KiCad

KiCad Logo

If you create your PCB layout with the freely available program KiCad, please note the following instructions below.

The KiCad software is a complete project manager with a number of integrated modules, such as Schematic Editor, PCB Editor and Gerber Viewer.

KiCad is open source, and thus available free of charge

We naturally import your ODB++, Gerber-, KiCad-, OrCAD-, Target-, Eagle-, Altium-, IPC-2581-, DPF- and Sprint layout data free of charge!

Data transfer

Please send your data as .kicad_pcb or Gerber export (+drill file).

Prior always: KiCad DRC

Before you send us your data, please run the KiCad Design Rule Check (DRC). This avoids queries, thus saving you valuable time and can lead to the detection of errors in the layout. 

When using KiCad's DRC, please select the option: "Refill all zones before performing DRC".

KiCad DRC refill all zones

.kicad_pcb data

If you send us .kicad_pcb data, we will take care of generating the production data (Gerber export) for you with our standard settings.

Following KiCad’s official recommendation, we create the Gerber data with "refilled zones" . We therefore recommend that you select the option "Refill all zones before performing DRC" for the KiCad DRC (see above).

Gerber data

If you export the Gerber data (+ drill file) yourself, we recommend that you check the generated production data with KiCad's integrated Gerber viewer in addition to the KiCad DRC (see above). This allows you to check, e.g., whether you have exported all the necessary layers.

Our experience with numerous KiCad data sets of different program versions / different users teaches us: It is more crucial to run the DRC of KiCad than the question in which file format you send us your layout.

Design Rules

The design rules can be found directly in the main menu of Pcbnew. There are two tabs:

  • Net Classes Editor: Conductor spacing and width as well as Vias
  • Global Design Rules: Minimum values for conductors, pad and drill diameters

Multi-CB parameters

For an optimal result, please define the free-of-charge high-tech parameters of Multi-CB:

  • Track-width / space: 0,1mm (100µm) - free-of-charge ✓
  • Annular ring: 0,1mm (100µm) - free-of-charge ✓
  • Drills: 0.2mm (200µm) - free-of-charge ✓
  • Via-Pad: 0,4mm (400µm) - free-of-charge ✓

This guarantees the best technology at the best price. The minimum possible values can be found here: Circuit board design parameters.

Net Classes Editor (mm)

 ClearanceTrack WidthVia ØVia Drill-ØuVia ØuVia Drill-Ø
 Multi-CB
Standard
Clearance0,1Track Width0,1Via Ø0,4Via Drill-Ø0,2uVia Ø0,3uVia Drill-Ø0,1
Net Classes Editor

Globale Design Rules (mm)

 Multi-CB StandardMin. possible
 Min. track widthMulti-CB Standard0,1Min. possible0,075
 Min. Via diameterMulti-CB Standard0,4Min. possible0,3
 Min. Via drill diameterMulti-CB Standard0,2Min. possible0,1
 Min. uVia diameterMulti-CB Standard0,3Min. possible0,225
 Min. uVia drill diameterMulti-CB Standard0,1Min. possible0,075
KiCad Design Rules

Additional required track-widths, clearances and Vias can also be defined in the Design Rules.

Gerber export

You can start the Gerber Export under File / Plot. In the Plotting dialog, you define the layers to be exported. Please activate the function "Subtract soldermask from silkscreen" to avoid silkscreen on the pads. You can usually use default settings for all other options.

KiCad plot Gerber export

Drill Files Generation

After the Gerber export, you start the drill file export from the same window (Generate Drill File). You can usually use default settings for all other options.

KiCad Drill Files Generation

Standard layers

By default, KiCad uses Protel's tried and tested filename extensions for Gerber export. Please use the default setting.

LayerKiCad layer nameStandard Protel extension
LayerTop layerKiCad layer nameF.CuStandard Protel extension.GTL
LayerBottom layerKiCad layer nameB.CuStandard Protel extension.GBL
LayerTop Marking Print (Overlay)KiCad layer nameF.SilkSStandard Protel extension.GTO
LayerTop Solder-stopKiCad layer nameF.MaskStandard Protel extension.GTS
LayerBottom Solder-StopKiCad layer nameB.MaskStandard Protel extension.GBS
LayerContourKiCad layer nameEdge.CutsStandard Protel extension.GM1

Gerber Data check

To view the generated Gerber files, click the Gerber Viewer icon in the KiCad Project Manager. Then import your Gerber and drill files:

  • Import Gerber: Select File / Load Gerber File and select all exported Gerber layers
  • Import drill file: Select File / Load EXCELLON drill file and select all exported drilling data

You can now check your complete production data. Pack all into a zip file which you can upload with your PCB order.

Getting Started

The following resources are recommended for access to KiCad:

KiCad 6 - Getting Started

Kicad Homepage

KiCad course by Contectual Electronics