When creating holes, you first specify the type of placement, then the hole’s dimensions, drill point, termination, and thread type options.
- Click 3D Model tab
Modify panel Hole 
. - Choose the Placement method:
- From Sketch. This option sets automatically if a sketch is visible. Requires a hole center point or sketch point sketched on an existing feature. You can select endpoints or center points on existing geometry as hole centers. Or drag with left mouse button to select an area and sketch points within it can serve as centers of holes. Note: To use a single sketch to position dissimilar holes, you can use a single sketch to lay out the position of multiple holes. Then share the sketch among several hole features. Sketches cannot be shared when creating the hole as an assembly feature.
- Linear. Creates holes on a face relative to two linear edges.
- Concentric. Creates holes on a plane, concentric with a circular edge or cylindrical face.
- On Point. Creates holes which are coincident with a work point, and positioned relative to an axis, edge, or work plane.
- From Sketch. This option sets automatically if a sketch is visible. Requires a hole center point or sketch point sketched on an existing feature. You can select endpoints or center points on existing geometry as hole centers. Or drag with left mouse button to select an area and sketch points within it can serve as centers of holes.
- Specify placement options and select hole geometry: From Sketch
- Centers. Click to select endpoints, or center points of geometry as hole centers. Selects hole center points automatically. Displays a dynamic count of centers currently selected.
Linear- Face. Selects a planar face to place the hole.
- Reference 1. Selects the first linear edge referenced for dimensioning the placement of the hole.
- Reference 2. Selects the second linear edge referenced for dimensioning the placement of the hole.
- Flip Side. Reverses direction of the hole.
Concentric- Plane. Selects a planar face or work plane to place the hole.
- Concentric Reference. Selects the object referenced for the placement of the hole center. Choose a circular edge, or cylindrical face.
On Point- Point. Selects a work point to set as the hole center.
- Direction. Specifies the direction of the hole axis. Choose a planar face or work plane that is perpendicular to the axis of the hole, or choose an edge or axis that is parallel to the axis of the hole.
- If there are two or more solid bodies in the part file, click the Solids selector to choose the participating solid bodies.
- Specify the hole type and the appropriate diameters and depths:
- Drilled
. Holes have a specified diameter, and are flush with the planar face. - Counterbore
. Holes have a specified diameter, counterbore diameter, and counterbore depth. You can’t use a Taper Tapped Hole with Counterbore. - Spotface
. Holes have a specified diameter, spotface diameter, and spotface depth. Measurement of the hole and thread depth starts from the bottom surface of the spotface. - Countersink
. Holes have a specified diameter, countersink diameter, and countersink depth.
- Drilled
- Specify the Drill Point type:
- Flat. Creates a flat drill point.
- Angle. For angled points, on the drop-down list, specify angle dimension, or on the model, select geometry to measure a custom angle, or show dimensions. The positive direction of the angle is measured counterclockwise from the hole axis, normal to the planar face.
- Choose a Termination option:
- Distance. Defines the termination method for the hole. Uses a positive value for the hole depth. Measures depth as perpendicular from the planar face or work plane.
- Through All. Extends a hole through all faces.
- To. Terminates a hole at the specified planar face. Select the surface on which to end the hole termination. You can terminate the feature on the extended face.
- Flip. Available when using Distance and Through All termination options. Reverses direction of the hole.
- Surface
. Available when using the To termination option. Terminates the hole on a selected surface or face. - Extended Face
. Available when using the To termination option. Specifies an extended face for the hole termination. Extends the face when the termination entity does not intersect completely with the hole feature.
- Choose a thread method:
- Simple Hole
. Creates a simple hole without a thread. No additional settings are needed. - Clearance Hole
. Creates standard, untapped (and usually through) holes that are toleranced to fit specific fasteners. Use them to create clearance holes for standard fasteners based on a library of standard fastener data. Note: Fastener information can be included in hole notes in drawings.To manage clearance data, Autodesk Inventor uses the Clearance.xls Microsoft Excel spreadsheet file, which is located in the Design Data folder. The Application Options or project settings affect the location of the spreadsheet file. You can change the order in the file so that the clearance you use most frequently is presented first. Edit the clearance spreadsheet and change the sort order number (from 1 to n) in cell B1 of each sheet to match your priority. To activate the new sort order, restart the program
- Tapped Hole
. Creates a hole with a thread that you define. Specify tapped holes in either English or Metric standard sizes. For part hole features you can select a common thread size from a list and its diameter is calculated. - Taper Tapped Hole
. Creates a hole with a taper thread that you define. Specify the thread type and size and right-hand or left-hand direction, and Autodesk Inventor automatically determines the diameter, taper angle, and thread depth. Specify taper tapped holes in either English or Metric standard sizes.
- Simple Hole
- Specify thread settings: Clearance Hole
- Standard. Selects the standard for the fastener from a list.
- Fastener Type. Selects the type of the fastener from a list.
- Size. Selects the size of the fastener.
- Fit. Specifies whether the type of the hole fit is Normal, Close, or Loose.
Tapped and Taper Tapped Holes- Thread Type. On the drop-down list, select a thread type. ANSI Unified Screw Thread is an example of an inch-based thread type. ANSI Metric M Profile is an example of a millimeter-based thread type. NPT is an example of an inch-based thread type. ISO Taper Internal is an example of a millimeter-based thread type.
- Size. Depending on the thread type selected, a list of nominal sizes displays. Each nominal size has one or more pitches available. Each nominal size and pitch combination has one or more classes available.
- Designation. Defines the distance from a point on a screw thread to a corresponding point on the next thread measured parallel to the axis. Note: If you use English units, the pitch is equal to 1 divided by the number of threads per inch.
- Class. On the drop-down list, select the class of fit for the internal thread. Note: For English threads, the letter A represents external threads, and B represents internal threads. Use higher numbers for more accurate, closer fitting requirements. For instance, use 2B for screws, bolts, nuts, and other general applications. Use 3B for highly accurate and close-fitting requirements.
- Diameter. Displays the value for the diameter type of this hole feature. You can change this value only in Document Settings. The hole diameter sets automatically from the thread specification in the Thread.xls, based on the setting (Minor, Pitch, Major, Tap Drill) in Document Settings.
- Direction. Specifies how the threads wind. If you select Right Hand, the threads wind in a clockwise and receding direction when viewed from the end. A right-hand threaded bolt advances into the nut when turned clockwise. If you select Left Hand, the threads wind in a counter clockwise and receding direction when viewed from the end. A left-hand threaded bolt advances into the nut when turned counter clockwise.
- Full Depth. Specifies threads the full depth of the hole.
- (Optional) Select Infer iMate to place an iMate automatically on a hole.
- Click OK.