The Web command creates a thin feature from an open sketch profile, in a direction perpendicular to the sketch plane, extruded to the nearest faces on a solid body in Fusion.

Design > Solid > Create > Web

Presets

• Last Used Values: Uses the last used values.
• Default Values: Uses the default values for the new web.
• Plus: Adds a new preset.
• Reset: Resets the entered values to the values specified in the Set As Default selection list.
• Save: Saves the current values as a preset.
• Rename: Renames the selected preset.
• Delete: Deletes the selected preset.
• Soft By: Enables to specify how the presets are listed in the drop-down.
• Set As Default: Specify which values are used when creating a new web.

Profile

Select an open sketch profile.

Direction

• Symmetric: Extrudes half the thickness value to each side of the sketch profile.
• One Direction: Extrudes the full thickness value to one side of the sketch profile.

Start

• Bottom: Measures thickness starting from the bottom.
• Top: Measures thickness starting from the top.

Thickness

Specify the distance to extrude the web, in a direction parallel to the sketch plane.

Extent Type

• To Next: Extrudes the web from the sketch profile to the nearest faces on a solid body.
• Depth: Extrudes the web from the sketch profile to a specified depth.

Depth (Depth option only)

Specify the distance to extrude the web, in a direction perpendicular to the sketch plane, toward the nearest faces on a solid body.

Flip Direction

Flips the direction in which the web feature is extruded.

Draft Angle

Specify draft angle value for web.

Fillet Radius

Specify fillet radius value.

Extend Curves

• Check to extend the web feature beyond the ends of the sketch profile to the nearest faces on a solid body.
• Uncheck to stop the web feature at the ends of the sketch profile.