FANUC Series 16/18/160/180-Model C for Lathe Operator Manual

PROGRAMMING
15. COMPENSATION FUNCTION
B–62754EN/01
224
This section provides a detailed explanation of the movement of the tool
for tool nose radius compensation outlined in Section 15.2.
This section consists of the following subsections:
15.3.1 General
15.3.2 Tool Movement in Start–up
15.3.3 Tool Movement in Offset Mode
15.3.4 Tool Movement in Offset Mode Cancel
15.3.5 Interference Check
15.3.6 Overcutting by Tool Nose Radius Compensation
15.3.7 Correction in Chamfering and Corner Arcs
15.3.8 Input Command from MDI
15.3.9 General Precautions for Offset Operations
15.3.10G53, G28, G30, and G30.1 Commands in Tool–tip Radius
Compensation Mode
The tool nose radius center offset vector is a two dimensional vector equal
to the offset value specified in a T code, and the is calculated in the CNC.
Its dimension changes block by block according to tool movement.
This offset vector (simply called vector herein after) is internally crated
by the control unit as required for proper offsetting and to calculate a tool
path with exact offset (by tool nose radius) from the programmed path.
This vector is deleted by resetting.
The vector always accompanies the tool as the tool advances.
Proper understanding of vector is essential to accurate programming.
Read the description below on how vectors are created carefully.
G40, G41 or G42 is used to delete or generate vectors.
These codes are used together with G00, G01, G02, G03 or G33 to specify
a mode for tool motion (Offsetting).
G code Function Workpiece position
G40 Tool nose radius compensation cancel Neither
G41 Left offset along tool path Right
G42 Right offset along tool path Left
G41 and G42 specify an off mode, while G40 specifies cancellation of the
offset.
The system enters the cancel mode immediately after the power is turned
on, when the RESET button on the MDI is pushed or a program is forced
to end by executing M02 or M30. (the system may not enter the cancel
mode depending on the machine tool.) In the cancel mode, the vector is
set to zero, and the path of the center of tool nose coincides with the
programmed, path. A program must end in cancel mode. If it ends in the
offset mode, the tool cannot be positioned at the end point, and the tool
stops at a location the vector length away from the end point.
15.3
DETAILS OF TOOL
NOSE RADIUS
COMPENSATION
15.3.1
General
D Tool nose radius center
offset vector
D G40, G41, G42
D Cancel mode

Leave a Reply

Your email address will not be published. Required fields are marked *