Working with several cutting edges

Two fits with the same shaft diameter

In the workshop environment, machine operators sometimes have to machine two different fits with the same diameter. The fit tolerances should be different.


This requirement can be implemented by calling different cutting edges of a tool. While working with several cutting edges, it is possible to assign fits with their own dedicated offset memory to a tool.


In the subsequent description, a shaft should have two different fits at the front shaft seat. A third fit has a diameter of 40 mm. The workpiece dimensions can be taken from the figure obove.

Selecting several cutting edges

Tools can be conveniently selected in the SINUMERIK Operate editor using a softkey and inserted in the G code or ShopTurn program. Open the tool list and navigate to the tool. An additional cutting edge is selected once the required tool has been selected.


Use the softkeys Edges > New cutting edge. A second cutting edge is created (see figure above). The result can be immediately seen in the tool list. This operation must be repeated to select a third cutting edge.


Three different offsets for the fits can be selected using the tool wear

Contour programming

When programming the contour, before each Z motion, another cutting edge is called for the fits. This is realized using the D command; this is responsible for the particular cutting edge number.


For the contour in the current example, between the two programmed straight lines in the Z direction (20h7 and 20j6), a straight line must be inserted in the X direction. This traversing path is necessary in order that the modified cutting edge length in the X direction from the tool offset of the second cutting edge can be taken into account with the traversing path. An incremental length of 0.001 mm is already sufficient for the straight line.


Another cutting edge can be selected using the All parameters softkey; this is in the entry field Supplementary commands. The All parameters softkey must be pressed to select another cutting edge. Entering D2 under the supplementary commands calls the second cutting edge.

Traversing direction

The programmed straight line with a traversing path of 1/1000 mm does not play a role when machining the fit tolerance. In the current example, the cutting edge is only taken into account for a straight line in the positive X direction, as the cutting edge geometry of the tool only permits this traversing direction.


Programming the cutting edge call in the negative X direction is ignored, as the tool cannot machine the contour as a result of the cutting edge geometry. Even if the contour comprises individual straight lines in which a cutting edge call is programmed, this is ignored as traversing cannot take place in the X direction. As a consequence, the corresponding cutting edge length cannot be taken into account.


Between the individual contour elements in which a cutting edge is selected it is possible that the tool briefly remains in this position.

Would you like to contact the CNC4you team?

Questions or suggestions? Write us!

Do you have a suggestion for a video tutorial, a workpiece or an online article? We are curious about it!  

Related Content