3. TOOL RADIUS CORRECTION

When a contouring profile is programmed for the numerical control, the radius of tool executing the profile is normally not known: the tool radius may vary due to many reasons (availability, sharpening, different tools used for roughing and finishing, etc.). The Z32 CNC allows to program directly the finished workpiece profile, and automatically executes all necessary profile modifications as a function of the effective tool radius. It is thus clear that the tool center path (i.e. the machine axes motion) is different from that necessary to describe the programmed profile with a speckled tool (R=0). In the figure, the tool center path (A…G) corresponding to the programmed profile (1…6) is shown. Please note the following: internal edges may not be machined due to tool radius (areas ‘X’) some fillets are automatically inserted (not programmed in the original profile) around external edges (B and D) some programmed segments have been eliminated because they cannot be machined with the programmed tool radius (segment 5) Generally, if the tool radius correction is activated in a program (with G41/G42), the Z32 CNC executes a series of operations on each element of the programmed profile, in order to transform it in the tool center path. These operations may bring to the elimination of some profile elements because they cannot be machined with the tool radius. The possibility to eliminate some profile elements imposes the CNC to “explore” in advance the trajectory, searching elements which cannot be machined. The G109 function allows to determine how many elements are explored in advance in this search: G109A three elements (active at reset) G109B four elements G109C five elements G109D six elements G109E seven elements

34