Operation and Programming

Classic Control - Lathe Operator's Manual

The Online Interactive Operator's Manual is currently available in English only.

A PDF version of the Operator's Manual is available for download in multiple languages. Click the link below to view the Operator's Manual in your language. Click "Continue" to view the online version in English.

Get a translated PDF Download Continue

The Y Axis is an additional axis on the lathes (if so equipped) that can be commanded and behaves in the same manner as the standard X and Z Axes. There is no activation command necessary for Y Axis.

The lathe automatically returns the Y Axis to spindle centerline after a tool change. Make sure the turret is correctly positioned before commanding rotation.

Standard Haas G-codes and M-codes are available when programming with the Y Axis.

Mill type cutter compensation can be applied in both G17 and G19 planes when performing live tool operations. Cutter compensation rules must be followed to avoid unpredictable motion when applying and canceling the compensation. The Radius value of the Tool being used must be entered in the RADIUS column of the tool geometry page for that tool. The tool tip is assumed as “0” and no value should be entered.

Programming recommendations:

  • Command Axes home or to a safe tool change location in rapids using G53 which moves all axes at the same rate simultaneously. Regardless of the positions of the Y Axis and X Axis in relation to each other, both move at the MAX possible speed towards commanded position and usually do not finish at the same time. For example:

    G53 X0 (command for home) ; G53 X-2.0 (command for X to be 2" from home) ; G53 X0 Y0 (command for home) ;

    Refer to G53 on page 7.

    If commanding the Y and X Axes home using G28 the following conditions must be met and the described behavior expected:

    • Address identification for G28:

      X = U

      Y = Y

      Z = W

      B = B

      C = H

      Example:

      G28 U0 (U Zero) ; sends the X Axis to home position.

      G28 U0 ; is okay with Y Axis below spindle centerline.

      G28 U0 ; produces a 560 alarm if Y Axis is above spindle centerline. However homing the Y Axis first or utilizing a G28 without a letter address does not generate the 560 alarm.

      G28 ; sequence sends X, Y, and B home first then C and Z

      G28 U0 Y0 ; produces no alarm regardless of the Y-Axis position.

      G28 Y0 ; is okay with Y Axis above spindle centerline.

      G28 Y0 ; is okay with Y Axis below spindle centerline

      Pressing POWER UP/RESTART or HOME G28 produces the message: Function locked.

    • If X Axis is commanded home while the Y Axis is above spindle centerline (positive Y-Axis coordinates), alarm 560 is generated. Command Y Axis home first, then X Axis.

    • If X Axis is commanded home and the Y Axis is below spindle centerline (negative Y-Axis coordinates), the X Axis goes home and Y does not move.

    • If both X Axis and Y Axis are commanded home using G28 U0 Y0, the X Axis and Y Axis go home at the same time regardless of Y being above or below the centerline.

  • Clamp the main and/or secondary spindles (if so equipped) anytime live tooling operations are being performed and C Axis is not being interpolated.

    note: The brake unclamps automatically any time C-Axis motion for positioning is commanded.
  • These canned cycles can be used with the Y Axis. Refer to page 5 for more information.

    Axial Only Cycles:

    • Drilling: G74, G81, G82, G83,

    • Boring: G85, G89,

    • Tapping: G95, G186,

    Radial Only Cycles:

    • Drilling: G75 (a grooving cycle), G241, G242, G243,

    • Boring: G245, G246, G247, G248

    • Tapping: G195, G196

Program Example of Y-Axis Milling:

Y-axis Milling Program Example: [1] Feed, [2] Rapid.

% o50004 (Y AXIS MILLING) ; (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) ; G19 (Call YZ plane) ; G98 (Feed per min) ; M154 (Engage C-Axis) ; G00 G54 X4. C90. Y0. Z0.1 ; (Rapid to clear position) ; M14 (Spindle brake on) ; P1500 M133 (Live tool CW at 1500 RPM) ; M08 (Coolant on) ; (BEGIN CUTTING BLOCKS) ; G00 X3.25 Y-1.75 Z0. (Rapid move) ; G00 X2.25 (Rapid approach) ; G01 Y1.75 F22. (Linear feed) ; G00 X3.25 (Rapid retract) ; G00 Y-1.75 Z-0.375 (Rapid move) ; G00 X2.25 (Rapid approach) ; G01 Y1.75 F22. (Linear feed) ; G00 X3.25 (Rapid retract) ; G00 Y-1.75 Z-0.75 (Rapid move) ; G00 X2.25 (Rapid approach) ; G01 Y1.75 F22. (Linear feed) ; (BEGIN COMPLETION BLOCKS) ; G00 X3.25 M09 (Rapid retract, Coolant off) ; M15 (Spindle brake off) ; M155 (Disengage C axis) ; M135 (Live tool off) ; G18 (Return to XZ plane) ; G53 X0 Y0 (X & Y Home) ; G53 Z0 (Z Home) ; M30 (End program) ; %

Be aware: Many service and repair procedures should be done only by authorized personnel. The service technicians at your Haas Factory Outlet (HFO) have the training, experience, and are certified to do these tasks safely and correctly. You should not do machine repair or service procedures unless you are qualified and knowledgeable about the processes.

Danger: Some service procedures can be dangerous or life-threatening. DO NOT attempt a procedure that you do not completely understand. Contact your Haas Factory Outlet (HFO) and schedule a service technician visit if you have any doubts about doing a procedure.

Feedback