Creating a Sweep

You can create a sweep by sweeping a profile along a center curve.

See Also
About Sweeps
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 , then click Sweep in the Shellable Feature dialog box that appears.
  2. Select the profile you want to sweep.
    Important: All the shape features have a profile/surface as part of the definition of the prism geometry.
    • If no profile is defined, click Positioned Sketch to sketch the profile you need.
    • You can also select:
      • Any face originated by functional features of any functional body. 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 functional body.
  3. Click Guided curve and select a sketch or click to sketch the center curve.
  4. Under Profile Control Options, select a profile control type and a profile control element.
  5. In the Draft tab, select the Intrinsic to feature option, the profile plane as the neutral element and then enter the value of your choice to define the draft angle.
  6. In the Fillet tab, select the required check boxes and set the values for respective fillet parameters.
    • Select the Lateral radius check box if you want to fillet lateral edges and set the radius value of your choice.

    • Select the First radius check box to fillet top edges and set the required radius value.

    • Select the Second radius check box to fillet the opposite bottom edges and set the required radius value.

    • You can select the Draft fillets check box if required. For more information, see draft fillets.
    Important: The core tab letss you define a core body (offset) for a shellable feature.
  7. Optional: Under Thin Properties (available for prism, sweep, and revolve shapes) select the Use param for thin feature check box, select a reference element and enter the required thickness values ().
    1. Select the Use param for thin feature check box to specify the thin feature parameters.
    2. From the Reference list, select a reference type.
    3. Enter the inside and outside thickness values.
    This option enables you to add material on both sides of the profile.