G234 - Tool Center Point Control (TCPC) (Group 08)

Next Generation Control Mill 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

G234 Tool Center Point Control (TCPC) is a software feature in the Haas CNC control that allows a machine to correctly run a contouring 4- or 5-axis program when the workpiece is not located in the exact location specified by a CAM-generated program. This eliminates the need to repost a program from the CAM system when the programmed and the actual workpiece locations are different.

The Haas CNC control combines the known centers of rotation for the rotary table (MRZP) and the location of the workpiece (e.g., active work offset G54) into a coordinate system. TCPC makes sure that this coordinate system remains fixed relative to the table; when the rotary axes rotate, the linear coordinate system rotates with them. Like any other work setup, the workpiece must have a work offset applied to it. This tells the Haas CNC control where the workpiece is located on the machine table.

The conceptual example and illustrations in this section represent a line segment from a full 4- or 5-axis program.

note:

For clarity, the illustrations in this section do not depict workholding. Also, as conceptual, representative drawings, they are not to scale and may not depict the exact axis motion described in the text.

The straight line edge highlighted in Figure 1 is defined by point (X0, Y0, Z0) and point (X0, Y-1., Z0). Movement along the Y Axis is all that is required for the machine to create this edge. The location of the workpiece is defined by work offset G54.

Location of Workpiece Defined by G54

In Figure Figure 2, the B and C Axes have been rotated 15 degrees each. To create the same edge, the machine needs to make an interpolated move with the X, Y, and Z Axes. Without TCPC, you would need to repost the CAM program for the machine to correctly create this edge.

G234 (TCPC) Off and the B and C Axes Rotated

TCPC is invoked in Figure 3. The Haas CNC control knows the centers of rotation for the rotary table (MRZP), and the location of the workpiece (active work offset G54). This data is used to produce the desired machine motion from the original CAM-generated program. The machine follows an interpolated X-Y-Z path to create this edge, even though the program simply commands a single-axis move along the Y Axis.

G234 (TCPC) On and the B and C Axes Rotated

G234 Program Example

%
O00003 (TCPC SAMPLE)
G20
G00 G17 G40 G80 G90 G94 G98
G53 Z0.
T1 M06
G00 G90 G54 B47.137 C116.354 (POSITION ROTARY AXES)
G00 G90 X-0.9762 Y1.9704 S10000 M03 (POSITION LINEAR AXES)
G234 H01 Z1.0907 (TCPC ON WITH LENGTH OFFSET 1, APPROACH IN Z-AXIS)
G01 X-0.5688 Y1.1481 Z0.2391 F40.
X-0.4386 Y0.8854 Z-0.033
X-0.3085 Y0.6227 Z-0.3051
X-0.307 Y0.6189 Z-0.3009 B46.784 C116.382
X-0.3055 Y0.6152 Z-0.2966 B46.43 C116.411
X-0.304 Y0.6114 Z-0.2924 B46.076 C116.44
X-0.6202 Y0.5827 Z-0.5321 B63.846 C136.786
X-0.6194 Y0.5798 Z-0.5271 B63.504 C136.891
X-0.8807 Y0.8245 Z-0.3486
X-1.1421 Y1.0691 Z-0.1701
X-1.9601 Y1.8348 Z0.3884
G49 (TCPC OFF)
G00 G53 Z0.
G53 B0. C0.
G53 Y0.
M30
%

G234 Programmer’s Notes

These key presses and program codes cancel G234:

  • EMERGENCY STOP

  • RESET

  • HANDLE JOG

  • LIST PROGRAM

  • M02 – Program End

  • M30 – Program End and Reset

  • G43 – Tool Length Compensation +

  • G44 – Tool Length Compensation -

  • G49 – G43 / G44 / G143 Cancel

These codes will NOT cancel G234:

  • M00 – Program Stop

  • M01 – Optional Stop

These key presses and program codes impact G234:

  • G234 invokes TCPC and cancels G43.

  • When using tool length compensation, either G43 or G234 must be active. G43 and G234 cannot be active at the same time.

  • G234 cancels the previous H-code. An H-code must therefore be placed on the same block as G234.

  • G234 cannot be used at the same time as G254 (DWO).

These codes ignore 234:

  • G28 – Return to Machine Zero Through Optional Reference Point

  • G29 – Move to Location Thru G29 Reference Point

  • G53 – Non-Modal Machine Coordinate Selection

  • M06 – Tool Change

Invoking G234 (TCPC) rotates the work envelope. If the position is close to the travel limits, the rotation can put the current work position outside of travel limits and cause an over travel alarm. To solve this, command the machine to the center of the work offset (or near the center of the table on a UMC), and then invoke G234 (TCPC).

G234 (TCPC) is intended for simultaneous 4- and 5-axis contouring programs. An active work offset (G54, G55, etc.) is required to use G234.

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