1. When generating output data for soldermask, there is no need to oversize or compensate the soldermask pads.
It is better to leave the soldermask pads at the same size as the copper pads. We will then set the soldermask to suit the technological needs for proper production and assembly of the boards.
Preferred version without oversizing Less good: pads are oversized
2. Soldermask preparation rules that we use:
We set the values for soldermask preparation according to the PCB pattern class. The different features are shown in the diagram:
MAR (Mask Annular Ring) – the clearance between the soldermask and the copper pad
MSM (Mask SegMent) – the bridge of soldermask between adjacent pads
MOC (Mask Overlap Clearance) – the soldermask cover between a track or plane and an adjacent soldermask window
We always start by applying the standard values to the complete soldermask. Depending on the design we can reduce these standard values at particular places down to the minimum accepted values to generate the best soldermask.
The standard value for MAR, MSM and MOC is 0.1000mm (4mil) for all pattern classifications.
The MINIMUM accepted values for MAR, MSM and MOC depend on the pattern classification according to the following table (values only in mm)
- Mask Segments smaller then 0.0800mm (3.15mil) will be removed.
à This will be converted to the image below if the Mask SegMent (MSM) between the pads is less than 0.0800mm (3.15mil)
- For NPTH drills without copper pad the Mask Annular Ring (MAR) is ALWAYS 0.125mm (4.92mil) independent of the pattern class.
3. Tented vias: the copper pad of the via is covered with soldermask.
IMPORTANT: If you require tented vias please make sure that you generate your soldermask data without soldermask pads for vias.
Tented via technology DOES NOT automatically mean that the via hole is fully closed or covered with soldermask. The maximum via ENDSIZE that can be closed with soldermask is 0.25mm (10mil). Completely closed via holes can only be guaranteed using ViaFill (See section ViaFill)
4. NPTH holes without copper pad should ALWAYS have a soldermask clearance pad.
5. When generating output include the board outline in your soldermask layers.
This is best done using a small line - e.g. 0.50mm (20mil) wide - where the center of the line is the exact board outline. We will remove the line from the final production ready data.
If you require board edge areas of your PCB to be free of soldermask, use a wide line to indicate the board outline. The line-width should be at least 2.00mm (79mil), resulting in 1.00mm (39.5mil) border free of soldermask. It is also advisable to indicate the soldermask-free border in the mechanical plan.