Sweep Feature Data

Define the sweep data

Dialog Box Options

Boss/Cutout

Defines whether the sweep adds (boss) or removes (cutout) material.

• If the part model does not yet have volume geometry, the only option is Boss.

Sweep elements

View, change or remove the elements you have selected for sweep with the Add, Change or Delete buttons.

Delete the line that controls the sweep

1. Select an element from the list.
2. Delete the element:
   • Click the following button: Delete or
   • Open the context-sensitive menu and select Delete.

   

Add lines to the curve controlling the cross-section

1. Click the Add button.
2. Select the lines to be added:
   • Click the line or lines you want to add to the guide curve.
   • Stop selecting guide curves by selecting Confirm (Confirm = V key, middle mouse button or the context-sensitive function OK).
   • If you want to select a tangential polyline by selecting one line of the polyline only, first click the button: and then click the line.
3. Select a line.
4. Select Confirm.

Add a tangential line chain to the existing guide line

1. Select the line from the list.
2. Click the Tang button in the dialog box.

Keep cross section direction

The direction of the cross section is kept during the sweep (A) when this checkbox is selected. Otherwise, the cross section normal will coincide with the line selected for the sweep (B).

Trimming of the first (1.) end

Defines the trimming of the first end of the sweep feature to either an element selected from the model or prevents trimming. The ends are indicated in the model with the numbers 1 and 2. Select one of the following:

• No - End is not trimmed, the sweep ends at the end point of the selected line or other end point.
• To Face - The sweep is trimmed to one or more faces you selected from the model. Confirm the selections with the Confirm function.
• To Point - The sweep is trimmed to a single point you selected from the model.
• To Part - The sweep is trimmed to one or more parts you selected from the model. Confirm the selections with the Confirm function.
  • This function is available when a part is being modeled in an assembly and the other part "cuts" the geometry to sweep.

Example: Trimming to a Face

• Above on the left: The cross section and the line are selected.
• Above on the right: By default, a tangential line chain has been selected.
• Below on the left: No trimming.
• Below on the right: Trimming to face.

Example: Trim to point

• Top left image: By default, a tangential line chain has been selected.
• Top right image: Trimming the second end to a point is selected and the point is clicked.
• Bottom right image: Result.

Offset

Defines an offset value for the sweep when the sweep does not have end trimming, or the end is trimmed to face, part or edge.

An example of an offset for a guide curve

• Above on the right: No offset value, so the sweep extends to the ends of the guide line.
• Below on the left: At both ends, offset has a positive value.
• Below on the right: At both ends, offset has a negative value.

Example of offset on surfaces

• Above on the right: No offset value, so the sweep extends to the ends of the guide line.
• Below on the left: At both ends, offset has a positive value.
• Below on the right: At both ends, offset has a negative value.

Formula

Defines the offset variable.

Trimming of the second (2.) end

Defines the trimming of the other end of the sweep feature.

Tool

Defines the sweep feature as a tool.

Apply

Preview by clicking the Apply button in the dialog box. This will show you how the model would look if you confirmed the feature data by clicking OK. If necessary, you can still edit the feature data.