Revolve dialog box

Section

A section can include one or more open or closed collections of curves or edges.

Select Curve — Lets you select curves, edges, a sketch, or a face to define the section.

• Tip: If you select a planar face when the Curve Rule is set to Infer Curves, the Sketch automatically opens to let you sketch new curve sections on the selected planar face. To prevent the Sketch from opening automatically, choose File tab → Utilities → Customer Defaults → Modeling → General. On the Miscellaneous page, clear the Automatically Sketch on Planar Faces check box.

Sketch Section — Opens the Sketch and lets you sketch a section that is internal to the feature. On exiting the Sketch, your sketch is automatically selected as the section to revolve.

Reverse Direction — Reverses the direction of the first curve in the section string, as indicated by a direction arrow. If there is no offset specified, this option has little effect on the revolve. But if an offset is specified, this option controls the offset direction, pointing it either inwards or outwards. (See Offset below for more details.)

Specify Origin Curve — Lets you specify which of the selected curves in the section string is the first curve in the revolve section, regardless of the order in which the curves were selected. The location and direction of the first curve of each section string is marked by a direction vector. The first curve in the revolve section can be important in certain revolve operations using the Until Selected limits option, which relies on the first curve of the first loop of the section. If your revolve fails with Until Selected, you may want to try selecting a different origin curve.

Axis

Lets you select and position a rotation axis. The revolved body is associative to the rotation axis. The rotation axis must not intersect the section curves. However, it can be coincident with an edge.

Specify Vector — Lets you select a curve or an edge, or define a vector using either the Vector Constructor or the vector list.

Reverse Direction — Reverses the direction of the axis and the revolve.

Specify Point — Positions the axis vector when the software does not infer a point during vector creation (for example, with the Face/Plane Normal method), or when you want to locate the vector at a point other than the inferred point.

Limits

The start and end limits represent the opposite ends of the revolve, from 0 to 360 degrees around the rotation axis.

Start / End

• Value — Lets you specify a value for the angle of rotation.
  • Snap to Object — Available on the shortcut menu when Start or End is set to Value. Lets you define a Start or End distance value by selecting a point, a planar face, or a datum plane. The software calculates the distance along the revolve arc and sets the value. There is no associativity to the point, face, or datum plane.
    • Note: If you use a planar face or datum plane as the Snap to object, we recommend that the face or datum be normal to the revolve arc where the face or plane intersects the arc.
• Until Selected — Lets you specify a face, solid body, sheet body, or relative datum plane where you want the revolve to start or end. You can select a solid body, sheet body, face, or relative datum plane for the defining limit.
  • Tip: You can bypass this option by selecting a limit handle in the graphics window and then selecting the desired limiting object.

Sweep — Appears when you set the Start or End limit list to Symmetric Value. Specifies the span of the revolve in degrees. NX revolves the selected section on either side of the specified axis. (Example: a section rotated on either side of an axis by 90° with the angle specified as 180°.)

Boolean

Use the Boolean options to specify how the revolve feature interacts with bodies it contacts.

Boolean

• None — Creates an independent revolve solid body.
• Unite — Combines the revolve volume with two or more bodies into a single body.
• Subtract — Removes the revolve volume from a target body.
• Intersect — Creates a body containing the volume shared by the revolve and existing bodies it intersects.
• Tip: You can also choose a Boolean option by right-clicking the preview. All options except None can leave empty space where the target body existed.

Select Body — Appears when Boolean is set to Unite, Subtract, or Intersect. Lets you select a target body.

Offset

Use this option to create a solid body, when you add an offset to one or both sides of the section.

Offset

• None — Does not add an offset to the revolve section.
• Two Sided — Adds offsets to one or both sides of the revolve section. If you have two section strings in a revolve that have first curves with opposite directions, any offset you add will also point in opposite directions. You can correct that condition by double-clicking one of the vectors so they both point in the same direction.

Start / End — Lets you specify the linear dimension start and end points for the offset. Positive and negative values are valid.

Settings

Body Type — Lets you specify if the revolve feature is one or more solid bodies or sheet bodies. To get a solid body, the section must be either a closed profile string or an open profile string with an offset. If you specify an offset, the system creates a solid body.

Tolerance — Lets you override the default distance tolerance during creation or edit. The default value is taken from the Modeling preference Distance Tolerance setting. The new distance tolerance is effective for subsequent revolve operations throughout the current session.

How do I

• Revolve and unite a section
• Revolve a section with an offset
• Revolve a section between faces
• Revolve a section using a symmetric angle

Learn more

• Revolve

Look up more details

• Solid bodies and sheet bodies with Revolve
• Revolve tips

Revolve dialog box, NX 2212 Series © 2023 Siemens