Hole dialog box

Options

Type
Type list	Displays a list of the types of Hole feature you can create. General Hole — Creates simple, counterbored, countersunk, or tapered Hole features of specified dimensions. General holes types are Blind, Through, Until Selected, or Until Next. Drill Size Hole — Creates a simple drill size hole feature using ANSI or ISO standards. Screw Clearance Hole — Creates simple, counterbored, or countersunk through holes that are designed to accommodate their application, such as clearance holes for screws. Threaded Hole — Creates threaded holes whose dimensions are defined by the standard, thread size, and radial engage. Hole Series — 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. Note: You can customize the standard data tables that are used to create Drill Size Hole, Screw Clearance Hole, and Threaded Hole. For more information, see Customize data tables for Hole features.
Position
Specify Point	Specifies the location of the center of the holes. You can use the following methods to specify the center of the hole: In the Create Sketch dialog box by specifying the placement face and orientation. By selecting a face. The coordinates of the cursor location are displayed in the Point dialog box. By selecting a datum plane. The coordinates of the origin of the datum plane are displayed in the Point dialog box. In the Dimensions dialog box. Click Point to specify the center of the hole using existing points.
Direction
Hole Direction	Specifies the hole direction. Normal to Face — Defines the direction of the hole along the direction opposite to the face normal which is nearest to each of the specified points within the tolerance. Note: If the selected point has more than one possible nearest face, the face whose normal at the selected point is closer to the Z axis, is inferred as the nearest face. Along Vector — Defines the hole direction along the specified vector. You can specify the vector using the options in Specify Vector: Vector Constructor or the list in Inferred Vector
Form and Dimensions
Form	Specifies the form of the Hole feature. 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.
Screw Type list	Available when Type is set to Screw Clearance Hole. The available options in the Screw Type list depend on whether Form is set to Simple, Counterbored, or Countersunk.
Screw Size list	Available when Type is set to Screw Clearance Hole. Specifies the screw size for the selected Screw Type used to create a Screw Clearance Hole feature.
Size list	Available when Type is set to Drill Size Hole. Specifies the drill size used to create the Drill Size Hole feature.
Fit	Available when Type is set to Drill Size Hole or Screw Clearance Hole. Specifies the required fit for the hole (Close, Normal, Loose, Exact, or Custom). Note: You must select Custom to specify values for the hole dimensions, chamfer, or relief dimensions.
Dimensions
C-Bore Diameter	Available when Form is set to Counterbored. Specifies the counterbored diameter. The diameter of the counterbored part of the hole must be greater than the hole diameter.
C-Bore Depth	Available when Form is set to Counterbored. Specifies the counterbored depth.
C-Sink Diameter	Available when Form is set to Countersunk. Specifies the countersunk diameter. The countersunk diameter must be greater than the hole diameter.
C-Sink Angle	Available when Form is set to Countersunk. Specifies the angle between the sides of the countersunk part of the hole; it must be greater than 0 and less than 180 degrees.
Diameter	Specifies the hole diameter.
Depth Limit	Specifies the hole depth limit. Available options are: Value — Creates a hole of the specified depth. Until Selected — Creates a hole till the selected object. Until Next — Extends the hole until it reaches the next face. Through Body — Creates a through hole.
Depth	Available when Depth Limit is set to Value. Specifies the required hole depth.
Tip Angle	Available when Depth Limit is set to Value. Specifies the hole tip angle to create either a flat or pointed end hole. A zero tip angle value results in a flat end (blind) hole. A positive tip angle value creates an angled tip, which is added to the depth of the hole. The tip angle must be greater than or equal to 0 and less than 180.
Select Object	Available when Depth Limit is set to Until Selected. Lets you select a face or a datum plane to specify the depth limit of the hole.
Thread Dimensions
Available when Type is set to Threaded Hole.
Size	Specifies the size for thread dimensions size.
Radial Engage	Lets you select the radial engage percentage. Specifies the radial engage percentage, which is the approximate percentage used to calculate the value of the tap drill diameter. The tap drill diameter determines the thread depth of a fastener when it is installed in a tapped hole that is made with the specified tap drill diameter. — Radial engage = 50% — Radial engage = 80% Note: You must select Custom to specify a value for the tap drill diameter, chamfer, or relief dimensions.
Tap Drill Diameter	Specifies the diameter of the tap drill. Note: You can edit the tap drill diameter only when Radial Engage is set to Custom.
Length list	Specifies the length of the thread for the Hole feature. Select from the list of available options or choose Custom to customize the thread depth.
Thread Depth	Available when Length is set to Custom. Sets the thread depth.
Rotation	Lets you specify whether the thread should be right handed (clockwise) or left handed (counterclockwise). — Right-handed thread winds in a clockwise and receding direction when the thread is viewed axially towards an end. — Left-handed thread winds in a counterclockwise and receding direction when the thread is viewed axially towards an end.
Relief
Available when Type is set to Screw Clearance Hole and Form is set to Countersunk, or when Type is set to Threaded Hole.
Enable	Adds a relief to the Hole feature when selected. For Screw Clearance Hole, you can edit the Depth value only when Fit is set to Custom. For Threaded Hole, you can edit the Diameter,Depth, and Angle values only when Radial Engage is set to Custom.
Start Chamfer
Available when Type is set to Drill Size Hole, Screw Clearance Hole, or Threaded Hole. Start Chamfer is available for Threaded Hole only when the Enable check box under Relief is not selected.
Enable	Adds a start chamfer to the Hole feature when selected. For Drill Size Hole and Screw Clearance Hole, you can edit the Diameter and Angle values only when Fit is set to Custom. For Threaded Hole, you can edit the Offset and Angle values only when Radial Engage is set to Custom.
Relief Chamfer
Available when Type is set to Threaded Hole and the Enable check box under Relief is selected.
Enable	Adds a relief chamfer to the Hole feature when selected. You can edit the Offset and Angle values only when Radial Engage is set to Custom.
Neck Chamfer
Available when Type is set to Screw Clearance Hole and Form is set to Counterbored.
Enable	Adds a neck chamfer to the Hole feature when selected. You can enter edit the Offset and Angle values only when Fit is set to Custom.
End Chamfer
Available when Type is set to Drill Size Hole, Screw Clearance Hole, or Threaded Hole.
Enable	Adds an end chamfer to the Hole feature when selected. For Drill Size Hole and Screw Clearance Hole, you can edit the Offset and Angle values only when Fit is set to Custom. For Threaded Hole, you can edit the Diameter and Angle values only when Radial Engage is set to Custom.
Specification
Available when Type is set to Hole Series.
Start tab	Specifies the start hole parameters. Start hole is a screw clearance through hole of the 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 that are aligned with the start holes.
End tab	Specifies the end hole parameters. End hole can be a screw clearance or threaded hole.
Boolean
Boolean	Specifies the Boolean operation to be used to create the Hole feature. Available options are: 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 to perform the Boolean operation. Target bodies are generally solid bodies, but you can also select sheet bodies as target bodies for the General Hole type.
Settings
Standard	Specifies the standard that define the options and parameters used to create Drill Size Hole, Screw Clearance Hole, Threaded Hole, or Hole Series features. Available when Type is set to Drill Size Hole, Screw Clearance Hole, Threaded Hole, or Hole Series. You can specify the default standard in the Customer Defaults dialog box. When you create a hole series, you can specify the required standard for the middle hole and end hole only if the Match Dimensions of Start Hole check box is not selected. You can customize the data tables used to specify the options and the corresponding parameters to create Drill Size Hole, Screw Clearance Hole, or Threaded Hole features. For more information, see Customize data tables for Hole features.
Extend Start	When selected extends the hole to provide a clear cut at the start of the hole.
Tolerance	Specifies the tolerance value. The tolerance value is used to find the nearest face to define the normal direction of the hole using the Normal to Face option. If no face is found within the tolerance you cannot use the Normal to Face option.