To Create a Helical Swept Wall
1. Click > and then click the arrow next to Sweep.
2. Click 
Helical Sweep. The Helical Sweep tab opens.
Helical Sweep. The Helical Sweep tab opens.3. For a new body not linked to the part in your design, under Settings, type a value for the wall thickness in the 
box or accept the default value. Click 
to change the side the thickness is added.
box or accept the default value. Click to change the side the thickness is added.4. Select or sketch a helix sweep profile and an axis of revolution. To sketch a helix sweep profile and axis of revolution:
a. The References tab is open by default.
b. Click Define. In Sketcher, set references and sketch an open section to define the helix sweep profile. The sketched entities must form an open loop.
c. Sketch a geometry centerline to define the axis of revolution.
 | The helix sweep profile entities must not have a tangent that is normal to the centerline at any point. |
d. Click 
.
.e. To flip the starting point of the sweep trajectory, click Flip.
5. Set the section orientation in relation to the helix sweep profile.
◦ Through helix axis—Orients the section to lie on a plane that passes through the helix axis.
◦ Normal to trajectory—Orients the section normal to the sweep profile.
| | If you select Normal to trajectory, the profile entities must be tangent to each other. |
6. Sketch a section to sweep:
a. Under Sketch, click 
to open Sketcher. Set references.
to open Sketcher. Set references.b. Sketch a section at the sweep start point (crosshairs).
c. Click .
.| | In Sketcher, you can change the direction of material thickness and specify thickness for a section containing a single chain with tangent entities. Click > > to access this tool. |
7. Under Pitch Value set the pitch (distance between coils).
8. Click 
Right-handed Rule to use the right-hand rule or click 
Left-handed Rule to use the left-hand rule.
Right-handed Rule to use the right-hand rule or click Left-handed Rule to use the left-hand rule.9. To set sheetmetal-specific options, click Options. The Options tab opens. Perform any of the following operations:
◦ Click Add bends on sharp edges to round sharp edges when the sketch includes nontangent geometry. Set the value of the radius and the location for dimensioning the radius.
◦ To set options for merging an additional wall to the model, set the options below:
▪ Select Merge to body to merge the wall to an existing wall in the body. You now have the option to keep the edges of merged geometry and edges of bend surfaces. This option is not available for a first wall.
▪ Select Do not merge to body to keep the new geometry as a disjoint volume. You now have the option to flip the driving surface of the sheet metal.
10. To create the new wall as a new body or to add the new wall to a different body, click Body Options. The Body Options tab opens.
◦ To create a new body, select the Create new body check box. A new body is created.
Click Link to part to link the preferences of the new body to the part preferences.
◦ To add the new wall to a different, existing body, select the body in the Model Tree or graphics window. The name updates in the body collector.
11. To set feature-specific bend allowance and calculate the developed length using a different method from that of the part, perform the following operations:
a. Click Bend Allowance. The Bend Allowance tab opens.
b. Click Use feature settings.
c. Perform one of the following operations:
▪ Click By K factor or By Y factor and type a new factor value or select one from the list.
▪ To use a bend table to calculate developed length for arcs, click By bend table. Use the default table, select a new one from the list, or click Browse to browse to a different table.
| | Only bend tables copied to the part are available. |
12. Click 
.
.