Profile processing on turning machines

Special processes such as broaching and slotting are usually used when manufacturing inner and outer profiles. However, slotting can also be carried out cost-effectively on CNC turning machines without special components.


On CNC turning machines, the workpiece generally turns, while fixed tools such as tool bits or drill bits remove the necessary material. However, when it comes to special turned parts with inner or outer profiles, such as gear hubs with keyways or splines, a fixed workpiece and moving tools are needed. Classic processes such as slotting and broaching are normally used for this.

The disadvantage here is that the operator must change machines during machining, resulting in greater production costs.

Overview: Traditional machining of grooves

In mass production, optimized machines are used for each production process to ensure cost-effectiveness. There are four traditional processes: keyseating, slotting, broaching and EDM wire cutting.

  • Keyseating is carried out using a drawknife- like cutting tool, the shape and width of which determine the groove. Material removal takes place in several feeds; this process is suitable only for through holes. 
  • With slotting, the slotting tool determines the shape and width of the groove. Again, material removal takes place in several feeds; this process is also suitable for blind holes. 
  • The cutting tool used for broaching is a broach with several cutting edges sitting above one another. The material is removed down to the final dimensions in one stroke. 
  • Finally, EDM wire cutting forms shapes by means of electrical discharge machining. This process is suitable only for electrically conductive materials

Slotting on the turning machine

A good alternative to traditional processes is to create the grooves or toothing directly on the CNC turning machine - particularly in the case of small series. It should be noted that special machine requirements must be met when slotting. Modern CNC turning machines are adapted to cope with these demands thanks to rapid axis movements and constant changes of direction, which are similar to those for tapping and to the high cutting forces of solid drilling.

The main cutting movement in slotting is in the z direction and is implemented in the programmed feed by the fixed tool. The tool withdraws from the base of the groove at the end of the feed movement; the backward movement is an empty return stroke. The workpiece spindle is clamped tightly.

The depth of the groove is set by means of the x-axis feed; the width of the groove correlates with the width of the slotting tool.

In the case of groove widths that are greater than the tool width, the c-axis (main spindle) must be turned.

In addition, if the groove base is to be even, a y-axis will be required for lateral displacement. The machine requires a programmable c-axis in order to be able to produce several grooves on the inner or outer diameter.

The tool used is a slotting tool, which is defined in the tool management as, for example, a front-mounted parting tool.

If grooves are produced on the turning machine on a regular basis, the tool turret can be equipped with special slotting units. The rotary movement generated by the turret drive is translated into linear movement with a withdrawal function.

Creating perfect grooves

CNC specialists who wish to achieve optimum results when slotting should note several things: First, the groove should always be created in the top of the component so that the chips automatically fall downward from the cutting edge (due to gravity). Sufficient cooling is required during the slotting process for better material removal. In addition, plenty of scope for ejection must be ensured in through holes or undercuts in blind holes, to prevent breakage of tools or damage to turned parts.

Slotting can also be carried out on a milling machine or machining center. In this case, the tool is clamped in the fixed milling spindle.

Programming on the turning machine

Slotting is easy to program in the CNC control thanks to programGuide. R variables are defined, which are used in an IF loop in the NC program. The NC program might look like this:

; definition of R parameters
; diameter of hole
; depth of groove in X
; feed per stroke
; spindle position
; safety distance in X
; starting position in Z
; depth of groove in Z
; number of runs already completed
; runs required
; spindle increment angle
; calculation
; diameter of hole + safety distance
; NC programm
; initial value R9 for current slot
G0 SPOS="R4" G94 F5000
; spindle starting position
IF R11>R10
G0 X="R9" Z="R6+R5"
; starting position in X and Z
G1 Z="R7"
; stroke to feed depth
G0 X="R8"
; withdrawal
G0 Z="R6+R5"
; back to starting position
; offset of safety distance + depth of groove
; run Counter
IF R4<360


Do you have any questions or a suggested topic?