Overview

Task

This instruction describes the automatic measurement of workpieces. In addition, a zero offset is written to offset the origin of the machining coordinate system to match the workpiece,

Possible applications

The following applications are conceivable:

• Precise measurement of workpieces before or after machining
• Generating a zero offset to match the workpiece to simplify the programming for machining

Programming

The cycles are called with the L CYCLE[..] function and the required parameters are taken directly from the NC program. A more detailed description of the call is provided in the subsections for each of the cycles.

The section below explains the typical programming of a teach-in by the example of the SysMeasWcs7.ecy cycle which determines the corner point of a rectangular workpiece by 3 measurements. After calling the cycle, the zero offset generated in the cycle is activated and traverses over the corner point of the workpiece. In addition, the example writes the coordinates of the corner point to a text file. This can be implemented in the NC program as follows:

Programing Example

TCS measurement

#VAR

V.CYC.SysRetX

V.CYC.SysRetY

V.CYC.SysRetZ

#ENDVAR

T1 D1

G00 G90 X-50 Y-50

G00 G91 Z-100

L CYCLE [NAME=SysMeasWcs7.ecy @P4=10 @P5=10 @P6=-10 \

@P7=54 @P9=0 @P10=0 @P11=-2 @P17=20 @P18=30 @P19=-15]

G00 G91 Z100

#FILE NAME [MSG="SysMeasWcsResult.txt"]

#MSG SAVE ["V.CYC.SysRetX =%f", V.CYC.SysRetX]

#MSG SAVE ["V.CYC.SysRetY =%f", V.CYC.SysRetY]

#MSG SAVE ["V.CYC.SysRetZ =%f", V.CYC.SysRetZ]

G54

G0 G90 X0 Y0 Z200

... Workpiece machining ....

G53

M30

To enable program execution, a configuration file must also be saved as NC program.