Creating a Contour Reference

You can create a contour reference and save it in the database. A contour reference is a part containing a sketch with a closed contour.

Before you begin: Create a structure contour.
See Also
Creating a Structure Contour Reference
In Other Guides
Content for Structure Apps
  1. Double-click the representation node in the tree.
  2. Create two geometrical set under the representation node and rename them.
    The geometrical sets, Reference Contour and Limit Surface, are created.
  3. Under Limit Surface geometrical set, create two limiting surfaces:
    1. Select the xy plane.
    2. From the Geometrical Tools section of the action bar, select Positioned Sketch .
      You enter the Sketcher app.
    3. Create a spline.
    4. Click Exit app to exit the sketcher.
    5. Click Extrude to extrude the profile.
      An extruded surface is created.
    6. Rename it as Limit 1 Surface.
    7. Select the xy plane.
    8. Repeat step (b) to (e) to create another extruded surface intersecting the previously created surface.
    9. Rename the other surface as Limit 2 Surface.
    Two limiting surfaces are created.

    Important: Ensure that while sketching the splines should pass through the origin and the sketch is created in the 1st quadrant.
  4. From the Compass, click Generative Shape Design.
    You are switched to Generative Shape Design.
  5. From the Transform section of the action bar, select Inverse .

    The Invert Definition dialog box appears.

    1. In the To Invert box, select Limit 1 Surface.
    2. Click OK.
      The surface is inverted.
    3. Similarly, invert Limit 2 Surface.

    Important: Always keep the surface vector in inward direction. If the vector is already pointing inward, do not invert the surface.

  6. Activate the Reference Contour geometrical set and click Positioned Sketch in the action bar.
    The Sketch Positioning dialog box appears prompting you to select the planar support.
  7. Select the xy plane to create intersection of the surfaces:

    You are switched to Sketcher.

    1. From the Sketch section of the action bar, click Intersect 3D Elements .
      The Intersection dialog box appears.
    2. In the Element(s) to intersect box, select Limit 1 Surface.
    3. Optional: Select the No Canonical Curve check box, if the use-edge is going to be used for a face of a flange, panel, or plate selected by pressing Ctrl or Alt.
    4. Click OK.
      An intersection is created. For more information, see Sketcher User's Guide: Performing Operations on Profiles: Projecting 3D Elements: Intersecting 3D Elements with the Sketch Plane.
    5. Rename it as Limit_1.
    6. Repeat step (a) to (c) for Limit 2 Surface.
    7. Rename it as Limit_2.
    The intersection is created.

  8. Create a sketch on the xy plane and apply constraint to it.


  9. Create an output profile:
    1. From the Sketch section of the action bar, click 3D Profile .
      The Profile Definition dialog box appears.
    2. Select the lines.
    3. Click OK.
    The profile is created. It is recommended to define an additional output profile to be used as a support for stiffener on free edge or flange.

  10. Apply parameters and formulas to the sketch.

    For more information about creating parameters, see Knowledge Basics: Creating and Working with Parameters and Managing Relations: Formulas.

    Important:
    • Ensure that you create parameters by using the prefixes Pub_ for the public parameters and Priv_ for the private parameters.
    • The created parameters must be under the sketch node in the Reference Contour geometrical set.
    • Similarly, the created formulae must be under the sketch node in the Reference Contour geometrical set.

  11. Click Exit app to exit Sketcher.
    The contour is created.
  12. Select Share > Save > Save with Options to save the contour.
    The contour is saved in the database.