Creating a Line Between Two Points

You can create a line between two selected points.

Before you begin: Insert in an assembly an existing 3D shape containing geometric elements.
  1. From the Assembly section of the action bar, click Line .
    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.
    • The Line Definition dialog box appears.
  • Important: You switch from Assembly Design app to the last representation app you used.
    1. Select Point-Point.
    2. Select two points.
      A line is displayed between the two points. Proposed Start and End points of the new line are shown.

    3. Optional: In the Support box, select a support surface.

      In this case a geodesic line is created, i.e. going from one point to the other according to the shortest distance along the surface geometry (blue line in the illustration below). If no surface is selected, the line is created between the two points based on the shortest distance.



    4. In the Point 1 and Point 2 boxes, select the start and end points of the new line, that is, the line endpoint location in relation to the points initially selected.
      These points are necessarily beyond the selected points, meaning the line cannot be shorter than the distance between the initial points.
    5. Select the Mirrored extent check box to create a line symmetrically in relation to the selected Point 1 and Point 2 points.
      Important: The projections of the 3D point(s) must already exist on the selected support.
    6. Click OK to create the line.
      The line (identified as Line.xxx) is added to the specification tree.
      Important: You come back in the Assembly Design app.