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 here.
We naturally import your ODB++, Gerber-, KiCad-, OrCAD-, Target-, Eagle-, Altium-, IPC-2581-, DPF- and Sprint layout data free of charge!
Instead of the uncommon IPC-2581 format we recommend ODB ++ data!
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.
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_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
Net Classes Editor (mm)
| Clearance | Track Width | Via Ø | Via Drill-Ø | uVia Ø | uVia Drill-Ø | |
|---|---|---|---|---|---|---|
| Multi-CB Standard | 0,1 | 0,1 | 0,4 | 0,2 | 0,3 | 0,1 |
Globale Design Rules (mm)
| Multi-CB Standard | Min. possible | |
|---|---|---|
| Min. track width | 0,1 | 0,075 |
| Min. Via diameter | 0,4 | 0,3 |
| Min. Via drill diameter | 0,2 | 0,1 |
| Min. uVia diameter | 0,3 | 0,225 |
| Min. uVia drill diameter | 0,1 | 0,075 |
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.
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.
Standard layers
By default, KiCad uses Protel's tried and tested filename extensions for Gerber export. Please use the default setting.
| Layer | KiCad layer name | Standard Protel extension |
|---|---|---|
| Top layer | F.Cu | .GTL |
| Bottom layer | B.Cu | .GBL |
| Top Marking Print (Overlay) | F.SilkS | .GTO |
| Top Solder-stop | F.Mask | .GTS |
| Bottom Solder-Stop | B.Mask | .GBS |
| Contour | Edge.Cuts | .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: