13.1 Automatic Tool Presetter (ATP)

Automatic Tool Presetter (ATP)

The Automatic Tool Presetter increases part accuracy and setup consistency, while reducing setup times by up to 50%. The system features easy-to-use automatic and manual modes of operation, with a user-friendly interface for quick, conversational-style programming.

  • Automatic, manual, and tool-breakage-detection operations.
  • Increases tool setting accuracy and consistency.
  • Conversational-style templates for easy tool-setting operations.
  • No macro programming required.
  • Outputs G-code to MDI, where it may be edited, or transferred into a program.

Follow the link or video below to Align, Test, and Calibrate the ATP.

Automatic Tool Presetter (ATP) - Alignment - Test - Calibration
Calibrate the Automatic Tool Probe (ATP) on Your Lathe

ATP - Manually Probe Tool Offsets

1

Warning: To manually probe a tool on the ATP, the tool must be fed into the probe stylus by holding the axis direction button and not the Hand Jog Wheel. The jog rate must be set to .001 or the tool offset measured may not be accurate.

Make sure that the ATP arm does not hit parts of the machine.

Push [CURRENT COMMANDS].

Select the Devices tab

Select the Mechanisms tab

Highlight Probe Arm

Push [F2] to lower the ATP arm.

2

Make sure a turning-stick tool is installed in the turret.

Make sure the pocket faces the spindle.

Jog the X and Z Axes to the center of the probe stylus to probe to X Geometry.

Make sure that you have distance of .125 inches between the tool tip and probe stylus.

3

Push [OFFSET] and navigate to the TOOL Offset tab .

Select the Tool Row that the tool offset will be measured.

Clear the tool offset value for both X Geometry and Z Geometry by pressing [0]. Push [F1]. This clears the Offset value.

If you get a warning message [1], Push [Y] to select YES.

Press [HANDLE JOG] and press [.001/1.].

Push and hold [-X] until the stick tool touches the probe.

 Note: You hear a beep sound when the stick tool touches the tool probe.

The tool offset will populate X Geometry.

Jog the X Axis away from the ATP arm.

4

Jog the X and Z Axes to the center of the probe stylus to probe the Z Geometry.

Make sure that you have distance of .125 inches between the tool tip and probe stylus.

Press [HANDLE JOG] and press [.001/1.].

Push and hold [-Z] until the stick tool touches the probe.

 Note: You hear a beep sound when the stick tool touches the tool probe.

The tool offset will populate Z Geometry.

Jog the Z Axis away from the ATP arm.

13.2 C-Axis

C-Axis

The C Axis provides high-precision, bi-directional spindle motion that is fully interpolated with X and/or Z motion. You can command spindle speeds from 0.01 to 60 RPM.

C-Axis operation is dependent on the mass, diameter and length of the workpiece and/or the workholding (chuck). Contact the Haas Applications Department if any unusually heavy, large diameter, or long configuration is used.

Cartesian to Polar Transformation (G112)

The G112 XY to XC coordinate interpolation feature lets you program subsequent blocks in Cartesian XY coordinates, which the control automatically converts to polar XC coordinates. While it is active, the control uses the G17 XY for G01 linear XY strokes and G02 and G03 for circular motion. G112 also converts X, Y position commands into rotary C-Axis and linear X-axis moves.

Cartesian to Polar coordinate programming greatly reduces the amount of code required to command complex moves. Normally a straight line would require many points to define the path, however, in Cartesian, only end points are necessary. This feature allows face machining programming in the Cartesian coordinate system.

C-Axis Programming Notes

Note: Programmed moves should always position the tool centerline.

Tool paths should never cross the spindle centerline. If necessary re-orient the program so the cut does not go over the center of the part. Cuts that must cross spindle center can be accomplished with two parallel passes on either side of spindle center.

Cartesian to Polar conversion is a modal command. Refer to Chapter 16 for more information on modal G-codes.

The G112 code is intended to be used with a Lathe using the C-axis and Live Tooling to program cutter anywhere along a non-rotating part.

The G112 code allows 3-D contouring using the X, Y, and Z axes. The tool centerline programing (G40) and cutter diameter compensation (G41/G42) are available with G112. They are also available for a tool in any of the three plane selection (G17, G18, G19).

A Lathe with Y-axis can use G112 and it can be useful to extend the range of travel of the live tool all the way across a part.

Circular motion (G02 and G03) in any of the three planes (G17, G18, G19) are also available with G112.

Since the spindle is not turning in G112, “feed per inch” (G98) must be selected.

Once G112 is active, all motions are programmed with XYZ and C cannot be used.

All X values are in radius when using G112.

Example Program:

o51120 (CARTESIAN TO POLAR INTERPOLATION) ;
(G54 X0 Y0 is at the center of rotation);
(Z0 is on face of the part) ;
(T1 is an end mill) ;
(BEGIN PREPARATION BLOCKS) ;
T101 (Select tool and offset 1) ;
G00 G20 G40 G80 G97 G99 (Safe startup) ;
G17 (Call XY plane) ;
G98 (Feed per min) ;
P1500 M133 (Live tool CW at 1500 RPM) ;
G00 G54 X2.35 C0. Z0.1 (Rapid to 1st position) ;
G112 (XY to XC interpretation);
M08 (Coolant on) ;
(BEGIN CUTTING BLOCKS) ;
G0 X-.75 Y.5 ;
G01 Z0 F10.;
G01 X0.45 (Point 1) ;
G02 X0.5 Y0.45 R0.05 (Point 2) ;
G01 Y-0.45 (Point 3) ;
G02 X0.45 Y-0.5 R0.05 (Point 4) ;
G01 X-0.45 (Point 5) ;
G02 X-0.5 Y-0.45 R0.05 (Point 6) ;
G01 Y0.45 (Point 7) ;
G02 X-0.45 Y0.5 R0.05 (Point 8) ;
G01 X0.45 Y.6 (Point 9) ;
G00 Z0.1 (Rapid retract);
(BEGIN COMPLETION BLOCKS) ;
G113 (Cancel G112) ;
M135 (Live tool off) ;
G18 (Return to XZ plane) ;
G00 G53 X0 M09 (X home, coolant off) ;
G53 Z0 (Z home) ;
M30 (End program) ;

C-Axis Cartesian Interpolation

Cartesian coordinate commands are interpreted into movements of the linear axis (turret movements) and spindle movements (rotation of the workpiece).

The lathe automatically engages/disengages the C-Axis when the axis is commanded or jogged.

When not using G112, Setting 102 - Diameter is used to calculate the feed rate.

C-Axis incremental moves are possible using the H address code as shown in this example:

G0 C90. (C-Axis moves to 90. deg.) ;
H-10. (C-Axis moves to 80. deg. from the previous 90 deg position) ; 

Cartesian Interpolation Example 1. [1] Projected Cutting Path [A] The endmill feeds 1" into the workpiece on one side. [B] The C Axis turns 180 degrees to cut the arc shape. [C] The endmill feeds 1" out of the workpiece.

o51121 (CARTESIAN INTERPOLATION EX 1) ;
(G54 X0 Y0 is at the center of rotation) ;
(Z0 is on face of the part) ;
(T1 is an end mill) ;
(BEGIN PREPARATION BLOCKS) ;
T101 (Select tool and offset 1) ;
G00 G18 G20 G40 G80 G99 (Safe startup) ;
G98 (Feed per min) ;
G00 G54 X2. C90 Z0.1 (Rapid to 1st position) ;
P1500 M133 (Live tool CW at 1500 RPM) ;
M08 (Coolant on) ;
(BEGIN CUTTING BLOCKS) ;
G01 Z-0.1 F6.0 (Feed to Z depth) ;
X1.0 (Feed to Position 2) ;
C180. F10.0 (Rotate to cut arc) ;
X2.0 (Feed back to Position 1 ) ;
(BEGIN COMPLETION BLOCKS) ;
G00 Z0.5 M09 (Rapid retract, coolant off) ;
M135 (Live tool off) ;
G18 (Return to XZ plane) ;
G53 X0 Y0 (X & Y home) ;
G53 Z0 (Z home) ;
M30 (End program) ;

Example Program:

o51122 (CARTESIAN INTERPOLATION EX 2);
(G54 X0 Y0 is at the center of rotation) ;
(Z0 is on face of the part) ;
(T1 is a drill) ;
(BEGIN PREPARATION BLOCKS) ;
T101 (Select tool and offset 1) ;
G00 G18 G20 G40 G80 G99 (Safe startup) ;
G19 (Call YZ plane) ; G98 (Feed per min) ;
G00 G54 X3.25 C0. Y0. Z0.25 ;
(Rapid to 1st position) ;
P1500 M133 (Live tool CW at 1500 RPM) ;
M08 (Coolant on) ;
G00 Z-0.75 (Rapid to Z depth) ;
(BEGIN CUTTING BLOCKS) ;
G75 X1.5 I0.25 F6. (Begin G75 on 1st hole) ;
G00 C180. (Rotate C axis to new position) ;
G75 X1.5 I0.25 F6. (Begin G75 on 2nd hole) ;
G00 C270. (Rotate C axis to new position) ;
G75 X1.5 I0.25 F6. (Begin G75 on 3rd hole) ;
(BEGIN COMPLETION BLOCKS) ;
G00 Z0.25 M09 (Rapid retract, coolant off) ;
M135 (Live tool off) ;
G18 (Return to XZ plane) ;
G53 X0 (X home) ;
G53 Z0 (Z home) ;
M30 (End program) ;

13.3 Dual Spindle

Dual Spindle

A lathe with two spindles is Dual Spindle machine. The main spindle is in a stationary housing. The other spindle, the “secondary spindle”, has a housing that moves along a linear axis, designated “B”, and replaces the typical tailstock. You use a special set of M-codes to command the secondary spindle.

Synchronized Spindle Control

Dual-spindle lathes can synchronize the main and secondary spindle. This means that when the main spindle receives a command to turn, the secondary spindle turns at the same speed, in the same direction. This is called Synchronous Spindle Control (SSC) mode. In SSC mode, both spindles accelerate, maintain speed, and decelerate together. You can then use both spindles to support a workpiece at both ends for maximum support and minimum vibration. You can also transfer the workpiece between the main and secondary spindle, effectively doing a “part flip” while the spindles continue to turn.

There are two G-codes associated with SSC:

G199 activates SSC.

G198 cancels SSC.

When you command G199, both spindles orient before they accelerate to the programmed speed.

Note: When you program synchronized dual spindles, you should first bring both spindles up to speed with M03 (for the main spindle) and M144 (for the secondary spindle) before you command G199. If you command G199 before commanding spindle speed, the two spindles attempt to stay synchronized while they accelerate, causing acceleration to take much longer than normal.

If SSC mode is in effect, and you press [RESET] or [EMERGENCY STOP], SSC mode remains in effect until the spindles stop.

The Synchronized Spindle Control Display

The spindle synchronization control display is available in the CURRENT COMMANDS display. The SPINDLE column gives the main spindle status. The SECONDARY SPINDLE column gives the secondary spindle status. The third column shows miscellaneous status. On the left is a column of row titles:

G15/G14 - If G15 appears in the SECONDARY SPINDLE column, the main spindle is the leading spindle. If G14 appears in the SECONDARY SPINDLE column, the secondary spindle is the leading spindle.

SYNC (G199) - When G199 appears in the row, spindle synchronization is active.

POSITION (DEG) - This row shows the current position, in degrees, of both the spindle and the secondary spindle. Values range from -180.0 degrees to 180.0 degrees. This is relative to the default orientation position of each spindle.

The third column indicates the current difference, in degrees, between the two spindles. When both spindles are at their respective zero marks, then this value is zero. If the third column value is negative, it represents how much the secondary spindle currently lags the main spindle, in degrees. If the third column value is positive, it represents how much the secondary spindle currently leads the main spindle, in degrees.

VELOCITY (RPM) - This row shows the actual RPM of the main spindle and the secondary spindle.

G199 R PHASE OFS. - This is the programmed R value for G199. This row is blank when G199 is not commanded; otherwise it contains the R value in the most recently executed G199 block.

CHUCK - This column shows the clamped or unclamped status of the work holding (chuck or collet). This row is empty when clamped, or shows “UNCLAMPED” in red when the work holding is open.

LOAD % - This shows the current load percent for each spindle.

VIDEO: See How G199 Works

R Phase Offset Explained

When dual lathe spindles are synchronized, they orient, then rotate at the same speed with their home positions stationary relative to each other. In other words, the relative orientation you see when both spindles are stopped at their home positions is preserved as synchronized spindles rotate.

You can use an R value with G199, M19, or M119 to alter this relative orientation. The R value specifies an offset, in degrees, from the following spindle’s home position. You can use this value to allow the chuck jaws to mesh during a workpiece hand-off operation.

G199 R Value Example:

[1] Leading Spindle

[2] Following Spindle

Finding a G199 R Value

To find an appropriate G199 R value:

1. In MDImode, command an M19 to orient the main spindle and an M119 to orient the secondary spindle. This establishes the default orientation between the spindles’ home positions.

2. Add an R value in degrees to the M119 to offset the secondary spindle’s position.

3. Check the interaction between the chuck jaws. Change the M119 R value to adjust the secondary spindle position until the chuck jaws interact correctly.

4. Record the correct R value and use it in the G199 blocks in your program.

Secondary Spindle Programming

The program structure for the secondary spindle is the same as that for the main spindle. Use G14 to apply main spindle M-codes and canned cycles to the secondary spindle. Cancel G14 with G15.

Secondary Spindle Commands

The secondary spindle can be jogged by following the instructions listed in the SUB-SPINDLE section under the current commands' devices tab. 

Three M-Codes are used to start and stop the secondary spindle:

  • M143 starts the spindle forward.
  • M144 starts the spindle in reverse.
  • M145 stops the spindle.

The P address code specifies the spindle speed, from 1 RPM to maximum speed.

Setting 345 selects between OD and ID clamping for the secondary spindle.

G14/G15 - Spindle Swap These G-codes select which spindle leads during Synchronized Spindle Control (SSC) mode (G199). G14 makes the secondary spindle the leading spindle, and G15 cancels G14.

The SPINDLE SYNCHRONIZATION CONTROL screen under current commands tells you which spindle currently leads. If the secondary spindle leads, G14 displays in the SECONDARY SPINDLE column. If the main spindle leads, G15 displays in the SPINDLE column.

Feedback