Toolpath options in Carbide Create
Carbide Create affords a number of different toolpath options which provide for a wide variety of geometries which may be cut away from material depending on the endmill used. Carbide Create includes support for the following endmill/tool types:
  • square
  • ball-nosed
  • V-endmill
  • engravers
Early versions of Carbide Create had limitations in terms of which endmill type could be assigned to which toolpath, but 629 added support for using V endmills with non-V-carving-specific toolpaths.
The following toolpaths are either for decorative use or for Carbide Create Pro only and so will not be considered at this time:
  • Texture (decorative)
  • Engrave (Pro only)
  • 3D Rough (Pro only)
  • 3D Finish (Pro only)
Carbide Create Pro also adds the option of Rest machining for Pockets.
The following toolpaths which Carbide Create supports will be discussed here:
  • Contour
  • Pocket
  • Drill
  • VCarve
  • Advanced VCarve
  • Keyhole
Normally square endmills will be used for removing material and creating flat-bottomed pockets and making profile cuts all the way through material to cut parts free, ball-nosed endmills will be used to create rounded forms (including 3D), and V endmills will be used for V carving or chamfering or cutting at a precise angle as for certain types of joinery. Keyhole toolpaths require the use of specialty keyhole cutters which cut wider at the bottom than their shaft. Surfacing toolpaths such as the McFly are used to flatten stock or the spoilboard.
Note that in Carbide Create, dimensions may be entered using math expressions (which may contain units indicated by in or mm) which are evaluated by entering = at the end, so 1in+8mm= will result in a dimension of either 1.3150in or 33.400mm depending on the current unit. The variable t may be used to reference the current stock thickness, and the expression may be left as an expression by entering it without adding the = at the end, so t/2 will result in half the current stock thickness being used, and will update dynamically when the stock thickness is changed.
Carbide Create v7 adds the option of associating a Toolpath with the content of a selected layer.


Contour toolpaths follow along one or more drawn element(s) of geometry, and will be aligned relatively along based on path orientation/direction which will determine the Offset Direction:
  • Inside / Left
  • No Offset (directly along the path)
  • Outside / Right
Where the toolpath will fall relative to the geometry will always be clear when viewed in the 3D preview, and the offsets will alter the geometry of features — given a 1" circle cut with a 1/4" square endmill the following dimensions will be realized:
Carbide Create | Contour Toolpath | Offsets
  • Inside / Left — a 1" hole will be made, and a post 1/2" in diameter will be left
  • No Offset — a 1.25" hole will be made, and a post 0.75" in diameter will be left
  • Outside / Right — a 1.5" hole will be made, and a post 1" in diameter will be left
When not cutting all the way through with a square endmill, a square walled slot will result:
If cut with a ball-nosed endmill, a rounded groove may be achieved:
One option for Contour Toolpaths is tabs. In Carbide Create v7 they may be added in the Design tab:
then the tabs may be instantiated in the Contour Toolpath setting.


Pocket toolpaths allow cutting out the interior of geometry:
which will be a flat bottomed pocket with vertical walls if cut out with a square endmill.
If one uses a ball-nosed endmill, the edges will be rounded, the bottom will be scalloped, and there may be artifacts left behind:
If there is nested geometry, then the pocketing algorithm will alternate between cutting and not cutting, leaving islands:
One option for pocket toolpaths in some CAM programs is Rest machining to remove material which the endmill first used for a pocket cannot reach. Carbide Create Pro adds this:
Rest machining allows removing uncut material where a larger endmill cannot reach by indicating the previous size tool used and selecting a smaller tool to cut those areas which were not previously cut away:


Drill toolpaths plunge the tool at the center of the selected geometry:
As noted above, square, ball-nosed, and V-endmills may be used, and will be correctly previewed in how they cut:
A notable use for a V-endmill when drilling is to chamfer a small hole.

VCarve (and Advanced VCarve)

V carving toolpaths may be assigned to closed geometry, and as noted above, will cut either along the center (normal V carving), or along the perimeter (Advanced V carving), to either the depth required, or the max depth which is set. Advanced VCarving adds the option of pocket clearing to the depth set w/ a different endmill.
If one limits the depth on a normal V carve, one can achieve special effects such as changing a square:
into a diamond:


Keyhole toolpaths as noted above, require the use of a special tool, and are not previewed in 3D, since that would require undercuts which the 3D preview does not support.
Copy link
On this page
VCarve (and Advanced VCarve)