Caution: The sample programs in this manual have been tested for accuracy, but they are for illustrative purposes only. The programs do not define tools, offsets, or materials. They do not describe workholding or other fixturing. If you choose to run a sample program on your machine, do so in GRAPHICS mode. Always follow safe machining practices when you run an unfamiliar program.

This example shows the preferred programming method with solid stock material, where the cutoff operation must cut to the centerline.

The material is 2" (51mm) diameter solid stock and the finished part is 1" (25mm) long. The cutoff tool is 0.125" wide. The spindle/tool clearance is 0.875". The amount of stock to remove from the face is 0.025".

The program uses these Bar Feeder variable values:

%
O00023 (PART PROGRAM)
G105 P24 (CALL CUTOFF SUB PROGRAM THEN BAR FEED)
T303 (FACE & TURN)
G50 S1500
G96 S500 M03
G00 G54 X2.1 Z0 M08
G01 X-0.05 F0.005
G00 X1.95 Z.05
G01 Z-1.0 F0.01
X2.1
G53 G00 X0
G53 Z0
/M99
M30
%

%
O00024 (CUT-OFF SUB PROGRAM)
T404
G50 S1500
G96 S500 M03
G00 X2.1 Z0.1 M08
Z-1.125 (1" PART LENGTH PLUS THE TOOL WIDTH)
G01 X-0.05 F0.005
G00 X2.1
G53 X0
G53 Z0
M99
%

Command G105 in MDI mode to load a bar and push it to the initial push length. In this example, the initial push length includes the 0.875" spindle/tool clearance, the 0.125" width of the cutoff tool, and a 0.025" facing allowance.

This program starts with a call to the cutoff subprogram. The effect of this is different depending on whether this is a new bar or if it is the next program loop on a bar:

• If this is a new bar, the cutoff subprogram faces and cleans the bar end at the initial push length (#3101(F)), and then the Bar Feeder pushes out the part length plus allowances (#3100(D)).
• When the subprogram call repeats on a bar, the cutoff subprogram cuts off finished parts and leaves a clean bar end, and then the Bar Feeder pushes out the part length plus allowances (#3100(D)). 

Note: When you write a bar feed program with a cutoff routine and then a bar feed command, or with a bar feed command that includes a Pxxxxx cutoff subprogram call, it is safest and most consistent to start the program with the bar feed command. This practice makes sure that a fresh piece of material, with a faced surface, in a consistent position, is always available for the rest of the operation.

Note: The main program has a block-deleted M99 command in the second-to-last line. This lets you turn on block delete if you want the program to run only one time.

Dimensions are not to scale.

[1] Shows the Bar After the Initial Push at MDI Setup.

[2] Shows the Bar During Subsequent Feeds.

[A] Reference Point, Variables as Defined Above.

 Caution: The sample programs in this manual have been tested for accuracy, but they are for illustrative purposes only. The programs do not define tools, offsets, or materials. They do not describe workholding or other fixturing. If you choose to run a sample program on your machine, do so in GRAPHICS mode. Always follow safe machining practices when you run an unfamiliar program.

This example shows the preferred programming method when the cutoff operation does not have to cut to the centerline, as when the finished part has a hole through the center. Unlike the first program example, which uses the same subprogram to both face a new bar and cut off finished parts, this program includes a facing operation and a separate cutoff operation for finished parts. The facing operation cuts to the workpiece centerline. To save machining time, the cutoff operation cuts only as far as the finished part’s inner diameter.

The material is 2" (51 mm) diameter solid stock and the finished part is 1" (25 mm) long. The cutoff tool is 0.125" wide. The spindle/tool clearance is 0.875". The amount of stock to remove from the face is 0.025".

The program uses these Bar Feeder variable values:

%
O00020 (PART PROGRAM);
T303 (FACE & TURN);
G50 S1500;
G96 S500 M03;
G00 G54 X2.1 Z0 M08;
G01 X-0.05 F0.005;
G00 X1.95 Z.05;
G01 Z-1.0 F0.01;
X2.1;
G53 G00 X0;
G53 Z0;
T404 (CUT OFF OPERATION);
G50 S1500;
G96 S500 M03;
G00 X2.1 Z0.1 M08;
Z-1.125 (1" PART LENGTH PLUS THE TOOL WIDTH);
G01 X-0.05 F0.005;
G00 X2.1;
G53 X0;
G53 Z0;
G105 (BAR FEED);
/M99;
M30;
%

Command G105 in MDI mode to load a bar and push it to the initial push length. In this example, the initial push length includes the 1" finished part length, 0.875" spindle/tool clearance, the 0.125" width of the cutoff tool, and a 0.025" facing allowance.

This program starts with the face and turn operation, then the cutoff operation, and the bar feed command at the end.

Note: The program has a block-deleted M99 command in the second-to-last line. This lets you turn on block delete if you want the program to run only one time.

 Caution: The sample programs in this manual have been tested for accuracy, but they are for illustrative purposes only. The programs do not define tools, offsets, or materials. They do not describe workholding or other fixturing. If you choose to run a sample program on your machine, do so in GRAPHICS mode. Always follow safe machining practices when you run an unfamiliar program.

This example demonstrates a double push on the workpiece. The program contains G105 commands. The first G105 uses the variables values set on the Bar Feeder current commands page. The second G105 uses J and K values to override the variable values.

Note: A G105 with a J code will not increment the counter. The J code is intended for double push operation to make a long part. This is the preferred programming method when, for example, you need the rigidity of a short bar for part of your operation, and then to machine the rest of the longer finished part.

The material is 2" (51 mm) diameter solid stock and the finished part is 4" (100 mm) long. The cutoff tool is 0.125" wide. The spindle/tool clearance is 0.875". The amount of stock to remove from the face is 0.025".

The program uses these Bar Feeder variable values. These values apply to the first G105 command, given without address codes:

%
O00021 (DOUBLE PUSH WITH Bar Feeder);
G105 (BAR FEED USING MACRO VARIABLES);
T303 (FACE & TURN);
M01;
G50 S1500;
G96 S500 M03;
G00 G54 X2.1 Z0 M08;
G01 X-0.05 F0.005;
G00 X1.95 Z.05;
G01 Z-1.0 F0.01;
X2.1;
G53 G00 X0;
G53 Z0;
G105 J3.0 K1.0 (BAR FEED WITH OPTIONAL VARIABLES);
M01;
T404 (CUT OFF TOOL);
G55 (WORK OFFSET CHANGE);
G50 S1500;
G96 S500 M03;
G00 G55 X2.1 Z0.1 M08;
Z-4.125;
G01 X-0.05 F0.005;
G00 X2.1;
G53 X0;
G53 Z0;
/M99;
M30;
%

Command G105 in MDI mode to load a bar and push it to the initial push length. In this example, the initial push length includes the 2" length to machine first and a 0.025" facing allowance.

Before you run this program for the first time after you load a bar in MDI mode, move the cursor to the block after the first G105 command in the program to bypass the first push. Remember that after the initial push, the bar is already in position to start machining.

Note: The program has a block-deleted M99 command in the second-to-last line. This lets you turn on block delete if you want the program to run only one time.

 Caution: The sample programs in this manual have been tested for accuracy, but they are for illustrative purposes only. The programs do not define tools, offsets, or materials. They do not describe workholding or other fixturing. If you choose to run a sample program on your machine, do so in GRAPHICS mode. Always follow safe machining practices when you run an unfamiliar program.

This example uses a two-pass facing operation that runs conditionally at the beginning of each new bar. The Q13 command in the G105 line specifies program O00025 as the new bar facing subprogram.

%
O00022;
G105;
G105 Q13 P25 (RUN FACING SUBPROGRAM AT A NEW BAR);
T303 (FACE & TURN);
G50 S1500;
G96 S500 M03;
G00 G54 X2.1 Z0 M08;
G01 X-0.05 F0.005;
G00 X1.95 Z.05;
G01 Z-1.0 F0.01;
X2.1;
G53 G00 X0;
G53 Z0;
M01;
(CUT-OFF PROGRAM);
T404;
G50 S1500;
G96 S500 M03;
G00 X2.1 Z0.1 M08;
Z-1.125 (1" PART LENGTH PLUS THE TOOL WIDTH);
G01 X-0.05 F0.005;
G00 X2.1;
G53 X0;
G53 Z0;
M99;
%

%
O00025;
T303 (FACING PROGRAM FOR BEGINNING OF NEW BAR);
G50 S1500;
G96 S500 M03;
G00 G54 X2.1 Z.1 M08;
G01 X-0.05 F0.005 (1ST FACING PASS);
G00 Z.15;
X2.1;
Z.05;
G01 X-0.05 (2ND FACING PASS);
G53 X0;
G53 Z0;
M99;
%

Each time the control loads a new bar, it gives variable #3114 a value of 1. This prompts the control to run the specified subprogram at Q13. The control then changes the value of variable #3114 to 0 until it loads another new bar. While variable #3114 has a value of 0, the control does not run the facing subprogram.

The Bar Feeder can count either the number of parts made, or the length of material run. A non-zero value set in, Maximum Number of parts determines the active counting modes. The first non-zero value stops the cycle if more than one is present.

To stop the machine after a chosen number of parts, set Maximum Number of Parts to the chosen quantity. The counter increments at each G105 command. If G105 is at the beginning of the program, the counter increments before each part starts machining. If G105 is at the end of the program, the counter increments after each part finishes machining.

Note: A G105 with a J code will not increment the counter. The J code is intended for double push operation to make a long part.

To view the counters exit the Devices tab and navigate to the Timers tab.