To Create an Offset Wall
1. Click > > 
Offset. The Offset tab opens.
Offset. The Offset tab opens.2. Select a surface, a quilt, or a solid body as a reference for the offset.
 | Alternatively, you can first select the geometry and then click > Offset. |
3. The thickness of a first wall can be changed only when the body is not linked to the part. Under Thickness, type a value for the wall thickness in the 
box or accept the default value. Click 
to flip the thickness direction.
box or accept the default value. Click to flip the thickness direction.4. Type a value in the Offset 
box to set the offset distance. Click 
to flip the offset direction.
box to set the offset distance. Click to flip the offset direction.5. Click Options. The Options tab opens. Perform any of the following operations:
◦ Click the Special Handling collector and select one or more surfaces to exclude.
▪ Auto—Populates the Special Handling collector with surfaces that cannot be offset without special handling.
▪ Exclude All—Excludes all the surfaces in the collector from the offset operation.
▪ Approximate All—Creates approximate offsets for all surfaces in the collector.
▪ Attach approximate offset surfaces check box—Creates attached approximate offset surfaces when the approximate surfaces cannot be merged with the standard offset surfaces.
For more information about excluding surfaces, search the Help Center.
◦ Set sheetmetal-specific options:
▪ 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.
6. 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. |
7. 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.
8. Click 
.
.