Lathe Tool Setter

A lathe tool setter is a precision device used in machining (particularly on lathes) to quickly and accurately set the position of cutting tools relative to the workpiece or spindle. It ensures that each tool is properly aligned, both in the Z-axis (lengthwise) and X-axis (radial), which is essential for accurate machining, especially in CNC (Computer Numerical Control) lathes.

TOOL SETTER OPERATES PROCEDURE

Lathe with FANUC OT command

Tool sensor distance setting

Macro variables definition and description

MACRO NO	DESCRIPTION
#100	TOOL NUMBER
#101	ABSOLUTE VALUE FOR #108
#102	ABSOLUTE VALUE FOR #109
#103	X- AXIS GEOMETRRY/OFFSET AMOUT (2700) TOOL NUMBER
#104	Z- AXIS GEOMETRRY/OFFSET AMOUT (2800) TOOL NUMBER
#108	X-AXIS TOOL BREAKGE AMOUNT (GEOMETRY VALUE)
#109	Z-AXIS TOOL BREAKGE AMOUNT (GEOMETRY VALUE)
#111	X-AXIS DIRECTION G00 PAUSE STOP POSITION (#123)
#112	Z-AXIS DIRECTION G00 PAUSE STOP POSITION (#124)
#113	X-AXIS SKIP BLOCK MEASURED VALUE
#114	Z-AXIS SKIP BLOCK MEASURED VALUE
#128	CALL G STATUS VALUE (05 GROUP)
#129	CALL G50 WORK POINT X-VALUE
#130	CALL GS0 WORK POINT Z-VALUE
#131	TOOL NUMBER
#500	G31 SKIP SIGNAL DISTANCE.
#501	THE DISTANCE FOR FROM ZRN TO -X PLUNGER OF SENSOR
#502	THE DISTANCE FOR FROM ZRN TO -Z PLUNGER OF SENSOR
#503	THE DISTANCE FOR FROM ZRN TO +X PLUNGER OF SENSOR
#504	THE DISTANCE FOR FROM ZRN TO +Z PLUNGER OF SENSOR
#505	BREAKGE VALUE

Program selection

macro programs

Here is a detailed explanation of each line Fanuc OT macro program for measuring tool gauges using a CNC lathe tool setter:

Line	Code / Command	Explanation
1	%09002	Program number. This identifies the program in the machine’s memory.
2	G65 H01 P#128 Q#4005	Macro call: Assigns the value stored in system variable #4005 (tool offset number) to local variable #128.
3	G98	Sets the canned cycle return point to the initial plane (R-value plane).
4	G28 U0	Returns the X-axis (U-axis in incremental mode) to the machine reference point (home position).
5	G28 W0	Returns the Z-axis (W-axis in incremental mode) to the machine reference point (home position).
6	G65 H02 P#129 Q#5001 R#5121	Macro call: Adds the values in variables #5001 and #5121 (X-direction tool offset and machine coordinate offset), storing the result in #129.
7	G65 H02 P#130 Q#5002 R#5122	Macro call: Adds the values in variables #5002 and #5122 (Z-direction tool offset and machine coordinate offset), storing the result in #130.
8	G50 X-#129 Z-#130	Sets coordinate system offsets with negative values calculated in #129 and #130.
9	M43	Turns on the tool setter signal or enables the measurement process.
10	G65 H24 P#131 Q#1032	Macro call: Copies the value from #1032 (diameter of the master tool) into #131.
11	G65 H12 P#100 Q#131 R15	Macro call: Divides the value in #131 by 15, stores the result in #100.
12	G65 H02 P#103 Q#100 R2700	Macro call: Adds 2700 to the value in #100, stores the result in #103. Used for positioning calculations.
13	G65 H02 P#104 Q#100 R2800	Macro call: Adds 2800 to the value in #100, stores the result in #104. Used for positioning calculations.
14	G65 H02 P#112 Q#504 R20.	Macro call: Adds 20.0 to the value in #504 (Z-position input), stores the result in #112.
15	G00 Z#112	Rapid move to the Z-coordinate defined by #112.
16	G65 H02 P#111 Q#501 R6.	Macro call: Adds 6.0 to the value in #501 (X-position input), stores the result in #111.
17	G00 X#111	Rapid move to the X-coordinate defined by #111.
18	G04 X1.	Dwell for 1 second to stabilize before measurement starts.
19	G65 H03 P#113 Q#501 R#500	Macro call: Subtracts #500 from #501, stores the result in #113. Used for calculating probe trigger point.
20	G31 X#113 F100	Probe command: Moves X-axis to #113 at feed rate 100; stops if probe detects contact.
21	G65 H03 P#101 Q#5061 R#501	Macro call: Subtracts #501 from #5061 (probe break point data), stores the result in #101.
22	G65 H01 P#108 Q#101	Macro call: Copies value in #101 into #108.
23	G65 H22 P#101 Q#101	Macro call: Multiplies #101 by itself, stores the result back in #101.
24	G65 H83 P100 Q#101 R#505	Macro call: Compares #101 with #505 (tolerance value); skips to line N100 if not within tolerance.
25	G65 H02 P#108 Q#108 R#9103	Macro call: Adds #9103 (X-offset storage location) to #108.
26	G65 H01 P#9103 Q#108	Macro call: Updates #9103 (X-tool offset) with the new calculated value from #108.
27	G00 U30.	Rapid move along U-axis (X-direction increment) by 30 units away from the tool setter.
28	W-30.	Rapid move along W-axis (Z-direction increment) by -30 units.
29	G65 H03 P#123 Q#501 R40.	Macro call: Subtracts 40.0 from #501, stores the result in #123.
30	G65 H03 P#124 Q#504 R2.5	Macro call: Subtracts 2.5 from #504, stores the result in #124.
31	G00 X#123	Rapid move to X position defined by #123.
32	Z#124	Rapid move to Z position defined by #124.
33	G65 H02 P#114 Q#504 R#500	Macro call: Adds #500 to #504, stores the result in #114.
34	G31 Z#114 F100	Probe command: Moves Z-axis to #114 at feed rate 100; stops if probe detects contact.
35	G65 H03 P#102 Q#5062 R#504	Macro call: Subtracts #504 from #5062 (probe break point data), stores the result in #102.
36	G65 H01 P#109 Q#102	Macro call: Copies value in #102 into #109.
37	G65 H22 P#102 Q#102	Macro call: Multiplies #102 by itself, stores the result back in #102.
38	G65 H83 P110 Q#102 R#505	Macro call: Compares #102 with #505 (tolerance value); skips to line N110 if not within tolerance.
39	G65 H02 P#109 Q#109 R#9104	Macro call: Adds #9104 (Z-offset storage location) to #109.
40	G65 H01 P#9104 Q#109	Macro call: Updates #9104 (Z-tool offset) with the new calculated value from #109.
41	G00 W-30.	Rapid move along W-axis (Z-direction increment) by -30 units.
42	G28 U0.	Returns the U-axis (X-direction) to the machine reference point (home position).
43	G28 W0.	Returns the W-axis (Z-direction) to the machine reference point (home position).
44	G65 H80 P150	Macro call: Unconditional jump to line N150.
45	N100 G28 U0	Label N100: Returns the U-axis to home position.
46	M44	Turns off the tool setter signal.
47	G04 X10	Dwell for 10 seconds.
48	G#128	Branches to the G-code stored in #128 (usually returns to the main program).
49	G50 X#129 Z#130	Resets the coordinate system to values stored in #129 and #130.
50	G65 H99 P1	Ends the macro program.
51	N110 G00 W-30.	Label N110: Rapid move along W-axis by -30 units.
52	G28 U0	Returns the U-axis to home position.
53	G28 W0	Returns the W-axis to home position.
54	M44	Turns off the tool setter signal.
55	G04 X10	Dwell for 10 seconds.
56	G#128	Branches to the G-code stored in #128.
57	G50 X#129 Z#130	Resets the coordinate system to values stored in #129 and #130.
58	G65 H99 P11	Ends the macro program.
59	N150 T00	Label N150: Tool change command to T00 (no tool).
60	M44	Turns off the tool setter signal.
61	G04 X10	Dwell for 10 seconds.
62	G#128	Branches to the G-code stored in #128.
63	G50 X#129 Z#130	Resets the coordinate system to values stored in #129 and #130.
64	M99	End of subprogram; returns control to the main program.

This table provides an overview of how the macro measures and updates tool offsets using probing logic and mathematical operations, ensuring accurate tool gauge compensation during machining processes.

Operates procedure

(I) in manual mode

1. Select optionally a tool as standard tool.

2. X, Z axis return to reference point.

3. Move toggle SW. “setter down/up” to “down position”

4. Then move two axes to touch the surface of appropriate direction of sensor. When X (Z) axis directional sensor is touched the sensor lamp of X <Z axis> direction will light and buzzer ring .

5. Register the present value of X Z axis position that display on page “position actual” on screen. For example x=-230.688 Z=-310.256

(II) In MDI mode

1. Input “-230688” to parameter No.743 Input “-310256” to parameter No.744

2. Press MENU OFFSET key and press MACRO soft key.

3. In search of variable No. 500 Input “230688” to #503. Input “310256” to #501.

4. The setting method for parameter No. 745, No. 746 and variable No. 504, No. 502 as same as above.

(III) In manual mode

1. Make toggle SW. “tool setter ON/OFF” to “ON” position and make toggle SW. tool offset/work shift to tool offset position, the screen display will change to page “off set/geometry”.

2. Move the two axes to safe area, then change tool.

3. Push cursor key ↑ or ↓until cursor No is equal to present tool No.

4. Move two axes to touch sensor and. the process as same as step (I).4.

5. The difference between the two figures will offset automatically.

(IV) In AUTO mode

Other tools are in accordance with former step. After a tool works sometimes, desire the tool to make a breakage offset. First change the cutting work piece into more small workpiece (otherwise when tool setter arm down, will hit the cutting workpiece if chuck don’t clamp any workpiece, in screen appear al1007.  Then write a program to call subprogram no, 9001 to no. 9004 in depending on what kind of tool

Note: subprogram no. 9001 to no. 9004 can’t be insert in cutting program.