Creating Profiles From Design Guidance Shapes

You can use the Create Profiles command to create profile sketches from the resulting shape generated by Design Guidance.

This task shows you how to:

Before you begin: You need a shape that has been generated by Design Guidance. Once you have a generated shape, use planes intersecting the shape to create profile sketches.

Selecting the Profiles

You can extract sketches from planes that intersect the shape.

  1. Generate a shape based on your load and restraint requirements.

    For more information, see Designing Models with Design Guidance.

  2. Click Create Profiles to open the Create Profiles dialog box.
  3. Select the outline of the intersecting planes for creating profile sketches of your generated shape.
    OptionDescription
    Circle Creates a circle sketch on each intersecting plane. The size and shape of the circle is based on where the plane intersects with the shape. The number of planes is selected number in Additional Planes.
    Rectangle Creates a rectangle sketch on each intersecting plane. The size and shape of the rectangle is based on where the plane intersects with the shape. The number of planes is selected number in Additional Planes.
    Polyline Creates a polyline sketch on each intersecting plane. The size and shape of the polyline is based on where the plane intersects with the shape. The number of planes is selected number in Additional Planes.
    Slot Creates a slot sketch on each intersecting plane. The size and shape of the slot is based on where the plane intersects with the shape. The number of planes is selected number in Additional Planes.
  4. Optional: Set the inspection area for generating the profiles sketches.
    • In the Inspection Volume Size section set the:
      • X-length
      • Y-length
      • Z-length
    • In the Inspection Volume Origin section, set X, Y, and Z coordinates:
      • X
      • Y
      • Z
    • In the Inspection Volume Orientation section, set the angle:
      • X-angle
      • Y-angle
      • Z-angle
      • Click to reset the orientation of the inspection volume box to the global orientation.
  5. Click Add Profiles to add the intersecting profiles as sketches in the Design Manager.

    You can move the inspection volume and click Add Profiles again to add more profile sketches. The number of sketches that were added are displayed at the bottom of the Create Profiles dialog box each time you click Add Profiles along with the total number of profile sketches in the Design Manager.

  6. Optional: Click to close the Create Profiles dialog box and save the profile sketches.

    Click to close the Create Profiles dialog box without saving the profile sketches.

  7. Use the newly created sketch profiles listed in the Design Manager to create the Design Guidance geometry using Sketch and Feature tools.

Run a stress and deflection study to make sure the design solution does not fail under applied loads.

Using Profile Sketches to Create a Geometry

You can create the geometry using the profile sketches with the Sketch and Feature tools.

  1. From the Design Manager, double-click profile sketches generated from Inspection Volume sketch planes.

    You might find it easier to Hide the Feature and Design Guidance objects when creating your geometry.

    The sketch editor opens.
  2. Optional: Make any edits needed to your sketch and click to save your changes.
  3. From the Feature section of the action bar, use tools such as the Loft and Draft to finalize your geometry.

Run a stress and deflection study to make sure the design solution does not fail under applied loads.