CAM Helix

CAM Helix CAM Helix

Menu location

CAM  Helix

Workbenches

CAM

Default shortcut

None

Introduced in version

-

See also

None

Description

The CAM Helix CAM Helix command creates helical (and optionally spiral) Toolpaths to clear or profile circular holes and bosses. It is found on the New Operations toolbar and in the CAM menu; its tooltip reads "Creates a Helical toolpath from the features of a base object". The rotation direction (G2 or G3) is computed from Cut Mode, Side and Start At. Step Over sets the concentric step as a percentage of the Tool Bit diameter; successive helices are generated at increasing or decreasing radius until the hole is cleared.

Usage

  • Select the Workbench CAM CAM Workbench.

  • Select the CAM Helix icon or CAM  Helix from the top menu. This opens the Helix configuration panel.

  • introduced in 26.3: Choose the Tool Controller and coolant mode on the Tool Controller tab, which also lets you edit the selected Tool Controller’s feeds and speeds in place. In older versions you were prompted with a Choose a Tool Controller pop-up window.

  • Open the Base Geometry tab. Auto-select fills the table with every drillable circular feature of the Job Model; Add appends features selected in the 3D view introduced in 26.3 (faces or edges); Remove deletes the selected rows; Clear All empties the list. Untick a row to disable it without removing it.

  • introduced in 26.3: The table shows position and whether a cylinder is blind (columns #, Feature, Diameter, X, Y, Blind). Choose Sorting = Manual to drag rows into the desired machining order, or Automatic to let the automatic sorter order them (optionally from Start Point to End Point).

  • On the Heights tab set Start depth, Final depth and Step down. By default the operation makes one pass from Start to Final (Step Down defaults to the expression StartDepth - FinalDepth); set a smaller Step down for multiple depth passes.

  • Ensure Safe and Clearance Heights are correct.

  • On the Operation tab set Side (Inside for holes, Outside for bosses), Start from (Inside or Outside), Cut mode (Climb or Conventional), Max pitch, Max ramp angle, Step over and Radial stock to leave (outer).

  • Click Apply to create or update the Toolpath, OK to apply and close the panel, or Cancel to abort and close the panel.

Options

Radial Stock To Leave Outer introduced in 26.3 (formerly Offset Extra) adds a margin of material left on the outer wall unmachined. This is typically to allow a light finishing pass as a separate operation.

Helix Max Pitch introduced in 26.3 (replaces Helix Pitch) limits the maximum descent per revolution; 0 disables the limit.

Helix Max Ramp Angle introduced in 26.3 limits the ramp entry angle (0-90°); 0 disables the limit. The effective pitch is computed per helix radius from both limits.

Radial Stock To Leave Inner introduced in 26.3 (formerly Start Radius) is not available in the Helix task panel but can be edited directly in the Property View.

This is the stock left at the centre. The default inner radius for an inside profile is the Tool Bit radius; by default (zero) the Tool Bit just touches the axis of the hole, producing a central Toolpath cutting a hole twice the size of the Tool Bit diameter.

If this parameter is set to a negative value, it can allow a smaller helix radius; it cannot be less than minus the Tool Bit radius. A negative value equal to minus the Tool Bit radius will produce a zero radius helix: a.k.a. plunge cut with the endmill, should the Tool Bit be suitable. This will work as a first cut in a multi-pass operation, but attempting to make a helix Toolpath with a Tool Bit the same size as the hole in the model is rejected. For outside profiles the reference is the profile radius.

Comments

  • The helix pitch limit is not respected exactly. It is always rounded to give a complete number of turns from Start Depth to Final Depth (introduced in 26.3: the helix Toolpath is produced by a rewritten generator).

  • Similarly Step Over is not respected exactly. It is always rounded to give a number of equal steps.

By default Override Arc Feed Rate (hidden property, default checked) adjusts the feed of each helical arc from the Tool Controller’s horizontal and vertical feeds so the cutting-edge speed stays constant between inner and outer passes; disable it in the Property View to keep the raw Tool Controller feed. Consider this behavior when selecting feeds and speeds in the Tool Controller for the Job.

Properties

Data

Helix Drill

  • Side: Inside (default, for holes) or Outside (for bosses).

  • Start At: (formerly Start Side) Start cutting from the Inside or Outside.

  • Cut Mode: Climb or Conventional (default).

  • Direction: (read-only) The computed CW / CCW rotation of the circular cuts.

  • Step Over: Percent of Tool Bit diameter to step over on each pass (default 50).

  • Radial Stock To Leave Inner, Radial Stock To Leave Outer: see Options.

  • Helix Max Pitch, Helix Max Ramp Angle: see Options.

  • Helix Cone Angle: Cone angle of the helix (0 = cylindrical); positive for inside profiles, mirrored for outside profiles.

  • Start Cone From Bottom: introduced in 26.3 (visible only with a non-zero cone angle) Process the cone helix from bottom to top.

  • Single Helix: (hidden) Create only one helix.

  • Spiral Mill: Cut a spiral instead of concentric helices.

  • Finish Helix Circle, Finish Spiral Circle: (hidden, default True) Add a full finishing circle for the helix or spiral.

  • Retract From Wall: (hidden, default True) Move away from the wall before retracting, if there is free space.

  • Override Arc Feed Rate: (hidden, default True) Override arc feed rates to get constant cutting speed at the Tool Bit’s edge.

  • Override Profile Diameter: (hidden) Use this diameter for every hole instead of the detected one, to get identical hole sizes; cannot be less than the Tool Bit diameter.

  • Rotation Angle: (hidden, default -1 = automatic) Angular position of the start and end points; 0 places them along the X axis.

Sorting

  • Sorting Mode: introduced in 26.3 Automatic (default) sorts the holes automatically; Manual uses the table order.

  • Start Point, End Point, Use End Point: introduced in 26.3 Start and optional end of the automatic sorting (X and Y used, Z ignored); hidden in Manual mode.

Base

  • Disabled: List of Base Geometry features that are unchecked in the table.

Linking

  • Collision Avoidance Strategy: introduced in 26.3 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: introduced in 26.3 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 (default expression: StartDepth - FinalDepth, one pass)

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.

  • 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

View

The Helix operation has no additional View properties beyond the standard Toolpath display properties.

Notes

  • Holes whose radius is too small for the Tool Bit and the configured stock-to-leave are skipped with a warning in the Report view introduced in 26.3.

  • Coincident holes keep only the largest diameter.

  • If Safe Height is above Clearance Height, Clearance Height is used.

  • Step Down is split into equal passes; with Retract From Wall the Tool Bit steps away from the wall before each retract.

Scripting

See also: FreeCAD Scripting Basics.

Example:

import Path.Op.Helix as PathHelix

op = PathHelix.Create('Helix', parentJob=job)
op.Base = [(doc.Body, ['Face8'])]
op.Side = 'Inside'
op.CutMode = 'Climb'
op.StepOver = 50
doc.recompute()