Silk To Solder Mask Clearance

Old Content - visit altium.com/documentation
Modified by Admin on Jul 25, 2014

Rule category: Manufacturing

Rule classification: Binary

Summary

Checks the clearance between any silkscreen primitive and any solder mask primitive, or exposed copper-layer primitive (exposed through openings in the solder mask). The check ensures that the distance is equal to or greater than the value specified in the constraint.

Many manufacturers routinely strip (or 'clip') silkscreen to the mask opening and not just to the copper pad. However, doing so can render silkscreen text unreadable. Being able to catch such occurrences through DRC, allows you to  manipulate offending silkscreen text prior to sending the board to manufacturing.

This design rule replaces the Silkscreen Over Component Pads rule found in previous releases of Altium Designer. When loading a PCB document from an earlier release of the software into Altium Designer 13.0 (or later), any defined Silkscreen Over Component Pads rules will automatically be converted to Silk To Solder Mask Clearance rules, with their scopes and constraints set to match legacy behavior. It is advised that you check your rule scopes and associated constraints to ensure accuracy in relation to design requirements.

Constraints

  • Clearance Checking Mode - Choose a checking mode for the clearance:
    • Check Clearance To Exposed Copper - in this mode, clearance checking is between silkscreen (Top/Bottom Overlay layer) objects and copper in component pads which is exposed through openings in the solder mask.
    • Check Clearance To Solder Mask Openings - in this mode, clearance checking is between silkscreen (Top/Bottom Overlay layer) objects and solder mask openings created by objects that include a solder mask, such as pads, vias, or copper objects with the Solder Mask Expansion option enabled.
  • Silkscreen To Object Minimum Clearance - The default value is 0.254mm, click the value directly to enter a new value.

To match the legacy behavior of the old Silkscreen Over Component Pads rule found in releases of the software prior to Altium Designer 13.0, the Silk To Solder Mask Clearance rule should have its Clearance Checking Mode set to Check Clearance To Exposed Copper, and the full query for one of its rule scopes set to IsPad. As mentioned previously, this is handled automatically when opening older designs.

How Duplicate Rule Contentions are Resolved

All rules are resolved by the priority setting. The system goes through the rules from highest to lowest priority and picks the first one whose scope expression(s) match the object(s) being checked.

Rule Application

Online DRC and Batch DRC.

You are reporting an issue with the following selected text and/or image within the active document: