Product 关闭
搜索 搜索文档

KB: How to Link Multi-Part Components as a Single Entity and Avoid Separate Annotation

Updated: 十月 16, 2026
Altium Designer Altium Designer
When placing multi-part components in a schematic, each part may be annotated independently based on its placement location. This occurs when the annotation process cannot identify the parts as belonging to the same logical component. To ensure all parts of a multi-part component receive the same designator and are treated as a single entity during annotation, assign a common PartId parameter value to each part and enable the PartId matching option during schematic annotation.

Solution Details

Multi-Part Components Receive Different Designators

Multi-part components may receive separate designators during annotation, causing individual parts of the same logical component to be treated as separate components within the schematic.

Annotation Cannot Identify Related Parts

By default, some component placement methods do not automatically link the parts of a multi-part component. Without a shared identifier, the annotation process treats each part as a separate entity and assigns independent designators.

Assign a Shared Component Identifier

  • Assign the same PartId parameter value to every part of the multi-part component.
  • Enable PartId in the annotation matching options so all parts are recognized as a single component during annotation.

Configure and Run Schematic Annotation

  1. Open the schematic document and locate the multi-part components.
  2. Double-click each part to open its properties.
  3. Navigate to the Parameters section in the Properties Panel.
  4. Click Add Parameter.
  5. Enter Parameter Name: PartId.
  6. Enter a shared value for all parts belonging to the same component.
    Example: PartId = 1 for all parts of a single multi-part component.
    Altium Designer schematic Properties panel for a component showing multipart settings: Part set to Part A of 3, Designator C?, Comment “multi,” and a PartId parameter value of 1 listed under Parameters.     Altium Designer schematic Properties panel for a multipart component with Part set to Part B of 3. Designator is C?, Comment “multi,” and the Parameters list shows PartId value 1, indicating the same logical component instance. 
  7. Select Tools » Annotate Schematic.
  8. Enable PartId in the matching options section.
    Altium Designer Annotate dialog showing Schematic Annotation Configuration. Matching Options include PartId enabled, and the Proposed Change List previews updated component designators and sub‑parts before applying changes. 
  9. Enable the appropriate Lock settings for values that should not change, then click Reset All.
     Altium Designer Annotate dialog showing Schematic Annotation Configuration. Proposed Change List displays current and proposed designators and sub‑parts, with Sub values highlighted, and the Reset All button available to revert pending annotation changes. 
  10. Click Update Changes List » Accept Changes (Create ECO) » Execute Changes » Close.

Additional Notes

  • If components are placed using Explorer panel: Right-click » Place, the PartId parameter is added automatically.
  • If components are placed using Components panel: Right-click » Place, the PartId parameter is not added automatically.
  • If components are placed by drag-and-drop from either the Explorer panel or the Components panel, the PartId parameter is not added automatically and must be assigned manually.

References

Creating Multi-Part Components

如您发现任何问题，请选中相关文本/图片，并按 Ctrl + Enter 键向我们提交反馈。
Contents
Was this article helpful?