Creating a Point on a Surface

You can create a point on a surface at a specified distance and direction from a reference point.

See Also
In the Knowledge Base
Why does geodesic computation fail when creating a point on a closed surface?
  1. From the Assembly section of the action bar, click Point .
    The Choose a 3D Shape dialog box appears.
  2. Click Create new in the Choose a 3DShape dialog box.

    In the Choose a 3D Shape dialog box:

    • The Product box displays the name of the active product.
    • 3DShapes either lists the available 3D shapes instanced under the active product or lists the available 3D shapes instanced under a selected product. In both cases, these 3D shapes can be modified.
    • The Create new command allows you to create a 3D shape.
      Important: When you create a new 3D shape in Assembly commands context, its Nature is set as Specification whatever your choice in the dialog box, and you cannot change the nature of this 3D shape after it has been created with this command. See Nature of a New 3D Shape Created in Assembly Commands Context.
    • The Automatically create new 3D Shape when none exists option allows you to create a 3D shape either under the active or selected product automatically. In this case, the Choose a 3D Shape dialog box does not appear.

    The New Content tab appears.
  3. Click 3D Shape under Physical Product Structure node in the New Content tab.
  4. Click OK in the 3D Shape dialog box.
    The new 3D Shape is created under the active product.
  5. Click OK in the 3D Shape dialog box.
    • The new 3D Shape is created under the active product.
    • The Axis System Definition dialog box appears. The axis system's parameters Origin, X axis, Y axis, and Z axis are automatically computed, and Default (Computed) appears in the boxes.
  • Important: You switch from Assembly Design app to the last representation app you used.
    1. Select On surface.
    2. In the Surface box, select the surface where the point is to be created.
    3. Optional: Select a reference point.

      By default, the surface's middle point is taken as a reference.

    4. Optional: Select an element to use its orientation as a reference direction or a plane to take its normal as a reference direction.

      You can also use the context menu to specify the X, Y, Z components of the reference direction.

    5. In the Distance box, enter the value or use the arrows to change the value of a distance along the reference direction to display a point.
    6. Select the dynamic positioning of the point:
      • Coarse (default behavior): the distance computed between the reference point and the pointer is a Euclidean distance. Therefore, the created point may not be located at the location of the pointer. The handle (symbolized by a red cross) is continually updated as you move the pointer over the surface.

      • Fine: the distance computed between the reference point and the pointer is a geodesic distance. Therefore, the created point is located precisely at the location of the pointer. The handle is not updated as you move the pointer over the surface, only when you click the surface.
    7. Click OK to create the point.
      The point (identified as Point.xxx) is added to the tree.
      Note:
      • The dynamic positioning option is persistent but is not stored in the feature. Therefore, while editing, the dynamic positioning may not be the one you selected.
      Important: You come back in the Assembly Design app.