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.
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
G234 Programmer’s Notes
These key presses and program codes cancel G234:
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.