How to Use Sub-Shape Binders in FreeCAD

Referencing geometry between different bodies in FreeCAD requires specialized tools to prevent model corruption and topological naming issues. This guide demonstrates how to use the Sub-Shape Binder tool in the PartDesign workbench to reliably link faces, edges, and sketches across multiple bodies. By following these steps, you will learn how to maintain parametric relationships across separate parts without triggering dependency errors.

Why Use a Sub-Shape Binder?

In FreeCAD's PartDesign workbench, each body is intended to be a single, contiguous solid. Directly referencing the sketch or feature of one body inside another creates cyclic dependencies and breaks the dependency graph. A Sub-Shape Binder acts as a non-solid proxy inside your active body, holding a direct parametric link to the source geometry of an external body. When the original body changes, the binder updates automatically.

Step-by-Step: Creating a Cross-Body Reference

  1. Prepare Your Model: Ensure you have at least two bodies in your tree view. For this workflow, consider Body A as the source containing existing geometry, and Body B as the target where new features will be built.
  2. Activate the Target Body: Double-click Body B in the tree view (or right-click it and select Toggle active body). The active body's label will turn bold.
  3. Select Source Geometry: While Body B remains active, click on the geometry from Body A that you want to reference. This can be a face, an edge, a vertex, or the entire Body A solid.
  4. Create the Binder: Click the Create a sub-shape binder tool icon in the PartDesign toolbar (represented by a green outline of a shape with a blue connection symbol).
  5. Verify Placement: Look at the tree view. A new Binder or SubShapeBinder object will appear nested under Body B. Even though it references Body A, it belongs to Body B.

Using the Binder in a New Sketch

Once created, the binder can be used just like native geometry:

  1. Create a new sketch inside the active body (Body B).
  2. Click the Create external geometry tool (the "X" icon).
  3. Click the edges or vertices of the Sub-Shape Binder displayed in the 3D view.
  4. The referenced geometry will appear as magenta construction lines, allowing you to attach constraints, dimensions, and sketch points directly to them.
  5. Close the sketch and perform standard operations such as Pads or Pockets.

Managing Relative Placement and Options

Select the Sub-Shape Binder in the tree view to modify its behavior in the Property panel:

  • Bind Mode: By default, binders update dynamically (Synchronized). You can set this to Frozen if you want to detach the reference temporarily and lock the geometry in place.
  • Offset: You can define a numeric offset to expand or contract the binder geometry relative to the original shape.
  • Placement: The binder accurately tracks the global position of the source body relative to the target body, ensuring alignment even if either body is repositioned within an assembly or Part container.