Creating a Prism

You can create a prism based on a closed profile.

Many capabilities require creating prisms.

See Also
About Prisms
About Feature Modifiers
Using Feature Modifiers
  1. Launch any capability requiring a shape definition. For example, from the Create section of the action bar, click Shellable Feature .
    The Prism is the default shape.
  2. Select a sketch or surface to define the prism.

    You can select an existing sketch, a sketch output, a sketch output profile or surface.

    Tips:
    • If no profile is defined, click Positioned Sketch to sketch the profile.
    • You can also select:
      • Any face originated by functional features of any solid functional set. In this case, the face needs to be the original untrimmed (unmerged) of the feature.
      • Any topological (trimmed) face of any Part Design body that is not the PartBody containing the active Solid Functional Set.

  3. In the Limits tab under First Limit, select the type and enter the required parameters.
  4. Optional: Click Mirrored extent or under Second Limit, select the type and enter the required parameters.
  5. In the Direction box, select a geometrical element as a reference for new extrude direction.
    By default, the direction is normal to the selected profile.

    You can click to reverse the extrude direction.

  6. Optional: In the Draft tab,
    1. From the Draft behavior list, select Intrinsic to feature.
    2. Set profile plane as the neutral element and enter the required value to define the draft angle.
  7. Under Thin Properties, specify the required values for the following parameters:

    • Enter a required value in the Inside Thickness box. Thickness is evenly distributed to both sides of the profile.
    • To enter a value in the Outside Thickness box, from the Reference list, select Outside Thickness. Thickness is added to the outside of the profile.
    Note: If you select Outside Thickness in the Reference list, the thickness you defined for inside thickness is added to the inside of the profile

  8. Optional: In the Fillet tab,
    1. Select among the following check boxes and enter the required values, to fillet the corresponding edges:

      • Lateral radius to fillet lateral edges
      • First radius to fillet top edges
      • Second radius to fillet bottom edges

    2. Select the Fillet profile ends check box, to fillet the end faces of open sketches.
    3. Select the Draft fillets check box, to fillet the drafted edges.
    4. From the Type list under Intersection Fillet, select among the following, to create fillets at required intersections:

      • Intersection with Core/Cavity
      • Intersection with Core
      • Intersection with Cavity

    5. Select the Fillet radius check box to create fillet by adding material to the feature.
    6. Select the Round radius check box to create fillet by removing material from the feature.
    7. Select the Preserve shell thickness check box to maintain the thickness at fillets.
  9. Select the Constant Thickness check box to apply lateral fillets to the feature with a constant wall thickness.
  10. In the Core tab, define a core body (offset) for a shellable feature when the geometrical complexity of the shellable feature is such that standard offsets fail.

    If your part contains two or more shellable features, choose between below three methods:

    • Isolated core: Generates the core automatically at feature level through an offset of only this shellable features geometry (i.e. the feature is independently shelled)
    • Interconnected core: Generates the core automatically at functional body level through an offset of the union of all shellable features contained within the same functional body.
    • Select core: Lets you select a body to represent the core for the shellable feature.

      Note: You cannot define the faces selected for core as faces to remove or faces with special thickness.