Hole and Thread

Overview#

The Hole tool places standards-based holes: simple, counterbore, and countersink, with optional clearance or tapped behavior. The Thread tool adds threads to cylindrical faces, internal or external. Together they produce the fastener features that manufacturing drawings expect, with real sizes (M5, 1/4-20) taken from tables instead of numbers you invent.

Why use Hole instead of an extruded circle cut?

• Tapped and Taper Tapped holes take their Thread Type, Size and Designation from the threads library (Public Library or a hub library), so thread data comes from tables rather than numbers you invent.
• One Hole feature carries the hole type, counterbore or countersink settings, depth and drill point together, and you can edit it later with Press Pull or Edit Hole.
• Preselected points carry into the dialog, so a sketch of points becomes many holes in one feature.

Where to find it#

• Workspace: Design.
• Tab / panel: Solid tab > Create > Hole; Solid tab > Create > Thread.
• Shortcut: H for Hole.

Step by step#

Placing a hole#

1. Press H. The Hole dialog appears.
2. Choose Placement: At Point (Single Hole) (click a face, plane or point, then position or dimension it) or From Sketch (Multiple Holes) (use sketch points; hold Ctrl (Windows) or Command (macOS) to pick several).
3. Click a face. With At Point, the References selector lets you select edges to position the hole; drag the manipulators or enter exact values.
4. Choose the Hole Type: Simple, Counterbore, or Countersink.
5. Choose the Hole Tap Type: Simple, Clearance, Tapped, or Taper Tapped. Taper Tapped is available only for Simple and Countersink hole types.
6. For Tapped or Taper Tapped, set the Threads Library (Public Library or a hub library) and pick Thread Type, Size and Designation; check Modeled to preview the thread.
7. Set Extents (Distance, To, or All), the Drill Point (Flat or Angle, with a Tip Angle) and, if you like, Flip Direction. In the Objects to Cut section, check or uncheck bodies.
8. Click OK.

Adding a thread to an existing cylinder#

1. Select Create > Thread.
2. Click the cylindrical face of a pin or bore (internal or external).
3. Optionally set the Threads Library (Public Library or a hub library), then choose the Thread Type, Size, Designation (for example M10x1.5), and Class.
4. Decide on Modeled (real geometry) or leave it cosmetic.
5. Leave Full Length on to thread the whole face, or turn it off and set Offset and Length.
6. Pick the Direction (right-hand or left-hand thread). Click Remember Size to reuse the settings next time, and click OK. Right-click and choose Repeat Thread to apply the same settings to another cylinder.

Worked example: a mounting plate#

1. Extrude a 80 x 50 x 8 mm plate.
2. Press H, click the top face, pick two References edges and dimension the hole 10 mm from each.
3. Choose Counterbore, Clearance, and a 5.5 mm hole Diameter for an M5 screw (general ISO 273 value; see the sizing table below). Extent: All.
4. Use a Rectangular Pattern of the hole to make four corner holes (see the Mirror and Patterns page).

Options reference#

Tips and pitfalls#

Tip: Make the first hole of a pattern a clean "Hole" feature and pattern the feature, not the faces. Face patterns tend to be more fragile (general advice).

Tip: Create holes from a sketch with many points (From Sketch), which keeps all hole locations in one editable sketch. Points or selection sets preselected before you start Hole carry into the dialog.

Warning: A tapped hole is drilled at tap-drill size (general machining practice), so a mating shaft dimensioned to the nominal diameter will not fit a hole whose thread is only cosmetic. Decide whether the model is for display, drawing, or printing.

Warning: A Modeled thread adds geometry and can slow the model (general experience). Autodesk notes you may want modeled threads for 3D printing, but you normally do not need them for milling.

Warning: The Thread tool works on cylindrical faces. A hole or boss from a loft, spline or polygon cannot take it.

• For 3D-printed parts, internal modeled threads often need tolerance tweaking; as general guidance, oversize them by roughly 0.2 to 0.4 mm.
• To edit a hole, use Press Pull, or right-click the hole in the browser and choose Edit Hole.
• For Tapped and Taper Tapped holes the Hole tool reads the Threads Library (Public Library or a hub library). See Autodesk's "Manage the threads library" topic to create, edit or delete custom threads.
• Adding a small chamfer at the hole mouth removes burrs and eases screw start; do this with Chamfer.

Choosing hole sizes with real numbers#

Clearance holes (screw passes through) and tap drills (screw cuts a thread) are different diameters. The values below are general ISO figures (not Autodesk data); Autodesk's Hole reference documents a Diameter field and does not list a fit setting:

The clearance columns are ISO 273 close, medium and coarse series values; type the one you need into the Diameter field.

Counterbores for socket head cap screws (ISO 4762): M4 head diameter 7 mm and head height 4 mm, so a counterbore of about 8 mm diameter and 4.4 mm deep. M5: head 8.5 mm, height 5 mm, counterbore about 9.5 x 5.4. M6: head 10 mm, height 6 mm, counterbore about 11 x 6.4. Add 0.5 to 1 mm to the head diameter for tool clearance in thin plates.

Countersinks for flat-head screws: angle 90 degrees in metric, 82 degrees in imperial. The countersink diameter must equal or exceed the head diameter, otherwise the head stands proud. For an M5 flat head of 10 mm diameter in a 4 mm plate, the countersink depth is (10 - 5.5) / 2 / tan(45) = 2.25 mm, which leaves 1.75 mm of material under it.

Thread depth versus hole depth#

A tapped hole has two depths: the drilled depth and the usable thread depth. General machining rule of thumb (not Autodesk data): drill depth is thread depth plus about 1.5 times the pitch for a bottoming tap's lead, or plus 2 to 3 pitches for a plug tap. For an M6 x 1 hole needing 12 mm of engaged thread, set thread length 12 mm and drilled depth about 15 mm. In a 3D printed part, drill 2 to 3 mm deeper for debris and support.

As a general rule of thumb, minimum engagement is about 1 times the diameter in steel, 1.5 times in aluminum, and 2 times in plastics and wood. An M6 hole in aluminum therefore needs 9 mm of thread.

Hole tap types in practice#

• Simple: a plain hole of the diameter you type. Use this for dowels, pockets and vents.
• Clearance: a hole sized for a fastener passing through.
• Tapped: a hole with a thread specification (Thread Type, Size, Designation) from the Threads Library. The Modeled option previews and creates physical thread geometry when you need it.
• Taper Tapped: for tapered threads such as pipe threads; Autodesk states it is available only for Simple and Countersink hole types, so it cannot be combined with a counterbore.

Cosmetic versus modeled threads#

Per Autodesk, cosmetic threads apply the appearance of threads to the selected geometry, while modeled threads are cut into it. Autodesk's tip: model a thread if you are 3D printing; you do not normally need to if you are milling. General FDM guidance (not Autodesk data): modeled internal threads usually need 0.3 to 0.4 mm of extra diameter on a 0.4 mm nozzle, and fine pitches below about 1.5 mm tend to fuse.

Thread tool options#

The Thread tool applies to an existing cylindrical face. Full Length controls whether the thread runs the whole face; when it is off, Offset sets the starting position and Length the extent. Thread Type, Size, Designation and Class come from the Threads Library (for example class 6g is the usual external metric class and 6H the internal one, general convention). Direction selects right- or left-hand. If you resize the hole with the manipulator, check that Size and Designation still match.

Failure modes and fixes#

Practice exercise#

Design a small mounting plate and a mating standoff, and verify every dimension.

1. Create an 80 x 50 x 8 mm plate.
2. Place four counterbored clearance holes for M5 with Hole > From Sketch: sketch four points 8 mm from each edge, in one sketch. Set the hole diameter to 5.5 mm and the counterbore to about 9.5 mm, with a counterbore depth of 5.4 mm, which leaves 2.6 mm of plate under the head.
3. At the plate center, place a Tapped M6 x 1 hole using At Point and References 40 mm and 25 mm, thread length 9 mm (engagement in aluminum, general rule), drilled depth 12 mm, Angle drill point with a 118 degree Tip Angle (a common drill-point angle).
4. Add a 90 degree countersunk hole for an M4 flat head at the midpoint of one long edge, 10 mm in. Compute and set the countersink depth for an 8 mm head diameter: (8 - 4.5) / 2 = 1.75 mm at 90 degrees.
5. Create a standoff: a 6 mm diameter, 25 mm tall cylinder (the cylinder diameter must match the thread size); add an external M6 x 1 thread, Full Length off, Offset 0, class 6g, length 9 mm to match the hole. Toggle Modeled and compare the timeline compute time.
6. Pattern the center hole with a rectangular pattern of 2 x 2, 20 mm spacing, using the pattern of the feature rather than faces.

Expected result: a plate with 4 + 1 + 1 hole features whose sizes match the standards you looked up, plus a threaded standoff that screws into the tapped hole. Check the engagement: a 9 mm thread in a hole drilled 12 mm deep leaves 3 mm of space behind the pin.

Related#

• Fillet and chamfer (hole entry chamfers)
• Mirror and patterns (repeat holes)
• Coil and pipe (build threads manually)
• Extrude (cut holes without standards)