The Sweep functions create freeform parts by sweeping a profile along a path defined by a spine curve. The profile defines the cross-section of the sweep body and the spine defines the path along which the profile is swept. The control mode defines the orientation of the profile as it follows the spine.
The following rules apply:
• Multiple closed planar profiles can be used in the same sweep operation, provided that all of these profiles are located on the same workplane.
• The profile(s) to be swept can be located at any distance from the spine defining the sweep path. However, for the Sweep Rem command, make sure that the profile sweeps through the part from which you want to remove the swept volume.
• The spine can be open or closed. If you want to sweep the profile along a specific section of the spine, split the spine at the begin and end points of this section.
• The spine must not be located in the same workplane as the profile(s) to be swept.
• If the spine is not smooth, such as a spine with sharp corners, the spine must lie on a plane.
• The combination of profile shape, spine and sweep control mode must be such that there is no self-intersection of the profile along its sweep path. Failure to comply with this rule returns an error message stating that the sweep body would contain self-intersecting surfaces.
To prepare for a sweep operation,
1. Create the profile(s) to be swept. If you want to sweep multiple profiles in a single operation, make sure that all of these profiles are located on the same workplane.
2. Make sure you have a series of 2D and/or 3D curves to serve as the spine. For example, you can select a 3D polyline composed of a straight section to which an interpolation spline is appended. The spine can also be defined by edges of an existing part.
3. If you want to sweep along a given section of the spine only, split the spine at the begin and end point of this section.
To sweep a part,
1. Click Modeling and then, in the Model group, click More.
2. Click Sweep Add in Basic Sweep section. The General Sweep dialog box opens.
3. Click Sweep Remove in Basic Sweep section. The General Sweep dialog box opens.
4. Select or enter a Part name.
5. Select the Workplane. All closed profiles on the workplane will be swept. You will get an error if the workplane contains an open profile.
6. Select the Spine you want to use for the sweep path. If you want to limit the sweep path to a section of the total spine, select this option only. If this section is part of a curve segment, split the curve segment at the begin point and end point of the section.
7. Set the Control mode:
◦ by Spine: This is the default control mode. The normal of the profile will follow the spine during the sweep operation.
◦ by Face: The sweep path is described by an existing edge adjacent to a face.
◦ Constant: The normal of the profile maintains its orientation. The swept profile remains parallel to the original profile.
8. Select Check Part to verify the part's integrity during the sweep operation. Although the operation is faster without this option, you may create a corrupt part. We recommend you keep the Check Part option on, because the part checker will not be able to detect that the part is corrupt.
9. Click to complete the operation.
Control modes
• by Spine
When you select this control mode, the normal of the profile follows the spine during the sweep operation. The sweep operation does not "twist" the profile along the sweep path.
In the example shown below, a profile (1) is swept along a path defined by a spine (2). The normal of the end face (3) of the newly created part has the same orientation as the spine at the end point of the sweep operation.
The profile and spine shown above are the same as in the third figure below. The only difference between both examples is the control mode for the sweep path.
• by Face
When you select this control mode, the normal of the profile follows a spine defined by one or multiple edges adjacent to one or multiple faces on the same side of the edges.
This control mode can also be applied to face parts that have a face on one side of a given edge only. If you attempt to select the other (non-existent) side of such parts, the system will tell you that the opposite face path is not complete.
The profile will be twisted along the sweep path defined by the spine. This twist is controlled by the faces adjacent to the edges that make up the spine.
Optionally, you can toggle to the faces on the other side (if any) of the spine to apply the twist defined by the face path on the other side of the spine.
In the example shown below, material is to be removed from an existing body. For this purpose, a profile (P) is swept along a spine defined by two edges (E1 and E2). These edges are adjacent to:
◦ two faces (F1 and F2) on one side
◦ one face (F3) on the other side
If you select the side defined by faces F1 and F2, the profile (P) twist is controlled by F1 and F2. The sweep volume (V1) of the profile is twisted due to the variation of the normals of F1 and F2 along the spine.
If you select the side defined by face F3, the profile (P) twist is controlled by F3. The sweep volume (V2) of the profile is twisted due to the variation of the normal of F3 along the spine.
Note that the twist volume (V1) shown in (2) differs from the twist volume (V2) shown in (3).
• Constant
When you select this control mode, the normal of the profile retains its original orientation during the sweep operation. The sweep operation does not twist the profile along the sweep path.
In the example shown below, a profile (1) is swept along a path defined by a spine (2). The end face (3) of the newly created part is parallel to the original profile.
The profile and spine shown above are the same as in the first figure above. The only difference between both examples is the control mode for the sweep path.
Sweep Add in Basic Sweep section. The General Sweep dialog box opens.
Sweep Remove in Basic Sweep section. The General Sweep dialog box opens.
to complete the operation.
