Siemens CNC | CYCLE802 | Arbitrary Positions

In this article, we describe how to use CYCLE802 for arbitrary positions in Siemens CNC controlled machines with all details and examples.

0
360

CYCLE802 Introduction

This cycle (CYCLE802) allows you to freely program positions, i.e., rectangular or polar. Individual positions are approached in the order in which you program them.
The drilling tool in the program traverses all programmed positions in the order in which you program them. Machining of the positions always starts at the reference point. If the position pattern consists of only one position, the tool is retracted to the retraction plane after machining.

CYCLE802 Format

CYCLE802 (111111111, 111111111, X0, Y0, X1, Y1, X2, Y2, X3, Y3, X4, Y4)

Parameters

PSYS : Internal parameter, only the default value 111111111 is possible
PSYS : Internal parameter, only the default value 111111111 is possible
X0 : First position in the X axis
Y0 : First position in the Y axis
X1 : Second position in the X axis
Y1 : Second position in the Y axis
X2 : Third position in the X axis
Y2 : Third position in the Y axis
X3 : Fourth position in the X axis
Y3 : Fourth position in the Y axis
X4 : Fifth position in the X axis
Y4 : Fifth position in the Y axis


Note:
X0, Y0…X4, Y4

All positions will be programmed absolutely.

You may be interested also:
“Siemens CNC | CYCLE801 | Dot Matrix”

CYCLE802 Example

Drilling in G17 at the Positions

X20 Y20
X40 Y25
X30 Y40
N10 G90 G17 ; Absolute dimension data X/Y plane
N20 T10 ; Selects the tool
N30 M06 ; Tool change
S800 M3 ; Spindle speed clockwise rotation of the spindle
M08 F140 ; Feedrate Coolant on
G0 X0 Y0 Z20 ; Approach starting position
MCALL CYCLE82 (2, 0, 2, -5, 5, 0) ; Modal call of the drilling
N40 CYCLE802 (111111111, 111111111, 20, 20, 40, 25, 30, 40) ; call cycle positions
N50 MCALL ; Deselect modal call
N60 M30


Need to More?

Our volunteers have worked together and carefully prepared the articles published here in their native language without using machine translation. You can search the entire site for more information on the subject. You can start a discussion on CNCarea.com forums and join us to get support, ask questions, improve a published article or give your opinion.


Previous articleCNC Milling | G41 Code | Tool Offset Example
Next articleSiemens CNC Milling | CYCLE832 | High Speed Settings