14 The Tool Compensation
14.3 Tool Length Compensation (G43, G44, G49)
Instruction
G43 q H or
G44 q H
will set up the tool length compensation mode.
Address q means axis q to which the tool length compensation is applied (q= X, Y, Z, U, V, W, A, B, C).
Address H means the compensation cell, from which the tool length compensation value is taken. Irrespective of q being an absolute or an incremental data, instruction G43 will add the compensation value (specified at address H) to the end point coordinate obtained in the course of execution:
G43: + compensation
Irrespective of q being an absolute or an incremental data, instruction G44 will subtract the compensation (specified at address H) from the end point coordinate obtained in the course of execution:
G44: – compensation
Since incremental displacement Z0 has been programmed, each of instructions G43 G91 Z0 H1 and G44 G91 Z0 H1 will produce displacement just equal to the length of the tool. At G43, the displacement will be positive or negative, depending on the compensation value at H1 being positive or negative, respectively. The case is just the opposite for G44. After the command has been executed, the position displayed at coordinate Z will be the same as the one beforehand, because the position of the tool's tip will be displayed after the length compensation is set up.
Tool compensations may be defined on several axes at a time. E.g.
G43 Z250 H15
G43 W310 H16
When several axes are selected in a block, the tool length compensation will be taken into account for each axis selected:
G44 X120 Z250 H27
When the composition value is altered by calling a new H address, the previous one will be deleted, and the new value will be effective:
H1=10, H2=20
G90 | G00 |
|
|
G43 | Z100 | H1 | moving to Z=110 |
G43 | Z100 | H2 | moving to Z=120 |
The effects of G43 and G44 are modal until another command is received from that group.
Command
G49 or
H00
will cancel the tool length compensation in each axis - with motion or with transformation, if a movement has been programmed in the block or not, respectively.
The difference between the two commands is that H00 will delete the compensation only, leaving state G43 or G44 unaffected. If a reference is made afterwards to an address H other than zero, the new tool length compensation will be set up as the function of state G43 or G44.
79
