Hole dialog box

Type

Lets you select the type of hole feature to create:

• Simple — Creates a simple hole of the specified diameter, depth, and tip angle for a pointed tip.
• Counterbored — Creates a counterbored hole of the specified diameter, depth, tip angle, C-bore diameter, and C-bore depth.
• Countersunk — Creates a countersunk hole of the specified diameter, depth, tip angle, C-sink diameter, and C-sink angle.
• Tapered — Creates a tapered hole of the specified taper angle and diameter.
• Threaded — Creates a threaded hole whose dimensions are defined by the standard, thread size, and radial engage.
• Hole Series — Available only when you create a new hole feature. Creates a series of multi-form, multi-target-body, aligned holes with coordinated start, middle, and end hole dimensions. When you create a hole series using the JIS standard, the values for the dimensions are as per the JIS_B_1001_1985 standard.

Once you create a Hole Series hole feature, you cannot change its hole type. You also cannot change the hole type of another existing hole to Hole Series.

Note: You can customize the standard data tables used to create Drill Size Hole, Screw Clearance Hole, and Threaded Hole. See "Customize standard data tables for hole features."

Form

Does not appear for the Hole Series hole type.

Hole Size

Specifies the hole feature's form:

• Custom — Appears for the Simple, Counterbored, or Countersunk hole type. Lets you specify the hole dimensions.
• Drill Size — Appears for the Simple hole type. Lets you create a drill size hole feature based on ANSI or ISO standards.
• Screw Clearance — Appears for the Simple, Counterbored, or Countersunk hole type. Lets you create through holes that are designed to accommodate their application, such as clearance holes for screws.

Standard

Specifies the standard that defines the options and parameters used to create Drill Size, Screw Clearance, or Threaded features. You can specify the default standard in the Customer Defaults dialog box. You can customize the data tables used to specify the options and the corresponding parameters.

Screw Type list / Screw Size list

Available when Hole Size is set to Screw Clearance. The available options in the Screw Type list depend on whether Form is set to Simple, Counterbored, or Countersunk. Screw Size specifies the screw size for the selected Screw Type.

Size list

Available when Hole Size is set to Drill Size. Specifies the drill size used to create the drill size hole feature.

Fit

Available when Hole Size is set to Drill Size or Screw Clearance. Specifies the required fit for the hole (Close, Normal, Loose, Exact, or Custom). You must select Custom to specify values for the hole dimensions, chamfer, or relief dimensions.

C-Bore Diameter / C-Bore Limit / C-Bore Depth

Available for the Counterbored hole type.

• C-Bore Diameter — Specifies the counterbored diameter (must be greater than the hole diameter).
• C-Bore Limit — Specifies the counterbored depth geometrically: Value (specified depth), Until Selected (extends until the selected object), Distance from Selected (specified depth away from the selected object).
• C-Bore Depth — Available when C-Bore Limit is set to Value.
• Select Object — Available when C-Bore Limit is Until Selected or Distance from Selected; lets you select a face or datum plane.
• Distance — Available when C-Bore Limit is Distance From Selected.

C-Sink Diameter / C-Sink Angle

Available for the Countersunk hole type. C-Sink Diameter must be greater than the hole diameter. C-Sink Angle is the angle between the sides of the countersunk part of the hole; must be greater than 0 and less than 180 degrees.

Hole Diameter

Available for the Simple, Counterbored, or Countersunk hole type when Hole Size is Custom, and for the Tapered hole type. You can also use the handle in the graphics window to specify the hole diameter.

Taper Angle

Available for the Tapered hole type. Specifies the taper angle of the hole.

Size (Threaded)

Available for the Threaded hole type. Specifies the thread size selected from the thread standard to match your selected geometry.

Radial Engage

Available for the Threaded hole type. Specifies the radial engage percentage — the approximate percentage used to calculate the tap drill diameter, which determines the thread depth of a fastener installed in a tapped hole. (Radial engage = 50% vs 80% examples shown.) You must select Custom to specify a value for the tap drill diameter, chamfer, or relief dimensions.

Tap Drill Diameter

Available for the Threaded hole type. You can edit it only when Radial Engage is set to Custom.

Thread Depth Type / Thread Depth

Specifies the length of the thread for the Hole feature. Select from available options or choose Custom to customize the thread depth (Thread Depth field appears when Custom).

Thread Both Ends of Through Hole

Available for the Threaded hole type when Thread Depth Type is not Full. Adds threads at both ends of a through hole. If a threaded hole passes through multiple walls, the thread depth can also pass through multiple walls.

Handedness

Available for the Threaded hole type.

• Right Handed — Thread winds in a clockwise and receding direction when viewed axially towards an end.
• Left Handed — Thread winds in a counterclockwise and receding direction when viewed axially towards an end.

Relief / Apply Relief

Available for the Countersunk hole type (Custom or Screw Clearance) or the Threaded hole type. Apply Relief adds a relief to the hole feature when selected.

• Screw Clearance — You can edit the Depth value only when Fit is Custom.
• Threaded — You can edit the Diameter, Depth, and Angle values only when Radial Engage is Custom. You can specify 180 as the Angle value to add a counterbored relief.

Relief Chamfer

Available for the Threaded hole type when Apply Relief is selected. Adds a relief chamfer. You can edit the Offset and Angle values only when Radial Engage is Custom.

Chamfer (Start Chamfer / End Chamfer / Neck Chamfer)

Available for the Threaded hole type, or when Hole Size is Custom, Drill Size, or Screw Clearance. Creates a chamfer that is coaxial with the hole.

• Start Chamfer — Adds a start chamfer. For Threaded, available only when Apply Relief is cleared; edit Diameter/Angle only when Radial Engage=Custom. For Drill Size, edit Offset/Angle only when Fit=Custom.
• End Chamfer — Adds an end chamfer. For Drill Size/Screw Clearance, edit Offset/Angle only when Fit=Custom. For Threaded, edit Offset/Angle only when Radial Engage=Custom.
• Neck Chamfer — Available when type=Counterbored and Hole Size=Screw Clearance. Edit Offset/Angle only when Fit=Custom.

Position

Specify Point

Specifies the location of the center of the holes. Click anywhere on a face — the point clicked is the center of the hole. NX displays the point's dimensions in the graphics window (based on the existing datum coordinate system), which can be edited without entering the Sketch environment. You can also use snap point options on the scene toolbar (e.g. Arc Center) to specify the hole location.

For advanced dimensional constraints, use Create Sketch to enter sketch mode, or use an existing point (e.g. on a nonplanar face) as the hole center.

Note: When Normal to Face is selected as the hole direction, NX creates the hole normal to the sketch plane if the sketch point is away from the target body, or if the hole position is at the intersection of more than one face (e.g. the corner of a block).

Project Point onto Target

Creates a hole from the projected point. If the center of the hole is away from the target body, NX projects the point in the specified hole direction onto the target body; the projected point becomes the starting point of the hole.

Direction

Hole Direction

• Normal to Face — Defines the hole direction opposite to the nearest face normal within tolerance. (If more than one nearest face is possible, the face whose normal is closer to the Z axis is inferred.)
• Along Vector — Defines the hole direction along a specified vector (Vector Constructor or Inferred Vector).

Limit

Relate Hole Depth to Thread Depth

Available for the Threaded hole type when Thread Depth Type is not Full. Specifies the hole depth as a multiple of the thread pitch beyond the thread depth (edit the Pitch Multiplier).

Depth Limit

• Value — Creates a hole of the specified depth.
• Until Selected — Creates a hole that extends until the selected object.
• Until Next — Extends the hole until it reaches the next face.
• Through Body — Creates a through hole that extends until the last face of the selected body in the vector direction.

You can also use the dimension handle in the graphics window to specify the Depth Limit.

Hole Depth

Available when Depth Limit is Value. Specifies the required hole depth.

Depth To

• Cylinder Bottom — To the bottom of the cylindrical portion of the hole.
• Cone Tip — To the bottom of the drill tip.

Tip Angle

Available when Depth Limit is Value. Specifies the hole tip angle (flat or pointed end). A zero value results in a flat end (blind) hole; a positive value creates an angled tip added to the hole depth. Must be ≥ 0 and < 180.

Note: When a Hole is created using certain procedures, the Tip Angle value is read from standard XML files and is not editable, unless additional conditions are met (e.g. Simple→Hole Size=Drill Size→Fit=Custom, Threaded→Radial Engage=Custom). Standard tip angle values can be edited in:

• UGII\modeling_standards\NX_Drill_Size_Hole_Standard.xml
• UGII\modeling_standards\NX_Screw_Clearance_Hole_Standard.xml
• UGII\modeling_standards\NX_Thread_Standard.xml

Select Object

Available when Depth Limit is Until Selected. Lets you select a face or datum plane to specify the depth limit.

Specification (Hole Series)

• Start tab — Specifies the start hole parameters. Start hole is a screw clearance through hole of simple, counterbored, or countersunk form that begins at the specified center.
• Middle tab — Specifies the middle hole parameters. Middle holes are screw clearance through holes aligned with the start holes.
• End tab — Specifies the end hole parameters. End hole can be a screw clearance or threaded hole.

Boolean

• Boolean — None creates a solid representation of the Hole feature rather than subtracting it from the work part. Subtract subtracts the tool bodies from the target body in the work part or its components.
• Select Body — Selects the target body for the Boolean operation. Target bodies are generally solid bodies, but sheet bodies can also be selected as targets for the Simple type.

Settings

• Standard — Specifies the standard defining options/parameters used to create Drill Size, Screw Clearance, Threaded, or Hole Series features. Default standard set in Customer Defaults. When creating a hole series, the standard for middle/end hole can only be specified if "Match Dimensions of Start Hole" is not selected.
• Extend Start — Extends the hole to provide a clear cut at the start of the hole.
• Tolerance — Used to find the nearest face to define the normal direction of the hole using Normal to Face. If no face is found within tolerance, Normal to Face cannot be used.

Related

• Standard data tables for hole features
• Counterbored, countersunk, and tapered hole types
• Screw clearance hole types
• Threaded hole types
• Tapered Hole

---

Hole dialog box, NX 2212 Series © 2023 Siemens