Part Modeling > Edit Features > Offset > Offset Surface > To Constrain an Offset with a Sketch
To Constrain an Offset with a Sketch
1. Select a surface, and click Model > Offset. The Offset tab opens, and the surface is highlighted.
2. Select Expand as the type of offset.
3. Type the required offset value in the offset value box. An offset surface is created parallel to the reference surface.
4. Click the Options tab to specify the offset method:
Normal to Surface (default)—Offsets the surface normal to the reference surface.
Translate—Translates the surface along the specified direction. Click the Direction reference collector and select a plane, a flat face, a linear curve or edge, an axis, or a coordinate system as the reference.
5. On the Options tab, specify the Expand area type:
Whole Surface—Offsets the entire surface. This option is applicable only to a closed quilt surface or a solid surface.
Sketched Region—Offsets only the region inside the sketched boundary. Click Define to enter Sketcher or use Define Internal Sketch from the shortcut menu, and sketch a closed section for offsetting. You can also select an existing sketch.
6. To specify the side surface type:
Surface—Offsets the side surface normal to the surface.
Sketch—Offsets the side surface normal to the sketching plane of the sketch.
7. Click to finish the offset.