Online PCB viewers, ranked · Guide

Checklist: what to check when a board will not render

Most rendering problems come from what was uploaded, not the viewer: a missing sheet or layer file, 3D models outside the project, unfilled zones, an old file version, or a conversion between tools. Work down the list below before you report a bug.

Last reviewed

Symptoms and what to check

A whole layer is missing

  • Gerbers: was the layer exported? Open the output folder and count the files.
  • Gerber X1 files: the viewer guesses the layer from the file name. Rename to your CAD tool's standard names, or export Gerber X2, which records each file's function.
  • Inner layers: check the stack-up in the design has the layer count you expect.
  • In the viewer: check the layer is not simply hidden in its layer panel.

No board outline, or the board looks infinite

  • KiCad: the outline must be a closed shape on Edge.Cuts.
  • Gerbers: export the outline layer; some viewers need it to clip the render.

Copper pours show as outlines or are missing

  • KiCad: fill all zones (press B in the PCB editor) and save before uploading.
  • Converted Altium files: compare pours with the original; they may need repouring.

3D view shows bare pads or floating parts

  • The 3D model paths point outside your upload. Copy models into the project and reference them with ${KIPRJMOD}.
  • Check the model's offset and rotation in the footprint's 3D settings.
  • The viewer may support STEP but not every other format: check which it reads.

Text in the wrong font, or overlapping

  • KiCad 7 custom fonts are not always implemented; KiCanvas lists them as a known gap.
  • Fonts installed on your machine are not in the upload. Use KiCad's default font for anything a reviewer must read.

Schematic sheets missing

  • Hierarchical designs keep each sub-sheet in its own file. Upload all of them, not just the root sheet.
  • KiCad 5 projects also need the -cache.lib file to draw symbols; better, upgrade to a current KiCad and save.

The file will not open at all

  • Version: KiCanvas reads KiCad 6 and later only. Check the viewer's supported versions.
  • Format: make sure you uploaded the design file the viewer reads (for example .kicad_pcb, .PcbDoc), not a backup or a lock file.
  • Packaging: some viewers want a ZIP of the project; others want files dropped one by one.
  • Size: very large boards may hit a size or memory limit; try a desktop browser with WebGL on.

Drill holes are offset or the wrong size

  • Excellon units and zero format must match what the viewer expects; re-export with units and format stated in the header.
  • Plated and non-plated holes may be separate files: include both.

Something looks different after conversion

  • A converted view (Altium to another tool, KiCad import of Eagle) is a translation. Compare pours, rules, net classes and variants against the original.
  • Keep the original files as the source of truth, and say in the review which view you are looking at.

Still wrong?

Open the same files in a second viewer from the ranking. If both draw the same thing, the problem is in the files; if not, report it to the viewer with a small file that shows it. For KiCad projects, BoardRepo notes that some uploads do not render fully, so compare with desktop KiCad before you share the link.