CAM MillFace

obsolete since 26.3 This command was replaced by Mill Facing in 26.3 and is no longer in the toolbar or menu. Existing Face operations in saved documents keep working and can still be created from Python with FreeCADGui.runCommand('CAM_MillFace') or Path.Op.MillFace.Create(). They are not converted to Mill Facing automatically.

CAM MillFace CAM MillFace

Menu location

CAM  Face 1.1 and earlier

Workbenches

CAM

Default shortcut

None

Introduced in version

-

See also

CAM Mill Facing

Description

The CAM MillFace CAM MillFace command creates a Toolpath to perform a facing operation on a horizontal surface. The command’s menu text is "Face" and its tooltip reads "Create a Facing Operation from a model or face"; in the source the command uses the CAM_Face.svg icon. This operation is generally used:

  • to smooth out a rough stock surface,

  • to mill selected face(s) to desired depth in preparation for performing subsequent clearing operations within the boundary of the regions affected by this operation,

  • or to apply a finishing surface to the selected face(s).

This operation contains a Boundary Shape property that allows for a modified selection area based upon the selected face(s).

For 26.3 and later use Mill Facing, which faces the Stock cross-section at the Final Depth and does not use Base Geometry.

Sample image of Mill Face operation used to prepare stock surface for subsequent clearing operation.

Usage

1.1 and earlier

  1. Select one or more faces to be surfaced. Note: If selected faces exist at different heights, then all will be milled to the Final Depth setting.

  2. There are several ways to invoke the command:

    • Press the CAM MillFace Face button.

    • Select the CAM  Face option from the menu.

  3. Select the correct Boundary Shape setting to modify the milling area based on the face(s) selected as Base Geometry.

  4. Adjust the other properties as needed. They are listed further below.

Caveats

The following caveats apply to this legacy operation. The replacement Mill Facing operation faces the whole Stock top without a face selection, so the issues around inclined planes and unmachined corners below do not apply to it.

  • Using it on an inclined plane may produce unexpected results: it will still produce a Toolpath to cut a horizontal surface. The extent of the cut will be the vertical projection of the inclined plane, performed at a height corresponding to the lowest point in that plane.

  • Since the CAM operations work on the geometry of the selected edges/faces only, and do not relate to the rest of the 3D model, the Toolpaths will not go beyond the bounds of the chosen plane, even if it is surrounded by unused stock or air. This will leave unmachined corners. These can sometimes be removed with one of the Dressups found on the CAM menu.

Vertical face milling

  • This operation will not work on a vertical plane or vertical non planar surface. Vertical operations can be achieved by using the face profile or edge profile operation. These will need the selection of a face or closed loop of edges including the top or bottom edge of the vertical surface desired). The extent of the Toolpath can then be reduced using the Boundary Dress-up found on the CAM menu. With the Dressup, select Create Box option and reduce the size to limit the scope of the profile Toolpath. These settings will not allow the origin of the boundary box to be moved, however. This must be done by adjusting the Placement settings in the Tree View.

  • This will work on compound surfaces such as several vertical planes or cylindrical surfaces joined together, so long as they form one continuous surface.

Properties

Note: The names of some Properties in this list differ a little from the same settings used in the Task Window Editor.

Data

Base

Note: It is suggested that you do not edit the Placement property of path operations. Rather, move or rotate the CAM Job model as needed.

  • Placement: Overall placement [position and rotation] of the object - with respect to the origin (or origin of parent object container)

    • Angle: Angle in degrees applied to rotation of the object around Axis property value

    • Axis: Axis (one or multiple) around which to rotate the object, set in sub-properties: X, Y, Z

      • X: X-axis value

      • Y: Y-axis value

      • Z: Z-axis value

    • Position: Position of the object, set in sub-properties: X, Y, Z - with respect to the origin (or origin of parent object container)

      • X: X-distance value

      • Y: Y-distance value

      • Z: Z-distance value

  • Label: User-provided name of the object (UTF-8)

Depth

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

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

  • Finish Depth: Maximum material removed on final pass.

  • Safe Height: The height above which rapid moves are allowed.

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

  • Step Down: Incremental Step Down of Tool Bit

Face

  • Boundary Shape: Shape to use for calculating the boundary: Boundbox, Face Region, Perimeter or Stock.

  • Clear Edges: Clear edges of surface (Only applicable to Boundbox)

  • Exclude Raised Areas: Exclude milling raised areas inside the face.

Path

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

  • Base: The base geometry for this operation

  • Block Delete: introduced in 26.3 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.

  • Sorting Mode: introduced in 26.3 Automatic sorts shapes with a nearest-neighbour algorithm; Manual follows the selection order.

  • 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

Pocket

  • Angle: introduced in 26.3 (formerly Zig Zag Angle) Angle of the grid, line and zigzag patterns. Hidden when the pattern is Offset.

  • Clearing Pattern: introduced in 1.1 (formerly Offset Pattern) Clearing pattern to use: ZigZag, Offset, ZigZagOffset, Line or Grid.

  • Cut Mode: Climb or Conventional.

  • Extra Offset: Extra offset to apply to the operation. Direction is operation dependent.

  • Force Max Step Over: introduced in 26.3 Force the maximum stepover even if not all area is cleared.

  • Min Travel: Use 3D Sorting of the Toolpath

  • Retract Threshold: introduced in 26.3 Repositioning moves shorter than this distance stay down. Replaces Keep Tool Down 1.1 and earlier.

  • Start At: Start pocketing at center or boundary

  • Step Over: Percent of Tool Bit diameter to step over on each pass (a value of 0 is reset to 1 %)

  • Use Rest Machining: Skip regions already cleared by previous operations.

Start Point

  • Start Point: The custom start point for the Toolpath of this operation.

    • X: X-distance value

    • Y: Y-distance value

    • Z: Z-distance value

  • Use Start Point: Make True, if manually specifying a Start Point. Set the start point in the property data Start Point field.

Notes

  • The legacy Heidenhain Post-Processor (heidenhain_legacy_post.py) still special-cases Face operations when labelling the output. It does not recognise the newer Mill Facing operation, so users of that Post-Processor who rely on the FACE labelling should be aware of the difference.