GSK980MDc Milling CNC System User Manual
52
I Programming
G codes Functions
G40 Tool radius compensation cancellation
G41 Tool radius left compensation
G42 Tool radius right compensation
G41 or G42 drives the system into compensation mode; G40 cancels the system compensation mode.
Explanation：
z Compensation plane
The compensation plane can be confirmed based upon plane selection command; the
tool compensation C is calculated in this plane.
z Compensation value (D code)
This system can be set for 32 compensation values at most. Two digits specified by D code in the
program, is called serial number of compensation value, the compensation value should be set by MDI/LCD
unit.
D code determines the compensation value in tool offset page according to the bit 1 of parameter
No.002, it is very important to notice that the value applied is diameter or radius.
Setting range of compensation value is as follows:
Compensation value: 0～9999999×least input increment.
z Compensation vector
The compensation vector is two-dimensional vector; it is equal to the compensation value specified
with D code. The compensation vector is calculated in control unit, its direction is real-time modified along
with the tool path in each block. You can calculate how much compensation is needed for tool movement
when the compensation value is applied in control unit. Compensation path (tool center path) =
programmed path tool radius (or diameter) (determined by compensation direction).
Note:
z Compensation operation is executed in the plane selected by G17, G18, G19. For example,
when XY plane is selected, (X,Y) or (I, J) is used to carry out compensation operation and
vector operation. The coordinate value whose axis in not in the compensation plane is not
affected by the compensation.
z In 3-axis linkage control, compensation only performed for the tool path projected on the
compensation plane.
z The alteration of compensation plane should be executed posterior to the compensation
mode cancelled. Otherwise, the system will give an alarm and machine stops.
z When the cutter compensation is cancelled by G40, movement amount should be specified,
otherwise, an alarm will occur.
z In the canned cycle G codes, G40, G41, G42 codes are disabled.
Plane selection Plane compensation
G17
X
－
Y
plane
G18
Z
－
X
plane
G19
Y
－
Z
plane
To Next Page
Loading...