Extrude dialog box

Section

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

• If you select a planar face when the Selection Intent rule is set to Infer Curves, the Sketch opens to let you sketch new curve sections on the face.
• If you select multiple sections, you get multiple sheet bodies or solid bodies, but only one extrude feature.
• Note: A section cannot include 3 or more curves whose end points coincide.

Sketch Section — Opens Sketch so you can create an internal sketch.

Reverse Direction — Available when you select the Show Section Curve Flow Direction customer default. Reverses the direction of the section curve.

Specify Origin Curve — Available when you select the Show Section Curve Flow Direction customer default and a loop of curves. Lets you specify one of the selected curves as an origin curve.

Direction

Reverse Direction — Changes the direction of the extrude to the opposite side of the section.

Limits (Start / End)

• Value — 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 extrude vector.
• Value From Start Limit — Defines the end of an extrude relative to the start of the extrude.
  • Example: To create an extrude of thickness 10 — Start Limit → Value = 25; End Limit → Value from Start Limit = 10.
• Symmetric Value — Creates a solid or sheet body of the total width specified in the Distance box. NX extrudes the section on both sides of the section curve by half the specified value.
• Until Next — Determines the limit by finding an intersection with the next face in the model.
  • Start limit = Until Next: the extrude is trimmed to the faces encountered in the reverse extrude direction.
  • End limit = Until Next: the extrude is trimmed to the faces encountered in the positive extrude direction.
  • Start and End limits = Until Next: the extrude is trimmed to both sets of faces found in the positive and reverse extrude directions.
• Until Selected — Extends the extrude feature to a selected face, datum plane, or body. If the extrude section extends past or does not completely intersect the selected face, the software extrudes the section onto adjacent faces of the selected face. If the selected face and its adjacent faces still do not intersect the extrude section completely, the extrude will fail, and you should try the Until Extended option.
• Until Extended — Trims the extrude feature (if it is a body) to a selected face when the section extends beyond its edges. If the extrude section extends past or does not completely intersect the selected face, the software extends the selected face mathematically when possible, and then applies trimming. A planar selected face would be unlimitedly extended to make the trimming successful, whereas a B-spline surface could not be extended.
• Offset from Selected — Defines the start or end of an extrude that is offset from a selected face or body. (Examples given for Start limit, End limit, and both Start+End limit set to Offset from Selected, with offset distances and limit values.)
• Through All — Extends the extrude feature completely through all selectable bodies along the path of the specified direction.

Distance — Appears for both the Start and End options when either is set to Value, Symmetric Value, or Value from Start Limit. Sets the start and end limits for the extrude feature.

Select Object — Appears for both the Start and End options when either is set to Until Selected, Until Extended, or Offset from Selected. Lets you select a face, sheet body, solid body, or datum plane to define the bounding start or end limit of the extrude feature.

Open Profile Smart Volume — Extends open profile geometry along open end points to find closure with the target body.

• Note: A Material Side vector allows you to select the volume side of the profile.

Boolean

Boolean — Lets you specify how the extrude feature interacts with the bodies that it comes in contact with.

• None — Creates an independent extrude solid body.
• Unite — Combines the extrude volume and the target body into a single body.
• Subtract — Removes the extrude volume from the target body.
• Intersect — Creates a body containing the volume that is shared by the extrude feature and the existing bodies that it intersects.
• Inferred — Determines the most probable Boolean operation based on the direction vector of the extrude and the position of the objects that are being extruded. NX automatically selects a target body from multiple solid bodies in the graphics window, and shows a preview of the interaction between the extrude feature and the target body.

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

Draft

Draft — Lets you add a slope (draft) to one or more sides of the extrude feature.

• Note: You can add a draft only to an extrude feature based on a planar section.
• None — Does not create a draft.
• From Start Limit — Creates a draft beginning from the extrude start limit.
• From Section — Creates a draft beginning from the extrude section.
• From Section-Asymmetric Angle — Available when the extrude feature extends from both sides of the section. Creates a draft starting from the extrude section, sloping in opposite directions both in front and back of the section. You can separately control draft angles on each side of the section using the Angle Option.
• From Section-Symmetric Angle — Available when the extrude feature extends from both sides of the section. Creates a draft starting from the extrude section, sloping at the same angle in opposite directions both in front and back of the section.
• From Section-Matched Ends — Available when the extrude feature extends from both sides of the section. Creates a draft starting from the extrude section, sloping in opposite directions both in front and back of the section. The shape at the end limit is matched to that of the start limit, and the draft angle for the end limit changes to maintain the matched shape.
• You can also select draft options by right-clicking the extrude preview.

Angle Option — Lets you specify draft angles.

• Single — Adds a single draft angle for all faces of the extrude feature. You can change the angle by typing a value in the Angle box, dragging the angle handle, or typing a value in the scene dialog.
• Multiple — Adds unique draft angles to each tangent chain of faces of the extrude feature. You can edit the angles by selecting them from the dialog list box and typing new values in the Angle box, dragging the angle handles, or typing values in the scene dialog. This option is not available when the Draft option is From Start Limit.

Angle — Lets you specify a value for a draft angle. If the Angle Option is set to Multiple, the value is applied to the selected angle in the list box; otherwise it applies to all angles in the draft. A positive angle slopes the sides of the extrude feature outward away from the center of the selected curves.

Front Angle / Back Angle — Available when the Draft option is set to From Section — Asymmetric, with the Angle Option set to Single. Lets you assign separate angle values to the front and back sides of an asymmetric extrude feature.

List — Appears when the Angle Option is set to Multiple, letting you assign separate draft angles to each tangent chain of faces in the extrude feature. Displays the name and value for each draft angle. You can edit an angle by selecting it in the list box and typing a new value in the Angle box, typing a value in the scene dialog, or dragging its angle handle.

Offset

Offset — Lets you specify up to two offsets for the extrude feature, either by typing values relative to the section or by dragging offset handles.

• None — No offset created.
• Single-Sided — Adds a single end offset to the extrude feature. This kind of offset lets you fill holes and create bosses, simplifying part development.
• Two-Sided — Adds an offset to the extrude feature with start and end values.
• Symmetric — Adds an offset to the extrude feature with duplicate start and end values measured from opposite sides of the section. The value for both start and end is determined by the last one you specify.

Start — Lets you specify a value for the start of the offset, relative to the section.

End — Lets you specify a value for the end of the offset, relative to the section.

Settings

Body Type — Lets you specify either a sheet body or solid body for the extrude feature.

• Solid — To create a solid body, the section must be either a closed profile section or an open profile section with an offset. If you use an offset, you will not be able to get a sheet body.
• Sheet — To create a sheet body: select an open section without using an offset, or select any non-planar section (such as 3D curves or edges), or set the Body Type to Sheet and select a closed section.
• This option is available when you create or edit an extrude feature. In some cases you can change existing extruded sheet bodies to solid bodies, or vice versa.

Tolerance — Lets you specify a distance tolerance different from the default.

How do I

• Extrude a solid body
• Create an extrude feature with an offset
• Subtract an extrude feature
• Extrude between two bodies
• Extrude with an asymmetric angle
• Extrude using a section with self-intersecting curves

Learn more

• Extrude

Look up more details

• Extrude notes
• Extrude warnings
• Extrude handles

Extrude dialog box, NX 2212 Series © 2023 Siemens