Chris Collins

Tools · electronics

Gerber viewer and DFM check

Open a zip of Gerbers and drill files, see the copper, mask, silkscreen, paste and outline stacked or as a realistic top or bottom board, measure, and check the design against JLCPCB, PCBWay or OSH Park's published limits — trace width, spacing, drills, annular rings, edge clearance, mask slivers, silk on pads — with every problem marked on the board.

Added

How to use it

A last look before you upload your board to a fab: what the files really contain, drawn from the Gerbers themselves, and the problems a fab’s checks would bounce. Everything runs in your browser; your design is never uploaded.

How to use it

  1. Open the zip your CAD program wrote (KiCad, Eagle / Fusion, Altium, EasyEDA, DipTrace …) or the files themselves; or drop them on the view. A sample board opens first — a KiCad 9 board with a deliberate example of every problem.

  2. Layers are recognised from their X2 file-function attribute (%TF.FileFunction) where the CAD program wrote one, otherwise from the file name (.GTL, .GBS, F_Cu, top-silk …). Untick a layer to hide it.

  3. Views: Layers stacks every layer in its own colour; Top and Bottom draw the board as it will come back from the fab — FR-4, copper seen through the mask, the mask colour you pick, exposed pads in ENIG gold, HASL tin or bare copper, the silkscreen (clipped by the mask openings as fabs do), and the holes. The bottom is seen from underneath (mirrored).

  4. Pan by dragging, zoom with the wheel, a pinch or the buttons; the readout shows the cursor’s coordinates. 📏 Measure: click two points for the distance and its X and Y parts (Esc clears).

  5. DFM check: choose the fab. The limits are each fab’s standard service as published on its capabilities page (linked) — they change, so check before you order; Custom takes your own. The report lists each finding with its layer and position, the markers on the board are numbered to match, and clicking either one zooms there. Checks:

    • trace width — drawn tracks thinner than the minimum;

    • copper spacing — separate copper areas closer than the minimum (on each copper layer);

    • drill size — holes and slots below the smallest drill;

    • annular ring — copper left round a plated hole: (pad − hole) ÷ 2 for the pad flashed on it;

    • edge clearance — copper closer than the minimum to the board outline or its cut-outs;

    • mask slivers — solder-mask webs between openings thinner than the minimum dam;

    • silk on pads — silkscreen on, or within the clearance of, a mask opening (fabs clip it);

    • silk line width — silkscreen strokes too thin to print.

  6. Board: its size, area, copper layers, holes and drill sizes, the thinnest trace, and the board area for a quantity. There is no live pricing (prices depend on options and change daily) — the links go to each fab’s quote page.

  7. ⛶ Full screen (or F) gives the board view the whole screen — the browser’s full screen where it is allowed, otherwise a full-window layer (iPhone); it is redrawn as the window changes, and ◫ Panels hides the side panel. Escape leaves.

The fab limits used (standard 2-layer service, mm):

Fab Trace Space Drill Ring Edge Mask dam Silk line Silk–pad

JLCPCB

0.1

0.1

0.15

0.18

0.2

0.1

0.15

0.15

PCBWay

0.1

0.1

0.15

0.15

0.25

0.1

0.15

0.15

OSH Park

0.1524

0.1524

0.254

0.127

0.381

0.1016

0.127

0.1016

Limits

  • The Gerber reader covers RS-274X as CAD programs write it today: formats and units, circle, rectangle, obround and polygon apertures with holes, aperture macros (circle, vector and centre lines, outline, polygon; thermals as plain rings), linear and circular interpolation (single- and multi-quadrant), regions, dark and clear polarity, step-and-repeat and X2 attributes. Image transformations (%LM, %LR, %LS) and the deprecated %IP, %OF, %SF are reported but not applied. Excellon: tools, metric / inch, leading / trailing zeros, decimal coordinates, G85 slots; routed outlines in the drill file are not drawn.

  • The DFM checks are geometric and approximate (polygons to 0.002 mm, arcs as short segments). Copper pours' own thin necks, inner-layer clearances to holes, acid traps, impedance and stack-up are not checked; a clean report is not a guarantee — the fab’s own review is final.

  • Spacing compares separate copper areas, whatever their nets; two areas of the same net closer than the minimum are reported too (fabs care about the gap either way).

  • The realistic views are illustrations: colours and finishes are approximate.

Related: PCB trace width and current, SMD packages and footprints, SMD marking codes, resistor codes, PCB enclosure generator, 2.5D CAM (mill your own boards' outlines), KiCad BOM rollup, reflow profile.

Linking to an example

Share link copies a URL with the view, the fab and the layer settings — never your files (a link opens on the sample board).

Parameter Meaning

example

A preset (below)

fab

jlcpcb, pcbway, oshpark, custom

view

layers, top, bottom

hide

Layers to hide, comma-separated: top-copper, bottom-copper, inner-copper, top-mask, bottom-mask, top-silk, bottom-silk, top-paste, bottom-paste, outline, drill

mask, finish

Mask green, purple, black, blue, red, white; finish enig, hasl, bare

units, qty

mm or mil; boards ordered

Presets: sample against JLCPCB · sample against OSH Park, purple · sample from underneath, HASL.

Runs entirely in your browser; nothing you type leaves this page.