Snapping Components in an Engineering Connection

You can snap and constrain components within an engineering connection.

Before you begin: Open an existing assembly containing 3D shape representations.
Related Topics
Creating an Engineering Connection

  1. Click Engineering Connection .

    The Engineering Connection Definition dialog box and the Engineering Connection Assistant toolbar appear.

    Important:

    Be sure that the Smart Positioning option is not selected.

    The assembly looks like this:

  2. Select the first component.

    The snap capability is initialized. The Engineering Connection Definition dialog box is updated.

    The first component Axis is selected.

  3. Move the mouse over the geometry of a second component.

    According to the selected geometrical elements in the first component, the first component is pre-snapped on the compliant geometries of the second component.

    Important:
    • The Coincidence cursor is displayed. The type of cursor depends on the selected geometries.
    • The constraint order is defined in Tools > Options.... See Constraint.

  4. Select a compliant geometry on the second component and click the left button of the mouse

    The snap is validated and a constraint is created.

    The Engineering Connection Definition dialog box is updated.

    Important:

    While the Positioning Mode option is on , no engineering connection is created although you click OK in the Engineering Connection Definition dialog box.

  5. Click OK in the Engineering Connection Definition dialog box to create the engineering connection.

    The assembly looks like this: