holes should sit inside the outline.
• Names a fab understands. JLCPCB notes that its system does not look for Altium’s GP plane files, which are usually negative and which it may not process correctly; route planes as positive layers or check with the fab.
• A flat zip. Leave out old zips, reports and design files. The viewer lists anything that is not fabrication data.

The checks read only the files. They do not know your fab’s minimum track, spacing or drill size, so compare the smallest drill the viewer reports with your fab’s capabilities page, and run DRC in your design tool before exporting. Our PCB design rules guide explains the difference between fab limits and good practice.

How to export Gerber files from KiCad, Altium, EAGLE and EasyEDA

KiCad

In the PCB editor choose File › Fabrication Outputs › Gerbers. Tick every copper layer, both mask, silkscreen and paste layers and Edge.Cuts, then Plot. Click Generate Drill Files in the same dialog. JLCPCB’s KiCad 8 guide recommends Protel filename extensions, millimetre drill units, decimal format and an absolute origin. Zip the output folder’s Gerber and drill files.

Altium Designer

Use File › Fabrication Outputs › Gerber Files, select the used layers, then File › Fabrication Outputs › NC Drill Files, as PCBWay’s Altium guide shows. Altium writes Protel extensions and .TXT drill files, plus reports (.DRR, .LDP, .REP) that fabs do not need.

EAGLE and Fusion electronics

Open the CAM Processor, load a CAM job (your fab’s, or the default), and process it. JLCPCB’s guide notes that the outline must be a continuous line on layer 20, Dimension, and that the .gpi and .dri files EAGLE writes are not used for manufacturing.

EasyEDA

EasyEDA exports a ready-made Gerber zip with the Gerber_… and Drill_… names in the table above, and it opens in this viewer as is.

Common Gerber mistakes

• No outline, or the outline on the wrong layer. Drawn on silkscreen or a fabrication layer, the shape never reaches the router. The viewer fails the set without one.
• Gaps in the outline. Two lines that look joined but miss by a fraction of a millimetre. The viewer reports open ends with their coordinates.
• Drill units or zero format that do not match. Holes land off the board or scale by 10 or 25.4.
• Mask and paste mixed up. They look alike (both are pad openings). A mask file saved with a paste extension leaves the fab without the mask openings, or with the wrong ones. When X2 attributes are present, the viewer warns if the name and contents disagree.
• Nested folders and stale files. Zipping the whole output folder can pull in an old export. Creation times in X2 files reveal it.
• Old RS-274-D files. They need a separate aperture list. The viewer flags files that use apertures they never define.

Accuracy and limits of an online Gerber viewer

Rendering uses pcb-stackup and gerber-to-svg from the tracespace project, which implement RS-274X including aperture macros, regions, arcs and polarity. The checks use a separate reader written for this page, tested against real exports from KiCad, Altium and ProtoFlow, drill headers from EAGLE and EasyEDA, and the Gerber specification’s coordinate rules.

It is a viewer and checker, not a CAM system. It does not compare a netlist, measure copper-to-edge clearance, panelize, or read ODB++. Negative plane layers are shown as drawn. For a definitive reading of a disputed file, Ucamco’s Reference Gerber Viewer is the specification owner’s own tool; KiCad’s GerbView and gerbv are capable desktop viewers.

Do this automatically in ProtoFlow

ProtoFlow, our desktop PCB design app, checks a board before it writes a single Gerber. Its export preflight blocks output when the Edge.Cuts outline is not one closed loop or a copper zone failed to fill, and if the design rule check still lists errors or warnings it asks you to review them first. Export Gerbers then writes Gerber X2 layers with file attributes, a Gerber job file and a metric Excellon drill file into one zip, with oval holes as routed slots. Preview the export in the built-in Gerber viewer, toggle layers and measure, export the BOM and pick-and-place files in JLCPCB format, or upload the package to PCBWay and finish the order in your browser. You can start the board itself from a plain-English description. Download ProtoFlow free for macOS, Windows or Linux.