About Sweeps

Draft behavior

The Draft behavior box lets you chose how you want to generate drafts:

• None: There is no draft.
• Intrinsic to feature: You can perform a draft operation by defining the following:
  • An angle value
  • A neutral element
    • Profile plane: The default neutral element defines a neutral curve on which the drafted face will lie.
    • Plane/Surface: Selecting this activates the selection box. You can select the plane or surface of interest. Also, you can select a sketch, and a Generative Shape Design surface of the required extent is automatically built.
• Draft Properties: You can also select Draft Properties.x which is set of draft properties predefined in Object Properties panel.
  • A neutral element
    • Profile plane: The default neutral element defines a neutral curve on which the drafted face lies.
    • Plane/Surface: If this is selected, the Selection box is active. You can select the plane or surface of interest.
    • Use parting element: This option is available when Draft properties is selected. The neutral element is equivalent to the selected Draft Properties Parting element.
  • Faces to draft: This controls which faces are drafted. There are three options:
    • All lateral faces
    • Selected by pull direction: Automatically selects the faces to draft to be those that are parallel to the pull direction vector.
    • Select profile curves: Specifies which faces to draft by picking curves of the boundary profile i.e. the defining profile curve for the face. You need to select Curves. There are two options available:
      • First limit
      • Second limit.

Parting Element

When the Profile Plane or Plane/Surface are selected to define the neutral element, Parting=Neutral is active by default. Moreover, when Parting=Neutral is selected, Draft both sides is also selected. If Draft both sides is selected, the draft becomes symmetrical about the parting element.

Three options are available:

• Parting=Neutral: The plane or surface you selected as the neutral element is also used as the parting element.
• Draft both sides: The draft operation applies to both opposite directions from the parting element.
• Draft fillets: The fillets are applied before the draft is created. Sometimes small edges that do not lie on the parting surface might be created. With this option, the fillets have variable fillet radius instead of the constant fillet radius and it prevents to generate the extra edges.

  Important: This option is also available in the Fillet tab. It operates simultaneously in both Draft and Fillet tabs.

Profile Control

You can control the sweep position by choosing one of the following options:

• Keep angle: Keeps the angle value between the sketch plane used for the profile and the tangent of the center curve.
  
  
• Pulling direction: Sweeps the profile with respect to a specified direction. To define this direction, you can select a plane or an edge.

You can also use contextual commands to control the sweep.

Move Profile to Path

Move profile to path check box lets you sweep the sketch such that:

• The anchor point travels along the path.
• The anchor direction remains either parallel to the pull direction or normal to the reference surface.

Move profile to path allows you to obtain a simple associative between the profile and the path, and also allows a single sketch to be swept along multiple paths.

To access the Move profile to path check box in Sweep, follow these steps:

1. Set Profile Control to either Pulling direction or Reference surface.
2. Select the Move profile to path check box.
3. Build the profile with the following understanding:

• The origin of the sketch plane (i.e. 0,0) will be swept along the path.
• The vertical axis of the sketch plane (i.e. 0,1) will be kept parallel to either the pulling direction (if profile control is set to Pull direction) or the normal to the reference surface (if the Profile control is set to Reference surface).