Skip to content

Fabrication and Export

Once your design is complete and DFM passes cleanly, export manufacturing files to send to your PCB manufacturer — or to document your design.

Export Types Overview

File type Format Purpose
Gerber RS-274X .gbr PCB fabrication — copper, mask, silk, outline layers
Drill Excellon .drl Via and hole positions for CNC drilling
BOM CSV .csv Bill of Materials for component ordering
Schematic PDF PDF .pdf Printable schematic documentation
Toner Transfer PDF PDF .pdf Hobbyist — per-layer PDFs for manual PCB making

Schematic PDF Export

Exports your schematic as a vector PDF for printing or sharing.

Steps:

  1. Open the Schematic tab you want to export
  2. Select File → Export → Export Schematic to PDF
  3. Choose a filename and directory
  4. Click Export

PDF content:

Element Rendering
Components Symbol outlines, pins, designator and value text
Wires and junctions Black/grey lines and dots
Graphics Rectangles, circles, text annotations
Title block Page border, title, company, revision, date

Colors are converted to black and grey for print-friendly output.

PCB Gerber Export

Gerber is the industry-standard format sent to PCB manufacturers. Each layer produces a separate .gbr file.

Steps:

  1. Open the PCB tab
  2. Select File → Export → Fabrication Outputs (Gerber/Drill/BOM) or Tools → Fabrication Output
  3. Select the layers to export:
Layer Example filename Purpose
F.Cu MyBoard-F_Cu.gbr Front copper
B.Cu MyBoard-B_Cu.gbr Back copper
F.SilkS MyBoard-F_SilkS.gbr Front silkscreen
F.Mask MyBoard-F_Mask.gbr Front solder mask openings
B.Mask MyBoard-B_Mask.gbr Back solder mask openings
Edge.Cuts MyBoard-Edge_Cuts.gbr Board outline for cutting
  1. Choose the output directory
  2. Click Export — one .gbr file is generated per selected layer
  3. (Optional) Compress all files into a ZIP to send to the manufacturer

Which files to send?

Typically: F_Cu, B_Cu, F_SilkS, F_Mask, B_Mask, Edge_Cuts, and the drill .drl file. Always check your manufacturer's specific requirements.

Drill File Export

The drill file contains all hole locations and diameters — vias and mechanical holes.

Format: Excellon NC drill (text-based coordinate format)

Data included: - X, Y coordinates for each via and hole - Drill diameter per tool - Plated vs. non-plated hole separation

BOM Export (Bill of Materials)

The BOM is a parts list used to order components for assembly.

Steps:

  1. Open the fabrication output workflow.
  2. Include the BOM CSV in the coordinated package.
  3. Open in Excel, LibreOffice Calc, or Google Sheets

BOM file columns:

Designator Value Footprint Layer
R1 10kΩ R_0603_1608Metric Top
R2 330Ω R_0603_1608Metric Top
C1 100nF C_0805_2012Metric Top
U1 STM32F103 LQFP-48 Top

Before exporting the BOM

Only footprints with a non-empty Value field are included. Verify that all components have values assigned.

Toner Transfer PDF (Hobbyist)

Toner Transfer PDF is a WireFrame feature designed for makers and hobbyists who produce PCBs manually using toner transfer or UV film methods.

  • Generates each selected layer as a separate PDF page
  • Output is true 1:1 scale — no page scaling
  • Automatically mirrors layers that need to be printed reversed (e.g. F.Cu)
  • WYSIWYG silkscreen — text renders exactly as it appears on the physical board

Steps:

  1. Open the Fabrication dialog
  2. Select Toner Transfer PDF as the export type
  3. Choose the layers to include (e.g. F.Cu, B.Cu)
  4. Click Export — each layer becomes a separate page in the PDF
  5. Print on glossy paper at 100% scale (no fit-to-page)

Built-in Gerber Viewer

WireFrame includes a Gerber viewer to inspect exported files without external software.

How to use:

  1. Select Tools → Gerber Viewer and open a generated .gbr file, or use another trusted Gerber viewer.
  2. Select representative copper, mask, silkscreen, and outline outputs.
  3. Pan and zoom to verify:
    • Trace continuity
    • Pad alignment and spacing
    • Board outline shape

Gerber Viewer

Visually confirm trace continuity, pad flashes, apertures, and the board outline before sending the package to a manufacturer.

Complete Export Workflow

  1. Run DFM/DRC and resolve every release-blocking error.
  2. Generate the coordinated fabrication package.
  3. Review representative Gerber X2 layers and both drill outputs.
  4. Check IPC-D-356A, BOM, and the package manifest.
  5. Archive only the verified board revision and send that archive to the manufacturer.

Image — Verified fabrication package

Image needed

Capture the fabrication output dialog beside the generated package contents. Show the board revision and filenames, but no private customer path.

Fabrication package contents

The release workflow can generate a coordinated package rather than a set of unrelated exports:

Output Purpose
Gerber X2 Copper, mask, silkscreen, and board geometry with generation metadata
PTH / NPTH drill files Separates plated electrical holes from unplated mechanical holes
IPC-D-356A netlist Electrical connectivity reference for fabrication test and CAM review
BOM CSV Designators, values, footprints, and placement layer
Manifest / README WireFrame version, generation time, and package inventory

Inspect the archive

A successful export does not prove manufacturability. Confirm that Edge.Cuts is closed, drill classifications are correct, every expected layer is present, and the package matches the board revision being released.

See Also