To Create a Parallel Blend Wall with Regular Sections
1. Click > > 
Blend. The Blend tab opens.
Blend. The Blend tab opens.2. Choose a wall creation method:
◦ To sketch internal sections:
a. Under Blend With, click 
Sketched sections, or click Sketched sections on the Sections tab.
Sketched sections, or click Sketched sections on the Sections tab.b. Click Define under Section Offset or, on the Sections tab, click Define and select a planar reference, a point, a vertex, or the end of a curve to define the sketch plane.
Define under Section Offset or, on the Sections tab, click Define and select a planar reference, a point, a vertex, or the end of a curve to define the sketch plane.c. Sketch the first section.
d. To set the sketch plane reference for the second section, click Offset dimension or Reference on the Sections tab, and then set the offset or select a reference for the section. Click Sketch and sketch the section. The blended walls preview.
e. To sketch another section, click Insert and repeat the previous step.
◦ To select sections:
a. Make sure that under Blend With, 
Selected Sections is selected or click Selected sections on the Sections tab.
Selected Sections is selected or click Selected sections on the Sections tab.b. Select the first section.
c. Click Insert on the Sections tab and select an additional section. The blended segments preview.
d. To add additional sections for the blend, repeat the previous step until all sections are added.
 | For more information on using the Blend tools, search the Help Center. |
3. The thickness of a first wall can be changed only when the body is not linked to the part. Under Section, 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. Click Options. The Options tab opens. Perform any of the following operations:
◦ Click Straight to connect the section edges with straight lines, or click Smooth to connect the section edges with spline surfaces.
◦ 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 model to merge the wall to an existing wall in the design. 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 model to keep the new geometry as a disjoint volume. You now have the option to flip the driving surface of the sheet metal.
5. 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.
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. Click 
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