CAM Mill Facing

CAM Mill Facing CAM Mill Facing

Menu location

CAM  Mill Facing

Workbenches

CAM

Default shortcut

None

Introduced in version

26.3

See also

CAM MillFace

Description

The CAM Face CAM Mill Facing command creates an operation that machines the top surface of the Stock down to the Final Depth with a rectangular clearing pattern. introduced in 26.3: It replaces the Face operation. The boundary is taken from the Stock cross-section at the Final Depth, so no Base Geometry selection is needed; the Stock may be rectangular or cylindrical (curved outlines are converted to the enclosing rectangle aligned to Angle).

The command’s menu text is "Mill Facing" and its tooltip reads "Create a Mill Facing Operation to machine the top surface of stock".

Usage

  1. The Job must have a Stock object; the operation uses its outline.

  2. Press the Mill Facing button on the New Operations toolbar or select CAM  Mill Facing.

  3. On the Heights tab set Start depth (top of Stock), Final depth (target surface), Step down and the Linking options.

  4. On the Tool Controller tab choose the Tool Controller and coolant mode.

  5. On the Operation tab choose Clearing Pattern, Cut Mode, Angle, Reverse, Step over, Pass Extension, Stock Extension and Axial stock to leave.

  6. Press Apply to preview, OK to accept.

Clearing patterns

  • ZigZag: continuous back-and-forth passes, alternating direction, linked at the ends.

  • Bidirectional: passes alternate between the two opposite edges of the boundary and meet in the middle, keeping a constant climb or conventional direction with rapid links outside the clearing area.

  • Directional: every pass cuts in the same direction; the Tool Bit retracts to the Retract height and moves laterally to the start of the next pass (best surface consistency).

  • Spiral: a rectangular spiral from the outer corner inward.

All patterns step by Step Over percent of the Tool Bit diameter and honour Cut Mode; Reverse flips the direction for the chosen pattern.

Properties

Facing

  • Angle: Rotation angle of the cutting passes (default 0°).

  • Axial Stock To Leave: How much stock to leave on the floor; the operation stops at Final Depth plus this value (default 0).

  • Clearing Pattern: ZigZag (default), Bidirectional, Directional or Spiral.

  • Cut Mode: Climb (default) or Conventional.

  • Pass Extension: Distance to extend cuts beyond the boundary for Tool Bit disengagement (default 3 mm).

  • Reverse: Reverse the cutting direction for the selected pattern.

  • Step Over: Stepover as percent of the Tool Bit diameter (default 25, clamped to 0-100).

  • Stock Extension: Extends the boundary outward on all sides.

Linking

  • Collision Avoidance Strategy: How moves between areas are checked: Clearance Height (no collision detection, rapids at Clearance Height), Retract Height (no collision detection, rapids at Safe Height), Line of Sight (fastest - checks the Toolpath centerline), Tool Diameter (balanced - checks clearance using the Tool Bit diameter), Tool Shape (safest - checks clearance using the cross section of the Tool Shape).

  • Collision Clearance: Minimum clearance distance between the Tool Bit and any solid during linking moves (default expression: OpToolDiameter).

Depth

  • Clearance Height: The height needed to clear clamps and obstructions

  • Final Depth: Final Depth of Tool Bit - lowest value in Z

  • Safe Height: (Retract in the task panel) The height above which rapid moves are allowed between locations.

  • Start Depth: Starting depth of Tool Bit - first cut depth in Z

  • Step Down: Incremental step down of Tool Bit during operation

The operation has no Finish Depth, no Start Point and no Base Geometry.

Path

  • Active: Make False, to prevent operation from generating code

  • Block Delete: Enable the Post-Processor to add block delete commands

  • Comment: An optional comment for this Operation

  • Coolant Mode: The coolant mode for this operation: None, Flood or Mist

  • Cycle Time: (read-only) The cycle time estimation for this operation.

  • Tool Controller: Defines the Tool Controller used in the Operation

  • User Label: User assigned label

  • Workplane: introduced in 26.3 The link to the Work Plane that the Operation works in. An Operation with no link works in the XY of the Job.

Op Values

These read-only properties hold values calculated by the operation. They are useful as sources for expressions.

  • Op Start Depth, Op Final Depth: the calculated default depths

  • Op Tool Diameter: the diameter of the Tool Bit

  • Op Stock ZMax, Op Stock ZMin: the Z extent of the Stock

Tasks Window Editor Layout

Heights

  • Clearance

  • Retract

  • Start

  • Step down

  • Final

  • Linking group: Collision Avoidance Strategy, Collision Clearance

Tool Controller

  • Tool controller

  • Coolant mode

Operation

  • Clearing Pattern

  • Cut Mode

  • Angle (°)

  • Reverse

  • Step over (%)

  • Pass Extension

  • Stock Extension

  • Axial stock to leave

The quantity fields accept expressions.

Notes

  • Each step-down starts with a rapid to Clearance Height, then to Safe Height and a feed plunge to the layer depth; feed rates are taken from the Tool Controller.

  • introduced in 26.3 3+2 machining: the Set Work Plane from Face context menu command creates a Work Plane from a selected planar face and links the Operation to that Work Plane.

Scripting

See also: FreeCAD Scripting Basics.

import Path.Op.MillFacing as MillFacing

op = MillFacing.Create('MillFacing', parentJob=job)
op.ClearingPattern = 'Spiral'
op.StepOver = 40
doc.recompute()

Setup Sheet defaults can be provided for Cut Mode, Clearing Pattern, Angle, Step Over, Axial Stock To Leave, Pass Extension, Reverse and the Linking properties.