12. Tool Compensation Functions
12.4 Tool Radius Compensation
202
12.4.5 General Precautions for Tool Radius Compensation
Precautions
(1) Designating the offset amounts
The offset amounts can be designated with the D code by designating an offset amount No.
Once designated, the D code is valid until another D code is commanded. If an H code is
designated, the program error (P170) No COMP No will occur.
Besides being used to designate the compensation amounts for tool radius compensation, the
D codes are also used to designate the compensation amounts for tool position compensation.
(2) Changing the offset amounts
Offset amounts are normally changed when a different tool has been selected in the
compensation cancel mode. However, when an amount is changed in the compensation mode,
the vectors at the end point of the block are calculated using the offset amount designated in
that block.
(3) Offset amount symbols and tool center path
If the offset amount is negative (
−
), the figure will be the same as if G41 and G42 are
interchanged. Thus, the axis that was rotating around the outer side of the workpiece will
rotate around the inner side, and vice versa.
An example is shown below. Normally, the offset amount is programmed as positive (+).
However, if the tool path center is programmed as shown in (a) and the offset amount is set to
be negative (
−
), the movement will be as shown in (b). On the other hand, if the program is
created as shown in (b) and the offset amount is set to be negative (
−
), the movement will be
as shown in (a). Thus, only one program is required to execute machining of both male and
female shapes. The tolerance for each shape can be randomly determined by adequately
selecting the offset amount.
(Note that a circle will be divided with type A when compensation is started or canceled.)
Workpiece
Workpiece
G41 offset amount (+) or G42 offset amount (
−
)
(a)
Tool center path
G41 offset amount (
−
) or G42 offset amount (+)
(b)
Tool center path
