CAM ThreadMilling

CAM ThreadMilling CAM ThreadMilling

Menu location

CAM  Thread Milling

Workbenches

CAM

Default shortcut

None

Introduced in version

1.1

See also

CAM Drilling

Description

The CAM Thread Milling command creates an Operation that mills internal or external threads in circular holes or on cylindrical bosses with a thread-milling cutter. The command tooltip reads "Creates a Thread Milling toolpath from features of a base object".

The Toolpath is a helical G2/G3 move at the thread pitch, repeated for the number of passes; the radial depth of each pass is computed so that every pass removes the same area. The Tool Controller must use a Tool Bit with the thread-mill Tool Shape (properties Diameter and Crest; the shipped 5mm-thread-cutter is an example). Base Geometry is selected like in CAM Drilling (circular faces, edges or vertexes, with Auto-select).

1.1 and earlier: only available when Enable experimental features is checked in the CAM preferences. 26.3 and later: available by default.

Usage

  1. Optionally select hole faces or edges on the Model.

  2. Press the CAM ThreadMilling Thread Milling button in the Drilling Operations group of the New Operations toolbar, or select CAM  Thread Milling from the menu.

  3. In the Base Geometry section add or Auto-select the holes; use Sorting to order them.

  4. In the Heights section set Clearance, Retract, Start and Final.

  5. In the Tool Controller section pick a Tool Controller with a thread-mill Tool Bit; the error "This operation requires a tool controller with a threadmilling tool" is shown otherwise.

  6. In the Operation section choose Orientation, Type, the thread name (standard threads) or enter Major diameter, Minor diameter and Pitch or TPI (custom threads), and adjust Fit, Passes, Direction and Lead in/out.

  7. Press OK.

Options

Thread group

  • Orientation: LeftHand or RightHand.

  • Type: see the Thread Type property values below.

  • Thread name combo box, filled from the data tables shipped with the workbench (metric-internal-6H, metric-external-6G, metric-external-4G6G, imperial-internal-2B, imperial-internal-3B, imperial-external-2A, imperial-external-3A).

  • Fit: slider 0–100.

  • Major diameter, Minor diameter, Pitch, TPI.

  • For Custom types the name and Fit are disabled and the diameters, Pitch and TPI are entered directly. For metric standards Pitch is filled and TPI disabled; for imperial standards TPI is filled and Pitch disabled; the diameters are interpolated between the standard’s minimum and maximum according to Fit.

Operation group

  • Passes: number of passes used to cut the thread.

  • Direction: Climb or Conventional.

  • Lead in/out: add lead-in and lead-out arcs.

Properties

Thread

  • Thread Orientation: Set thread orientation. LeftHand or RightHand (default).

  • Thread Type: Custom External, Custom Internal, Imperial External (2A), Imperial External (3A), Imperial Internal (2B), Imperial Internal (3B), Metric External (4G6G), Metric External (6G), Metric Internal (6H) (default). (The source tooltip still reads "Currently only internal", which is stale; external types are implemented.)

  • Thread Name: Defines which standard thread was chosen.

  • Major Diameter: Set thread’s major diameter.

  • Minor Diameter: Set thread’s minor diameter.

  • Pitch: Set thread’s pitch - used for metric threads. Default: 1 mm.

  • TPI: Set thread’s TPI (turns per inch) - used for imperial threads. Default: 0; when greater than 0 it overrides Pitch.

  • Thread Fit: Override to control how loose or tight the threads are milled (0–100). Default: 50.

Operation

  • Passes: Set how many passes are used to cut the thread. Default: 1.

  • Direction: Direction of thread cutting operation, Climb (default) or Conventional.

  • Lead In Out: Set to True to get lead in and lead out arcs at the start and end of the thread cut. Default: false.

  • Clearance Op: Operation to clear the inside of the thread (link to another operation; defined but currently unused by the operation).

Base

  • Disabled: List of disabled features (holes unchecked in the Base Geometry table).

Sorting

introduced in 26.3

  • Sorting Mode: Automatic or Manual.

  • Start Point, Use End Point, End Point: points for automatic sorting; hidden when Sorting Mode is Manual.

Depth

  • Clearance Height, Safe Height, Start Depth, Final Depth.

Linking

introduced in 26.3

  • Collision Avoidance Strategy, Collision Clearance: inherited from the circular-hole base; the thread milling Toolpath retracts to Clearance Height between holes.

Path

  • Active, Base, Comment, Coolant Mode, Cycle Time, Tool Controller, User Label, Workplane.

introduced in 26.3: The Workplane property links the Operation to a named Work Plane that the Job holds.

Op Values

  • Op Final Depth, Op Start Depth, Op Stock ZMax, Op Stock ZMin, Op Tool Diameter. All read-only.

Notes

  • The radii of the passes are derived from the major and minor diameters and the Tool Bit diameter; the cutter Crest is compensated (introduced in 26.3: crest handling fixed).

  • Internal threads are milled from the inside out, external threads from the outside in. Between passes the tool retracts to Clearance Height.

  • If the Tool Bit is larger than the minor diameter an error is reported.

Scripting

See also: FreeCAD Scripting Basics.

Example:

import FreeCAD
import Path.Op.ThreadMilling as PathThreadMilling

job = FreeCAD.ActiveDocument.getObject('Job')
op = PathThreadMilling.Create('ThreadMilling', parentJob=job)
op.Proxy.findAllHoles(op)
op.ThreadType = 'MetricInternal6H'
op.ThreadName = 'M8 x 1.25'
op.MajorDiameter = 8.0
op.MinorDiameter = 6.647
op.Pitch = 1.25
op.Passes = 2
FreeCAD.ActiveDocument.recompute()

Note: in scripting the enumeration data values are the identifiers without spaces or parentheses: MetricInternal6H, ImperialInternal2B, CustomInternal, and so on.