Working with the Board Outline Clearance Design Rule on a PCB in Altium Designer

您正在阅读的是 15.1. 版本。关于最新版本,请前往 Working with the Board Outline Clearance Design Rule on a PCB in Altium Designer 阅读 21 版本
Applies to Altium Designer version: 15.1
 

Rule Category: Manufacturing

Rule classification: Unary

Summary

This rule defines the minimum clearance allowed from design objects that are fabricated, to edges of the board. Either a single clearance value can be specified for all object-to-edge possibilities, or different clearances for different pairings can be defined, through use of a dedicated Minimum Clearance Matrix. The terms Board Outline and Board Edge are general names used interchangeably to describe the outer edge of the board. The term edge is defined in the table below the image. The Board Outline Clearance design rule checks object-to-edge clearances on the electrical and overlay (silkscreen) layers.

Constraints

 Default constraints for the Board Outline Clearance rule.

Default constraints for the Board Outline Clearance rule.

Edge Type Definition
Outline Edge The outer-most (exterior) edge of the board
Cavity Edge The edge of a user-defined cavity
Cutout Edge The edge of a user-defined cutout
Split Barrier When a Split Line defines the edge of the board on this layer, this edge is referred to as a Split Line Barrier
Split Continuation When this layer continues beyond a Split Line, this edge is referred to as a Split Line Continuation (a permeable boundary).
To allow an object-kind to cross an edge, set the clearance value to zero. Zero indicates to the software that an object-kind is allowed to violate (pass over) this edge type. Use this technique to allow routed tracks, for example, to travel across from one Layer Stack Region to another.

Working with the Clearance Matrix

Definition of clearance values in the matrix can be performed in the following ways:

  • Single cell editing - to change the minimum clearance for a specific object pairing.
  • Multi-cell editing - to change the minimum clearance for multiple object pairings:
    • Use Ctrl+click, Shift+click, and click&drag to select multiple cells in a column.
    • Use Shift+click, and click&drag to select multiple contiguous cells in a row.
    • Use click&drag to select multiple contiguous cells across multiple rows and columns
    • Click on a row header to quickly select all cells in that row.
    • Click on a column header to quickly select all cells in that column.

Once the required cells have been selected, type in the new value and press Enter on the keyboard.

To set a single clearance value for all possible object pairings, simply set the required value for the Minimum Clearance constraint. On clicking Enter, this value will be replicated across all applicable cells of the matrix. Alternatively, click the blank grey cell at the top-left of the matrix, or use the Ctrl+A shortcut. This selects all cells in the matrix, ready to accommodate a newly-entered value.

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 matches the object(s) being checked.

Rule Application

Online DRC, Batch DRC, interactive routing and autorouting.

 

可用的功能取决于您的 Altium Designer 软件订阅级别

Content