# Siemens CNC | HOLES2 | Row of Holes

## HOLES2 Introduction

Use this cycle (HOLES2) to machine a circle of holes. The machining plane must be defined before the cycle is called. The type of drill hole is determined by the drilling cycle that has already been called modally.

### Supported CNC Series

 Siemens CNC 802D, 810D, 840D, 840D sl, 840Di, 840Di sl series controllers.

## HOLES2 Format

 HOLES2 (CPA, CPO, RAD, STA1, INDA, NUM)

### Parameters

 CPA = Center point of circle of holes, abscissa (absolute) CPO = Center point of circle of holes, ordinate (absolute) RAD = Radius of circle of holes (enter without sign) STA1 = Starting angle; (Range of values: –180 < STA1 ≤ 180 degrees) INDA = Incrementing angle NUM = Number of drill holes

## HOLES2 Examples

### HOLES2 CNC Program Example – 1

The program uses CYCLE82 to produce 4 holes having a depth of 30 mm. The final drilling depth is specified as a relative value to the reference plane. The circle is defined by the center point X70 Y60 and the radius 42 mm in the XY plane. The starting angle is 45 degrees. The safety clearance in drilling axis Z is 2 mm.

Siemens CNC Holes2 Program Example

DEF REAL CPA=70,CPO=60,RAD=42,STA1=45 ; Definition of parameters with Value assignments
DEF INT NUM=4 ;
N10 G90 F140 S710 M3 D1 T40 ; Specification of technology values
N20 G17 G0 X50 Y45 Z2 ; Approach start position
N30 MCALL CYCLE82 (2, 0,2, , 30) ; Modal call of drilling cycle, without dwell time, DP is not programmed
N40 HOLES2 (CPA, CPO, RAD, STA1, , NUM) ; Call of circle of holes, the incrementing angle is calculated in the cycle, as the INDA parameter has been omitted
N50 MCALL ; Deselect modal call
N60 M30 ; Program end