Hole¶

In one sentence: Cut a standards-aware cylindrical hole into a Body, with built-in support for threads, countersinks, counterbores, and drill-point geometry in one unified tool.

Overview¶

Workbench: Part Design · Menu: Part Design → Subtractive Features → Hole
Toolbar: Part Design Modeling Features · Shortcut: none

Hole is Part Design's most feature-rich subtractive operation. Given a sketch containing one or more circles (or points), it drills matching holes into the Body — optionally with threads, a countersink or counterbore recess for a screw head, a drill-point cone at the bottom, or a taper along the wall. All thread geometry follows published fastener standards (ISO metric, UNC, UNF, UNEF, BSW, BSP, NPT, and others), so you never need to look up tap-drill diameters or counterbore dimensions manually.

Intuition¶

Think of the Hole tool as a CNC drilling and tapping cycle packed into a single dialog. A machinist drilling a hole for an M6 socket-head cap screw must choose: the tap-drill diameter (5 mm), the counterbore diameter for the screw head, the counterbore depth, and the thread depth. The Hole tool automates all of those choices the moment you pick ISOMetricProfile and M6x1.0 — the rest of the fields fill in with ISO-standard values that you can override.

The sketch driving the hole carries the position of each hole centre. The Hole task panel carries every other dimension. One hole feature can produce dozens of identical holes simultaneously: FreeCAD finds every circle (or point) in the sketch and cuts a hole at each one.

A subtlety that confuses new users: the hole depth and the thread depth are controlled separately. You can have a 20 mm deep hole with only 15 mm of thread, which is the normal engineering practice (partial-thread blind hole). The Thread Depth Type dropdown controls this relationship — setting it to Hole Depth makes the thread run the full depth; Dimension lets you set an independent thread depth; Tapped (DIN76) adds a DIN 76 thread run-out allowance automatically.

When to use it¶

You need a bolt or screw to thread into the part, and you want the correct tap-drill diameter and thread class selected according to an industry standard.
You are preparing a clearance hole for a fastener to pass through, and you want a correctly sized counterbore or countersink for the screw head.
You need several identical holes placed at multiple positions defined by a sketch (one Hole feature can create all of them at once).
You want the 3-D model to show an accurate helical thread form for technical presentation or FEA (enable Modeled thread).
You need a non-standard simple cylindrical blind or through hole of a given diameter — the tool works without any thread standard selected.

When NOT to use it¶

The opening is not a circular hole — use Pocket for rectangular, slotted, or other non-circular cutouts.
You need a rotationally tapered pipe thread (NPT or BSP taper) — the Hole tool can size the hole for those standards, but does not generate a tapered bore geometry; model the taper manually with Revolution or a tapered Pocket.
You need a partial-sphere or non-cylindrical recessed seat — use a Pocket with the appropriate sketch profile instead.
The hole axis is not perpendicular to a planar face — Hole always drills perpendicular to the attachment plane of its sketch. For angled holes, tilt the datum plane and attach the sketch to that.

Step-by-step walkthrough¶

Prerequisites: An active Body with at least one solid feature (e.g. a Pad or an Additive Box) and a face to drill into.

Create the position sketch. Select a planar face of the Body, then open Sketch → New Sketch. Draw one circle for each hole position. The circle's radius is ignored by the Hole tool (the task panel controls diameter), but placing a circle rather than a point allows the Hole tool to read the sketch by default. Fully constrain all centres. Close the Sketcher.

Tip

If you prefer to mark hole centres with sketch points instead of circles, set Base profile types to Points, circles and arcs or Points in the task panel after activating the Hole tool.
Activate the Hole tool. Open Part Design → Subtractive Features → Hole, or click the Hole icon in the toolbar. The Hole Parameters task panel opens.
Choose a thread standard. In the Standard dropdown, select the fastener family: None for a plain dimensioned hole, or one of the thread standards (e.g. ISO metric regular). When a standard is selected the Size and Head type rows become active.
Select the size. Pick the nominal designation in the Size dropdown (e.g. M6x1.0). FreeCAD sets the tap-drill diameter and thread pitch automatically.
Set the head type. In Head type choose None, Counterbore, Countersink, or Counterdrill. For a standard screw type (e.g. ISO 4762 socket-head cap screw) FreeCAD fills the counterbore or countersink dimensions from the norm. Tick Custom head values to override those dimensions.
Set the depth type and depth. In Depth type choose Dimension for a blind hole or Through all for a through-hole. If Dimension is selected, enter the hole depth in the Depth field.
Configure the drill point. Tick Drill angle to add a conical drill- point at the bottom (typical for twist-drilled blind holes). Enter the included angle in Drill angle (118° is the standard for high-speed-steel twist drills). Tick Include in depth if the drill-point cone should be counted as part of the nominal hole depth.
Set the Threading section (visible when a thread standard is selected).

a. In Hole type, choose Clearance / Passthrough for a non-threaded clearance hole, Tap drill (to be threaded) for a tapped hole without modelled thread geometry, or Modeled thread to generate a real 3-D helix.

b. If threaded, choose Thread Depth Type: Hole depth (thread fills the hole), Dimension (enter an explicit depth), or Tapped (DIN76) (DIN 76 runout allowance is added automatically).

c. Select Class (tolerance class, e.g. 6H for ISO metric).

d. Select Direction: Right hand or Left hand.

e. For modeled threads, optionally tick Custom Clearance and enter a clearance offset to adjust thread fit for manufacturing tolerance.
Optionally enable Tapered. Tick Tapered and enter an angle in Tapered angle to produce a conical hole wall. 90° means a straight (non-tapered) hole, below 90° the hole narrows toward the bottom.
Click OK. FreeCAD cuts a hole at every circle (or point) in the sketch and fuses the result into the Body. The model tree shows a single Hole feature regardless of how many holes were created.

Tip

For a standard M6 tapped blind hole to accept a socket-head cap screw (ISO 4762), select ISO metric regular, size M6x1.0, head type Counterbore, hole type Tap drill (to be threaded), depth type Dimension, depth 15 mm, drill angle ticked at 118°. All counterbore dimensions are filled automatically from ISO 4762.

Parameters¶

The task panel is organised into logical groups, documented below in the order they appear in the UI.

Profile and geometry¶

Parameter	Type	Default	Description
Base profile types	Dropdown	`Circles and arcs`	Which sketch elements define hole centres. `Circles and arcs`: circles and arcs only. `Points, circles and arcs`: centres of all three. `Points`: sketch points only. Corresponds to `BaseProfileType` bitmask property.
Standard	Dropdown	`None`	Thread standard. `None`: plain dimensioned hole. Other values: `ISO metric regular` (ISOMetricProfile), `ISO metric fine` (ISOMetricFineProfile), `UTS coarse` (UNC), `UTS fine` (UNF), `UTS extra fine` (UNEF), `ANSI pipes` (NPT), `ISO/BSP pipes` (BSP), `BSW whitworth` (BSW), `BSF whitworth fine` (BSF), `ISO tyre valves` (ISOTyre).
Size	Dropdown	(first entry for selected standard)	Nominal thread designation (e.g. `M6x1.0`, `#10`, `1/4`). Available options depend on the selected standard. Sets `ThreadSize`.
Head type	Dropdown	`None`	Cut type for the screw-head recess: `None` / `Counterbore` / `Countersink` / `Counterdrill`. See deep dive below.
Depth type	Dropdown	`Dimension`	Controls how hole depth is determined. `Dimension`: use the explicit Depth value. `Through all`: hole penetrates the entire Body. Sets `DepthType`.

Head type in depth¶

The Head type dropdown determines whether the surface has a recessed seat for the fastener head, and what shape that seat is. Choosing the wrong type means the fastener either won't sit flush or the modelled geometry won't match manufacturing.

None (default)¶

A plain cylindrical hole with no enlargement at the entry. The fastener's head sits on top of the surface.

Use this mode when: - Standard hex bolts, nuts, or washers bear on the surface (no recess needed) - Locating pins, dowels, or through-holes where head geometry is not relevant - The screw head protrudes above the surface and that is acceptable

Watch out for: Nothing — None is the correct choice for most through-holes. Choose a recess type only when the fastener head must sit flush or below the surface.

Counterbore¶

A flat-bottomed cylindrical recess is cut at the entry. The screw head (socket cap, button head, or any flat-topped head) drops into the cylinder and its top face sits at or below the surrounding surface.

Use this mode when: - Socket head cap screws or button head screws must be flush or recessed below the surface (common in machine design and enclosures) - A bearing face of specific depth and diameter is required for a fastener or insert

Sub-parameters unlocked:

Sub-parameter	Notes
Head diameter	Outer diameter of the cylindrical recess. Must be larger than the hole bore diameter.
Head depth	Depth of the flat-bottomed recess (how far down the head sits).
Custom head values	Tick to override standard-derived dimensions. Leave off to use ISO/ANSI values.

Watch out for: When Standard is set to a normed value, head dimensions are read from the standard and the fields are read-only. Tick Custom head values only if the standard dimensions don't match your fastener.

Countersink¶

A conical recess is cut at the entry. Flat-head or oval-head screws seat in the cone so their top face is flush with the surrounding surface.

Use this mode when: - Flat-head machine screws must sit flush with the surface (panel hardware, sheet-metal assemblies, cosmetic fastening) - The screw standard specifies a conical seat (most metric flat-head screws use a 90° included angle; many imperial flat-head screws use 82°)

Sub-parameters unlocked:

Sub-parameter	Notes
Head diameter	Outer diameter of the cone at the surface.
Head depth	Distance from the surface to the cone apex (or to the bore entry).
Countersink angle	Included angle of the cone. Must match the screw head angle exactly.
Custom head values	Tick to override standard-derived dimensions.

Watch out for: The countersink angle must match the screw head angle. A 90° hole with an 82° screw (or vice versa) makes contact only at the cone edge or the cone tip — not on the full bearing face. Always confirm the angle from the fastener's data sheet.

Counterdrill¶

A short cylindrical entry is combined with a conical countersink below it. Some ISO standards (e.g. DIN 74) specify this two-step entry geometry.

Use this mode when: - A specific drawing standard explicitly calls for a counterdrill profile - Machining practice requires a cylindrical pilot before the conical face begins

Sub-parameters unlocked:

Sub-parameter	Notes
Head diameter	Outer diameter of the cylindrical pilot.
Head depth	Depth of the cylindrical pilot portion (above where the cone begins).
Countersink angle	Included angle of the cone below the cylindrical pilot.
Custom head values	Tick to override standard-derived dimensions.

Watch out for: Counterdrill is uncommon in general design work. Choose it only if a specific standard or machining procedure requires this geometry — for everything else use Counterbore or Countersink.

Hole cut / head dimensions¶

Visible when Head type is not None.

Parameter	Type	Default	Description
Custom head values	Checkbox	off	When ticked, enables manual editing of Head diameter and Head depth (and Countersink angle for countersink types). When unticked with a normed screw type selected, the fields show norm values and are read-only. Sets `HoleCutCustomValues`.
Head diameter	Length	(from norm)	Outer diameter of the counterbore or countersink. Must be larger than the hole diameter. Sets `HoleCutDiameter`.
Head depth	Length	(from norm)	For counterbore: depth of the flat-bottomed recess. For countersink: depth of the screw top below the surface. For counterdrill: depth of the cylindrical entry before the conical section. Sets `HoleCutDepth`.
Countersink angle	Angle	`90°`	Included angle of the countersink cone. Only active for `Countersink` and `Counterdrill` types. Sets `HoleCutCountersinkAngle`. Range: near 0° to near 180°.

Drill point¶

Parameter	Type	Default	Description
Drill angle	Checkbox	off	When ticked, adds a conical drill-point tip at the bottom of blind holes, as produced by a standard twist drill. Sets `DrillPoint` to `Angled`.
Drill angle value	Angle	`118°`	Included angle of the drill-point cone. 118° is standard for HSS twist drills; 135° is common for carbide. Sets `DrillPointAngle`. Active only when `Drill angle` is ticked.
Include in depth	Checkbox	off	When ticked, the drill-point cone geometry is included within the nominal hole depth (the full-diameter portion is shortened). When unticked, the depth value specifies the cylindrical portion and the cone adds extra depth beyond it. Sets `DrillForDepth`.

Depth and taper¶

Parameter	Type	Default	Description
Depth	Length	`25 mm`	Hole depth when Depth type is `Dimension`. Not active for `Through all`. Sets `Depth`.
Switch direction	Checkbox	off	Reverses the drill direction (hole goes the opposite way through the solid). Sets `Reversed`.
Tapered	Checkbox	off	Enables a conical wall angle on the hole. Sets `Tapered`.
Tapered angle	Angle	`90°`	Half-included wall angle. `90°` = straight hole. Less than 90°: hole narrows toward the bottom (taper inward). Greater than 90°: hole widens toward the bottom (taper outward). Sets `TaperedAngle`. Active only when `Tapered` is ticked.

Threading section¶

Visible when Standard is not None.

Parameter	Type	Default	Description
Hole type	Dropdown	`Clearance / Passthrough`	The fundamental purpose of the hole relative to threading. See deep dive below.
Clearance	Dropdown	`Medium` (ISO) / `Normal` (UTS)	Clearance class for passthrough holes. ISO: `Fine`, `Medium`, `Coarse` (ISO 273). UTS: `Close`, `Normal`, `Loose` (ASME B18.2.8). Active only when Hole type is `Clearance / Passthrough`.
Update thread view	Checkbox	off	When `Modeled thread` is active, recomputes the thread helix in real time. Untick during editing to avoid slow recomputes.
Class	Dropdown	(standard dependent)	Thread tolerance class. ISO metric: `6H` common. UNC/UNF: `2B` common. Active when threaded.
Direction	Radio	`Right hand`	Thread hand: `Right hand` (standard) or `Left hand`.
Thread Depth Type	Dropdown	`Hole depth`	How thread depth is calculated. See deep dive below.
Thread Depth	Length	`23.5 mm`	Explicit thread length. Active only when `Thread Depth Type` is `Dimension`.
Custom Clearance	Checkbox + Length	off / `0 mm`	Override `ThreadClass` clearance manually. Active only when `Modeled thread` is selected.

Hole type in depth¶

The Hole type dropdown — visible only when Standard is set to anything other than None — is the single most consequential threading decision. It controls whether the hole is a clearance fit, a tap-drill pilot, or a fully modelled helical thread.

Clearance / Passthrough (default)¶

The bore diameter is set to let the screw shank pass through freely, with no thread. The diameter is determined by the Clearance class from the selected standard. A nut or threaded receiver on the other side provides the clamping force.

Intuition: the bolt drops through the first part like a key through a keyhole — the hole in this part is just a passage. The thread engagement is elsewhere.

Use this mode when: - A bolt passes through one part and threads into a nut or a tapped hole in another part (the standard bolted joint) - A flange, bracket, or cover plate that is clamped but not threaded

Sub-parameters unlocked:

Sub-parameter	Notes
Clearance	`Fine` = snug fit (positional accuracy). `Medium` = normal assembly. `Coarse` = easy assembly with potential misalignment.

Watch out for: Clearance class affects the bore diameter. Fine is smaller (tighter fit for location), Coarse is larger (easier assembly). For parts that need to be positionally accurate, use Fine; for ordinary bolted connections, Medium is sufficient.

Tap drill (to be threaded)¶

The bore diameter is set to the tap-drill size for the selected thread standard — the size you would drill before cutting the thread with a tap. No 3-D thread geometry appears in the model. This is the correct choice for the vast majority of tapped holes in production designs.

Intuition: the number you see is what you tell the machinist to drill before tapping. FreeCAD looks it up from the thread standard for you.

Use this mode when: - The hole will be tapped in manufacturing (CNC or hand tap) - Thread geometry in the model is not needed for visual clarity or FEA - Working with any standard thread: ISO metric, UNC/UNF, BSW, pipe

Sub-parameters unlocked:

Sub-parameter	Notes
Class	Thread tolerance class (fit). `6H` is the standard ISO metric class for general engineering; `4H` is tight, `7H` is loose.
Thread Depth Type	See Thread Depth Type deep dive below.

Watch out for: The diameter shown is the tap drill diameter — not the thread nominal diameter and not the minor diameter. This is the correct value to put on a manufacturing drawing. Do not use the nominal diameter as the drill size or the thread will cut air.

Modeled thread¶

A real 3-D helical thread form is swept into the hole, producing full visible thread geometry in the model. This is generated by sweeping the thread profile along a helix of the correct pitch.

Intuition: you can see individual thread turns, zoom in and count them, and the geometry is accurate to the selected thread standard.

Use this mode when: - Technical illustrations or exploded views must show the thread clearly - FEA analysis needs to model actual thread contact and stress concentration - Exporting to downstream software (e.g. rendering tools) that expects real thread geometry

Sub-parameters unlocked:

Sub-parameter	Notes
Update thread view	Leave off during parameter editing to avoid recomputing after every keystroke. Tick to update the view for a final check.
Custom Clearance	Fine-tune the effective fit of the modelled thread with a positive (looser) or negative (tighter) offset.

Watch out for: Modelled thread is very slow for fine threads in deep holes (many hundreds of helical faces). For a 1.0 mm pitch thread 30 mm deep, expect 30 full turns and significant recompute time. Use Tap drill for production documentation and switch to Modeled thread only when the geometry is genuinely needed.

Thread Depth Type in depth¶

Thread Depth Type is only visible when Hole type is Tap drill or Modeled thread. It controls how far down the hole the thread extends.

Hole depth (default)¶

The thread extends through the entire hole depth. Thread depth equals hole depth.

Use this mode when: - The full hole is tapped (the most common case for short blind holes) - Simplicity is preferred over specifying an explicit thread engagement length

Watch out for: For deep holes with only a few turns of engagement needed, threading the full depth wastes machining time and adds geometric complexity in Modeled thread mode. Use Dimension to limit it.

Dimension¶

An explicit thread depth is entered, independent of the hole depth. The thread ends at that depth; the remaining hole below is unthreaded (clearance bore or chip relief space).

Use this mode when: - Only a defined engagement length is needed — typically 1.0 to 1.5 × nominal diameter for standard steel-into-steel joints - The hole is deliberately deeper than the thread (chip relief for a tap, or a bottoming tap requires clearance) - Thread depth is a specified dimension on an engineering drawing

Watch out for: Thread Depth must not exceed Hole Depth — FreeCAD will error if you try to thread deeper than the hole.

Tapped (DIN 76)¶

Thread depth is calculated per DIN 76, which adds a thread run-out zone (incomplete thread turns at the bottom of the blind hole, as produced by a standard taper tap). The usable thread engagement length is the value you enter; the total hole depth must accommodate the run-out in addition.

Use this mode when: - The drawing must conform to DIN 76 (common in German and European manufacturing) - The hole geometry must explicitly represent the run-out zone for clearance of the male thread's chamfered end

Watch out for: The physical hole is deeper than the Thread Depth value by the DIN 76 run-out amount. This extra depth must be available — verify the feature does not break through a thin wall.

Advanced usage¶

Creating many holes in one operation¶

Place all hole centre circles (or points) in a single sketch and run the Hole tool once. FreeCAD processes every circle or point in the profile and creates all holes simultaneously. This is significantly faster to model and easier to update parametrically than separate Pocket operations.

For a bolt-circle pattern, use the Sketcher's circular-pattern constraint to place the centres, then apply Hole once. Changing the number of instances or the pitch-circle diameter updates all holes.

Modeled threads for FEA and presentation¶

Enable Modeled thread when you need a real helical thread form in the geometry — for example, for FEA meshing or technical documentation renders. Note that computing the helical geometry is slow for deep holes; untick Update thread view while adjusting parameters and retick only to see the final result.

The clearance between the modeled thread crest and the surrounding material can be adjusted per class (via ThreadClass) or overridden exactly with CustomThreadClearance. A value of 0 mm gives nominal geometry; a small positive clearance simulates a real-world fit.

Mixing head types with standard sizes¶

Selecting a screw standard automatically looks up the correct counterbore or countersink geometry for that size from the embedded ISO 4762 (socket-head cap screws) and ISO 10642 (flat-head screws) tables. If no norm entry exists for a given size, FreeCAD computes a geometric approximation and forces Custom head values to true so you can inspect and adjust the result.

To use a non-standard head size (e.g. a flanged hex bolt that does not appear in the presets), select the nearest thread standard for the tap diameter, then tick Custom head values and enter the required head diameter and depth.

Tapered holes¶

The Tapered option produces a conical bore wall, which is useful for press-fit pins, draft angles on moulded features, or matching a conical seat. The angle is defined relative to the bore axis: 90° gives a straight cylinder, less than 90° gives a truncated cone that narrows toward the bottom.

Tapered holes can be combined with all other options (countersink, drill point, thread type) but the combination of a taper with Modeled thread is unusual and the resulting geometry should be checked carefully.

Common mistakes and pitfalls¶

Hole feature fails with 'No profile selected'

Cause: The sketch driving the Hole was not set as the Profile property, or the sketch contains no circles or points (and the default Circles and arcs profile mode found nothing to work with).
Fix: Select the Hole in the model tree and check that Profile points to the correct sketch. If the sketch uses only points, change Base profile types to Points, circles and arcs or Points.

All holes are drilled at the wrong depth or diameter

Cause: When ThreadType is not None, the Diameter field is driven by the selected thread size and is read-only. Setting it manually when the type is None and then switching to a standard silently overrides the value.
Fix: Set the thread standard first, then adjust size. If you need an exact non-standard diameter, keep ThreadType as None and enter the diameter directly.

Countersink/counterbore dimensions reset when size is changed

Cause: Changing Size resets HoleCutCustomValues to false and reloads the norm values from the embedded lookup table.
Fix: Make all custom head-dimension edits after locking in the size selection, then tick Custom head values.

Modeled thread is extremely slow to compute

Cause: Generating a real helical thread solid is OCCT-intensive and scales with thread depth. Long holes or very fine pitches can take tens of seconds.
Fix: Leave Update thread view unticked until you are satisfied with all other parameters, then tick it once to get the final geometry.

Hole does not appear even though the sketch is correct

Cause: The sketch is attached to a face but the hole direction points away from the solid (outside the material). This can happen if the sketch plane normal faces away from the Body.
Fix: Tick Switch direction in the task panel to reverse the drill direction, or flip the sketch's MapReversed property.

Python API¶

Minimal example¶

import FreeCAD as App
import Part
import Sketcher

# TODO: verify — tested against TestHole.py patterns in the FreeCAD source tree

doc = App.newDocument()

# Create a body and a base solid (10 × 10 × 10 mm box)
body = doc.addObject("PartDesign::Body", "Body")
box = doc.addObject("PartDesign::AdditiveBox", "Box")
box.Length = 10
box.Width = 10
box.Height = 10
body.addObject(box)
doc.recompute()

# Sketch on the top face (XY plane, reversed so normal points down into the solid)
sketch = doc.addObject("Sketcher::SketchObject", "HoleSketch")
sketch.AttachmentSupport = (doc.XY_Plane, [""])
sketch.MapMode = "FlatFace"
sketch.MapReversed = True
body.addObject(sketch)

# Add a circle at (-5, 5) — radius value is ignored by the Hole tool
sketch.addGeometry(
    Part.Circle(App.Vector(-5, 5, 0), App.Vector(0, 0, 1), 1), False
)
doc.recompute()

# Create the Hole feature
hole = doc.addObject("PartDesign::Hole", "Hole")
hole.Profile = sketch
body.addObject(hole)

# Plain 6 mm blind hole, 8 mm deep, flat drill point
hole.ThreadType = 0          # None — no thread standard
hole.Diameter = 6.0          # mm
hole.DepthType = 0           # 0 = Dimension, 1 = ThroughAll
hole.Depth = 8.0             # mm
hole.HoleCutType = 0         # 0 = None, 1 = Counterbore, 2 = Countersink, 3 = Counterdrill
hole.DrillPoint = 0          # 0 = Flat, 1 = Angled
hole.Tapered = False

doc.recompute()
print(f"Hole volume removed: {10**3 - hole.Shape.Volume:.4f} mm³")

Setting up an M6 tapped hole¶

# Continuing from the minimal example above (hole object already exists)

hole.ThreadType = 1          # ISOMetricProfile
hole.ThreadSize = 14         # M6x1.0 — index in the ISOMetricProfile list
hole.Threaded = True         # tap drill / threaded
hole.ModelThread = False     # no helical geometry (faster)
hole.ThreadClass = 5         # 6H  (index 5 in ThreadClass_ISOmetric_Enums)
hole.ThreadDirection = 0     # Right hand
hole.HoleCutType = 1         # Counterbore
hole.DepthType = 0           # Dimension
hole.Depth = 15.0
hole.DrillPoint = 1          # Angled
hole.DrillPointAngle = 118.0
hole.DrillForDepth = False
hole.ThreadDepthType = 0     # Hole depth (thread fills full depth)

doc.recompute()

Feature properties¶

Property	Type	Default	Description
`Profile`	`App::PropertyLinkSub`	—	The driving sketch containing circles or points.
`BaseProfileType`	`App::PropertyInteger`	`6` (OnCirclesArcs)	Bitmask: `1` = OnPoints, `2` = OnCircles, `4` = OnArcs.
`ThreadType`	`App::PropertyEnumeration`	`"None"`	Thread standard. Enum values: `"None"`, `"ISOMetricProfile"`, `"ISOMetricFineProfile"`, `"UNC"`, `"UNF"`, `"UNEF"`, `"NPT"`, `"BSP"`, `"BSW"`, `"BSF"`, `"ISOTyre"`.
`ThreadSize`	`App::PropertyEnumeration`	`"---"`	Nominal designation within the selected standard (e.g. `"M6x1.0"`). Enum list resets when `ThreadType` changes.
`Threaded`	`App::PropertyBool`	`False`	`True` if the hole is tapped (sets diameter to tap-drill size).
`ModelThread`	`App::PropertyBool`	`False`	`True` to generate a real helical thread solid.
`ThreadClass`	`App::PropertyEnumeration`	`"None"`	Tolerance class. Options depend on `ThreadType`.
`ThreadFit`	`App::PropertyEnumeration`	`"Medium"`	Clearance fit for passthrough holes. Options depend on `ThreadType`.
`ThreadDirection`	`App::PropertyEnumeration`	`"Right"`	`"Right"` or `"Left"`.
`ThreadDepthType`	`App::PropertyEnumeration`	`"Hole Depth"`	`"Hole Depth"`, `"Dimension"`, or `"Tapped (DIN76)"`.
`ThreadDepth`	`App::PropertyLength`	`23.5 mm`	Explicit thread depth used when `ThreadDepthType` is `"Dimension"`.
`ThreadPitch`	`App::PropertyLength`	(from standard)	Thread pitch; set automatically from the selected size.
`ThreadDiameter`	`App::PropertyLength`	`0 mm`	Read-only. Thread major diameter as derived from the selected standard and size.
`UseCustomThreadClearance`	`App::PropertyBool`	`False`	Override thread clearance with `CustomThreadClearance`.
`CustomThreadClearance`	`App::PropertyLength`	`0 mm`	Manual clearance offset. Active only when `UseCustomThreadClearance` is `True`.
`Diameter`	`App::PropertyLength`	`6 mm`	Hole diameter. Manually editable only when `ThreadType` is `"None"`; otherwise set by the standard.
`HoleCutType`	`App::PropertyEnumeration`	`"None"`	`"None"`, `"Counterbore"`, `"Countersink"`, `"Counterdrill"`.
`HoleCutCustomValues`	`App::PropertyBool`	`False`	Enable manual override of head dimensions.
`HoleCutDiameter`	`App::PropertyLength`	`0 mm`	Outer diameter of the head recess.
`HoleCutDepth`	`App::PropertyLength`	`0 mm`	Depth of the head recess.
`HoleCutCountersinkAngle`	`App::PropertyAngle`	`90°`	Included angle of the countersink or counterdrill cone.
`DepthType`	`App::PropertyEnumeration`	`"Dimension"`	`"Dimension"` or `"ThroughAll"`.
`Depth`	`App::PropertyLength`	`25 mm`	Hole depth when `DepthType` is `"Dimension"`.
`DrillPoint`	`App::PropertyEnumeration`	`"Angled"`	`"Flat"` or `"Angled"`.
`DrillPointAngle`	`App::PropertyAngle`	`118°`	Included angle of the drill-point cone. Active when `DrillPoint` is `"Angled"`.
`DrillForDepth`	`App::PropertyBool`	`False`	Include the drill-point cone within the nominal `Depth`.
`Tapered`	`App::PropertyBool`	`False`	Enable a conical wall angle.
`TaperedAngle`	`App::PropertyAngle`	`90°`	Wall cone half-angle. `90°` = straight; `< 90°` = narrows; `> 90°` = widens.

Hole¶

Overview¶

Intuition¶

When to use it¶

When NOT to use it¶

Step-by-step walkthrough¶

Parameters¶

Profile and geometry¶

Head type in depth¶

None (default)¶

Counterbore¶

Countersink¶

Counterdrill¶

Hole cut / head dimensions¶

Drill point¶

Depth and taper¶

Threading section¶

Hole type in depth¶

Clearance / Passthrough (default)¶

Tap drill (to be threaded)¶

Modeled thread¶

Thread Depth Type in depth¶

Hole depth (default)¶

Dimension¶

Tapped (DIN 76)¶

Advanced usage¶

Creating many holes in one operation¶

Modeled threads for FEA and presentation¶

Mixing head types with standard sizes¶

Tapered holes¶

Common mistakes and pitfalls¶

Python API¶

Minimal example¶

Setting up an M6 tapped hole¶

Feature properties¶

See also¶