INCON-M84/M86/M86R Manual

1.

Pocket machining includes "Rectangular Pocket" (G70.00) and "Circular Pocket" (G70.01), before using these two instructions, please note the following:

(1)

Orientation (G): The cutting orientation can be clockwise (CW, G02) or counterclockwise (CCW , G03).

(2)

Step In Axis (P): can be Not Defined, + 1st Axis, + 2nd Axis, - 1st Axis, and - 2nd Axis, which will be shown as P0~P4 command in the program. The orientation of 1st axis and 2nd axis are depends on the working plane (G17/G18/G19).

(3)

The radius of tool should be defined before pocket machining. It can be defined by tool table (D_).

(4)

G70.00 and G70.01 are both one-shot commands; users need to type G70.xx command in each pocket machining block. If continuous pocket machining command is written in the program instead of using "Command Insertion Aid", users still need to type G70.xx command in each of the blocks and values of new Center (X/Y/Z). Under the circumstances, if users do not change any of the other values, the system will adopt the previous settings.

(5)

The d value in the figures of pocket machining commands is the same as the value set in "F2→Parameter→Cancycle Parameters→Cut In Retract Length".

(6)

If values of Fine Feed Width (J value) and Fine Feed Depth (K value) were left blank, the system will not process fine cutting.

(7)

If G70.00 in values of Chamfering (L value)/Corner Rounding (R value) were left blank, the system will not process chamfered/rounded angle machining.

(8)

If value of Fine Feed Rate (E value) was left blank, the system will replace the value with half of Feed Rate (F value) value.

(9)

Pocket machining starts from the center of object and gradually widens the pocket layer by layer.

2.

Pocket machining starts from center of the object and gradually widens the dowel layer by layer. There are four percentage options of the widening width (150%, 125%, 100%, 75%). Users can select from "F2→Parameter→Cancycle Parameters→StepInWidth".

(1)

The tool move rapidly to center position Center X/Y (X,Y) and start height, which is Center Z (Z value) + Clearance (C value) of the pocket.

(2)

The tool descends to Step In Depth (Q value) with Spindle Feed Rate (I value).

(3)

The tool processes pocket machining with chosen Orientation and Feed Rate (F value).

(4)

The tool move back to center position and start height after finishing one layer.

(5)

The tool descends again to Step In Depth (Q value) with Spindle Feed Rate (I value) and processes pocket machining of the next layer.

(6)

The tool repeats the above steps until it reaches Length/Depth Z (W value).

(7)

Lastly, the tool processes cutting with Fine Feed Rate (E value).

(8)

When pocket machining command is finished, the tool retracts perpendicular to start height and stay at center position of the pocket.