Overview#
Holes are among the most common features on machined parts, and Fusion treats them with a dedicated Drill operation that is more than just "go down and come back". One Drill operation can handle drilling, spot drilling, counterboring, tapping, reaming, boring and more, depending on the Cycle Type you choose and the tool you assign. Hole selection can use model faces, which gives depth and keeps the operation associative to the model, and holes can be sorted for efficient travel.
Alongside the Drill operation, 2D milling operations produce holes by interpolation: Bore (helical boring), Circular (circular pocket/boss), Thread (thread milling), and Slot. Milling holes costs time but gives size control, uses a single tool for many diameters, and avoids dedicated drills for odd sizes.
The usual hole workflow: spot drill (or center drill) to start the hole accurately, drill to depth, then optionally chamfer, tap, ream or bore.
Where to find it#
- Milling > Drilling > Drill (and Hole Recognition in the same panel).
- Milling > 2D > Bore, Circular, Thread for milled holes.
- Toolbar search (S): "Drill".
Selecting hole geometry#
On the Geometry tab, Selection Mode chooses how drilling locations are found:
- Faces: model-based selection of cylinders or hole chamfers. Provides starting height and hole depth; Autodesk calls it the preferred method because it stays associative with the model.
- Points: hole edges, sketch points or sketch circles. Returns only the XY location and Z starting height.
- Diameter range: automatic selection by Minimum Diameter and Maximum Diameter.
- Remaining holes from operation: selects holes left unmachined or partly machined by a reference operation (fallback drilling after a collision).
Other Geometry options: Select Same Diameter (associative; new holes of that diameter are picked up on regenerate), Check for Occlusions (deselects holes the tool cannot reach in the current orientation), Containment Boundary, Auto-Merge Hole Segments (start from above the highest segment, e.g. after a spot drill or counterbore), Order by Depth, Order (Order selected, Optimized order, Inside to Outside, Order by X motion, Order by Y motion), Reverse Order, Reset Directions and Surface Manager. The Hole Recognition command separately groups features and creates operations.
Tip: Modeling holes with the Design Hole command rather than a plain extrude-cut keeps hole data in the model, which makes face-based selection easier.
Depth#
Depth comes from the Heights tab and the selection. With face selection the hole depth is read from the model. Through holes need extra depth so the drill tip emerges fully; use a Bottom Height offset and the Break through cycle option (reduced feed and speed before breaking through) as appropriate. Only cut beyond the hole when the exit side is free of fixture or table.
Cycle types#
The Cycle Type list on the Cycle tab selects the canned cycle. The posted code uses a controller canned cycle if the post supports it; otherwise it expands to explicit moves. Autodesk's cycle list:
| Cycle type | What it does | Common Fanuc-style code |
|---|---|---|
| Drilling - rapid out | Feed to depth, rapid out; spot and center drilling | G81 |
| Counterboring - dwell and rapid out | Feed to depth, dwell, rapid out | G82 |
| Chip breaking - partial retract | Peck with small retract | G73 |
| Deep drilling - full retract | Peck with full retract to the R plane | G83 |
| Break through | Reduced feed and speed before breaking through | n/a |
| Guided deep drilling - gun drilling | For gun drills | post-specific |
| Tapping, Left tapping, Right tapping | Taps; spindle direction comes from the tool library settings | G84 / G74 |
| Tapping with chip breaking | Screws in part way, reverses to break the chip, repeats | post-specific |
| Reaming - feed out | Feed in and immediately feed out | G85 |
| Boring - dwell and feed out | Reaming with a dwell at the bottom | G89 |
| Stop boring - stop and rapid out | Stops the spindle at depth, rapids out | G86 |
| Fine boring - shift | Orients the insert, shifts away, retracts | G76 |
| Back-boring | Bores from the back side with a reverse tool | G87 |
| Circular pocket milling, Bore milling, Thread milling | Trigger custom controller cycles | control-specific |
| Custom | Probe measurement or machine macros | control-specific |
The G-code numbers are common for Fanuc-style controls; other controls differ, and Autodesk advises consulting your machine's programming manual. The post decides the actual output.
Peck options#
For Chip breaking and Deep drilling:
| Option | What it does |
|---|---|
| Pecking Depth | Increment for each peck; sets the first peck |
| Pecking Depth Reduction | Subtracted from the pecking depth for each later peck (0 keeps it constant) |
| Minimum Pecking Depth | Smallest allowed peck |
| Chip Break Distance | Retract between pecks (chip breaking) |
| Accumulated Pecking Depth | Total depth before retracting to the Feed Height to clear chips and let coolant in |
| Dwell Before Retract | Dwell before the peck retract |
| Dwelling Period / Dwelling Depth | Dwell time in seconds; depth below the stock to dwell (not implemented in all cycles or posts) |
| Starting Depth, Positioning Spindle Speed / Feedrate | For positioning inside a pilot hole |
Autodesk describes G81 as common for spot drilling and basic drilling in softer materials where depth is under 3x diameter. As general guidance, aluminum and plastic often need full retract with generous coolant, while stainless often prefers chip breaking.
Tapping#
Tapping needs the spindle speed and feed linked: feed = pitch x rpm (metric). Use the Tapping, Left tapping or Right tapping cycle; the spindle direction is determined by the settings in the tool library.
Note: not confirmed in Autodesk's documentation: rigid versus floating tapping output (M29 or equivalent prefixes) and any "minimum feed per revolution" error; these depend on the post and machine.
Warning: Tapping depth must account for the chamfered lead on the tap (general practice). Drill blind holes deeper than the thread length so the tap does not bottom out.
Step by step: spot, drill, tap#
- Model a part with Hole-command holes: some 6.8 mm tapped M8 x 1.25 blind holes and some 6 mm through holes.
- Create a Setup. Add Drill (operation 1) with a 90-degree spot drill and the Drilling - rapid out cycle. Select the holes by face (use Select Same Diameter), and set the Bottom Height offset so the spot produces a chamfer slightly larger than the hole diameter.
- Add Drill (operation 2) with a 6.8 mm drill for the tapped holes, cycle Deep drilling - full retract, depth to the model hole bottom, with a Pecking Depth of 6 mm.
- Add Drill (operation 3) with a 6 mm drill for through holes; use the Break through option if you want reduced feed at exit.
- Add Drill (operation 4) with an M8 x 1.25 tap, Right tapping cycle, selecting the tapped holes.
- Generate, simulate, and review the posted file for G81/G83/G84 cycles.
Heights for drilling#
The Drill operation uses the same five heights (Clearance, Retract, Feed, Top, Bottom). Autodesk notes that in a drilling operation the Feed Height is used as the initial feed height and the retract peck height, and the canned cycle structure references an R plane (retract height). Whether the post returns to the initial level or the R plane (G98/G99) is post-dependent. Use a larger Retract height when clamps or tall features lie between holes. The Linking tab has a Retraction Policy (Avoid collisions, or Preserve cycles, which keeps the retract height and warns), High Feedrate Mode and Safe Distance.
Options reference#
| Option | What it does | Notes |
|---|---|---|
| Selection Mode | Faces, Points, Diameter range, Remaining holes from operation | Faces preferred |
| Order | Order selected, Optimized, Inside to Outside, X motion, Y motion | Geometry tab |
| Cycle Type | Drilling, counterbore, peck, tapping, boring and so on | Cycle tab |
| Pecking Depth / Reduction / Minimum | Peck control | Chip breaking and deep drilling |
| Break Through Distance / Feedrate / Spindle Speed | Reduce feed and speed before exit | Break through |
| Dwelling Period | Dwell in seconds | Counterbore, boring |
| Shaft and Holder Mode | Trimmed, Detect tool length, Fail on collision, Skip colliding holes | Collision handling |
| Use Shaft and Holder / Shaft Clearance / Holder Clearance | Include shaft and holder in collision checks | |
| Check Machine Spindle / Check Machine Table | Machine collision checks | Needs a machine in the setup |
| Machining Type | 3-axis, Polar, 4-axis, 5-axis | Multi-Axis tab |
| Retraction Policy | Avoid collisions or Preserve cycles | Linking tab |
Milling holes and threads#
When a drill size is unavailable, or you need a precise diameter, use milling operations:
- Bore (2D): helical descent to cut a hole of a selected diameter with a tool smaller than the hole.
- Circular: for circular pockets and bosses, with a similar helical descent.
- Thread: thread milling with a thread mill; internal and external, right or left hand. The tool must be a thread mill in the library.
- The Drill operation itself also offers Circular pocket milling, Bore milling and Thread milling cycle types with options such as Cycle Diameter, Pitch, Incremental Depth, Stepover, Repeat Pass and Radial Stock to Leave.
Thread milling gives size control, works with any pitch within the cutter's range, and suits hard materials, at the cost of cycle time and a more complex tool (general guidance).
Tips and pitfalls#
Tip: A shallow spot drill pass improves accuracy of the following drill and prevents walk on curved or angled surfaces.
Tip: Group holes by tool and use a single Drill operation for all holes of the same diameter, which gives one tool change and compact code.
Tip: For holes on non-planar tilted faces, create a separate Setup with the WCS Z along the hole axis (or use the Drill operation's Multi-Axis tab with 4-axis or 5-axis machining type) rather than forcing a 3-axis Drill.
Warning: Drill depth is measured to the drill tip unless the operation says otherwise. A hole depth of 10 mm with the full diameter reaching only to 9 mm because of the cone is a normal consequence of a 118-degree tip. Use simulation to check the depth.
Warning: Through-hole break-through into a vise jaw, table, or fixture plate can be catastrophic. Check the exit side in Simulate with the fixture shown.
Warning: Tapping holes with no pilot check: if the drill size in the model does not match the actual tap drill size, the tapped thread class changes. Use the tap drill size from the Hole command.
Warning: Canned cycle availability and numbers depend entirely on your post. If a cycle does not appear in your code, your post may be expanding it, or it may not support it; Autodesk notes that dwell, for example, is output as G4 when cycles are expanded.
Practice exercise#
Create a 80 x 50 x 15 mm plate. Using the Hole command in Design, add four M6 x 1.0 tapped blind holes (12 mm thread depth) near the corners and one 10 mm through hole in the center.
In Manufacture, create operations: a spot drill on all holes, a 5 mm drill (tap drill) on the M6 holes with peck depth 5 mm, a 10 mm drill on the center hole using a 6 mm pilot first if you want, and an M6 tap with the Right tapping cycle.
Generate and post to a generic Fanuc-style post. Expected result (Fanuc-style post): the code contains G81 (spot), G83 (pecking), G81 (through), and G84 (tapping) cycle calls, with hole positions listed once under each cycle, and the tap feed equal to 1.0 mm times the spindle speed.
Related#
- Tools and tool libraries (drill, tap and spot drill tools)
- Feeds and speeds (feed per revolution for drilling)
- Post processing (canned cycle output and rigid tapping)
- Hole and thread (Solid modeling section)