trickchit,
The Zero Line Table refers to the actual work table top surface. This surface is the origin point that is used to establish the Guide Heights within the machine, so all Taper and 4-Axis machining will reference this point using the G95 command to understand where the work piece and geometry are located in the Z-Axis.
Take a look at the attached image, as the Taper Data (G95 Command) will look like one of these (4) examples when machining Tapers and 4-Axis programs. In all the (4) examples, the P-Program Plane value would change if the work piece was raised above the Zero Line Table, but the Q-Sub Plane value would remain the same. Below is basic information on the G95 command.
G95 P_____ Q_____ Z#5015
- G95 = Taper Data Plane Command
- P = Program Plane (Start location of angle from Zero Line Table Height of the program geometry)
- Q = Sub-Plane (Machining height/thickness of angle. Use ± values to control direction. Always the Incremental height value from the Program Plane)
- Z#5015 = Automatically reads the current set position of the G53 Z-Axis and establishes the Upper Guide Height location for program execution.
When processing Taper programs, the Q-Value (Sub-Plane) can be a (+) or (-) value. A (+) value places the taper above the programmed geometry (Example 1 & 4), whereas a (-) value places the taper below the Programmed geometry (Example 2 & 3).
When processing 4-Axis programs, which requires (2) different geometry profiles, the Q-Value (Sub-Plane) should always be a (+) value, and must be the EXACT distance between the (2) geometry profiles used to create the NC program.
-Brian