Service Home G234 Tool Center Point Control (TCPC)

G234 Tool Center Point Control (TCPC)

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

G234 Tool Center Point Control (TCPC) lets a machine correctly run a contouring 4- or 5-axis program when the workpiece is not located in the exact location specified by the 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.

VR/GM-2-5AX - G234 - Tool Center Point Control (TCPC)

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 axes (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.

TCPC is activated with G234. G234cancels the previous H-code. An H-code must therefore be placed on the same block as G234. G234is canceled by G49, G42, and G44.


NOTE		 The rotary axes must be at 0 before commanding G234 .

TCPC G-code is programmed from the tool tip. The control knows the centers of rotation for the rotary axes (MRZP), the location of the workpiece (active work offset), and the tool length offset. The control uses this data to calculate the position of tool tip relative to the active work offset and maintains a static tool tip position through rotary feed moves.


NOTE		 Tool tip position is not maintained during rapid rotary moves. Do not program rapid moves while TCPC is active.

The diagram below illustrates TCPC positioning.

GM-2-5AX TCPC


TCPC Program Example


NOTE		 When starting TCPC it is safest to establish a new XYZ using a rapid move. The example below has a rapid G00 XYZ move after the G234 H code.

%
O00003 (TCPC SAMPLE);
G20;
G00 G17 G40 G80 G90 G94 G98;
G53 Z0.;
T1 M06;
G00 G90 G54 B0. C0. (POSITION ROTARY AXES);
G00 G90 X-0.9762 Y1.9704 S10000 M03 (POSITION LINEAR AXES);
G234 H01(TCPC ON WITH LENGTH OFFSET 1);
G00 X-0.9762 Y1.9704;
G00 Z1.0;
G01 X-0.5688 Y1.1481 Z0.2391 B43.421 C115.162 F40.;
X-0.4386 Y0.8854 Z-0.033 B43.421 C116.576;
X-0.3085 Y0.6227 Z-0.3051 B45.421 C116.654;
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 Z0.3884G49 (TCPC OFF);
G00 G53 Z0.;
G53 B0. C0.;
G53 Y0.;
M30;
%

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

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 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 , 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 . 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 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.