6FC5500-0AA22-0AA0 - Siemens - Datasheet.Global

Operation and Programming 11/2005 Edition

sinumerik

SIEMENS

SINUMERIK 801

Turning

SINUMERIK 801 Document Structure

User Documentation: Operation and Programming

User Documentation: Diagnostics Guide

Technical Documentation: Start-Up

Turning

Introduction 1

Turning On, Reference

Point Approach 2

Setting Up 3

Manually Controlled Mode 4

Automatic Mode 5

Part Programming 6

Services and Diagnosis 7

Programming 8

Cycles 9

SINUMERIK 801

Operation and Programming

Turning

Valid for

Control system

SINUMERIK 801

11.2005 Edition

SINUMERIK Documentation

Key to editions

The editions listed below have been published prior to the current edition.

The column headed “Note” lists the amended sections, with reference to the previous edition.

Marking of edition in the “Note” column:

A ... ... New documentation.

B ... ... Unchanged reprint with new order number.

C ... ... Revised edition of new issue.

Edition Order No. Note

2005.11 A5E00702070 A

Trademarks

SIMATIC®, SIMATIC HMI®, SIMATIC NET®, SIMODRIVE®, SINUMERIK®, and SIMOTION® are registered

trademarks of SIEMENS AG.

Other names in this publication might be trademarks whose use by a third party for his own purposes may violate

the registered holder.

The reproduction, transmission or use of this document or its con-

tents is not permitted without express written authority. Offenders

will be liable for damages. All rights, including rights created by

patent grant or registration of a utility model, are reserved.

Exclusion of liability

We have checked that the contents of this document correspond to

the hardware and software described. Nonetheless, differences

might exist and we cannot therefore guarantee that they are com-

pletely identical. The information contained in this document is re-

viewed regularly and any necessary changes will be included in the

next edition. We welcome suggestions for improvement.

Subject to technical changes without notice.

Siemens-Aktiengesellschaft.

SINUMERIK 801

SINUMERIK 801 I

Operation and Program ming

—

Turning

Safety Guidelines This Manual contains notices intended to ensure your personal safety, as well

as to protect products and connected equipment against damage. Safety

notices are highlighted by a warning triangle and presented in the following

categories depending on the degree of risk involved:

Danger

Indicates an imminently hazardous situation which, if not avoided, will result in

death or serious injury or in substantial property damage.

Warning

Indicates a potentially hazardous situation which, if not avoided, could result in

death or serious injury or in substantial property damage.

Caution

Used with safety alert symbol indicates a potentially hazardous situation which,

if not avoided, may result in minor or moderate injury or in pro perty damage.

Caution

Used without safety alert symbol indicates a potentially hazardous situation

which, if not avoided, may result in property damage.

Notice

Indicates important information relating to the product or highlights part of the

documentation for special attention.

Qualified person The unit may only be started up and operated by qualified person or persons.

Qualified personnel as referred to in the safety notices provided in this

document are those who are authorized to start up, earth and label units,

systems and circuits in accordance with relevant safety standards.

Proper use Please observe the following:

Warning

The unit may be used only for the applications described in the catalog or the

technical description, and only in combination with the equipment,

components and devices of other manufacturers as far as this is

recommended or pe rmitted by Siemens.

This product must be transported, stored and installed as intended, and

maintained and operated with care to ensure that it functions correctly and

safely.

Contents

SINUMERIK 801 III

Operation and Program ming

—

Turning

Contents

SINUMERIK 801 Operato r Panel OP ………………………………………………………… III

1. Introduction …………………………………………………………………………………………………… 1-1

1.1 Screen Layout ………………………………………………………………………………………… 1-1

1.2 Operating areas ……………………………………………………………………………………… 1-4

1.3 Overview of the most important softkey functions ………………………………………………… 1-5

1.4 Pocket calculator ……………………………………………………………………………………… 1-6

1.5 Coordinate systems ………………………………………………………………………………… 1-10

2. Turning On and Reference Point Approach ………………………………………………………… 2-1

3. Setting Up…………………………………………………………………………………………………………… 3-1

3.1 Entering tools and tool offsets ……………………………………………………………………… 3-1

3.1.1 Creating a new tool …………………………………………………………………………………… 3-3

3.1.2 Tool compensation data ……………………………………………………………………………… 3-4

3.1.3 Determining the tool offsets ………………………………………………………………………… 3-5

3.2 Entering/modifying the zero offset ………………………………………………………………… 3-7

3.2.1 Determining the zero offset ………………………………………………………………………… 3-8

3.3 Programming the setting data - “Parameters” operating area ………………………………… 3-10

3.4 R parameters – “Parameters” operating area …………………………………………………… 3-12

4. Manually Operated Mode ………………………………………………………………………………… 4-1

4.1 Jog mode – “Machine” operating area ……………………………………………………………… 4-1

4.1.1 Assigning the handwheel……………………………………………………………………………… 4-4

4.2 MDA mode (Manual Data Input) – “Machine” operating area …………………………………… 4-5

5. Automatic Mode ……………………………………………………………………………………………… 5-1

5.1 Selecting/starting a part program – “Machine” operating area …………………………………… 5-4

5.2 Block search – “Machine” operating area ………………………………………………………… 5-5

5.3 Stopping/ab orting a part program – “Machine” operating area ………………………………… 5-6

5.4 Repositioning after interruption – “Machine” operating area ……………………………………… 5-7

6. Part Programming …………………………………………………………………………………………… 6-1

6.1 Entering a new program – “Program” operating area …………………………………………… 6-3

6.2 Editing a part program – “Program” operating area ……………………………………………… 6-4

6.3 Programming support ………………………………………………………………………………… 6-7

6.3.1 Vertical menu ………………………………………………………………………………………… 6-7

6.3.2 Cycles ………………………………………………………………………………………………… 6-8

6.3.3 Contour ………………………………………………………………………………………………… 6-9

6.3.4 Free softkey assignment …………………………………………………………………………… 6-24

7. Services and Diagnosis …………………………………………………………………………………… 7-1

7.1 Data transfer via the RS232 Interface ……………………………………………………………… 7-1

7.2 Diagnosis and start-up – “Diagnostics” operating area …………………………………………… 7-8

8. Programming ………………………………………………………………………………………………… 8-1

8.1 Fundamentals of NC programming ………………………………………………………………… 8-1

8.1.1 Program structure …………………………………………………………………………………… 8-1

8.1.2 Word structure and address ………………………………………………………………………… 8-2

8.1.3 Block structure ………………………………………………………………………………………… 8-3

8.1.4 Character set ………………………………………………………………………………………… 8-5

8.1.5 Overview of instructions ……………………………………………………………………………… 8-6

Contents

IV SINUMERIK 801

Operation and Program ming

—

Turning

8.2 Position data ………………………………………………………………………………………… 8-13

8.2.1 Absolute/incre mental dimensions: G90, G91 …………………………………………………… 8-13

8.2.2 Metric/inch dimensions: G71, G70 ………………………………………………………………… 8-14

8.2.3 Radius/diameter dimensio ns: G22, G23 ………………………………………………………… 8-15

8.2.4 Programmable zero offset: G158 ………………………………………………………………… 8-16

8.2.5 Workpiece clamping - settable zero offset: G54 to G57, G500, G53 ………………………… 8-17

8.3 Axis movements …………………………………………………………………………………… 8-18

8.3.1 Linear interpolation at rapid traverse: G0 ………………………………………………………… 8-18

8.3.2 Linear interpolation at feedrate: G1 ……………………………………………………………… 8-19

8.3.3 Circular interpolation: G2, G3 ……………………………………………………………………… 8-20

8.3.4 Circular interpolation via interm ediate point: G5 ………………………………………………… 8-23

8.3.5 Thread cutting with constant lead: G33 …………………………………………………………… 8-24

8.3.6 Fixed-point approac h: G75 ………………………………………………………………………… 8-27

8.3.7 Reference point approach: G74 …………………………………………………………………… 8-28

8.3.8 Feedrate F …………………………………………………………………………………………… 8-28

8.3.9 Exact stop / continuous path mode: G9, G60, G64 …………………………………………… 8-29

8.3.10 Dwell time: G4 ……………………………………………………………………………………… 8-31

8.4 Spindle movements ………………………………………………………………………………… 8-32

8.4.1 Spindle speed S, directions of rotation …………………………………………………………… 8-32

8.4.2 Spindle speed l imitation: G25, G26 ……………………………………………………………… 8-33

8.4.3 Spindle positioning: SPOS ………………………………………………………………………… 8-34

8.5 Special turning functions …………………………………………………………………………… 8-35

8.5.1 Constant cutting rate: G96, G97 …………………………………………………………………… 8-35

8.5.2 Rounding, chamfer ………………………………………………………………………………… 8-37

8.6 Tool and tool offset ………………………………………………………………………………… 8-39

8.6.1 General notes ……………………………………………………………………………………… 8-39

8.6.2 Tool T ………………………………………………………………………………………………… 8-40

8.6.3 Tool offset number D ………………………………………………………………………………… 8-41

8.6.4 Selection of tool radius compensation: G41, G42 ……………………………………………… 8-46

8.6.5 Behavior at corners: G450, G451 ………………………………………………………………… 8-48

8.6.6 Tool radius compensation OFF: G40 ……………………………………………………………… 8-49

8.6.7 Special cases of tool radius compensation ……………………………………………………… 8-50

8.6.8 Example of tool radius compensatio n …………………………………………………………… 8-52

8.7 Miscellaneous function M …………………………………………………………………………… 8-53

8.8 Arithmetic parameters R …………………………………………………………………………… 8-54

8.9 Program branches …………………………………………………………………………………… 8-56

8.9.1 Labels - destination for program branches ……………………………………………………… 8-56

8.9.2 Unconditional program branches ………………………………………………………………… 8-57

8.9.3 Conditional branches ……………………………………………………………………………… 8-58

8.9.4 Example of program with branches ……………………………………………………………… 8-60

8.10 Subroutine technique ……………………………………………………………………………… 8-61

9. Cycles …………………………………………………………………………………………………………… 9-1

9.1 General Information about Standar d Cycles ……………………………………………………… 9-1

9.1.1 Overview of Cycles …………………………………………………………………………………… 9-1

9.1.2 Error messages and error handling in cycles ……………………………………………………… 9-2

9.2 Drilling, counter boring - LCY C82 …………………………………………………………………… 9-4

9.3 Deep hole drilling – LCYC83 ……………………………………………………………………… 9-6

9.4 Tapping with compensating chuck - LCYC840 …………………………………………………… 9-10

9.5 Boring - LCYC85 …………………………………………………………………………………… 9-12

9.6 Recess cycle – LCYC93 …………………………………………………………………………… 9-14

9.7 Undercut cycle – LCYC94 ………………………………………………………………………… 9-18

9.8 Stock removal cycle – LCYC95 …………………………………………………………………… 9-20

9.9 Thread cutting – LCYC97 …………………………………………………………………………… 9-25

SINUMERIK 801 V

Operation and Program ming

—

Turning

SINUMERIK 801 Operator Panel OP

Key definition

NC keyboard area

Machine area key Cursor UP (with shift: page up)

Recall key Cursor DOWN (with shift: page down)

Softkey Cursor LEFT

Area switchover key Cursor RIGHT

ETC key Selection key/toggle key

Acknowledge alarm Delete key (backspace)

SPACE (INSERT) Vertical menu

LCD

NC keys

MCP area

VI SINUMERIK 801

Operation and Program ming

—

Turning

ENTER / input key Shift key

… Numerical keys (with shift for

alternative assignment) …Alphanumeric keys (with shift for

alternative assignment)

MCP (Ma chine Control Panel) area

Chuck clamping (with LED) Spindle override 100％

Chuck clamping internally / Chuck clamping

externally (with LED) Spindle override minus (with LED)

Chuck unclamping (with LED) X axis, plus direction

Manual tool change (with LED) X axis, minus direction

Manual lubrication (with LED) Z axis, plus di rection

Manual coolant (with LED) Z axis, minus direction

AUTOMATIC (with LED) RAPID TRAVERSE OVERLAY

SINGLE BLOCK (with LED) SPINDLE START LEFT

Counterclockwise direction

MANUAL DATA (with LED) SPINDLE STOP

Increment (with LED) SPINDLE START RIGHT

Clockwise direction

JOG (with LED) RESET

REFERENCE POINT (with LED) NC STOP

Feedrate override plus (with LED) NC START

Contents

SINUMERIK 801 VI

Operation and Program ming

—

Turning

Feedrate override 100％ LED POK (Power OK), green

Feedrate override minus (with LED) LED ERR (Error), red

Spindle override plus (with LED) LED DIA (Diagnostics), yellow

Emergency Stop button (option)

SINUMERIK 801 1-1

Operation and Program ming

—

Turning

Introduction 1

1.1 Screen layout

1 2 3 4 7

Fig.1-1 Screen layout

The abbreviations on the screen stand for the following:

Table 1–1 Explanation of display elements

Display Element Abbreviation Meaning

MA Machine

PA Parameter

PR Programming

DI Services

Active operating area DG Diagnosis

STOP Programm stopped

RUN Program running

Program st atus RESET Program aborted

Jog Manual traverse

MDA Manual input with automatic function

Operating mode Auto Automatic

Introduction

1-2 SINUMERIK 801

Operation and Program ming

—

Turning

Display Element Abbreviation Meaning

SKP Skip block

Program blocks marked by a slash in front of the block number

are ignored during program execution.

DRY Dry run feed

Traversing movements are executed at the feed specified in the

Dry Run Feed setting data.

ROV Rapid traverse override

The feed override also applies to rapid feed mo de.

SBL Single block with stop after each block

When this function is active, the part program blocks are

processed separately in the following manner:

Each block is decoded sepa rately, the program is stopped at the

end of each block. The only exception are thread blocks without

dry run feed. In this case, the program is stopped only when the

end of the current thread block is reached. SBL can only be

selected in the RESET stat e.

M1 Programmed stop

When this function is active, the program is stopped at each

block in which the miscellaneous function M01 is prog rammed.

In this case, the message “Stop M00/M01 active“ appears on the

screen.

PRT Program test

Status display

1…1000

INC Incremental mode

If the control is in the Jog mode, incremental dimension is

displayed instead of the active program control function.

Operational

message

Stop: No NC Ready

Stop: EMERGENCY STOP active

Stop: Alarm active with stop

Stop: M0/M01 sctive

Stop: Block ended in SBL mode

Stop: NC STOP active

Wait: Read-in enable missing

Wait: Feed enable missing

Wait: Dwell time active

Wait: Auxiliary function acknowl. missing

Wait: Axis enable missing

Wait: Exact stop not reached

Wait: For spindle

Wait: Feed override to 0%

Stop: NC block incorrect

Wait: Block search active

Wait: No spindle enable

Wait: Axis feed value 0

Program name

Introduction

SINUMERIK 801 1-3

Operation and Program ming

—

Turning

Display Element Abbreviation Meaning

Alarm line

The alarm line is only displayed if an NC or PLC alarm is active.

The alarm line contains the alarm number and reset criterion of

the most recent alarm.

Working window

Working window and NC display

Recall symbo l

This symbol is displayed above the softkey bar when the

operator is in a lower-level menu.

When the Recall key is pressed, you can return to the

next-higher menu without saving data.

Menu extension

ETC is possible If this symbol appears above the softkey bar,

further menu functions are provided. These functions can be

activated by the ETC key.

Softkey bar

Vertical menu

If this symbol is displayed above the softkey bar, further menu

functions are provided. When the VM key is pressed, these

functions appear on the screen and can be selected by Cursor

UP and Cursor DOWN.

Feedrate

override

Here the current actual feedrate overrid e is shown.

Gear box

Here the current spindle gear stage 1…5 is shown.

Spindel speed

override

Here the current spindel speed override is shown.

Introduction

1-4 SINUMERIK 801

Operation and Program ming

—

Turning

1.2 Operating areas

The basic functions are grouped in the CNC into the fo llowing operating areas:

Machine Parameters Program Services Diagnostics

Executing

part

programs

Manual

control

Editing

program

data

Creating

part

programs

Reading

in / reading

out data

larm

display

Start-up

Oper ati n g ar eas

Fig.1-2 SINUMERIK 801operating areas

Switching between the operating

Press the “Machine” area key for direct access to the “Machine” operating

area.

Use the area switching key to return from any operating area to the main

menu.

Press the area switching key twice to return to the previous operating area.

After turning on the control system, the Machine operating area will appear by

default.

Display contrast adjustm ent

The display contrast can be adjusted via relevant softkeys Display Bright and

Display Darker (see “Section7.2 Diagnosis and start-up – “Diagnostics” operating

area” for detailed descriptions) or alternatively via CNC front panel directly. By

pressing Shift key + Cursor Left key, display will be brighter. By pressing Shift

key + Cursor Right key, display will be darker.

+ Pressing both keys, display will be brighter;

+ Pressing boths keys, display will be darker.

Introduction

SINUMERIK 801 1-5

Operation and Program ming

—

Turning

1.3 Overview of the most important softkey functions

Machine Parameter Program Services Diagnosis

larms Service

displa

Start-up Machine

data

Display

bright. Display

darker

Data In

Start Data Out

Start Error log show

Pro

rams Selection Open

Cop

Delete Rename Memor

info

Parameter Tool

correction Setting

data Zero

offset

Program

control Z oom block Search

ct.val

WCS Zoom

act.val

xis feed. Zoom G

funct Zoom M

funct

Zoom blo ck

ct.val

WCS Zoom

act.val

xis feed Zoom G

funct Zoom M

funct

Hand wheel

xis feed

ct.val

WCS Zoom

act.val.

X=0 *

RCS on

Z=0

* : Pressing on “RCS on” switches the softkey to “RCS off”

Introduction

1-6 SINUMERIK 801

Operation and Program ming

—

Turning

1.4 Pocket calculator

This function can be activated for all input fields intended for entry of

numerical values by means of the “=” character. To calculate the required

value, you can use the four basic arithmetic operations, and the functions sine,

cosine, squaring, as well as the square root function.

If the input field is already loaded with a value, this function writes the value in

the input line of the pocket calculator.

Fig. 1-3 Pocket calculator

Permissible characters

The following characters are permitted for input:

+ Value X plus value Y

- Value X minus value Y

* Value X multiplied with value Y

/ Value X divided by value Y

S Sine function

The value X in front of the input cursor is repla ce d by the value sin(X).

C Cosine function

The value X in front of the input cursor is repla ced by the value cos(X).

Q Square function

The value X in front of the input cursor is repla ce d by the value X2.

R Square root function

The value X in front of the input cursor is repla ce d by the value √X.

Calculation examples Task Input

100 + (67*3) 100+67*3

sin(45°) 45 S -> 0.707107

cos(45°) 45 C -> 0.707107

42 4 Q -> 16

√ 4 4 R

-> 2

The calculatio n is carried out by pressing the Input key. The softkey function OK

will accept the result into the input field, quitting the calculator automatically.

To calculate auxiliary points on a contour, the calculator provides the following

functions:

z calculating the tangential transition between a circle sector and a straight

line

z moving a point in a plane

z converting polar coordinates into Cartesian coordinates

z adding the second end point of a contour section ‘straight line - straight

line’ given via angular interrelation.

Introduction

SINUMERIK 801 1-7

Operation and Program ming

—

Turning

These functions are directly linked with the input fields of the programming

support. Any values in this input field are written by the pocket calculator into

the input line, and the result is automatically copied into the input fields of the

programming support.

Softkeys

This function is used to calculate a point on a circle. The point results from the

angle of the created tangent and the direction of rotation of the circle.

Fig.1-4 Calculation of a point on a circle

Enter the circle center, the angle of the tangent and the radius of the circle.

The function switches the screen form from diameter programming to radius

programming.

Use softkey G2 / G3 to define the direction of rotation of the circle.

The abscissa and ordinate values are calculated; the abscissa is the first axis

of the plane, and the ordinate is the second axis of the plane.

If plane G18 is active, the abscissa is the Z axis, and the ordinate is the X

axis.

The value of the abscissa is copied into that input field from which the pocket

calculator function has been called, and the ordinate value into the next

following input field.

Example Calculating the intersection point between the circle sector and the

straight line .

Given: Radius: 10

Circle center point: Z 147 X103

Ongoing angle of the straight line: -45°

Introduction

1-8 SINUMERIK 801

Operation and Program ming

—

Turning

Result: Z = 154.071

X = 117.142

The function calculates the missing end point of the contour section straight

line - straight line, with the second straight line standing vertically on the first

straight line.

The following values of the straight line are known:

Straight line 1: Start point and rise angle.

Straight line 2: Length and one end point in the Cartesian coordinate system

Fig.1-5

The function switches the screenform from diameter programming to radius

programming.

The function chooses the given coordinate of the end point. The value of

ordinate and/or abscissa is given.

The second straight line is rotated in clockwise direction or, with refer to the

first straight line, rotate d by 90 degrees in counter-clo ckwise direction.

The function chooses the appropriate setting.

The missing end point is calculated. The value of the abscissa is copied into

that input field from which the pocket calculator function has been called, and

the ordinate value into the next following input field.

Introduction

SINUMERIK 801 1-9

Operation and Program ming

—

Turning

Fig.1-6

The drawing above must be added by the value of the circle center point to be

able to calculate the intersection point between the circle sector of the straight

line. The missing coordinate of the center point is calculated by means of the

pocket calculator function , since the radius in the tangential transition

stands vertical on the straight line.

Calculating M1 in section 1:

In this section, the radius stands on the straight line section rotated in

counter-clockwise direction.

Use the softkeys and to select the given constellation .

Enter the coordinates, the pole point P1, the rise angle of the straight line, the

given ordinate value and the circle radius as the length.

Fig.1-7

Result: Z = 24.601

X = 60

Introduction

1-10 SINUMERIK 801

Operation and Program ming

—

Turning

1.5 Coordinate systems

Right-handed, rectangular coordinate system s are used for machine tools.

Such systems describe the movements on the machine as a relative motion

between tool and workpiece.

Fig.1-8 Specification of the axis directions to one another; coordinate system

when programming for turning.

Machine coordinate The orientation of the coordinate system on the machine depends on the

particular

system (MCS) machine type. It can be turned to various positions.

Fig. 1-9 Machine coordinates/axes on a turning machine

The origin of this coordinate system is the machine zero.

All axes are in the zero position at this point. This point is merely a reference

point determined by the machine manufacturer. It does not need to be

approachable.

The traversing range of the machine axes can be ne gative.

Introduction

SINUMERIK 801 1-11

Operation and Program ming

—

Turning

Workpiece coord- The coordinate system described above (see Fig. 1–8) is also used to

describe

inate system (WCS) the geometry of a workpiece in the workpiece program.

The workpiece zero can be freely selected in the Z axis by the programmer. In

the Z axis, the zero point corresponds to the turning center.

Workpiece

W - w o rkp iec e ze ro

Fig.1-10 Workpiece coordinate system

Workpiece clamping To machine the workpiece, it is clamped in the machine. The workpiece must

be aligned such that the axes of the workpiece coordinate system are in

parallel with the machine axes. Any resultant offset of the machine zero to the

workpiece zero is determined in the Z axis and entered in a specially provided

data area for the settable zero offset. This offset is activated during the NC

program execution by means, for example, of a programmable G54 (see

Section “Workpiece Clamping - Settable Zero Offset ...”).

XMachine X

Workpiece

z.B.

G54

Workpiece

Machine

Fig.1-11 Workpiece on the machine

Current workpiece An offset in relation to the workpiece coordinate syste m can be generat ed by

coordinate system means coordinate system of the programmable zero offset G158. The result is

the current workpiece (see Section “Programmable Zero Offset: G158”).

Introduction

1-12 SINUMERIK 801

Operation and Program ming

—

Turning

SINUMERIK 801 2-1

Operation and Program ming

—

Turning

Turning On and Reference Point 2

Approach

Notice

Before you switch on the SINUMERIK and the machines, you should also

have read the machine documentation, since turning on and reference point

approach are machine-dependent functions.

Operating sequence First switch on the power supply of the CNC and of the machine. After the

control system has booted, you are in the “Machine” operating area, in the Jog

operating mode.

The Reference point approach window is active.

Fig.2-1 Jog Ref basic screen

Reference-point approach can only be e x ecuted in the Jog Ref mode.

Activate the “Approach reference point” function by selecting the Ref key on

the machine control panel area.

In the “Reference point approach” window (Fig. NO TAG), it is displayed

whether or not the axes have to be referenced.

Axis has to be referenced

Axis has reached the reference

oint

Turning On and Reference Point Approach

2-2 SINUMERIK 801

Operation and Program ming

—

Turning

… Press the direction keys.

The axis does not move if you select the wrong direction.

Approach the reference point in each axis successively.

You can quit the function by selecting another operating mode (MDA,

Automatic or Jog).

SINUMERIK 801 3-1

Operation and Program ming

—

Turning

Setting Up 3

Preliminary remarks Before you can use the CNC, set up the machine, tools, etc. on the CNC by:

z entering the tools and tool offsets

z entering/modifying the zero offset

z entering the setting data

3.1 Entering tools and tool offsets

Functionality The tool offsets consist of several data that describe the geometry, wear and

tool type.

Each tool has a defined number of parameters depen ding on the tool type.

Each tool is identified by its own tool number (T number).

See also Section 8.6 “Tool and Tool Offset”.

Operating sequences

This function opens the Tool Compensation Data window, which contains the

offset values of the currently active tool. If you select another tool using the

“<<T “ or “T>>” soft keys, the setting remains when you quit the window.

Parameter

Fig.3-1 Tool compensation data window

Tool

Corr.

Parameter

Setting Up

3-2 SINUMERIK 801

Operation and Program ming

—

Turning

Get

Comp.

<< T

T >>

<< D D >>

Softkeys

Select next lower or next higher edge numbe r.

Select next lower or next higher tool.

Determine length compensation values.

Use the ETC key to extend the softkey functions.

Reset

edge All edge compensation values are reset to zero.

Creates a new edge and loads it with the appropriate parameters.

The new edge is created for the currently displayed tool; it is automatically

assigned the next higher edge number (D1 – D9).

Max. 16 edges (in total) can be stored in the memory.

Deletes the tool compensation data of all edges of the selected tool.

Creates new tool compensation data fo r a new tool.

Note: Max. 8 tools can be created.

Pressing this softkey opens the dialog box and the overview of the tool

numbers assigned. Enter the tool number you search for in the input window

and start search with OK. If the searched tool exists, the search function

opens the tool offset data box.

Delete

tool

New

tool

New

edge

Setting Up

SINUMERIK 801 3-3

Operation and Program ming

—

Turning

3.1.1 Creating a new tool

Operating sequence

Press this softkey to create a new tool.

Pressing this softkey opens the input window and an overview of the tool

numbers assigned.

Fig 3-2 New Tool window

…

Enter the new T number (maximal only three digits) and specify the tool type.

Press OK to confirm your entry; the Tool Compensation Data window is

opened.

New

tool

Setting Up

3-4 SINUMERIK 801

Operation and Program ming

—

Turning

3.1.2 Tool compensation data

The tool compensation data are divided into length and radius compensation

data.

The list is structured according to the tool type.

Fig.3-3 Tool compensation data window

Operating sequence Enter the offsets by

Positioning the cursor on the input field to be modifie d,

… Entering value(s)

And confirming your entry by pressing Input or a cursor selection.

Setting Up

SINUMERIK 801 3-5

Operation and Program ming

—

Turning

3.1.3 Determining the tool offsets

Functionality This function can be used to determine the unknown geometry of a tool T.

Prerequisite The appropriate tool has been changed. In JOG mode, approach a point on

the machine, from which you know the machine coordinates, with the edge of

the tool.This can be a tool with a known position. The machine coordinate

value can be split into two components: stored zero offset and offset.

Procedure Enter the offset value into the intended Offset field. Then select the required

zero offset (e.g. G54) or G500 if no zero offset is to be calculated. These

entries must be made for each selected axis (see Fig. 3-6).

Please note the following: The assignment of length 1 or 2 to the axis

depends on the type of tool (turning tool, drill).

For the turning tool, the of fset value for the X axis is a diameter dimension.

Using the actual position of point F (machine coordinate), the offset entry and

the selected zero offset Gxx (position of the edge), the control system can

calculate the assigned compensation value of length 1 or length 2 for the

preselected axis.

Note: You can also use a zero offset already determined (e.g. G54 value) as

the known machine coordinate. In this case, approach to workpiece zero with

the edge of the tool. If the edge stands directly at the workpiece zero, the

offset value is zero.

XMachine

Workpiece

Machine

Length 2=?

ctual position

Z position

F - tool ca rrie r referen ce p oint

M - ma chine zero

W - wo rk pie c e zero

Length 1=?

ctual position X

Offset

The offset value of the X axis is a

diameter valu e.

Gxx

Fig.3-4 Determination of the length compensation values using the example of

a cutting tool

Setting Up

3-6 SINUMERIK 801

Operation and Program ming

—

Turning

XMachine

Workpiece

Machine

Length 1=?

ctual position Z

F- workpiece reference point

M-machine zero

W -workpiece zero

OffsetGxx

Fig.3-5 Determination of length compensation value using the example of a

drill: Length 1/Z axis

Operating sequence

Select the softkey Get Comp. The window Compensation values opens.

Fig.3-6 Compensation values windo w

z Enter offset if the tool edge cannot approach the zero point Gxx. If you

work without zero offset, select G500 and enter offse t.

z When the softkey Calculate is pressed, the control system determines

the searched geometry length 1 or 2 depending on the preselected axis.

This geometry is calculated on the basis of the approached actual

position, the selected Gxx function and the entered offset value.

The determined compensation value is stored by pressing the softkey

OK.

Get

Comp.

Setting Up

SINUMERIK 801 3-7

Operation and Program ming

—

Turning

3.2 Entering/modifying the zero offset

Functionality The actual-value memory and thus also the actual-value display are referred

to the machine zero after the reference-point approach. The workpiece

machining program, however, refers to the workpiece zero.

This offset must be entere d as the zero offset.

Operating sequences

Use the Parameter and Zero Offset softkeys to select the zero offset.

An overview of settable zero offsets appears on the screen .

Fig.3-7 Zero offset wind ow

Position the cursor bar on the input field to be altere d,

… enter value(s).

The next zero offset overview is displayed by Page down. G56 and G57 are

now displayed.

Return to next-higher menu level, without saving the zero offset values.

Softkeys

Use this function to determine the zero offset with refer to the coordinate origin

of the machine coordinate system. When you have selected the tool, which

you want to use for measuring, you can set the appropriate conditions in the

Determine window.

Deter-

mine

Paramete

Zero

offset

Setting Up

3-8 SINUMERIK 801

Operation and Program ming

—

Turning

A window with the programmed zero offset is displayed. The values in the

window cannot be edited.

Displays the sum of all active zero offsets. The values cannot be edited.

3.2.1 Determining the zero offset

Prerequisite You have selected the window with the corresponding zero offset (e.g. G54)

and the axis for which you want to determine the offset.

XMachine

Workpiece

Machine

Zero offset Z=?

Length 2

ctual

Z position

F - tool support reference po in t

M - mach in e z ero

W - workpiece ze ro

Fig.3-8 Determining the zero offset for the Z axis

Approach

z A zero offset can only be determined with a known tool. Enter the active

tool in the dialog box. Press OK to take over the tool; the Determine

window is then opened.

z The selected axis appears in the Axis area.

The actual position of the tool support reference point (MCS) associated

to the axis is displayed in the adjacent field.

z D number 1 is displayed for the tool edge.

If you have entered the valid offsets for the used tool under a D number

other than D1, enter that D number here.

z The stored tool type is displayed automa tically.

z The effective length compensation value (geometry) is displayed.

z Select the sign (-, +) for calculating the length offset, or select “without”

taking the length of fset into account.

A negative sign subtracts the length offset value from the actual position.

The zero offset in the sele cted axis is the result.

z Offset

If the tool does not reach zero, an offset can be entered to specify an

additional of fset to a point which can be approched by the tool.

Pro-

grammed

Sum

Setting Up

SINUMERIK 801 3-9

Operation and Program ming

—

Turning

Fig.3-9 Select Tool screen form

Fig.3-10 Determine zero offset form

Softkey can be used to select the zero offsets G54 to G57. The selected zero

offset is displ ayed on the selected softkey.

Selects the next axis.

Pressing the Calculate softkey calculate s the ze ro offset.

Press the OK softkey to quit the window.

UFrame

xis

Calcu-

late

Setting Up

3-10 SINUMERIK 801

Operation and Program ming

—

Turning

3.3 Programming the setting data - “Parameters” operating area

Functionality Use the setting data to define the settings for the operating states. These can

also be modified if necessary.

Operating sequences

Use the Parameter and Setting Data softkeys to select Setting Data.

The Setting Data softkey branches to another menu level in which various

control options can be set.

Fig.3-11 Setting data main screen

Use the paging keys to position the cursor on the desired line within the

display areas.

… Enter the new value in the input fields.

Use Input or the cursor keys to confirm.

Softkeys

This function can be used to change the following settings:

Jog feed

Feed value in Jog mode

If the feed value is zero, the control system uses the value stored in the

machine data.

Spindle

Spindle speed

Direction of rotation of the spindle

Jog

data

Paramete

Sett.

data

Setting Up

SINUMERIK 801 3-11

Operation and Program ming

—

Turning

Minimum / Maximum

Limits for the spindle speed set in the Max. (G26)/Min. (G25) fields must be

within the limit values specified in the machine data.

Programmed (LIMS)

Programmable upper speed limitation (LIMS) at constant cutting speed (G96).

Dry-run feedrate for dry-run operation (DRY)

The feedrate you enter here is used in the program execution instead of the

programmed feed during the Automatic mode when the Dry-Run Feedrate is

active (see Program Control, Fig. 5–3).

Start angle for thread cutting (SF)

A start angle representing the starting position for the spindle is displayed for

thread cutting operations. It is possible to cut a multiple thread by altering the

angle and repeating the thread cutting operation.

Spindle

data

Dry

feed

Start

angle

Setting Up

3-12 SINUMERIK 801

Operation and Program ming

—

Turning

3.4 R parameters – “Parameters” operating area

Functionality All R parameters (arithmetic parameters) that exist in the control system are

displayed on the R Parameters main screen as a list (see also Section 8.8

“Arithmetic Parameters /R Parameters”). These can b e modified if necessary.

Fig.3-12 R Parameters window

Operating sequence

Use the Parameter and R Parameter softkeys.

To position the cursor on the input field that you want to edit.

… Enter value(s).

Press Input or use the cursor keys to confirm.

Parameters

R Para-

meters

SINUMERIK 801 4-1

Operation and Program ming

—

Turning

Manually Operated Mode 4

Preliminary remarks

The manually operated mode is possible in the Jog and MDA mode.

In the Jog mode, you can traverse the axes, and in the MDA mode, you can

enter and execute individual p art program blocks.

4.1 Jog mode – “Machine” operating area

Functionality In Jog mode, you can

z traverse the axes and

z set the traversing speed by means of the override switch, etc.

Operating sequences

Use the Jog key on the machine control panel area to sele ct the Jog mode.

… Press the appropriate key for the X or Z axis to traverse the desired axis.

As long as the direction key is pressed and hold down, the axes traverse

continuously at the speed stored in the setting data. If this setting is zero, the

value stored in the machine data is used.

… If necessary use the override button key to set the traversing speed.

It can be adjusted by settable increments:

0%, 1%, 2%, 4%, 6%, 8%, 10%, 20%, 30%, 40%, 50%, 60%, 70%, 75%, 80%,

85%, 90%, 95%, 100%, 105%, 110%, 115%, 120%.

If you press the Rapid Traverse Overlay key at the same time, the selected

axis is traversed at rapid traverse speed as long as both keys are pressed

down.

Manually Operated Mode

4-2 SINUMERIK 801

Operation and Program ming

—

Turning

In the Incremental Feed operating mode, you can use the same operating

sequence to traverse the axis by settable increments. The set increment is

displayed in the display area. Jog must be pressed again to cancel the

Incremental F eed.

The Jog main screen displays position, feed and spindle values, including the

feedrate override and spindle override, gear stage status as well as the

current tool.

Fig.4-1 Jog main screen

Press softkey ETC displayed on the screen above, system will branch into the

following screen:

Press softkey “X=0” or “Z=0”, the value of the current coordinate system

displayed on the screen will be automatically changed to zero. You may make

coordinate system switches by switching between “RCS on”/”RCS off” (see

figure below for “RCS off”).

Manually Operated Mode

SINUMERIK 801 4-3

Operation and Program ming

—

Turning

Notice:

“RCS off”/”RCS on” is valid for corresponding cooredinate screen only.

Softkey functions “X=0”, “Z=0” and “RCS off”/”RCS on” are not available In

AUTO or MDA mode

If the system returns back to JOG mode again from AUTO or MDA mode,

the screen last stored in JOG mode will be automatic ally restored.

Parameters Table 4–1 Description of parameters in the Jog main screen

Parameter Explanation

MCS

Display of addresses of existing axes in machine

coordinate system (MCS).

+X– Z If you traverse an axis in the positive (+) or negative (–)

direction, a plus or minus sign appears in the respective

field.

No axis is displayed, if the axis is in position.

Act.

mm The current position of the axes in the MCS or WCS is

displayed in these fields.

Repos

offset If the axes are traversed in the Jog mode in the Program

Interrupted condition, the distance traversed by each axis

in relation to the break point is displayed in this column.

Spindle S

rpm Display of actual value and setpoint of spindle speed

Feed F mm/min Display of path feed actual value and setpoint

Tool Display of currently active tool with the current cutting

edge number

Actual feedrate

override Display of current feedrate override

Actual spindle

override Display of current spindlel speed overrid e

Gear stage Display of current gear stage in the machine

Softkeys

Call the Handwheel window.

Hand-

wheel

Manually Operated Mode

4-4 SINUMERIK 801

Operation and Program ming

—

Turning

Call the Axis Feed or Interp. Feed window.

Use this softkey to change between the Axis Feed window and the Interp.

Feed window.

The softkey label changes to Interp. feed when the Axis/Feed window is

opened.

The actual values are displayed as a function of the selected coordinate

system. There are two different coordinate systems, i.e. the machine

coordinate system (M CS) and the workpiece coordinate system (WCS).

The softkey changes between MCS and WCS. When doing this, the softkey

label changes as follows:

z The values of the machine coordinate system are selected, the softkey

label changes to Act. val. WCS.

z When the workpiece coordinate system is selected, the label changes to

Act. val. MCS.

Enlarged view of actual values.

Pressing Recall key, return to the next-higher menu level.

xis

feed

Interp./

feed

ct. val.

WCS

ct.val.

MCS

Zoom

act.val.

Manually Operated Mode

SINUMERIK 801 4-5

Operation and Program ming

—

Turning

4.1.1 Assigning the handwheel

An axis is assigned to the respective handwheel and becomes active as soon

as you press OK.

The increment size for the handwheel is also selectable with the key .

Operating Sequence

In Jog mode, call the Handwheel window.

After the window has opened, all axis identifiers are displayed in the Axis

column and also appear in the softkey bar.

Fig.4-2 Handwheel window

The WCS/MCS softkey is used to select the axes from the machine or

workpiece coordinate system for assignment to the handwheel. The current

setting is displayed in the Handwheel win dow.

The assignment you have made i s reset for the selected handwheel.

Hand–

wheel

WCS

MCS

De-

select

Manually Operated Mode

4-6 SINUMERIK 801

Operation and Program ming

—

Turning

4.2 MDA mode (Manual Data Input) – “Machine” operating area

Functionality You can create and execute a part program block in the MDA mode.

Contours that require several blocks (e.g. roundings, chamfers) cannot be

executed/programmed.

Caution

This mode is protected by the same safety interlocks as fully automatic mode.

Furthermore, the MDA mode is subject to the same prerequisites as the fully

automatic mode.

Before NC-start of an input NC-program in the mode MDA is to wait till the

message “Block store activ e” displays on the screen.

Operating sequences

Use the MDA key in the machine control panel area to select the MDA mode.

Fig.4-3 MDA main screen

… Enter a block using the control keyboard.

The entered block is executed by pressing NC START. The block cannot be

executed while machining is taking place.

Manually Operated Mode

SINUMERIK 801 4-7

Operation and Program ming

—

Turning

Parameters Table 4–2 Description of the parameters in the MDA working window.

Parameter Explanation

MCS

Display of existing axes in MCS or WCS.

– Z If you traverse an axis in the positive (+) or negative (–)

direction, a plus or minus sign appears in the respective

field.

No sign is displayed if the axis is in posi tion.

Act. value

mm The current position of the axes in the MCS or WCS is

displayed in these fields.

Spindle S

rpm Display of actual value and setpoint of spindle speed.

Feed F Display of path feed actual value and setpoint in

mm/min or mm/rev.

Tool Display of currently active tool with the current tool

edge number (T..., D...).

Edit window In the Stop or Reset program state, an edit window is

provided for input of the part program block.

Actual feedrate

override Display of current feedrate override.

Actual spindle

override Display of current spindlel speed overrid e.

Gear stage Display of current gear stage in the machine.

Softkeys

The actual values for the MDA mode are displayed as a function of the

selected coordinate syste m.

There are two different coordinate systems, i.e. the machine coordinate

system (MCS) and the workpiece coordinate system (WCS).

Enlarged view of the actual values.

Menu extension.

Display of Axis Feed or Interp. Feed window.

This softkey can be used to change between the two windows. The softkey

label changes to Interp. Feed when the Axis Feed window is opened.

The G function window contains all active G functions whereby each G

function is assigned a group and has its own fixed positon in the window.

Further G functions can be displayed using the Page Up or Page Down keys

together with Shif t key. Select Recall to quit the wind ow.

ct.val.

WCS

ct.val.

MCS

Zoom

act.val.

xis

feed

Interp.

feed

Zoom

G funct.

Manually Operated Mode

4-8 SINUMERIK 801

Operation and Program ming

—

Turning

The window shows the currently edited block full length.

Opens the M function window to display all active M functions of the block.

Zoom

block

Zoom

SINUMERIK 801 5-1

Operation and Program ming

—

Turning

Automatic Mode 5

Functionality In Automatic mode, part programs can be executed fully automatically, i.e. this

is the operating mode for standard processing of part programs.

Preconditions The preconditions for executing part programs are:

z Reference point approached.

z You have already stored the required part program in the control system.

z You have checked or entered the necessary offset values, e.g. zero

offsets or tool offset s.

z The required safety interlocks a re a ctivated.

Operating sequence

Use the Automatic key to select the Automatic mode.

The Automatic main screen appears that displays the position, feed, spindle,

override and tool values, the gear stage status as well as the current block.

Fig.5-1 Automatic main screen

Automatic Mode

5-2 SINUMERIK 801

Operation and Program ming

—

Turning

Parameters Table 5–1 Description of the parameters in the working wind ow

Parameter Explanation

MCS

Display of existing axes in MCS or WCS.

+ X

– Z If you traverse an axis in the positive (+) or negative (–)

direction, a plus or minus sign app ears in the respective field.

No sign is displayed if the axis is in posi tion.

Act. val.

mm The current position of the axes in the MCS or WCS is

displayed in these fields.

Distance

to go The remaining distance to be traversed by these axes in the

MCS or WCS is displayed i n these fields.

Spindle S

rpm Display of actual value and setpoint of spindle speed

Feed F

mm/min or

mm/rev

Display of path feed actual value and setpoint

Tool Display of currently active tool with the current cutting edge

number (T..., D...).

Current

block The block display contains the current block. The block is

output in one line only and truncated if nece ssary.

Actual

feedrate

override

Display of current feedrate override

Actual

spindle

override

Display of current spindlel speed overrid e

Gear stage Display of current gear st age in the machine

Softkeys

The window to select Program Control (e.g. skip block, program test) appears

on the screen.

The window shows the previous, current and next block full length. In addition,

the names of the current program or subroutine are displayed.

Use the Block Search function to jump to the desired point in the program.

The cursor is positioned to the main program block of the breakpoint

(“interrupt point”). The search target is automatically set in the subroutine

levels.

Continue Search

Progr.

control

Zoom

block

Interr.

point

Contin.

Automatic Mode

SINUMERIK 801 5-3

Operation and Program ming

—

Turning

The Start B Search softkey starts the search process in which the same

calculations are carried out as in normal program mode, but without axis

movements.

The block search can be canceled by NC Reset.

The values of the machine or workpiece coordinate system are selected. The

softkey label changes to Act. val. WCS or Act. val. MCS.

Enlarged view of actual values.

Menu extension.

When pressing these softkeys, the Axis Feed or Interp. Feed window appears.

This softkey can be used to change between the windows. The softkey label

changes to Interp. feed when the Axis Feed window is opened.

An external program is transferred into the control system via the RS232

interface and executed immediately by pres sing NC START.

Opens the G Function win dow to display all active G functions.

The G Function window contains all active G functions. Each G function is

assigned to a group and has a fixed position in the window. More G functions

can be displayed by pressing the PAGE UP or PAGE DOWN keys together

with Shift key.

DEM

Fig.5-2 Active G functions window

Opens the M Function win dow to display all active M functions.

Start B

ct.val.

WCS

ct.val.

MCS

Zoom

act.val.

xis

feed

Interp.

feed

Execute

f. ext.

Zoom

G Funkt.

Zoom

M funct.

Automatic Mode

5-4 SINUMERIK 801

Operation and Program ming

—

Turning

5.1 Selecting/starting a part program – “Machine” operating area

Functionality The control system and the machine must be set up before the program is

started. Please note the safety instructions provided by the machine

manufacturer.

Operating sequence

Use the Automatic key to select the Automatic mode.

An overview of all programs stored in the control system is displayed.

Position the cursor bar on the desired program.

Use the Select softkey to select the program for execution. The selected

program name appears in the Program Name screen line.

If necessary you can now make settings on program execution.

The following program control functions can be activated and deactivated:

Fig.5-3 Program control window

The part program is exe cuted when NC START is pressed.

Select

Progr.

control

Programs

Automatic Mode

SINUMERIK 801 5-5

Operation and Program ming

—

Turning

5.2 Block search – “Machine” operating area

Operating sequence Precondition: The desired program has already been selected (cf. Section 5.1),

and the control system is in the reset state.

The block search function can be used to advance the program up to the

desired point in the part program. The search target is set by positioning the

cursor directly on the desi r ed block in the part program.

DEMO.

Fig.5-4 Block search window

This function starts program advance and closes the Search window.

Result of the search The desired block is displayed in the Cu rrent Block window.

Start B

Automatic Mode

5-6 SINUMERIK 801

Operation and Program ming

—

Turning

5.3 Stopping/aborting a part program – “Machine” operating

area

Functionality Part programs can be sto pped and aborted.

Operating Sequence

The execution of a part program can be interrupted by selecting NC STOP.

The interrupted program can be continued by NC START.

The current program can be aborted by pressing RESET.

When you press NC START again, the aborted program is restarted and

executed from the beginning.

Automatic Mode

SINUMERIK 801 5-7

Operation and Program ming

—

Turning

5.4 Repositioning after interruption – “Machine” operating area

Functionality After a program interruption (NC STOP), you can move the tool away from the

contour in the manual mode (Jog). The control system stores the coordinates

of the breakpoint (“interrupt point”). The path differences traversed by the axes

are displayed.

Operating sequence

Select the Automatic mode.

Open the Block Search window to load the breakpoint.

The breakpoint is loaded. The routine is adjusted to the start position of the

interrupted block.

A block search to the breakpoint is started.

Continue execution of the program by NC START.

Interr.

Point

Start B

SINUMERIK 801 6-1

Operation and Program ming

—

Turning

Part Programming 6

Functionality This Section describes how to create a new part program.

The standard cycles can also be displayed provided you have the required

access authorization.

Operating sequence

You are in the main menu.

The Programming main screen appears.

Fig.6-1 Programming main screen

When the Program operating area is selected for the first time, the directory

for part programs and subroutines is automatically selected (see above).

Softkeys

This function selects the program highlighted by the cursor for execution. The

program is started on next NC START.

Opens the files selected by the cursor for editing.

Menu extension

Use the New sof t key to create a new program. A window ap pears in which you

are prompted to enter prog ram na me and type.

After you have confirmed your inputs by OK, the program editor is called, and

you can enter part program blocks. Select RECALL to cancel this function.

Use the Copy softkey to copy the selected program into another program.

Pro-

grams

Open

Cop

Select

New

Part Programming

6-2 SINUMERIK 801

Operation and Program ming

—

Turning

The program highlighted by the cursor is deleted after the system has

requested confirmation of the delete operation.

Press OK to confirm the Delete request and RECALL to cancel it.

When you select the Rename softkey, a window appears in which you can

rename the program that you have already highlighted by the cursor.

After you have entered the new name, confirm your rename request by OK or

cancel by RECALL.

The Programs softkey can be used to change to the program directory.

When you press this softkey, the totally available NC memory (in kbytes) is

displayed.

Delete

Memory

Info

Rename

Part Programming

SINUMERIK 801 6-3

Operation and Program ming

—

Turning

6.1 Entering a new program – “Program” operating area

Functionality This Section describes how to create a new file for a part program. A window

appears in which you are prompted to enter p rogram name and type.

DEMO

Fig.6-2 New program input screen form

Operating sequences

You have selected the Program operating area. The Program Overview

window showing the programs already stored in the CNC is displayed on the

screen.

Press the New softkey. A dialog window appears in which you enter the new

main program or subroutine program name. The extension .MPF for main

programs is automatically entered. The extension .SPF for subroutines must

be entered with the program name.

… Enter the new name.

Complete your input by selecting the OK softkey. The new part program file is

generated and is now ready for editing.

The creation of the program can be interrupted by RECALL; the window is

then closed.

Program

New

Part Programming

6-4 SINUMERIK 801

Operation and Program ming

—

Turning

6.2 Editing a part program – “Program” operating area

Functionality Part programs or sections of a part program can only be edited if not being

executed.

DEMO.MPF

Fig. 6-3 Editor window

Operating sequence

You are in the main menu and have selected the Programs operating area.

The program overview appears autom atically.

Use the paging keys to select the program you wish to edit.

Pressing the open softkey calls the editor for the selected program and pulls

down the editor window.

The file can now be edited. All changes are stored immediately.

Softkeys

User-assignable softkeys

You can assign predefined functions to the softkeys 1 - 4 (see Section 6.3.4

“User-Assignable Sof t keys”).

The softkeys are assigned process-specific functions by the control

manufacturer.

The contour functions are described in Section 6.3 ”Programming Support”.

Menu extension

This function selectes section of text up to the current cursor position.

Contou

Edit

Mark

Programs

open

Part Programming

SINUMERIK 801 6-5

Operation and Program ming

—

Turning

This function deletes the selected text.

This function copies sele cted text to the clipboard.

This function inserts text from the clipboard at the current cursor position.

For re-compilation, the cursor must stand on the cycle call line in the program.

The required parameters must be arranged directly in front of the cycle call

and may not be separated by instruction or comment lines. The function

decodes the cycle name and prepares the screen form with the respective

parameters. If there are any parameters are outside the validity range, the

function automatically uses standard values. When the screen form has been

quitted, the original parameter block is automatic ally replaced by the corrected

one.

Note: Only automatically generated blocks can be recompile d.

Note

To carry out these functions outside the Edit menu, it is also possible to use

the key combinations <SHIFT> and

softkey 1 Select

softkey 2 Delete block

softkey 3 Copy block

softkey 4 Insert block.

Menu extension

This function can be used to change the assignment of the softkey functions 1

- 4.

For more detail description refer to Secti on NO TAG.

The softkeys Search and Contin. Search can be used to search for a string

chain in the program file displayed on the screen.

Type the text you wish to find in the input line and start the Search operation

by selecting the OK softkey.

If the character string you have specified cannot be found in the program file,

an error message appears that must be ackno wle dged with OK.

You can exit the dialog box without starting the search by selecting RECALL.

Type the line number in the input line.

The search is started by pressing OK.

You can quit the dialog box without starting the se arch by selecting RECALL.

This function can be used to continuously search through the file to find

another character string that matches the target string.

Delete

Cop

Past

Recomp.

cycles

ssign

Text

Line no.

Contin.

Part Programming

6-6 SINUMERIK 801

Operation and Program ming

—

Turning

This function stores the changes in the file system and automatically closes

the file.

Part Programming

SINUMERIK 801 6-7

Operation and Program ming

—

Turning

6.3 Programming support

Functionality The programming support facility contains various help levels simplifying the

programming of p art programs without constraining your choi ce of inputs.

6.3.1 Vertical menu

Functionality The vertical menu is displayed in the program editor.

The vertical menu allows you to quickly insert certain NC instructions into the

part program.

Operating sequence

You are in the program editor.

Press the VM key and select the desired instruction from the list.

Fig.6-4 Vertical menu

Lines that end in “...” contain a collection of NC instructions. You can list these

instructions by pressing the Input key or entering the number of the line.

Fig.6-5 Vertical menu

Use the paging keys to browse through the list.

Part Programming

6-8 SINUMERIK 801

Operation and Program ming

—

Turning

Confirm your entry by pressing Input.

Alternatively, the number of the lines from 1 to 7 can be entered to select

instructions and take them over into the pa rt program.

6.3.2 Cycles

Functionality You can either specify your own machining cycles on assigning parameters or,

alternatively, use input forms in which you set all the necessary R parameters.

Operating sequences

The screen forms are selected either with the available softkey functions or by

means of the vertical menu.

Fig.6-6

The cycle support provides a screen form in which you can fill in all the

necessary R parameters. A graphic and a context-sensitive help will assist you

to fill in the form.

Select the OK softkey to transfer the generated cycle call to the part program.

LCYC 93

LCYC 94

Part Programming

SINUMERIK 801 6-9

Operation and Program ming

—

Turning

6.3.3 Contour

Functionality The control system provides you with various contour forms to assist you in

creating part programs quickly and reliably. Enter the necessary parameters in

the screen forms and confirm your inputs.

The contour screen forms can be used to program the following contour

elements and contour sections:

z Straight section with specification of end point or an gle

z Circle sector with specification of center point / end point

z Circle sector with specification of center point / opening angle

z Circle sector with specification of center point / radius

z Straight line/straight line contour section with specification of angle and

end point

z Straight line/circle contour section with tangential transition; calculated

from angle, redius and end point

z Straight line/circle contour section with any transition; calculated from

angle, center point and end point

z Circle/straight line contour section with tangential transition; calculated

from angle, radius and end point

z Circle/straight line contour section with any transition; calculated from

angle, center point and end point.

z Circle/circle contour section with tangential transition; calculated from

center point, radius and end point

z Circle/circle contour section with any transition; calculated from center

point and end positon

z Circle - straight line - circle contour section with tangential transitions

z Circle - circle - circle contour section with t angential transitions

Fig.6-7

Softkeys

The sofkey functions bran ch to the contour elements.

Programming aid for programming straight line sections.

Part Programming

6-10 SINUMERIK 801

Operation and Program ming

—

Turning

Fig.6-8

Enter the end point of the straight line.

The block is traversed either at rapid traverse or with the programmed

feedrate.

The end point can be entered either in the absolute dimension, as an

incremental dimension (referred to the starting point) or in polar coordinates.

The current setting is displayed in the interactive dialog screenfor m.

The end point can also be specified by a coordinate and the angle between

the 1st axis and the straight line.

If the end point is determined using polar coordinates, the length of the vector

between pole and end point is required, as well as the angle of the vector with

reference to the pole. When using the possibility, first a pole must be set.

Fig.6-9

Pressing the OK softkey takes over the block into the part program and

displays the Additional Functions form in which you can extend the block by

adding more instructions.

G0/G1

Part Programming

SINUMERIK 801 6-11

Operation and Program ming

—

Turning

Additional functions

Fig.6-10 Additional functions screen form

Enter additional commands in the fields. The commands can be separated by

means of blanks, commas or semi-colons.

This screen form is available for all contour elements.

The OK softkey transfers the command s to the part program.

Select RECALL if you wish to exit the interactive form without saving the

values.

The dialog screen form is used to create a circular block by means of the end

and center point coordinates.

Fig.6-11

Enter the center point coordinates in the input fields.

To enter the coordinates, there are three variants:

z absolute

z incremental

z polar

This softkey changes the direction of rotation from G2 to G3. G3 appears on

the display.

When you press the softkey again, you will return to G2.

Pressing the OK softkey will accept the block into the part program and will

offer additio nal commands in another intera ctive screenform.

G2/G3

Part Programming

6-12 SINUMERIK 801

Operation and Program ming

—

Turning

This function is intended to calculate the intersection point between two

straight lines.

Specify the coordinates of the end point of the second straight line and the

angles of the straight line. For the coordinate value, the toggle key can be

used to choose between absolute, increment al or polar coordinates.

If the starting point cannot be selected based on the previous blocks, the

operator must set the st arting point.

Fig. 6-12 Calculating the intersection point between two straight lines

Table 6–1 Input in the interactive screenform

End point of

straight line 2 E Specify the end point of the straight line.

Angle of

straight line 1 A1 The angle must be specified in the CCW direction in

the range between 0 and 360 degrees.

Angle of

straight line 2 A2 The angle must be specified in the CCW direction in

the range between 0 and 360 degrees.

Feedrate F Feedrate

This function is used to calculate the tangential transition between a straight

line and a circle sector. The straight line must be described by starting point

and angle. The circle must be described by the radius and by the end point.

To calculate intersection points with any transition angles, the POI softkey

function will display the center point coordinates.

Fig. 6–13 Straight line - circle with tangential transitio n

Part Programming

SINUMERIK 801 6-13

Operation and Program ming

—

Turning

Table 6–2 Input in the interactive screenform

Circle end

point E The end point of the circle must be specified.

Straight line

angle A The angle is specified in the CCW direction in the

range between 0 and 36 0 degrees.

Circle radius R Input field for the circle radius.

Feed F Input field for the interpolation feed.

Circle center

point M If there is no tangential transition between the straight

line and the circle, the circle center must be known.

The circle center point is specified depending on the

calculation method (absolute or incremental dimension

/ polar coordinates) selected in the previous block.

This softkey is used to switch the direction of rotation from G2 to G3. G3 is

displayed on the screen. Pressing this softkey once more will switch the

display back to G2.

The end point can be acquired either in the absolute dimension, incremental

dimension or as polar coordinates.

The current setting is displayed in the interactive screenform.

You can choose between tange ntial or any transition.

If the starting point cannot be determined from the previous blocks, the

starting point must be set by the operator.

The screenform will generate a straight line and a circle block from the

entered data.

If there are several intersection points, the operator must select the desired

intersection point from a dialog.

If a coordinate was not entered, the program tries to caluclate it from the

existing information. If there are several possibilities, the operator must

choose an appropriate possibility from the dialog.

This function is used to calculate the tangential transition between a circle

sector and a straight line. The circle sector must be described by the

parameters starting point and radius, and the straight line must be described

by the parameters end point and angle.

Fig. 6–14 Tangential transition

G2/G3

G90/G91

POI

Part Programming

6-14 SINUMERIK 801

Operation and Program ming

—

Turning

Table 6–3 Input in the interactive screenform

Straight line end point E Enter the end point of the straight line either in

absolute, incremental or polar coordinates.

Center point M The center point of the circle must be entered

either in absolute, incremental or polar

coordinates.

Circle radius R Input field for the circle radius.

Angle of straight line 1 A The angle is specified in the CCW direction in

the range between 0 and 360 degrees.

Feedrate F Input field for the interpolation feedrate.

This softkey is used to switch the direction of rotation from G2 to G3. G3 is

displayed on the screen. Pressing this softkey once more will switch back to

G2; the display will change to G2.

Use this softkey to choose between tangential or any transition.

If the starting point cannot be generated from the previous blocks, the starting

point must be set by the operator.

The screenform will generate both a straight line and a circle block based on

the entered data.

If there are several intersection points, the desired intersection point must be

selected by the operator from a dialog box.

This function is used to caluclate the tangential transition between two circle

sectors. Circle sector 1 must be described by the parameters starting point

and center point, and circle sector 2 must be described by the parameters end

point and radius.

To avoid an overdetermination, input fields not needed are hidden.

Fig. 6–15 Tangential transition

Table 6–4 Input in the interactive screenform

End point of circle 2 E 1st and 2nd geometry axis of the plane

Center point of circle 1 M1 1st and 2nd geometry axis of the plane

Radius of circle 1 R1 Radius input field

Center point of circle 2 M2 1st and 2nd geometry axis of the plane

Radius Kreis 2 R2 Radius input field

Feedrate F Input field for the interpolation feedrate

The points are specified depending on the previsouly selected caluclation

method (absolute, incremental dimension or polar coordinates). Input fields no

longer needed are hidden. If a value is omitted in the center point coordinates,

the radius must be entered.

G2/G3

POI

Part Programming

SINUMERIK 801 6-15

Operation and Program ming

—

Turning

This softkey is used to switch the direction of rotation from G2 to G3. G3 is

displayed on the screen. Pressing this softkey once more will switch back to

G2; the display will change to G2.

Use this softkey to choose between tangential or any transition.

If the starting point cannot be generated from the previous blocks, the starting

point must be set by the operator.

The screenform will generate two circle blocks based on the entered data.

Selecting the intersection point

If there are several intersection points, the desired intersection point must be

selected by the operator from a dialog box.

Fig. 6–16

The contour is drawn using intersection point 1.

Fig. 6–17 Selection of intersection point 1

The contour is drawn using intersection point 2.

G2/G3

POI

POI 1

POI 2

Part Programming

6-16 SINUMERIK 801

Operation and Program ming

—

Turning

Fig. 6–18 Selection of intersection point 2

Pressing this softkey will accept the intersection point of the displayed contour

into the part program.

This function is used to insert a straight line tangentially between two circle

sectors. The sectors are determined by their center points and their radii.

Depending on the selected direction of rotation, different tangential

intersection points result.

Use the screenform, which will appear, to enter the parameters center point

and radius for sector 1, as well as the parameters end point, center point and

radius for sector 2. In addition, the direction of rotation must be selected for

the circles. The current setting is displayed in a help screen.

The end and center points can be acquired either as absolute, incremental or

polar coordinates.

The OK function will calculate three blocks from the given values and will

insert them into the part program.

Fig. 6–19 Screenform for calculating the contour section ‘circle - straight line -

circle’

Part Programming

SINUMERIK 801 6-17

Operation and Program ming

—

Turning

Table 6–5 Input in the interactive screenform

End point E 1st and 2nd geometry axes of the plane

If no coordinates are entered, the function will provide

the intersection point between the inserted circle

sector and sector 2.

Center point

of circle 1 M1 1st and 2nd geometry axes

Radius of

circle 1 R1 Input field for radius 1

Center point

of circle 2 M2 1st and 2nd geometry axes of the plane

Radius of

circle 2 R2 Input field for radius 2

Feedrate F Input field for the interpolation feedrate

If the starting point cannot be determined based on the previous blocks, the

appropriate coordinates must be entered in the “Starting point” screenform.

The screenform will generate both a straight line and two circle blocks based

on the entered data.

G2/G3 Use this softkey to define the direction of rotation of the two circle sectors. You

can choose between

Sector 1 Sector 2

G2 G3,

G3 G2,

G2 G2 and

G3 G3

The end point and the center points can be acquired either in absolute,

incremental or polar coordinates. The current setting is displayed in the

interactive screenform.

Example DIAMON

Fig. 6–20 Setting the st arting point

Given: R1 50 mm

R2 100 mm

R3 40mm

M1 Z -159 X 138

Part Programming

6-18 SINUMERIK 801

Operation and Program ming

—

Turning

M2 Z -316 X 84

M3 Z -413 X 292

Starting point: The point X = 138 and Z = -109 mm (-159 -R50) is supposed as

the starting point.

Fig. 6–21 Setting the starting point

After the starting point has been confirmed, the screenform can be

used to calculate the contour sectio n - - .

Use softkey 1 to set the direction of rotation of the two circle sectors and to fill

out the parameter list.

The end point can be left o pen.

Fig. 6–22 Calling the screenform

Fig. 6–23 Result of step 1

After you have filled out the screenform, press OK to quit the screenform. The

intersection points are caluclated and the two blocks are generated.

Since the end point has been left open, the intersection point between the

straight line and the circle sector is also the starting point for the

subsequent contour definition.

Now, call the screenform for calculating the contour section - again.

The end point of the contour se ction are the coordinates Z=-413.0 and X=212.

Part Programming

SINUMERIK 801 6-19

Operation and Program ming

—

Turning

Fig. 6–24 Calling the screenform

Fig. 6–25 Result of step 2

This function is used to insert a circle sector tangentially between two adjacent

circle sectors. The circle sectors are described by their center points and their

circle radii. The inserted sector is described by its ra dius.

Use the screenform to enter the parameters center point and radius for circle

sector 1, and the parameters end point, center point and radius for circle

sector 2. in addition, the radius for the inserted circle sector 3 must be entered

and the direction of rot ation be defined.

The end point and the center points can be acquired either as absolute,

incremental or pola r co ordinates.

The selected setting is displayed in a help screen.

The OK function will caluclate three blocks from the given values and will

insert them into the part program.

Fig. 6–26 Screenform for calculatin g the contour section ‘cir cle - circle - circle’

Part Programming

6-20 SINUMERIK 801

Operation and Program ming

—

Turning

Table 6–6 Input in the dialog screenform

End point E 1st and 2nd geometry axes of the plane

If no coordinates are entered, the function

provides the intersection point between the

inserted circle sector and sector 2.

Center point of circle 1 M1 1st and 2nd geometry axes of the plane

Radius of circle 1 R1 Input field for radius 1

Center point of circle 2 M2 1st and 2nd geometry axes of the plane

Radius of circle 2 R2 Input field for radius 2

Radius of circle 3 R3 Input field for radius 3

Feedrate F Input field for the interpolation feed

If the starting point cannot be deteremined from the previous blocks, the

respective coordinate s mu st be entered in the “Starting point” scree nform.

G2/G3 This softkey defines the direction of rotation of the three circles. It is possible

to select between:

Sector 1 Inserted Sector Sector 2

G2 G 3 G2,

G2 G2 G2,

G2 G2 G3,

G2 G3 G3,

G3 G2 G2,

G3 G3 G2,

G3 G2 G3,

Example DIAMON - G23

Fig.6-27

Given: R1 39 mm

R2 69 mm

R3 39 mm

R4 49 mm

R5 39 mm

M1 Z -111 X 196

M2 Z -233 X 260

M3 Z -390 X 162

Part Programming

SINUMERIK 801 6-21

Operation and Program ming

—

Turning

The coordinates Z -72, X 196 will be selected as the starting point.

After you have confirmed the starting point, use the screenform to

caluclate the contour section - . The end point is left open, since the

coordinates.

Use softkey 1 to set the direction of rotation of the two circles (G2 - G3 - G2)

and to fill out the parameter list.

Fig. 6–28 Setting the starting point

Fig. 6–29 Screenform ‘circle - circle - circle’

Fig.6-30 Result of step 1

In the second step, screenform is used to calculate the contour section

- . For calculation, select direction of rotation G2 – G3 – G2. Starting

point is the end point of the first caluclation.

Part Programming

6-22 SINUMERIK 801

Operation and Program ming

—

Turning

Fig. 6–31 Screenform ‘circle - circle - circle’

Fig. 6–32 Result of step 2

The result provided by the function is the intersection point between circle

sector 4 and circle sector 5 as the end point.

To calculate the tangential transition between and , the circle-straight

line screenform is used.

Fig. 6–33 Screenform ‘circle - straight line’

Part Programming

SINUMERIK 801 6-23

Operation and Program ming

—

Turning

Fig. 6–34 Result of step 3

This function is used to insert a circle sector (with tangential transitions)

between two straight lines. The circle sector is described by the center point

and the radius. The coordinates of the end point of the second straight line

and, optionally, angle A2. The first straight line is described by the starting

point and the angle A1.

If the starting point cannot be determined from the previous blocks, the

starting point must be set by the operator.

Fig. 6–35 Straight line - circle - straight line

Table 6–7 Input in the interactive screenform

End point of straight line 2 E Enter the end point of the straight line.

Circle center point M 1st and 2nd axes of the plane

Angle of straight line 1 A1 The angle must be specified in the CCW

direction.

Angle of straight line 2 A2 The angle must be specified in the CCW

direction.

Feedrate F Input field for the feedrate

End and center points can be specified either in absolute, incremental or polar

coordinates. The screenform will generate a circle and two straight line blocks

from the entered data.

Use this softkey to switch the direction of rotation from G2 to G3. G3 is

displayed on the screen. Pressing this softkey once more will switch back to

G2; the display will change to G2.

G2/G3

Part Programming

6-24 SINUMERIK 801

Operation and Program ming

—

Turning

6.3.4 Free softkey assignment

You can assign the softkeys various cycles or contours. To this aim, the

softkeys 1 to 4 in the softkey bar in the Program operating area are provided.

Once you have activated the Assign softkeys function, a list of all available

cycles or contours appears on the screen.

Fig.6-36

Position the cursor on the element you wish to assign.

Press the desired softkey from 1 to 4 to assign them the desired element. The

assignment you have made appears in the softkey bar under the selection list.

Confirm the assignment you have made by selecting the OK softkey.

ssign

SINUMERIK 801 7-1

Operation and Program ming

—

Turning

Services and Diagnosis 7

7.1 Data transfer via the RS232 Interface

Functionality You can use the RS232 interface of the CNC to output data to an external

data storage medium or to read in them from there. RS232 interface

parameters h ave been fixe d by the control system and cannot be changed.

After you have selected the Services operating area, a list of all available part

programs and sub ro utines appears on the screen.

Fig.7-1 Service main screen

Communication tool The RS232 communication tool WinPCIN shall be loaded onto the PC (you

may download corresponding tool on website at:

www.ad.siemens.com.cn/download/) and baudrate be set as 9600. For

detailed information about baudrate setting and softeware tool version, see Fig.

7-2 and 7-3 below.

Services and Diagnosis

7-2 SINUMERIK 801

Operation and Program ming

—

Turning

Fig. 7-2

Fig.7-3

File types Provided the access authorization is set, files can be read in or read out via

the RS232 interface.

File type has been fixed as: RS232 text Baudrate: 9600

If the access authorization is set (cf. Technical Manual), the following data can

be transmitted:

z Data

— Machine data

— Setting data

— Tool data

— R param eters

— Zero offsets

— Leadscrew error compensation

z Part programs

Services and Diagnosis

SINUMERIK 801 7-3

Operation and Program ming

—

Turning

— Part programs

— Subroutines

Operating Sequence

Use the Service softkey to select the Services o perating area.

Softkeys

This key start s reading in data.

This key sta rts reading out data to the PG/PC or another device.

A log is output for the transferred dat a.

z For files to be output, it contains

— the file name and

— an error acknowledgement

z For imported files, it cont ains

— the file name and the path spe cification

— an error acknowledgement

Transmission messages:

OK Transmission completed suc cessfully

ERR EOF End-of-file character received, but the archive file is not

complete.

Time Out Timeout monitoring is signaling an interruption in the

transmission.

User Abort Transmission aborted by Stop softkey

Error Com Error at COM 1

NC / PLC Error NC error message

Error Data Data errors

1. Files read in with/without leader

2. Files transferred in tape format without file name

Error File Name The file name does not comply with NC name

conventions.

no access right No access right for this function

Display of the data that are amongst the data types marked with “...”. Use this

function to transfer individual files.

Data In

Start

DataOut

Start

Error

log

Show

Service

Services and Diagnosis

7-4 SINUMERIK 801

Operation and Program ming

—

Turning

7.2 Diagnosis and start-up – “Diagnostics” operating area

Functionality In the “Diagnosis” operating area, you can call service and diagnostic

functions, set start-up switches, etc.

Operating sequence

Selecting the Diagnosis softkey will open the Diagnosis main screen.

Fig.7-4 Diagnosis main screen

Softkeys for diagnostic functions

This window displays all pending alarms line by line, starting with the alarm

with the highest priority.

Alarm number, cancel criterion and error text are displayed. The error text

refers to the alarm number on which the cursor is po sitione d.

Explanations with regard to the screenform above:

z Number

The “Number” item displays the alarm number. The alarms are displayed in

chronological sequence.

z Cancel criterion

The symbol of the key required to reset the alarm is displaye d for every alarm.

— Switch the device off and o n again.

— Press the RESET key.

— Press the “Acknowledge alarm” key.

— Alarm is reset by NC START.

z Text

The alarm text is displayed.

The Service Axes window appears on th e screen.

Diagnosis

larms

Service

displa

Services and Diagnosis

SINUMERIK 801 7-5

Operation and Program ming

—

Turning

The window displays information about the axis drive.

Fig. 7–5 The “Service Axes” window

Notice

“Servo trace” function is valid for machine manufacturers only. Machine

manufacturer may select the “Servo trace” softkey on the screen of Fig.7-5 to

branch to the corresponding “Servo trace” main screen. However, before

entering this main screen, machine manufacturer password must first be input.

Otherwise, system will prompt “Access Denied!”

In addition, the Axis+ and Axis– softkeys are displayed. They can be used to

call the values for the next or previous axis.

This window contains the version numbers and the creation date of the

individual CNC component s.

displays the control type

Service

axes

Version

Type

Services and Diagnosis

7-6 SINUMERIK 801

Operation and Program ming

—

Turning

Fig. 7–6 Control type

OEM displays the OEM picture here.

Softkeys for start-up fun ctions

Note

See also Technical Manual

The start-up functio n bran ches to the following softkey functions:

Fig. 7–7

Start-up switch

You can assign the system power-up parameters various parameters.

Start-up

switch

Services and Diagnosis

SINUMERIK 801 7-7

Operation and Program ming

—

Turning

Caution

Changes in the start-up branch have a considerable influence on the machine.

Fig. 7–8 NC Start-up

Notice

If the fuction “record of reference point” has been executed (with MD34210),

do approach reference point again after system power up with saved data!

Use the OK key to start the NC start-up.

Return to the Start-up main screen without further action by RECALL.

You can display information about the current states of PLC memory cells

listed below; if desired they can be altered.

It is possible to display 6 operands simultaneously.

Inputs I Input byte (IBx), input word (Iwx), input double word (I Dx)

Outputs Q Output byte (Qbx), output word (Qwx), output double

word (QDx)

Bit

memories M Memory byte (Mx), memory word (Mw), memory double

word (MDx)

Timers T Timer (Tx)

Counters C Counter (Zx)

Data V Data byte (Vbx), data word (Vwx), data double word

(VDx)

Format B

Binary

Hexadecimal

Decimal

Binary representation cannot be used for double words.

Counters and timers are displayed in decimal format.

PLC

status

Services and Diagnosis

7-8 SINUMERIK 801

Operation and Program ming

—

Turning

Fig. 7–9 PLC status display

There are further softkeys provided un der this menu item.

z Edit

Cyclic updating of the values is interrupted. You can then edit the operand

values.

z Cancel

Cyclic updating continues without the entered values being transferred to the

PLC.

z Accept

The entered values are transferred to the PLC; cyclic updating continues.

z Delete

All operands are deleted.

z Operand +

The address of the operand can be incremented in steps of 1.

z Operand –

The address of the operand can be decremented in steps of 1.

Click on ETC key on Fig. 7-7 to branch into the lower-level screen, then you

may execute “Set password”, “Delete password”, “Change password” and

“Save data” softkey functions.

Set password

There is only one password level available for machine tool builders, i.e.:

z Manufacturer password

Set

password

Services and Diagnosis

SINUMERIK 801 7-9

Operation and Program ming

—

Turning

Fig. 7-10 Enter the password.

If you do not know the password, you will not be granted access.

The password is set when you press the OK softkey.

You can return to the Start-up main screen without saving your input by

selecting RECALL.

The access authorization is reset.

Change password

Fig. 7–11

With the access authorization, pa ssword can be chan ged.

Use the softkeys to enter the new password and complete your input with OK.

The system asks you to confirm the new password again.

Press OK to complete the password change.

You can return to the Start-up main screen without saving your input by

RECALL.

Delete

password

Change

password

Services and Diagnosis

7-10 SINUMERIK 801

Operation and Program ming

—

Turning

Save data

This function saves the contents of the volatile memory to a non-volatile

memory area.

Prerequisite: No program is currently being run.

It is not allowed to perform any operating actions while saving data.

Softkeys for service functions

Machine data (see also Technical Manual)

Fig.7-12

Changes to the machine data have a considerable influence on the machine.

Incorrect parameter settings can result in irreparable damage to mechanical

components.

userdef User-defined

M/s**2 Meters per secon d

U/s**3 Revolutions per second

S Second

Kgm**2 Moment of inertia

MH Inductivity

Nm Torque

µs Microseconds

µA Microamperes

Units

µVs Microvolt seconds

So Effective immediately

Cf With confirmation

Re Reset

Effective

ness

Po Power ON

General machine data

Open the General Machine Data window. Use the paging keys to page up and

down.

Axis-specific machine data

Open the Axis-Specific Machine Data window. The softkey bar is extended by

Save

data

Machine

data

General

xis

Services and Diagnosis

SINUMERIK 801 7-11

Operation and Program ming

—

Turning

the Axis + and Axis – softkeys.

Fig.7-13

The data of the X axis is displayed.

Enter the number or name of the machine data you want to find and press

Input.

The cursor jumps to the t arget data.

Fig. 7–14

The search for the next number or name continues.

The Axis + and Axis – softkeys are used to switch over to the machine data

area of the next or previous axis.

Continue

xis +

xis –

Services and Diagnosis

7-12 SINUMERIK 801

Operation and Program ming

—

Turning

This softkey is used to activate the machine data marked with “cf”.

When the screen as shown in Figure 7-4 is displayed, press ETC key to

proceed to the next sub-screen, on which you will see softkey “Display bright

“Display darker” as well as “”Change lang.”. Press “Display bright” for more

brightness.

This softkey can be used to adjust the brightness of the screen.

Display

bright.

Display

darker

ctive

Services and Diagnosis

SINUMERIK 801 7-13

Operation and Program ming

—

Turning

SINUMERIK 801 8-1

Operation and Program ming

—

Turning

Programming 8

8.1 Fundamentals of NC programming

8.1.1 Program structure

Structure and contents

The NC program consists o f a sequence of blocks (see Table NO TAG).

Each block constitutes a machining step.

Instructions are written in a block in the form of word s.

The last block in the sequence contains a special word for the end of program:

M2.

Table 8–1 NC program structure

Block Word Word Word ... ; Comment

Block N10 G0 X20 ... ; 1st block

Block N20 G2 Z37 ... ; 2nd block

Block N30 G91 ... ... ; ...

Block N40 ... ... ...

Block N50 M2 ; End of program

Program names Every program has its own program name.

Note

When generating the program, its name can be freely chosen provided the

following conditions are complied with:

z The first two characters must be letters.

z Otherwise letters, digits or underscore may be used.

z Do not use more than 8 characters.

z Do not use separators (see Section “Character Set”)

Example: SHAFT52/

Programming

8-2 SINUMERIK 801

Operation and Program ming

—

Turning

8.1.2 Word structure and address

Functionality/structure

The word is an element of a block and is mainly a control instruction.

The word (see Fig. (8-1) consists of

z an address character

The address character is gene rally a letter,

z and a numerical value.

The numerical value consists of a sequence of digits. A preceding sign or a

decimal point can be adde d to this sequence for certain addresses.

A positive sign (+) can be omitted.

Fig.8-1 word structure

Several address characters

A word may also contain several address letters. In such cases, however, an

“=” sign must be inserted to assign the n umerical value to the address letters.

Example: CR=5.23

Word

ddress Value

Example: G1 X–20.1 F300

Word

ddress Value

Word

ddress Value

Explanation: Traverse

with linear

interpolation

Path or end

position for X

axis: -20.1 mm

Feed:

300 mm/min

Programming

SINUMERIK 801 8-3

Operation and Program ming

—

Turning

8.1.3 Block structure

Functionality A block should contain all data required to execute a machining step.

The block generally consists of several words and always ends with the

end-of-block character “LF” (line feed). This character is automatically

generated when the carriage return or Input key is pressed during typing.

Fig.8-2 Diagram of block structure

Word sequence When a block contains more than one statement, the words in the block

should be arranged in the following sequence:

N... G... X... Y... Z... F... S... T... D... M...

Note with regard to the block numbers

Select the block numbers first in steps of 5 or 10. This will allow you to insert

blocks later while retaining the ascending order of the block numbers. (No

matter how big a block number is, it will not have any influence on the

program executing sequence. Every program can be executed in an order of

from top to down or in sequences marked by the block skipping symbol.)

Block skipping (see Fig. 5–3)

Program blocks that must not be executed during every program run can be

marked with a slash “ / ” in front of the block number word.

Block skipping is activated by means of an operator input or by the interface

control (signal). A program section can be skipped by skipping several

successive blocks with “ / ”.

If block skipping is active during program execution, none of the blocks

marked with “ / ” is executed. Any statements contained in such blocks are

ignored. The program continue s at the next block not marked.

Comment, remark Comments (remarks) can be used to explain the staements in the blocks of a

program.

Comments are displayed together with the other contents of the block in the

current block displ ay.

Note: Chinese comments (remarks) can be entered via a PC only. It’s

/N…

Word1 Word2 … Wordn ;Comment L F

end-of-block

character

Only if necessary,

stands at the end,

separated from the

rest of the block with

“;”

BLANK BLANK BLANK BLANK

Block instructions

Block number- stands in front of the

instructions; Only if necessary,

instead of “N”, a colon “:” is used in

main blocks

Skip block, only if necessary,

stands in the begining Total number of characters in a block: 127

Programming

8-4 SINUMERIK 801

Operation and Program ming

—

Turning

impossible to enter Chinese comments (remarks) via the operator panel.

Programming example

N10 ;G&S Order No. 12A71

N20 ;Pump part 17, Drawing No.: 123 677

N30 ;Program created by Mr. Adam Dept.TV 4

N50 G54 G94 F470 S20 D0 M3

N60 G0 G90 X100 Z200

N70 G1 Z185.6

N80 X112

/N90 X118 Z180 ;Block can be skipped

N100 X118 Z120

N110 X135 Z70

N120 X145 Z50

N130 G0 G90 X200

N140 M2 ;End of program

Programming

SINUMERIK 801 8-5

Operation and Program ming

—

Turning

8.1.4 Character set

The following characters can be used for programming and are interpreted

according to the following definitions:

Letters A, B, C, D, E, F, G, H, I, J, K, L, M, N,O, P, Q, R, S, T, U, V, W X, Y, Z

No distinction is made between upper-case and lower-case letters.

Lower-case letters are therefore equivalent to upper-case letters.

Digits 0, 1, 2, 3, 4, 5, 6, 7, 8, 9

Printable special charac ters

( Left round bracket

) Right round bracket

[ Left square bracket

] Right square bracket

< Less than

> Greater than

: Main block, label termination

= Assignment, equals

/ Division, block skip

* Multiplication

+ Addition, positive sign

- Subtraction, negative sign

“ Quotation marks

_ Underscore (together with letters)

. Decimal point

, Comma, separator

; Start of comment

% Reserved, do not use

& Reserved, do not use

’ Reserved, do not use

$ Reserved, do not use

? Reserved, do not use

! Reserved, do not use

Non-printable special characters

F End-of-block character

Blank Separator between words, blank

Tabulator Reserved, do not use.

Programming

8-6 SINUMERIK 801

Operation and Program ming

—

Turning

8.1.5 Overview of instructions

Address Meaning Value assignment Information Programming

D Tool

compensation

number

0 ... 9, integers only,

without sign Contains compensation data for a

particular tool T... ; D0->compensation

values= 0,

max. 9 D numbers for one tool

D...

F Feedrate

(in combination

with G4, the

dwell time is also

programmed

under F)

0.001 ... 99 999.999 Tool/workpiece path velocity

in mm/min or mm/rev

depending on whether G94 or G95 is

programmed

F...

G G function

(preparatory

function)

Only specific integer

values The G functions are divided into G

groups. Only one

G function of a G group can be

programmed in any one b l ock.

A G function can be modal (until

canceled by another function of the

same group) or non-modal - it is only

active for the block in which it is

programmed.

G group:

G...

G0 Linear interpolation with rapid traverse G0 X... Z...

G1 * Linear interpolation with feed G1 X... Z... F...

G2 Circular interpolation in clockwise

direction G2 X... Z... I... K...

F...

;center point and

end point

G2 X... Z... CR=...

F...

;Radius and end

point

G2 AR=... I... K...

F...

;Angle of aperture

and center point

G2 AR=... X... Z...

F...

;Angle of aperture

and end point

G3 Circular interpolation in

counterclockwise direction G3 .... ;otherwise

as for G2

G5 Circular interpolation via interpolation

point

1: Motion commands

(interpolation type)

G5 X...Z...

IX=...KZ=... F...

G33 Thread cutting with constant pitch Modal G33 Z... K... SF=...

;Cylindrical thread

G33 X... I... SF=...

;Cross thread

G33 Z... X... K...

SF=...

;Tapered thread,

path greater in Z

axis than in X axis

G33 Z... X... I...

SF=...

;Tapered thread,

path greater in X

axis than in Z axis

Programming

SINUMERIK 801 8-7

Operation and Program ming

—

Turning

Address Meaning Value assignment Information Programming

G4 Dwell time G4 F... or G4 S....

;in separate block

G74 Reference point approach G74 X...Z...

;in separate block

G75 Fixed point approach

2: Special movements,

non modal

G75 X... Z...

;in separate block

G158 Programmable offset G158 X...Z...

;in separate block

G25 Lower spindle speed limit G25 S...

;in separate block

G26 Upper spindle speed limit

3: Write to memory

non modal

G26 S...

;in separate block

G17 (required for end face drilling)

G18 * Z/X plane 6: Plane selection

G40 * Tool radius compensation OFF

G41 Tool radius compensation left of

contour

G42 Tool radius compensation right of

contour

7: Tool radius compensatio n

modal

G500 * Settable zero offset OFF

G54 1st settable zero offset

G55 2nd settable zero offset

G56 3rd settable zero offset

G57 4th settable zero offset

8: Settable zero offset

modal

G53 Non–modal suppression of settable

zero offset 9: Suppression of settable zero offset

non modal

G60 * Exact positioning

G64 Continuous path mode 10: Approach behaviour

modal

G9 Non-modal exact stop 11: Non–modal exact positio ning

non–modal

G601 * Exact positioning window fine for G60,

G602 Exact positioning window coarse for

G60, G9

12: Exact positioning window

modal

G70 Dimensions in inches

G71 * Dimensions in metric values 13: Dimensions in inches/metric values

modal

G90 * Absolute dimensions

G91 Incremental dimensions 14: Absolute/in cremental dimension

modal

G94 Feedrate F in mm/min

G95 * Feedrate F in mm/revolution of spindle

G96 Constant cutting speed for t urning ON

(F in mm/rev, S in m/min) G96 S... LIMS=...

F...

G97 Constant cutting speed for turning OFF

15: Feedrate/spindle

modal

G450 * Transition circle

G451 Point of intersect i on 18: Behaviour at corners with tool radius

compensation

modal

G22 Radius input

G23 * Diameter input 29: Radius/diameter input

modal

The functions marked with an * are active from the begin ni n g of t he program ( with the ver sion

of the control supplied unless otherwise programmed).

Programming

8-8 SINUMERIK 801

Operation and Program ming

—

Turning

Address Meaning Value assignment Information Programming

I Interpolation parameter

± 0.001 ... 99 999.999

thread:

0.001 ... 2000.000

For X axis, meaning depends on

whether G2,G3->circle center or

G33->thread pitch has been

programmed

see G2, G3 and

G33

K Interpolation parameter

± 0.001 ... 99 999.999

thread:

0.001 ... 2000.000

For Z axis, other wise as for I see G2, G3 and

G33

L Subroutine, name and

call 7 decimal places,

integers only, without

sign

Instead of a user–defined name

L1 ...L9999999 can also be

selected;

this also calls the subroutine in

its own block

Caution: L0001 is not the same

as L1

L....

;in sepa rate blo ck

M Miscellaneous function 0 ... 99

integers only, no sign E.g. to trigger actions

such as ”coolant ON”,

max. 5 M functions in one block,

M...

M0 Programmed stop Machining is stopped at the end

of a block containing M0,

operation is continued with

“START”

M1 Optional stop As for M0, but operation only

stops if a special signal has been

given

M2 End of program Programmed in the last block to

be executed

M30 - Reserved, do not use

M17 - Reserved, do not use

M3 Spindle clockwise rotation

M4 Spindle counterclockwise rotation

M5 Spindle stop

M6 Tool change Only if activated with M6 in

machine data, otherwise tool

change performed directly with T

command

M40 Automatic gear stage switchover

M41 bis

M45 Gear stage 1 to

gear stage 5

M70 - Reserved, do not use

M... Other M functions This functionality is not

predefined in the cont rol and can

therefore be assigned by the

machine manufacturer

N Block number -

subblock 0 ... 9999 9999

integer only, no sign Can be used with a number to

identify blocks,

programmed at the beginning of

a block

E.g.: N20

: Block number - main

block 0 ... 9999 9999

integer only, no sign Special identification for blocks -

used instead of N..., this block

should contain all the inst ructions

for a complete set of subsequent

machining operations

E.g.: :20

P Number of subroutine

passes 1 ... 9999

integer only, no sign Programmed in the same block

as a subroutine to be call ed

several times,

e.g.: N10 L871 P3 ; called three

times

E.g.: L781 P...

;in sepa rate blo ck

Programming

SINUMERIK 801 8-9

Operation and Program ming

—

Turning

Address Meaning Value assignment Information Programming

R249

Arithmetic parameter ± 0.0000001 ... 9999

9999

(8 decimal places) or

with exponent:

± (10-300 ... 10+300 )

R0 to R99 -user assignable

R100 to R249 -transfer

parameters for machining cycles

Arithmetic functions In addition to the 4 basic

arithmetic operations

+ - * / the following

arithmetic functions are also

available:

SIN( ) Sine in degrees E.g.:

R1=SIN(17.35)

COS( ) Cosine in degrees E.g.:

R2=COS(R3)

TAN( ) Tangent in degrees E.g.:

R4=TAN(R5)

SQRT( ) Square root E.g.:

R6=SQRT(R7)

ABS( ) Absolute value E.g.:

R8=ABS(R9)

TRUNC( ) Integer part E.g.:

R10=TRUNC(R1

RET End of subroutine

0.001 ... 99 999.999 Used instead of M2 to maintain

continuous path mode RET

;in sepa rate blo ck

S Spindle speed

or other meaning

with

G4, G96

0.001 ... 99 999.999 Spindle speed in rev/min

if G96 is programmed, S is

interpreted as constant cutting

speed in m/min (turning),

with G4, dwell time in spindle

revolutions

S...

T Tool number 1 ... 32 000

integer only, without

sign

Tool change can be performed

directly with T command or not

until M6 is programmed. This can

be set in machine data.

T...

X Axis ± 0.001 ... 99 999.999 Positional data X...

Z Axis ± 0.001 ... 99 999.999 Positional data Z...

AR Angle of aperture for

circular interpolation 0.00001 ... 359.99999 Given in degrees, a method of

defining the circle with G2/G3 see G2; G3

CHF Chamfer 0.001 ... 99 999.999 Inserts a chamfer of the specified

length between tw o contour blocks N10 X... Z....

CHF=...

N11 X... Z...

CR Radius for circular

interpolation 0.010 ... 99 999.999

Negative sign - for

circle selection:

greater semi-circle

A method of d efining a circle wit h

G2/G3. see G2; G3

GOTOB GOTO instruction

backwards - Jumps to the block defined by

the label, the target of the ju mp is

located in the direction of the

beginning of the program.

E.g.: N20

GOTOB

MARKE1

GOTOF GOTO instruction

forwards - Jumps to the block defined by

the label, the target of the ju mp is

located in the directio n of the end

of the program.

E.g.: N20

GOTOF

MARKE2

Programming

8-10 SINUMERIK 801

Operation and Program ming

—

Turning

Address Meaning Value assignment Information Programming

IF Jump condition - If the jump condition is fulfilled

the jump goes to the next

instruction,

Comparators:

= =

E.g.: N20 IF

R1>5 GOTOB

MARKE1

IX Interpolation point for

circular interpolation ± 0.001 ... 99 999.999 For the X a xis, programmed for

circular interpolation with G5 see G5

KZ Interpolation point for

circular interpolation ± 0.001 ... 99 999.999 For the Z axis, programmed for

circular interpolation with G5 see G5

LCYC... Machining cycle call Specified values only Machining cycles have to be

called in a separate block, the

transfer parameters to be used

must be assigned values

Transfer parameters:

LCYC82 Drilling, spot-facing R101: Retraction plane

(absolute)

R102: Safety clearance

R103: Reference plane

(absolute)

R104: Final drilling depth

R105: Dwell time at drilling depth

N10 R100=...

R101=... ...

N20 LCYC82

in separa te block

LCYC83 Deep-hole drilling R100: Number of the drilling axis

R101: Retract ion plane

(absolute)

R102: Safety clearance

R103: Reference plane

(absolute)

R104: Final drilling depth

(absolute)

R105: Dwell time at drilling depth

R106: Dwell time start/stock

removal

R107: First drilling dept h

(absolute)

R108: Amount of degression

R109: Feedrate factor for drilling

R110: Machining type:

chipbreaking=0

stock removal=1

R111: Feedrate for first drilling

depth

N10 R100=...

R101=... ....

N20 LCYC83

;in sepa rate blo ck

LCYC840 Tapping with compensating chuck R101: Retraction plane (absolute

R102: Safety clearance

R103: Reference plane

(absolute)

R104: Final drilling depth

(absolute)

R106: Thread lead value

R126: Direction of rotation of

spindle for tapping

N10 R100=...

R101=... ....

N20 LCYC840

;in sepa rate blo ck

Programming

SINUMERIK 801 8-11

Operation and Program ming

—

Turning

Address Meaning Value assignment Information Programming

LCYC85 Boring R101: Retraction plane (absolute

R102: Safety clearance

R103: Reference plane

(absolute)

R104: Final drilling depth

(absolute)

R105: Dwell time at drilling depth

R107: Feed for drilling

R108: Feed on retract from drill

hole

N10 R100=...

R101=... ....

N20 LCYC85

;in sepa rate blo ck

LCYC93 Groove (drilling cycle) R100: Starting point i n facing

axis

R101: Starting poin t in longitudinal

axis

R105: Machining type (1...8)

R106: Final machining a llowance

R107: Cutting edge width

R108: Infeed depth

R114: Groove width

R116: Thread angle

R117: Chamfer on groove edge

R118: Chamfer at base of groove

R119: Dwell time at base of groo ve

N10 R100=...

R101=... ....

N20 LCYC93

;in sepa rate blo ck

LCYC94 Undercut (form E and F) (turning cycle) R100: Starting point in facing

axis

R101: Starting point of contour in

longitudinal axis

R105: Form E=55, F=56

R107: Cutting edge position (1...4)

N10 R100=...

R101=... ....

N20 LCYC94

;in separate

block

LCYC95 Stock removal (turning cycle) R105: Machining type (1...12)

R106: Finishing allowance

R108: Infeed depth

R109: Infeed angle for roughing

R110: Contour clearance for

roughing

R111: Feedrate for roughing

R112: Feedrate for finishing

N10 R105=...

R106=...

N20 LCYC95

in separate

block

LCYC97 Thread cutting (turning cycle) R100: Diameter of thread at

starting point

R101: Thread starting point in

longitudinal axis

R102: Thread diameter at end

point

R103: Thread end point in

longitudinal axis

R104: Thread lead value

R105: Machini ng type (1 and 2)

R106: Finishing allowance

R109: Approach path

R110: Run-out path

R111: Thread depth

R112: Starting point offset

R113: Number of roughing cuts

R114: Number of threads

N10 R100=...

R101=... ....

N20 LCYC97

;in separate

block

LIMS Upper limit speed of

spindle with G96 0.001 ... 99 999.999 Limits the spindle speed if

function G96 is activated -

constant cutting speed for turning

see G96

RND Rounding 0.010 ... 99 999.999 Inserts a rounding with the radius

value specified tangentially

between two contour blocks

N10 X... Z....

RND=...

N11 X... Z...

Programming

8-12 SINUMERIK 801

Operation and Program ming

—

Turning

Address Meaning Value assignment Information Programming

SF Thread

commencement point

with G33

0.001 ... 359.999 Specified in degrees, with G33

the thread commencement point

is offset by the specified amount

see G33

SPOS Spindle position 0.0000 ... 359.9999 Specified in degrees, the spindle

stops at the specified position

(spindle must be designed to do

this)

SPOS=....

STOPRE Preprocessing stop - Specia l function, the next blo ck is

not decoded until the block prior

to STOPRE is completed

STOPRE ;in

separate block

$P_TOOL Active tool cutting

edge read-only integer,

DO to D9 IF $P_TOOL==7

GOTOF ...

$P_TOOL

NO Active tool number read-o nly integer,

TO - T32000 IF

$P_TOOLNO==

46 GOTOF ...

$P_TOOLP Tool number last

programmed read-only integer,

TO - T32000 IF

$P_TOOLNP==

11 GOTOF ...

Programming

SINUMERIK 801 8-13

Operation and Program ming

—

Turning

8.2 Position data

8.2.1 Absolute/incremental dimensions: G90, G91

Functionality When instruction G90 or G91 is active, the specified position information X, Z

is interpreted as a coordinate point (G90) or as an axis path to be traversed

(G91). G90/G91 applies to all axes.

These instructions do not determine the actual path on which the end points

are reached. This is done by a G group (G0, G1, G2, G3, ... see Section “Axis

Movements”).

Programming G90 ;Absolute dimensioning

G91 ;Increment al dimensioning

G90 absolute dimension

sion

G91 incremental dimension

sion

Fig.8-3 Different dimensioning in the part drawing

Absolute dimension G90

When absolute dimensioning is selected, the dimension data refer to the zero

point of the currently active coordinate system (workpiece coordinate system,

current workpiece coordinate system or machine coor dinate system). Which of

the systems is active depends on which offsets are currently effective, i.e.

programmable, settable or none at all.

G90 is active for all axes on program start and remains so until it is

deactivated by G91 (incremental dimensioning selection) in a subsequent

block (modal command ).

Incremental dimen- When incremental dimensioning is selected, the numerical value in the

posion

sion G91 information corresponds to the path to be traversed by an axis. The traversing

direction is determined by the sign.

G91 applies to all axes and can be deactivated by G90 (absolute

dimensioning) in a later block.

Programming exam- N10 G90 X20 Z90 ;Absolute dimensioning

ple for G90 and G91 N20 X75 Z-32 ;Absolute dimensioning still active

...

N180 G91 X40 Z20 ;Switchover to incremental dimensioning

N190 X-12 Z17 ;Incremental dimensioning still active

Programming

8-14 SINUMERIK 801

Operation and Program ming

—

Turning

8.2.2 Metric/inch dimensions: G71, G70

Functionality If a workpiece has dimensions that deviate from the default system settings in

the control system (inch or mm), then these can be entered directly in the

program. The control system then conve rts them to the basic system.

Programming G70 ;Inch dimension

G71 ;Metric dimension

Programming N10 G70 X10 Z30 ;Inch dimension system

example N20 X40 Z50 ;G70 still active

...

N80 G71 X19 Z17.3 ;Metric dimension system from here

...

Information Depending on the current default settings, the control system interprets all

geometric values as metric or inch dimensions. “Geometric values” also

include tool offsets and settable zero offsets including the display as well as

feed F in mm/min or inch/min.

The basic sett ing can be changed in the machine data.

All examples in this Guide assume that the default setting is metric.

G70 and G71 affect all geometric data that refer directly to the workpiece:

z Position information X, Z with G0, G1, G2, G3, G33

z Interpolation parameters I, K (incl. lead).

z Circle radius CR

z Programmable ze ro offset (G158)

Any other geometric data not relating directly to the workpiece, such as

feedrates, tool of fsets, settable zero offsets, are not affected by G70/G71.

Programming

SINUMERIK 801 8-15

Operation and Program ming

—

Turning

8.2.3 Radius/diameter dimensions: G22, G23

Functionality When parts are machined on turning machines, it is normal practice to

program the position data for the X axis (facing axis) as a diameter dimension.

The specified value is interpreted as a diameter for this axis only by the

control.

It is possible to switch over to radius dimension in the program if necessary.

Programming G22 ;Radius dimension

G23 ;Diameter dimension

Facing axis

Longitudinal axis

Facing axis

Longitudinal axis

Diameter dimension Radius dimension

G23 G22

D40

D30

D20

R20

R15

R10

Fig.8-4 Diameter and radius dimen sions for facing axis

Information When G22 or G23 is active, the specified end point for the X axis is

interpreted as a radius or diameter dimension.

The actual value is displayed correspondingly in the workpiece coordinate

system. A programmable offset with G158 X... is always interpreted as a

radius dimension. See the followin g section for a description of this function.

Programming N10 G23 X44 Z30 ;Diameter for X axis

example N20 X48 Z25 ;G23 still active

N30 Z10

...

N110 G22 X22 Z30 ;Changeover to radius dimension for X axis from he re

N120 X24 Z25

N130 Z10

...

Programming

8-16 SINUMERIK 801

Operation and Program ming

—

Turning

8.2.4 Programmable zero offset: G158

Functionality Use the programmable zero offset for frequently repeated shapes/arrangements

in different positions on a workpiece or when you simply wish to choose a new

reference point for the dimension data. The programmable offset produces the

current workpiece coordinate system. The newly programmed dimension data

then refer to this system. The offset can be applied in all axes.

A separate block is always requi red for the G158 instruction.

XWorkpiece

Workpiece

W orkpiece original

Workpiece “offset”

Offs e t X ...Z ...

current

Fig.8-5 Example of programmable of fset

Offset G158 A zero offset can be programmed for all axes with instruction G158. A newly

entered G158 instruction replaces any previous programmable offset instruction.

Delete offset If the instruction G158 without axes is inserted in a block, then any active

programmable of fset will be deleted.

Programming N10 ...

Example N20 G158 X3 Z5 ;Programmable offset

N30 L10 ;Subroutine call, contains the geometry to be offset

...

N70 G158 ;Offset delete d

...

Subroutine call - see Section 8.10 “Subroutine System”

Programming

SINUMERIK 801 8-17

Operation and Program ming

—

Turning

8.2.5 Workpiece clamping - settable zero offset: G54 to G57, G500, G53

Functionality The settable zero offset specifies the position of the workpiece zero point on

the machine (offset between workpiece zero and machine zero). This offset is

calculated when the workpiece is clamped on the machine and must be

entered by the operator in the data field provided. The value is activated by

the program through selection from four possible grou ps: G54 to G57.

See Section 3.2 “Enter/Modify Zero Offset” for operating sequence.

Programming G54 ;1st settable zero offset

G55 ;2nd settable zero offset

G56 ;3rd settable zero offset

G57 ;4th settable zero offset

G500 ;Settable zero offset OFF modal

G53 ;Settable zero offset OFF non-modal, also suppresses

programmable offset

Machine

Workpiece

e.g.

G54

Workpiece

Specify offset in Z axis only!

Machine

Fig.8-6 Settable zero offset

Programming N10 G54 ... ;Call first settable zero offset

Example N20 X... Z... ;Machine workpiece

...

N90 G500 G0 X... ;Deactivate settable zero offset

Programming

8-18 SINUMERIK 801

Operation and Program ming

—

Turning

8.3 Axis movements

8.3.1 Linear interpolation at rapid traverse: G0

Functionality The rapid traverse motion G0 is used to position the tool rapidly, but not to

machine the workpiece directly. All axes can be traversed simultaneously

resulting in a linear path.

The maximum speed (rapid traverse) for each axis is set in the machine data.

If only one axis is moving, it traverses at its own rapid traverse setting. If two

axes are traversed simultaneously, then the path speed (resultant speed) is

selected so as to obtain the maximum possible path speed based on the

settings for both axes.

A programmed feed (F word) is irrelevant for G0. G0 remains effective until it

is canceled by another instruction from the same group (G1, G2, G3,...).

Fig.8-7 Linear interpolation with rapid trav erse from point P1 to P2

Programming N10 G0 X100 Z65

example

Information A further group of G functions is provided for programming the approach to the

position (see Section 8.3.9 “Exact Stop/Continuous Path Control: G60, G64”).

G60 (exact stop) is linked to another group which allows various accuracy

settings to be selected in a window. There is also a non-modal instruction, i.e.

G9, for the exact stop function.

You should note these options when considering how to adapt the control to

your positioning t asks.

Programming

SINUMERIK 801 8-19

Operation and Program ming

—

Turning

8.3.2 Linear interpolation at feedrate: G1

Functionality The tool moves from the start point to the end point along a straight path. The

path speed is defined by the programmed F word.

All axes can be traversed simultaneously.

G1 remains effective until it is canceled by another instruction from the same

G group (G0, G2, G3, ...).

Fig.8-8 Linear interpolation with G1

Programming N05 G54 G0 G90 X40 Z200 S500 M3 ;tool is moving at rapid traverse,

spindle

example speed = 500 rpm, CW rotation

N10 G1 Z120 F0.15 ;Linear interpolation with feed 0.15

mm/rev

N15 X45 Z105

N20 Z80

N25 G0 X100 ;Traverse clear at rapid traverse

N30 M2 ;End of program

Programming

8-20 SINUMERIK 801

Operation and Program ming

—

Turning

8.3.3 Circular interpolation: G2, G3

Functionality The tool moves from the start point to the end point on a circular path. The

direction is determined by the G function:

G2 - in clockwise direction

G3 - in counterclockwise direction

The path speed is determined by programmed F word. The required cycle can

be described in different ways:

— Center point and end point

— Circle radius and end point

— Center point and aperture angle

— Aperture angle and end point

G2/G3 remain effective until they are canceled by another instruction from the

same G group (G0, G1, ...).

In clockwise direction In counterclockwise direction

Fig.8-9 Definition of direction of rotation around circle with G2/G3

G2/G3 and input of center point (+end point): G2/G3 and radius spoecification (+end point):

G2/G3 and input of aperture angle

End point X,Z

Start point X,Z Center point I, J

XEnd point X,Z

Start point X,Z

e.g. G2 X...Z...I...K... e.g. G2 X...Z...CR=...

Start point X,Z

e.g. G2 AR=... I...K...

Angle AR

(+center point):

Circle radius

Center point I, K

G2/G3 and input of aperture angle

Start point X,Z

e.g. AR=... X...Z...

Angle AR

(+end point):

End point X, Z

Fig.8-10 Circle pro gramming options

Programming

SINUMERIK 801 8-21

Operation and Program ming

—

Turning

Programming Center point and end point specificatio n:

example

End point

Center point

Start point

Fig.8-11 Example of center and end point specification

N5 G90 Z30 X40 G22 G0 ;Circle start point for N1 0

N10 G2 Z50 X40 K10 I-7 ;End point and center point

Programming End point and radius specification:

example

30 Z

End point

Center point

Start point

Fig.8-12 Example of end point and radius input

N5 G90 Z30 X40 G22 G0 ;Circle start point for N1 0

N10 G2 Z50 X40 CR=12.207 ;End point and radius

Note: When the value for CR =-... has a negative sign, a circle segment larger

than a semi-circle is selected.

Programming

8-22 SINUMERIK 801

Operation and Program ming

—

Turning

Programming End point and aperture angle:

example

30 Z

End point

Center point

Start

105°

Fig.8-13 Example of end point and aperture angle spe cificatio n

N5 G90 Z30 X40 G22 G0 ;Circle start point for N1 0

N10 G2 Z50 X40 AR=105 ;End point and aperture angle

Programming Center point and aperture angle:

example

Fig.8-14 Example of center point and aperture angle specification

N5 G90 Z30 X40 G22 G0 ;Circle start point for N1 0

N10 G2 K10 I-7 AR=105 ;Center point and aperture angle

Input tolerances The control system will only accept cricles within a cert ain dimensional tolerance.

for circle The circle radius at the start and end points are compared for this purpose. If

the difference is within the tolerance limit s, the center point is set internally in

the control. Otherwise, an alarm messa ge is output.

The tolerance value can be set via the machine data.

30 Z

End point

Center point

Start point

105°

Programming

SINUMERIK 801 8-23

Operation and Program ming

—

Turning

8.3.4 Circular interpolation via intermediate point: G5

Functionality If you know three contour points around the circle instead of center point or

radius or aperture angle, you sh ould preferably use the G5 function.

The direction of the circle in this case is determined by the position of the

intermediate point (between start and end positions).

G5 remains effective until it is canceled by another instruction from the same

G group (G0, G1, G2, ...).

Note: The dimension setting G90 or G91 applies to both the end point and

intermediate point!

30 Z

End point

Start point

In te rme d ia te po in t

Fig.8-15 Circle with end and intermediate point specification with G90 active

Programming N5 G90 G23 G0 Z30 X80 ;Circle start point for N10

example N10 G5 Z50 X80 KZ=40 IX=45 ;End and intermediate points, IX must

be programmed as a radius dimension

Programming

8-24 SINUMERIK 801

Operation and Program ming

—

Turning

8.3.5 Thread cutting with constant lead: G33

Functionality Function G33 can be used to cut the following types of threads with constant

lead:

z Thread on cylindrical bodies

z Thread on ta pered bodies

z External/internal threads

z Single-start/multiple-start threads

z Multi-block threads (thread “chaining”)

This function requires a spindle with position measuring system.

G33 remains effective until it is canceled by another instruction from the same

G group (G0, G1, G2,G3,...).

external

internal

Fig.8-16 Example of external /internal thread on cylindrical body

RH or LH threads When Z axis is traversing from right to left, the direction of the thread, i.e.

right-hand or left-hand, is determined by the setting for the direction of rotation

of the spindle (M3 - clockwise rotation, M4 - counterclockwise rotation; see

Section 8.4 “Spindle Movements”). To this aim, the speed setting must be

programmed under address S, or a speed must be set.

Note: The approach and run-out paths must be taken into account with

respect to the thread length.

End point Start point Zero degree mark

of spindle enco de r

SF=...

Offset

Thread length

Lead

Lead: I or K

(V a lue is co n sta nt o ve r

the en tire th r ea d len gt h

of a G33 block ) RH or LH thread

(M3 / M4)

Further start

point possible

(fo r multip le-star t threa ds )

Side view Top view

Fig.8-17 Programmable quantities for thread cutting with G33

Programming

SINUMERIK 801 8-25

Operation and Program ming

—

Turning

ngle at taper is

less than 45

degrees

ngle at taper is

greater than 45

degrees

Lead:

Lead: K

Lead:

Programming:

G33 Z... K...

G33 Z... X... K...

G33 Z... X... I...

G33 X... I...

(Lead K, since Z a xis has the lon ge r p ath)

(Lead I, since X axis has the long er path)

Lead:

Cylindrical threa d

Tapere d thre ad

Transversal th read

Fig.8-18 Lead assignment on the example of Z/X axis

In the case of tapered threads (2 axes must be specified), the lead address I

or K of the axis with the longer path (greater thread length) must be used. A

second lead is not specifie d.

Start-point offset A start-point offset of the spindle is required for machining multiple-start threads

SF= or threads in offset cuts. The start-point offset is programmed under address

SF in the thread block with G33 (absolute position, specified in Degree).

If a start point is not included in the block, the value from the setting data is

activated.

Note: Any value programmed for SF= is always entered in the setting data as

well.

Programming Cylindrical thread, two-start, start-point offset 180 degrees, thread length (including

example app roach and run-out) 100 mm, thread lead 4 mm/rev.

RH thread, cylinder premachined:

N10 G54 G0 G90 X50 Z0 S500 M3 ;Approa ch sta rt point, CW spindle rotation

N20 G33 Z-100 K4 SF=0 ;Lead:4 mm/rev.

N30 G0 X54

N40 Z0

N50 X50

N60 G33 Z-100 K4 SF=180 ;2nd start, 180 degrees offset

N70 G0 X54 ...

Multi-block thread If several thread blocks are programmed in succession (multi-block thread), it

makes only sense to program a start-point offset in the 1st thread block since

this is the only block in which the function is effective.

Multi-block threads are automatically linked by G64 (continuous path mode,

see Section 8.3.9 “Exact Stop/Continuous Path Co ntrol: G60, G64”).

Programming

8-26 SINUMERIK 801

Operation and Program ming

—

Turning

3rd block with G33

1st block wit h G33

N10 G33 Z... K... SF=...

N20 Z.... X.... K...

N30 Z.... X... K...

Fig.8-19 Example of multi-block thread (thread “chaining”)

Axis velocities For thread cuts with the G33 function, the velocity of the axes for the thread

length is determined by the spindle speed and the thread lead. Feed F is not

relevant in this respect. However, it remains stored. The maximum speed

defined in the machine data (rapid traverse) must not be exceeded.

Information Important

— The setting of the spindle speed override switch (override spindle)

should not be changed for thre ad machining operation s.

— The feed override switch has no function in this block.

Programming

SINUMERIK 801 8-27

Operation and Program ming

—

Turning

8.3.6 Fixed-point approach: G75

Functionality G75 can be used to approach to a fixed point on the machine, such as the tool

change point. The position is fixed for all axes in the machine data. No offset

is applied.

The speed of each axis is its own ra pid traverse setting.

G75 requires a separate block and is non-modal.

The G command from the Interpolation Type group (G0, G1,G2, ...) which was

active prior to the block with G75 is activated after the block with G75.

Programming N10 G75 X0 Z0

example Note: The programmed numerical values for X, Z are ignored.

8.3.7 Reference point approach: G74

Functionality G74 is used to execute the reference-point approach in the NC program.

Direction and speed of each axis are stored in machine data.

G74 requires a separate block and is non-modal. The G command for the

Interpolation Type group (G0, G1,G2, ...) active prior to the block with G74 is

activated again af ter the block with G74.

Programming N10 G74 X0 Z0

example Note: The pro grammed numerical value s for X, Z are igno red.

Programming

8-28 SINUMERIK 801

Operation and Program ming

—

Turning

8.3.8 Feedrate F

Functionality The feedrate F is the path speed and represents the absolute value of the

geometric total of the speed components of all axes involved.

The axis speeds are determined by the axis path distance in relation to the

total path distance.

The feedrate F is effective in interpolation modes G1, G2, G3 and G5 and

remains active until a new F word is inserted in the program.

Programming F...

Note: Decimal points can be omitted in case of integer values, e.g. F300.

Unit for F–G94, G95 The unit of measurement for the F word is defined by G functions:

z G94 F as feedrate in mm/min

z G95 F as feedrate in mm/rev of spindle

(only makes sense if spindle is in operation!)

Programming N10 G94 F310 ;Feedrate in mm/min

example ...

N110 S200 M3 ;Spindle operation at a speed of 200rev/min

N120 G95 F1.5 ;Feedrate in mm/rev

Note: Enter a new F word if you change from G94 to G95.

Information The group with G94 and G95 has additional functions G96 and G97 for

constant cutting rate for turning machines. These functions also influence the

S word (see Section 8.5.1 “Constant Cutting Rate”).

Programming

SINUMERIK 801 8-29

Operation and Program ming

—

Turning

8.3.9 Exact stop / continuous path mode: G9, G60, G64

Functionality These G functions enable you to set the traversing behavior at block limits and

to control program advance to the next block, thus allowing you to adapt your

program optimally to various requirements. For example, you want to position

quickly with the axes or process path contours over several blocks.

Programming G60 ;Exact stop - (modal)

G64 ;Continuous path mode

G9 ;Exact stop - (non-modal)

G601 ;Exact stop window fine

G602 ;Exact stop window coarse

Exact stop G60, G9 If the exact stop function (G60 or G9) is active, the speed for reaching the

exact target position is re duced towards zero at the end of the program bl ock.

Another modally active G group can be set in conjunction with these functions

to determine the moment at which the traversing motion in this block is

finished so that processi ng of the next block can commence.

z G601 Exact stop window fine

Processing of the next block commences as soon as all axes have

reached the “Exact stop window fine” (value in machine data).

z G602 Exact stop window coarse

Processing of the next block commences as soon as all axes have

reached the “Exact stop window co arse” (value in machine data).

The selection of the exact stop window significantly affects the total machining

time if many positioning operations need to be carried out. Fine adjustments

require more time.

G60

(fine)

(coarse)

dvance to next block for

“coarse” and for “fine”

Fig.8-20 Coarse or fine exact stop window, effective with G60/G9, zoomed

view of window

Programming

8-30 SINUMERIK 801

Operation and Program ming

—

Turning

Programming N5 G602 ;Exact stop coarse

example N10 G 0 G60 Z... ;Exact stop modal

N20 X... Z... ;G60 still active

...

N50 G1 G601 ... ;Exact stop window fine

N80 G64 Z... ;Switchover to continuous path

...

N100 G0 G9 Z... ;Exact stop acts only in this block

N111 ... ;Return to continuous path mode

...

Note: The command G9 generates an exact stop only for the block in which it

is programmed; in contrast, G60 remains active until it is canceled by G64.

Continuous path The purpose of continuous path mode is to prevent braking of the axes at

block

mode G64 limits to make the transition to the next block at the most constant possible

speed (in the case of tangential transitions). The function operates with

lookahead speed control to the next block. In the case of non-tangential path

transitions (corners), the speed is reduced to such an extent in some cases

that none of the axes is capable of making a speed step change that is higher

than the maximum acceleration rate. In such cases, speed-dependent

rounding at corners occurs.

Advance to next

block with feed F2 Advance to next

block with feed F1

Feed F2 is greater than F1

Fig.8-21 Rounding at contour corners with G64

Programming N10 G64 G1 Z... F... ;Continuous path mode

example N20 X.. ;Continuous path control mode still active

...

N180 G60 ... ;Switching to exact stop

Programming

SINUMERIK 801 8-31

Operation and Program ming

—

Turning

Fig.8-22 Comparison between speed re sponses with G60 and G64 with sho rt block paths

8.3.10 Dwell time: G4

Functionality You can interrupt machining between two NC blocks for a defined time period

by inserting a separate block with G4, e.g. for relief cutting operations.

The words with F... or S... are used for time specifcations only in this block.

Any previously programmed feed F or spindle speed S remain unaffected.

Programming G4 F... ;Dwell time in seconds

G4 S... ;Dwell time in spindle revolutions

Programming N5 G1 F200 Z-50 S300 M3 ;Feed F, spindle speed S

example N10 G4 F2.5 ;Dwell time 2.5 s

N20 Z70

N30 G4 S30 ;Dwell for 30 spindle revolutions, correspond s to t

= 0.1 when S = 300 rev/min and 100% speed

override

N40 X... ;Feed and spindle speed values remain effective

Note G4 S.. can only be programmed if the machine has a controlled spindle (if the

speed has also been programmed under address S... ).

Programmed feed F

G60 - exact stop

N2 N3 N5 N6 N7 N8 N9 N10 N11 N12 Block

Programmed speed cannot b e reached because block paths too short

G64 - continuous path mode

Programming

8-32 SINUMERIK 801

Operation and Program ming

—

Turning

8.4 Spindle movements

8.4.1 Spindle speed S, directions of rotation

Functionality The spindle speed is programmed under address S in revolutions per minute,

if the machine has a controlled spindle. The direction of rotation and the start

or end of the movement are specified by means of M commands (see Section

“Miscellaneous Function M”).

Note: A decimal point may be omitted in the case of integer S values, e.g.

S270.

Information If you insert M3 or M4 in a block with axis movements, then the M commands

will take effect before the axis movements.

Default setting: The axis movements will only start after the spindle has run up

(M3, M4). M5 is also output prior to the axis movement. However, the axes will

not wait for the spindle being stopped. The axis movements will already start

before the spindle has come to a standstill. The spindle is stopped with

program end or RESET.

Note:

Other settings can be conf igured via machine data.

Programming example

N10 G1 X70 Z20 F300 S270 M3 ;S pindle powe rs up to 270 rev/min in clockwi se

rotation before axis traversal X, Z

...

N80 S450 ... ;Speed change

...

N170 G0 Z180 M5 ;Z movement in block, spindle stop

Programming

SINUMERIK 801 8-33

Operation and Program ming

—

Turning

8.4.2 Spindle speed limitation: G25, G26

Functionality You can restrict the speed limit values that otherwise apply by programming a

speed limit value using G25 or G26 and spindle address S. These functions

also overwrite the values entered in the setting data.

G25 or G26 each requires a separate block. Any previously programmed

speed S remains effective.

Programming G25 S... ;Lower spindle speed limitation

G26 S... ;Upper spindle speed limitation

Information The maximum upper and lower spindle speed limits are set in a machine data.

Setting data can be activated via the operator panel to limit the speed range

still further.

The special function G96 (constant cutting rate) can be used to program an

additional upper limit on turning machin es.

Programming N10 G25 S12 ;Lower spindle limit speed: 12 rev/min

example N20 G 26 S700 ;Upper spindle limit speed: 700 rev/min

Programming

8-34 SINUMERIK 801

Operation and Program ming

—

Turning

8.4.3 Spindle positioning: SPOS

Functionality Precondition: The spindle must be technically designed for operation under

closed-loop position control.

The SPOS= function allows you to position the spindle in a specific angular

position. It is then held in this position by a closed-loop position control

function.

The speed of the positioning operation is defined in a machine data.

The applicable direction of rotation is maintained from the M3/M4 movement

until the positioning process is complete. When the spindle is positioned from

standstill, the position is approached via the shortest possible path. In this

case, the direction is determined by the start and end positions.

Exception: Initial movement of spindle, i.e. if the measuring system is not yet

synchronized. In such cases, the direction is specified by a machine data.

The spindle movements are executed in parallel to any axis movements that

are programmed in the same block. Processing of the block is complete when

both movements have been executed.

Programming SPOS=... ;Absolute position: 0 ... <360 Grad

Programming N10 SPOS=14.3 :Spindle position 14.3 degrees

example ...

N80 G0 X89 Z300 SPOS=25.6 ;Position spindle with axis movements.

The block is complete once all movements

have been executed.

N81 X200 Z300 ;N81 block does not start until spindle

position from N80 is reached.

Programming

SINUMERIK 801 8-35

Operation and Program ming

—

Turning

8.5 Special turning functions

8.5.1 Constant cutting rate: G96, G97

Functionality Precondition: The machine must have a controlled spindle.

When the G96 function is active, the spindle speed is adjusted to the diameter

of the workpiece currently being machined (facing axis) such that a

programmed cutting rate S remains constant at the tool edge (spindle speed

times diameter = constant).

The S word is interpreted as the cutting rate from the block with G96 onwards.

G96 is active as a modal command until it is cancelled by another G function

in the same group (G94, G95, G97).

Programming G96 S... LIMS=... F... ;Constant cutting rate ON

G97 ;Constant cutting rate OFF

STL Explanation

S Cutting rate, unit m/min

LIMS= Upper limit speed of spindle, effective only with G96

F Feed in mm/rev unit of measurement - as for G95

Note:

In this case, feed F is always interpreted in the unit of measurement

mm/revolution.

If G94 was active instead of G95 beforehand, then a suitable F word must be

inserted again in the program!

D2 D1

X(Facing axis)

D1 x S D1=D2 x SD2=Dn x SD n=constant

SD =Spindle speed

D 1 , D2 = Diame te r

Fig.8-23 Constant cutting rate G96

Traversing at rapid No speed changes take place during rapid traversal with G0.

traverse Exception: If the contour is approached in rapid traverse mode and the next

block contains an interpolation type G1 or G2, G3, G5 (contour block), then

the speed is adjusted to the value for the contour block while the approach

block with G0 is being processed.

Programming

8-36 SINUMERIK 801

Operation and Program ming

—

Turning

Upper limit speed The spindle speed may rise sharply when large diameters are machined

down

LIMS= to small diameters. For such applications, it is advisable to specify the upper

spindle speed limitation by means of LIMS=... . LIMS is effective only in

conjunction with G96.

When LIMS=... is programmed, the value entered in the setting data is

overwritten.

The upper speed limit programmed with G26 or via machine data cannot be

overwritten by the LIMS= function.

Deactivate constant The “Constant cutting rate” function is deactivated with G97. If G97 is active, a

cutting rate: G97 subsequently programmed S word is interpreted again as the spindle speed in

revolutions per minute.

If no further S word is inserted in the program, then the spindle continues to

rotate at the speed that was recorded when the G96 function was l ast active.

Programming N10 ... M3 ;Direction of rotation of spindle

example N20 G96 S120 LIMS=2500 ;Activate constant cutting rate, 120 m/min,

limit speed 2,500 rev/min

N30 G0 X150 ;No speed change because block N31 includes

N31 X50 Z... ;No speed change because block N32 includes

N32 X40 ;Approach contour, new speed is automatically

set to value required for start of block N40

N40 G1 F0.2 X32 Z... ;Feed 0.2 mm/rev

...

N180 G97 X... Z... ;Deactivate constant cutting rate

N190 S... ;New spindle speed, rev/min

Information The G96 function can also be deactivated by G94 or G95 (same G group). In

this case, the last programmed spindle speed S applies for the remainder of

the machining operation provided no new S word is programmed.

Programming

SINUMERIK 801 8-37

Operation and Program ming

—

Turning

8.5.2 Rounding, chamfer

Functionality You can insert the elements “chamfer” and “rounding” at contour corners. The

appropriate instruction, i.e. CHF=... or RND=... is programmed in the block

with axis motions that leads into the corner.

Programming CHF=... ;Insert chamfer, value: Length of chamfer

RND=... ;Insert rounding, value: Rounding radius

Chamfer CHF= A linear section is inserted between linear and circular contours in any

combination. The edge is chamfered.

Bisector

Chamfer

N 1 0 G1 ...CHF = ...

N2 0 G1 ...

CHF=

Fig.8-24 Insertion of a chamfer between two linear contours (example)

Programming exa- N10 G1 Z... CHF=5 ;Insert 5 mm chamfer

mple for chamfer N20 X... Z...

Rounding RND= A circular contour element is inserted with tangential transitions between linear

and circular contours in an y combination.

RND=...

Rounding

N50 G1 ...RND=...

N60 G3 ...

RND=...

Rounding

N10 G1 ...RND=...

N20 G1 ...

Straight line/straight line Straight line/straight line

Fig.8-25 Examples of rounding insertion

Programming

8-38 SINUMERIK 801

Operation and Program ming

—

Turning

Programming exa- N10 G1 Z... RND=8 ;Insert rounding with 8 mm radius

mple for rounding N20 X... Z...

...

N50 G1 Z... RND=7.3 ;Insert rounding with 7.3 mm radius

N60 G3 X... Z...

Information Note:

The programmed value for the chamfer or rounding is automatically reduced

when the contour programmed in one of the blocks involved is not sufficiently

long.

No chamfer/rounding is inserted if more than one of the subsequently

programmed blocks does not contain any information about traversal of the

axes.

Programming

SINUMERIK 801 8-39

Operation and Program ming

—

Turning

8.6 Tool and tool offset

8.6.1 General notes

Functionality When you are creating programs for workpiece machining, you need not take

tool lengths or cutter radii into account. Program the workpiece dimensions

directly, e.g. as given in the workpiece drawing.

The tool data are entered separately in a special data area. You merely call

the tool you need together with its offset data in the program. On the basis of

this data, the control executes the necessary path compensations in order to

produce the workpiece yo u have defined.

F-tool carrier reference point

M-machine zero

W-workpiece zero

Fig.8-26 Machining of a workpiece with various tool dimensions

Programming

8-40 SINUMERIK 801

Operation and Program ming

—

Turning

8.6.2 Tool T

Functionality You select a tool by programming the T word. A machine data defines whether

the T word represents a tool change or merely a preselection.

z Tool change (tool call) is implemented directly by T word (e.g. normal

practice for tool revolver on turning machines) or

z the tool is changed through additional instruction M6 after preselection

by T word (see also Section “Miscellaneous Functions M”).

Please note:

If a certain tool has been activated, this will remain stored as the active tool

even across the program end and after POWER ON of the control system.

If you change a tool manually, then enter the change into the control system

also manually to make sure that the control system detects the right tool. For

example, you can st art a block with a new T wo rd in the MDA mode.

Programming T... ;Tool number: 1 ... 32 000

Note

A maximum of 8 tools can be stored in the control at a time.

Programming Tool change without M6:

example N10 T1 ;Tool 1

...

N70 T588 ;Tool 588

Programming

SINUMERIK 801 8-41

Operation and Program ming

—

Turning

8.6.3 Tool offset number D

Functionality You can assign between 1 and 9 data fields with various tool offset blocks (for

several tool edges) to each specific tool. If a special edge is required, it can be

programmed by means of D plus a corresponding number.

D1 is the automatic default if no D word is programmed.

When D0 is programmed, then the offsets for the tool are not active.

Note

A maximum of 16 data fields with tool offset blocks can be stored in the control

at a time.

Programming D... ;Tool offset number: 1 ... 9

D0: No offsets active

Fig.8-27 Example assignment of tool offset numbers to tool

Information Tool length compensations take immediate effect when the tool is active. The

values of D1 are applied if no D number has been programmed. The tool

length is compensated when the first programmed traversal of the relevant

length compensation axis is executed.

A tool radius compensation must also be activated by means of G41/G42.

Programming Tool change:

example N10 T1 ;Tool 1 is activated with associated T 1D1

N11 G0 X... Z... ;The length compensation is superimposed here

N50 T4 D2 ;Change to tool 4, D2 of T4 becomes active

...

N70 G0 Z... D1 ;T4D1 for tool 4 is active, only edge changed

Contents of an Enter the following in the of fset memory:

offset memory

z Geometric quantities: Length, radius

These consist of several components (geometry, wear). The control

computes the component data to produce a resultant quantity (e.g. total

length 1, total radius). The total dimension calculated in each case takes

effect when the offset memory is activated.

T...

D2 D3 D9

D2 D3

T9 D1 D2

Programming

8-42 SINUMERIK 801

Operation and Program ming

—

Turning

The method used to compute these values in the axes depends on the tool

type and commands G17, G18 (see diagrams below).

z Tool type

The tool type determines which geometry data are necessary and how they

are computed (drills or turning tools). The hundreds place is the only

distinguishing digit:

— Type 2xy: Drills

— Type 5xy: Turning tools

z Tool point direction

You must also specify the tool point direction for tool type 5xy (turning tools).

Tool parameters The value for the relevant tool parameters is entered next to DP... . The tool

type determines which parameters are required. Any tool parameters not

needed must be set to “0”.

Tool type: DP1

Edge length: DP2

Geometry Wear

Length 1: DP3 DP12

Length 2: DP4 DP13

Radius: DP6 DP15

The following diagrams show which tool parameters are needed for which tool

type.

Fig.8-28 Length compensation values required for tu rning tools

G18:

Length 2

Tool tip P(Z)

(tool nose)

Effect

Length 1 in X

Length 2 in Z

Length 1

(X)

Turning tool

Set all other

values to 0

DP1

DP3

5xy

Length 1

Entries in tool

parameters

DP4

Wear values acc.

to requirements

Length 2

F - Tool carrier reference point

Programming

SINUMERIK 801 8-43

Operation and Program ming

—

Turning

Set all other

values to 0

DP1

DP3

5xy

Length 1

Entries in tool

parameters

DP4

Wear values acc.

To requirements Effect

G18: Length 1 in X

Length 2 in Z

Length 2

DP1

DP3

5xy

Length 1

DP4 Length 2

Grooving tool

Tool tip P

(edge 2 =D2)

D2:

Length 2

F - Tool carrie

reference point

D1: Length 1

(X)

Tool tip P

(edge 1 =D1)

D2: Length 1

(X)

(Z)

D1:

Length 2

(Z)

Fig.8-29 Turning tool with length comp ensation for two edges

Programming

8-44 SINUMERIK 801

Operation and Program ming

—

Turning

Length 1

Length 2

Tool tip P

(X)

(Z)

(tool nose)

R -Edge radius (tool radius)

S -Position of tool nose center point

Turning tool

The tool param eter DP2 specifies the tool point direction. Dire ction value 1 to 9 can be program m ed:

P=S

12 3 45 6

789

Tool point direction DP2:

Note:

Param eters length 1 and length 2 refer to

point P with tool point directions

1..8, but to S (S=P) with 9.

Effect

G18: Length 1 in X

Length 2 in Z

Se t all oth e r

values to 0

DP1 5xx

Length1

En tries in to ol

parameters

DP4

Wear values

acc. to

requirements

Length 2

DP2 1...9

DP6 Radius

F - Tool c arrier reference point

DP3

Fig.8-30 Offset data required for turning tools with tool radius compensation

Programming

SINUMERIK 801 8-45

Operation and Program ming

—

Turning

Set all other

values to 0

F - Tool carrier reference point

DP1

Entries in tool

parameters

DP3

2xy

Length 1

Effect

G17: Length 1 in Z

G18:

Wear values acc.

to requirements

Length 1

Turning tools

Fig.8-31 Offset data required for drills

Centre hole To drill a center hole, switch over to G17. The length compensation then acts

on the drill in the Z axis. After drilling, switch back to G18 for the normal

turning tool offset.

Example:

N10 T200 ;Drill, =tool type 200

N20 G17 G1 F... Z... ;Length compensation acts in Z axis

N30 Z...

N40 G18 .... ;Drilling completed

Fig.8-32 Drilling a center hole

Programming

8-46 SINUMERIK 801

Operation and Program ming

—

Turning

8.6.4 Selection of tool radius compensation: G41, G42

Functionality A tool with a corresponding D number must be active. The tool radius

compensation (tool nose radius compensation) is activated by G41/G42. The

control then automatically calculates the necessary tool paths equidistant from

the programmed contour for the current tool radius.

Note: G18 must be active.

Tool nose radius

Fig.8-33 Tool (nose) radius compensation

Programming G41 X... Z... ;Tool radius compensation to left of contour

G42 X... Z... ;Tool radius compensation to right of contour

Note: You may only select the function for linear interpolation (G0, G1).

Program both axes. If you only specify one axis, then the last programmed

value is automatically set for the second axis.

G42

G41

Fig. 8-34 Compensation to right/left of contour

Begin compen- The tool approaches the contour on a linear path and positions itself perpendicular

sation to the path tangent at the start of the contour. Select the start point such that

the tool can traverse safely with no risk of collision.

Programming

SINUMERIK 801 8-47

Operation and Program ming

—

Turning

Compensated

tool path

P0 -Start point

First contour section: Straight line

P1 -First contour section: Circle

R -Tool nose radius

First contour section: Circle

G42

Circle radius

Compensated

tool path

Tangent

P0 -Start point

G42

Fig.8-35 Beginning of tool radius compensatio n –example sho ws G42, tool point direction =3

Information The block containing G41/G42 is generally followed by the first block with the

workpiece contour. The contour definition may, however, be interrupted by an

intermediate block that does not contain any contour information, e.g. by a

block with just an M command.

Programming N10 T... F...

example N15 X... Z... ;P0 start point

N20 G1 G42 X... Z... ;Select compensation to the right of the contour, P1

N30 X... Z... ;Initial contour section, circle or straight line

Programming

8-48 SINUMERIK 801

Operation and Program ming

—

Turning

8.6.5 Behavior at corners: G450, G451

Functionality Functions G450 and G451 are provided to allow you to set the response in the

case of discontinuous transition from one contour element to another

(behavior at corners) when G41/G4 2 is active.

The control itself detects inside and outside corners. The point at which the

equidistant paths intersect is always approached in the case of inside corners.

Programming G450 ;Transition circle

G451 ;Intersection

Transition circle

(radius = tool radius) Intersection

Outside corner Outside corner

G450 G451

Fig.8-36 Behavior at an outside corner

Inside corner Intersection

Fig 8-37 Behavior at an inside co rner

Transition circle The tool center point traverses round the workpiece outer corner along an

G450 arc with the same radius as the tool radius.

In processing terms, the transition circle belongs to the next block that

contain s traversing movements, e.g. relating to feed value.

Intersection G451 With function G451 (intersection of equidistant paths), the tool approaches the

point at which the center point p aths (circle or straight line) intersect.

Programming

SINUMERIK 801 8-49

Operation and Program ming

—

Turning

8.6.6 Tool radius compensation OFF: G40

Functionality Function G40 is used to canceled compensation mode G41/G42. This G

function is also preset for program start.

The tool ends the block before G40 in normal position (i.e. compensation

vector perpendicular to tangent at end point), independently of retraction angle.

Always select the end point of the G40 block such that the tool can traverse

safely with no risk of collision.

Programming G40 X... Z... ;Tool radius compensation OFF

Note: Tool radius compensation can be canceled only in linear interpolation

mode (G0, G1).

Program both axes. If you only specify one axis, then the last programmed

value is automatically set for the second axis.

Final contour section: Straight line

R - Tool nose radius

Final contour section:

Circle

G40

Tangent

P2 - End point, block with G40

P1 - End point, last block with e.g. G42

Circle radius

G40

Fig.3-38 Cancelation of tool radius compensation using G40, example shows

G42, tool point direction=3

Programming ...

example N100 X... Z... ;Last block on contour, circle or straight line, P1

N110 G40 G1 X... Z... ;Deactivate tool radius compensation, P2

Programming

8-50 SINUMERIK 801

Operation and Program ming

—

Turning

8.6.7 Special cases of tool radius compensation

Change in compen- The compensation direction G41 <-> G42 can be changed without inserting

sation direction G40 instruction in-between.

The last block with the old compensation direction ends with the

compensation vector in the normal position at the end point. The new

compensation direction is executed as start of compensation (position at start

point).

Repetition of G41, The same contour can be programmed again without inserting a G40 instruction

G41 or G42, G42 beforehand.

The last block before the new compensation call ends with the compensation

vector in the normal position at the end point. The repeat compensation

process is executed as described under “Change in compensation direction”

above.

Change in offset The offset number D can be c hanged in compensation mode. In this case,

number D a n altered tool radius becomes effective at the beginning of the block in which

the new D number is programmed. The full change in radius is not achieved

until the end of the block, i.e. the change is implemented continuously over the

entire block. This also applies to circular interpolation.

Cancellation of If compensation mode is aborted by means of M2 (program end) without a prog-

com pensation rammed G40 instruction, then the last block ends with coordinates

using M2 corresponding to the compensation vector in normal position. No compensatory

movement is executed. The program ends with this tool positio n.

Critical machining When programming machining operations, watch out for cases where the contour

operations path at inner corners is smaller than the tool radius and, with two consecutive

inner corners, smaller than the diameter.

This type of programming error must be avoided!

Check sequences of several blocks to make sure that the contour does not

contain any “bottlene cks”.

When you carry out a test/dry run, use the largest available tool radius.

Programmed contour

B < R

Collision

R - Tool nose radius

B - Contour path

Remed

: Switch from G450 to G451 in this cas

Fig.3-39 Critical maching operation, ex ample shows transition circle

Programming

SINUMERIK 801 8-51

Operation and Program ming

—

Turning

8.6.8 Example of tool radius compensation

45°

R55

R30

R20

5203084020

Fig.8-40 Example of tool radius compensation, tool nose radius magnified

Programming N1 ; ;Contour section

example N2 T1 ;Tool 1 with offset D1

N10 G22 F... S... M... ;Radius dimension specification,

technological values

N15 G54 G0 G90 X100 Z15

N20 X0 Z6

N30 G1 G42 G451 X0 Z0 ;Begin compensation mod e

N40 G91 X20 CHF=(5* 1.41) ;Insert chamfer

N50 Z-25

N60 X10 Z-30

N70 Z-8

N80 G3 X20 Z-20 CR=20

N90 G1 Z-20

N95 X5

N100 Z-25

N110 G40 G0 G90 X100 ;End compensation mode

N120 M2

Programming

8-52 SINUMERIK 801

Operation and Program ming

—

Turning

8.7 Miscellaneous function M

Functionality Miscellaneous function M can be used, for example, to initiate switching

operations such as “Coolant ON/OFF”, among other tasks.

The control system manufacturer preassigns certain functions to a small

number of the M functions. The others can be freely assigned to functions by

the user.

A block may contain a maximum of 5 M functions.

Note

You will find an overview of all M functions reserved and used in the control

system in Section 8.1.5. “List of instructions”

Programming M...

Activation Activation in blocks with axis movements:

If functions M0, M1 and M2 are programmed in a block that includes axis

movements, then they take effect after the traversing movements have been

executed.

Functions M3, M4 and M5 are transferred to the internal interface control

before the traversing movements. The axis movements are not executed until

the spindle has run up in M3 or M4. In the case of M5, however, the axis

movements commence before the sp indle has reached a standstill.

All the other M functions are transferred to the internal interface control at the

same time as the traversing movements.

If you wish to program an M function specifically before or after an axis

movement, then insert a separate blo c k with the M function.

Remember: This block will interrupt G64 continuous path mode and generate

an exact stop!

Programming N10 S...

example N20 X... M3 ;M function in block with axis movement Spindle runs

up before X axis movement

N180 M78 M67 M10 M12 M37

;Max. 5 M functions in block

Programming

SINUMERIK 801 8-53

Operation and Program ming

—

Turning

8.8 Arithmetic parameters R

Functionality If you want an NC program in which you can vary the values to be processed,

or if you simply needed to compute arithmetic values, then you can use R

(arithmetic) parameters. The control system will calculate or set the values you

need when the program is executed.

An alternative method is to input the arithmetic parameter values directly. If the

R parameters already have value settings, then they can be assigned in the

program to other NC addresses that have variable values.

Programming R0=...

R249=...

(to R299=..., if there are no machining cycles)

Explanation 250 arithmetic pa rameters with the following cla ssification are available:

R0 ... R99 - for free assignment

R100 ... R249 - transfer parameters for machining cy cles.

R250 ... R299 - internal arithmetic parameters for m achining cycles.

If you do not intend to use machining cycles (see Section NO TAG “Machining

Cycles”), then this range of arithmetic parameters is also available for your

use.

Value assignment You can assign values in the followi ng range to the R parameters:

± (0.000 0001 ... 9999 9999)

(8 decimal places and sig n and decimal point).

The decimal point can be omitted for integer values. A positive sign can also

be omitted.

Example:

R0=3.5678 R1=-37.3 R2=2 R3=-7 R4=-45678.1234

You can assign an extended numerical range using exponential notation:

± ( 10-300 ... 10+300 ).

The value of the exponent is typed after the characters EX. Maximum number

of characters: 10 (including sign and decimal point).

Value range of EX: -300 to +300.

Example:

R0=-0.1EX-5 ;Meaning: R0 = -0,000 001

R1=1.874EX8 ;Meaning: R1 = 187 400 000

Note: Several assignments (including arithmetic expressions) can be

programmed in one bloc k.

Assignment to You can obtain a flexible NC program by assigning arithme tic parameters

other addresses or arithmetic expressions with R parameters to other NC addresses. Values,

arithmetic expressions or R parameters can be assigned to any NC address

with the exception of addresses N, G and L.

Programming

8-54 SINUMERIK 801

Operation and Program ming

—

Turning

When making assignments of this kind, type the character “=” after the

address character. Assignments with a negative sign are also permitted.

If you wish to make assignments to axis addresses (traversal instructions),

then you must do so in a separate p rog ram block.

Example:

N10 G0 X=R2 ;Assignment to X axis

Arithmetic opera- Operators/arith metic func tio ns mus t be pr ogrammed usin g the normal

tions / functions mathematical notation. Processing priorities are set by means o f round

brackets.

Otherwise the “multiplication/division before addition/ subtraction” rule applies.

Degrees are spe cified fo r trigonometric functions.

Programming N10 R1= R1+1 ;The new R1 is product of old R1 plus 1

example: R N20 R1=R2+R3 R4=R5-R6 R7=R8* R9 R10=R11/R12

parameter N30 R13=SIN(25.3) ;R13 is the sine of 25.3 degrees

N40 R14=R1*R2+R3 ;“Multiplication/division before addition/subtraction” rule

R14=(R1

*R2)+R3

N50 R14=R3+R2*R1 ;Result as for block N40

N60 R15=SQRT(R1*R1+R2*R2)

;Meaning: R15= R1

+R2

Programming N10 G1 G91 X=R1 Z=R2 F300

example: Assi- N20 Z=R3

gnment to axes N30 X=-R4

N40 Z=-R5

...

Programming

SINUMERIK 801 8-55

Operation and Program ming

—

Turning

8.9 Program branches

8.9.1 Labels - destination for program branches

Functionality Labels are used to mark blocks as the branch destination for branches in the

program sequence.

Labels can be selected freely, but must have a minimum of 2 and a maximum

of 8 letters or digits. However the first two characters must be letters or

underscore characters.

Labels end in a colon in the block that is to act as a branch destination. They

are always positioned at the beginning of the block. If the block also has a

block number, then the label is positioned after the number.

Labels must be unique within the same program.

Programming N10 MARKE1: G1 X20 ;MARKE1 is label, branch destination

example ...

TR789: G0 X10 Z20 ;TR789 is label, branch destination No block number

Programming

8-56 SINUMERIK 801

Operation and Program ming

—

Turning

8.9.2 Unconditional program branches

Functionality NC programs process the blocks they contain in the same order as they were

typed by the programmer.

The processing sequence can be altered through the insertion of program

branches.

The only possible branch destination is a block with label. This block must be

included in the program.

An unconditional branch instruction must be programmed in a separate block.

Programming GOTOF Label ;Branch forwards

GOTOB Label ;Branch backwards

STL Explanation

GOTOF Branch direction forwards (towards last block in program)

GOTOB Branch direction backwards (towards first block in program)

Label Selected ch aracter string for label

Fig.8-41 Example of unconditional branches

Program

sequence ...

...

N20 GOTOF MARKE0 ; Branch to label0

...

N50 MARKE0: R1 = R2+R3

N51 GOTOF MARKE1 ; Branch to label1

...

G0 X... Z...

...

MARKE2: X... Z...

N100 M2 ;End of program

MARKE1: X... Z...

N150 GOTOB MARKE2 ; Branch to label2

Programming

SINUMERIK 801 8-57

Operation and Program ming

—

Turning

8.9.3 Conditional branches

Functionality Branch conditions are formulated after the IF instruction. If the branch

condition is fulfilled (value not equal to zero), then the program branches. The

branch destination can only be a block with corresponding label. This block

must be cont ained within the program.

Conditional branch instructions must be programmed in a separate block.

Several conditional branch instructions can be programmed in the sam e block.

You can reduce program processing times significantly by using conditional

program bran che s.

Programming IF condition GOTOF L abel ;Branch forwards

IF condition GOTOB Label ;Branch backwards

STL Explanation

GOTOF Branch direction forwards (towa rd s la st block in program)

GOTOB Branch direction backwa rds (towards first block in program)

Label Selected character string for label

IF Introduction of branch condition

Condition Arithmetic parameter, arithmetic expression in comparison for

formulation of condition

Comparison operations

Operators Meaning

= = Equal to

< > Not equal to

> Greater than

< Less than

> = Greater than or equal to

< = Less than or equal to

The comparison operations are used to formulate branch conditions.

Arithmetic expressions can also be compared.

The result of comparison operations is either “fulfilled” or “not fulfilled”. “Not

fulfilled” is equivalent to a value of zero.

Programming R1>1 ;R1 greater than 1

example for 1 < R1 ;1 less than R1

comparison R1<R2+R3 ;R1 less than R2 plus R3

operators R6>=SIN( R7*R7 ) ;R6 greater than or equal to SIN (R7)2

Programming N10 IF R1 GOTOF MARKE1 ;If R1 is not zero, branch to block with

example MARKE1

...

N100 IF R1>1 GOTOF MARKE2 ;If R1 is greater than 1, branch to block with

MARKE2

...

Programming

8-58 SINUMERIK 801

Operation and Program ming

—

Turning

N1000 IF R45==R7+1 GOTOB MARKE3

;If R45 is equal to R7 plus 1, branch to block

with MARKE3

...

Several conditional branches in bloc k:

...

N20 IF R1==1 GOTOB MA1 IF R1==2 GOTOF MA2 ...

...

Note: The program branches at the first fulfilled condition.

Programming

SINUMERIK 801 8-59

Operation and Program ming

—

Turning

8.9.4 Example of program with branches

Objective of Approach points on an circle segment:

program Let us assume the following values:

Start angle: 30° in R1

Circle radius: 32 mm in R2

Position spacing: 10° in R3

Number of points: 11 in R4

Position of circle center point in Z: 50 mm in R5

Position of circle center point in X: 20 mm in R6

R4 = 11 (No. of points)

Pnt.1

Pnt.2

Pnt.11 R3

Pnt.10

Pnt.3

Fig.8-42 Approaching points along a circle segm ent

Programming N10 R1=30 R2=32 R3=10 R4=11 R5=50 R6=20

example ;Assignment of start values

N20 MA1: G0 Z=R2 *COS (R1)+R5 X=R2*SIN(R1)+R6

;Computation and assignment to axis addresses

N30 R1=R1+R3 R4= R4-1

N40 IF R4 > 0 GOTOB MA1

N50 M2

Explanation The initial conditions are assigned to the appropriate arithmetic parameters in

block N10. The coordinates in X and Z are calculated in N20 and processed.

In N30, R1 is increased by the angle R3 and R4 is decremented by 1. If R4 >

0, N20 is processed again. Otherwise the program continues with N50 and

end of program.

Programming

8-60 SINUMERIK 801

Operation and Program ming

—

Turning

8.10 Subroutine technique

Application There is no essential difference between a main program and a subroutine.

Subroutines contain frequently recurring machining sequences, for example,

certain contour shapes. This type of subroutine is called at the appropriate

locations in the main program and then proce s sed.

One type of subroutine is the machining cycle. Machining cycles contain

generally applicable machining operations (e.g. thread cutting, stock removal,

etc.). By supplying these cycles with values by means of the arithmetic

parameters provided, you can adapt the program to your specific application

(see Section “Machining Cycles”).

Structure Subroutines are structured in exactly the same way as main programs (see

Section “Program structure”). M2 (end of program) is programmed in the last

block of the subroutine sequence in exactly the same way as for main

programs. In this case, program end means a return to the program level that

called the subroutine.

Program end The M2 end–of–program instruction can be substituted by the end instruction

RET in subroutines.

RET must be programmed in a sepa rate block.

An RET instruction must be used when it is necessary to avoid an interruption

in continuous path mode G64 when the program branches back to main

program level from the subroutine. If an M2 instruction is programmed, G64

mode is interrupted and an exact stop generated.

N20 X...Z...

N10 R1=34 ...

L10

N20 L10 ;Call

N80 L10 ;Call

N21 ...

Main program

Subroutine

Return

MAIN123

...

Sequence

Fig. 8-43 Example of program sequence in which subroutine is called twice

Programming

SINUMERIK 801 8-61

Operation and Program ming

—

Turning

Subroutine name A subroutine is given its own specific name so that it can be selected from all

the others. The name can be chosen freely subject to the following conditions

when the subroutine is generated:

— The first two characters must be letters

— The others may be letters, digits or underscore

— Maximum of 8 characters in total

— No dashes (see Section “Character set”)

The same rules apply as for main program names.

Example: BUCHSE7

There is the additional option of using the address word L... for subroutines.

This value may have 7 decimal places (integers o nly).

Please note: Leading zeros are interpreted as distinguishing digits in the L

address.

Example: L128 is not L0128 or L00128!

These are 3 different subroutines!

Subroutine call Subroutines are called by their name in a program (main program or

subroutine). These calls must be programmed in separate blocks.

Example:

N10 L785 ;Call subroutine L785

N20 WELLE7 ;Call subroutine WELLE7

Program repeat P...

If a subroutine must be repeated several times in succession, then enter the

number of runs under address P after the subroutine name in the block

containing the subroutine call. A maximum of 9999 runs can be programmed

(P1 ... P9999).

Example:

N10 L785 P3 ;Call subroutine L785, 3 runs

Nesting depth It is not only possible to call subroutines in main programs, but also in other

subroutines. There is a total of 4 program levels (including the main program

level) available for programming this typ e of nested call.

Note: If you are working with machining cycles, please remember that these

also need one of the four program levels.

1st level 2nd level 3rd level 4th level

Main program

Subroutine Subroutine

Subroutine

Fig.8-44 Sequence with four program levels

Programming

8-62 SINUMERIK 801

Operation and Program ming

—

Turning

Information It is possible to change modal G functions, e.g. G90 -> G91, in subroutines.

Make sure that all modal functions are set in the way you require when the

program branches back to the level on which the subroutine was called.

The same applies to the arithmetic (R) parameters. Make sure that the

arithmetic parameters you are using in the upper program levels do not

change to dif f erent settings in lower levels.

SINUMERIK 801 9-1

Operation and Program ming

—

Turning

Cycles 9

Preface Cycles are process-related subroutines that support general implementation of

specific machining processes such as, for example, drilling, stock removal or

thread cutting. The cycles are adapted to the specific problem in hand by

means of supply parameters.

Standard cycles for turning applications are provided in the system.

9.1 General Information about Standard Cycles

This section provides general programming notes for SIEMENS standard

cycles.

9.1.1 Overview of Cycles

LCYC82 Drilling, spot-facing

LCYC83 Deep hole drilling

LCYC840 Tapping with compensation chuck

LCYC85 Boring

LCYC93 Recess

LCYC94 Undercut (forms E and F to DIN)

LCYC95 Stock removal with relief cuts

LCYC97 Thread cutting

Supply parameters The arithmetic parameters in the R100 to R249 range are used as supply

parameters for cycles.

Before a cycle is called, values must be assigned to its transfer parameters.

These value settings are unch anged after the cycle has been executed.

Arithmetic If you intend to use machining cycles, y ou must ensure t hat arit hmetic p a rameters

parameters R100 to R249 are reserved for this purpose, and are not used for other

functions within the program. The cycles use R250 to R299 as internal

arithmetic parameters.

Cycles

9-2 SINUMERIK 801

Operation and Program ming

—

Turning

Call and return G23 (for LCYC93, 94, 95, 97) or G17 (for LCYC82, 83, 840, 85)

conditions (diameter programming) must be active before a cycle is called. Otherwise,

the error message 17040 illegal axis index is output. The appropriate values

for feedrate, spindle speed and spindle direction of rotation must be

programmed in the part program if there are no supply parameters for these

quantities in the cycle.

G0 G90 G40 are always effective at the end of a cycle.

9.1.2 Error messages and error handling in cycles

Error handling Alarms with numbers between 61001 and 62999 are generated in the

cycles.

in cycles In turn, this number range is subdivided into alarm reactions and reset criteria.

Table 9–1 Alarm numbers, reset criteria, alarm reactions

Alarm number Reaction Program

continued by

61001...61999 Block preparation in the NC is aborted NC RESET

62000...62999 Block preparation is interrupted, can be

continued with NC start after alarm

reset

Reset key

The error text that is displayed at the same time as the alarm number provides

further details about the cause of the error.

Overview of The following Table gives an overview of errors that can occur in cycles,

the

cycle alarms location of their origin and guida nce on how to eliminate them.

Cycles

SINUMERIK 801 9-3

Operation and Program ming

—

Turning

Table 9–2 Cycle alarms

Alarm

Number Alarm Text Source (Cycle) Remedial Action

61001 Thread lead incorrectly

defined LCYC840 Check p arameter R106 (R106=0).

61002 “Machining type incorrectly

programmed” LCYC93, 95, 97 The value of parameter R105 for the

machining type is incorrectly set and

must be altered.

61102 No spindle direction defined LCYC840 Value in parameter R107 is greater than

4 or less than 3.

61107 “First drilling depth incorrectly

defined” LCYC83 Change the value for 1st drilling depth

(first drilling depth is in opposition to total

drilling depth)

61601 “Finished part diameter too

small” LCYC94 A finished part diameter of < 3mm is

programmed. This setting is illegal.

61602 “Tool width incorrectly

defined” LCYC93 The tool width (parameter R107) does

not match the programmed recess type.

61603 “Recess form incorrectly

defined” LCYC93 The recess form is incorrectly

programmed.

61606 “Error when preparing the

contour” LCYC95 Check contour subroutine.

Check machining type parameter (R105)

61608 “Incorrect tool point direction

programmed” LCYC94 A tool point direction 1 ... 4 that matches

the undercut form must be progra mmed.

61609 “Form incorrectly defined” LCYC94 Check parameters for undercut form.

61610 “No infeed depth

programmed” LCYC95 The parameter for infeed depth R108

must be set >0 for roughing.

Cycles

9-4 SINUMERIK 801

Operation and Program ming

—

Turning

9.2 Drilling, counter boring – LCYC82

Function The tool drills with the spindle speed and feedrate programmed down to the

entered final depth. When the final drilling depth is reached, a dwell time can

be programmed. The drill is retracted from the drill hole at rapid traverse rate.

Call LCYC82

Fig.9-1 Motional sequence and parameters in the cycle

Precondition The spindle speed and the direction of rotation, as well as the feed of the

drilling axis must be defined in the higher-level program.

The drilling position must be approached before calling the cycle in the

higher-level program.

The required tool with tool of fset must be sele cted before calling the cycle.

Parameters Parameter Meaning, Value Range

R101 Retract plane (absolute)

R102 Safety clearance

R103 Reference plane (ab solute )

R104 Final drilling depth (ab solu t e)

R105 Dwell time in seconds

Information

R101 The retract plane determines the position of the drilling axis at the end of the

cycle.

R102 The safety clearance acts on the reference plane, i.e. the reference plane is

shifted forward by an amount corresponding to the safety clearance.

The direction in which the safety clearance acts is automatically determined

by the cycle.

R101

R103+R102

R103

R104

Cycles

SINUMERIK 801 9-5

Operation and Program ming

—

Turning

R103 The starting point of the drill hole shown in the drawing is programmed under

the reference plane parameter.

R104 The drilling depth is always programmed as an absolute value with refer to

workpiece zero.

R105 The dwell time at drilling depth (chip breakage) is programmed in seconds

under R105.

Motional sequence Position reached prior to beginning of cycle:

last position in the higher-level program (drilling positi on)

The cycle produces the following motional seq uence:

1. Approach reference plane shifted forward by an amount corresponding

to the safety clearance using G0.

2. Traverse to final drilling depth with G1 and the feedrate programmed in

the higher-level program.

3. Execute dwell time to final drilling depth.

4. Retract to retract plane with G0.

Example Drilling - counter boring

The program produces a 27 mm deep drill hole in the position X0 in G17 plane

using the cycle LCYC82. The dwell time is 2 s, and the safety clearance in the

drilling axis (here: Z) amounts to 4 mm. On completion of the cycle, the tool

stands on X0 Z110.

102

Fig.9-2 Example drawing

N10 G0 G17 G90 F500 T2 D1 S500 M4 ; Define technology values

N20 X0 ; Approach drilling position

N25 G17

N30 R101=110 R102=4 R103=102 R104=75 ; Supply parameters

N35 R105=2 ; Supply parameters

N40 LCYC82 ; Call cycle

N50 M2 ; End of program

Cycles

9-6 SINUMERIK 801

Operation and Program ming

—

Turning

9.3 Deep hole drilling – LCYC83

Function The deep-hole drilling cycle produces center holes down to the final drilling

depth by repeated, step-by-step deep infeed whose maximum amount can be

parameterized. The drill can be retracted either to the reference plane for

swarf removal after each infeed depth or by 1 mm in each case for chip

breakage.

Call LCYC83

R101

2 n d d rillin g d e p th

1 s t d rillin g d e pth

R110

etc.

Clearance distance

Note

In th e d ia gra m, th e c le ara n ce d is ta n ce to th e c u rre n t d rillin g d e p th is

shown only for the 1st drilling depth. In reality, it’s effective for every

drilling depth.

R104

Ne x t d rillin g d e pth

...

This m otional sequence is repeated

fo r e a c h d rillin g d e p th

current drill. depth

R103 + R 102

R103

Fig.9-3 Motional sequence and parameters in the cycle

Precondition The spindle speed and the direction of rotation must be defined in the

higher-level program.

The drilling position must be approached before calling the cycle in the

higher-level program.

Before calling the cycle, a tool offset for the drill must be selected.

G17 must be active.

Cycles

SINUMERIK 801 9-7

Operation and Program ming

—

Turning

Parameters Parameter Meaning, Value Range

R101 Retract plane (absolute)

R102 Safety clearance, enter without sig n

R103 Reference plane (ab solute )

R104 Final drilling depth (ab solu t e)

R105 Dwell time to drilling depth (chip breakage)

R107 Feed for drilling

R108 Feed for first drilling depth

R109 Dwell time at sta rting point and for swarf removal

R110 First drilling depth (absolute)

R111 Absolute degression, enter without sign

R127 Machining type:

Chip breakage = 0

Swarf removal = 1

Information

R101 The retract plane determines the position of the drilling axis at the end of the

cycle.

The cycle is programmed on the assumption that the retract plane positioned

in front of the reference plane, i.e. its distance to the final depth is greater.

R102 The safety clearance acts on the reference plane, i.e. the reference plane is

shifted forward by an amount corresponding to the safety clearance.

The direction in which the safety clearance acts is automatically determined

by the cycle.

R103 The starting point of the drill hole shown in the drawing is programmed under

the reference plane parameter.

R104 The drilling depth is always programmed as an absolute value regardless of

how G90/91 is set prior to cycle call.

R105 The dwell time at drilling depth (chip breakage) is programmed in seconds

under R105.

R107, R108 The feed for the first drilling stroke (under R108) and for all subsequent drilling

strokes (under R107) are programm ed via the parameters.

R109 A dwell time at the starting point can be programmed in seconds under

parameter R 109.

The dwell time at the starting point is executed only for the “with swarf

removal” variant.

R110 Parameter R110 determines the depth of the first drilling stroke.

Cycles

9-8 SINUMERIK 801

Operation and Program ming

—

Turning

R111 Parameter R111 for the absolute degression value determines the amount by

which the current drilling depth is reduced with subse quent drilling strokes.

The second drilling depth corresponds to the stroke of the first drilling depth

minus the absolute degression value provided that this value is greater than

the programmed absolute degression value.

Otherwise, the second drilling depth also corresponds to the absolute

degression value.

The next drilling strokes correspond to the absolute degression value provided

that the remaining degression depth is still greater than twice the absolute

degression value. The remainder is then distributed evenly between the last

two drilling strokes.

If the value for the first drilling depth is in opposition to the total drilling depth,

the error message 61107 “First drilling depth incorrectly defined” is displayed,

and the cycle is not executed.

R127 Value 0:

The drill travels 1 mm clear for chip breakage after it has reached each drilling

depth.

Value 1:

The drill travels to the reference plane, which is shifted forward by an amount

corresponding to the safety clearance for swarf removal after each drilling

depth.

Motional sequence Position reached prior to beginning of cycle:

last position in the higher-level program (drilling positi on)

The cycle produces the following motional seq uence:

1. Approach reference plane shifted forward by an amount corresponding

to the safety clearance using G0.

2. Traverse to first drilling depth with G1; the feedrate results from the

feedrate programmed prior to cycle call after it has been computed with

the setting in parameter R109 (feedrate facto r).

Execute dwell time at drilling depth (para meter R105).

With chip breakage selected:

Retract by 1 mm from the current drilling depth with G1 for chip

breakage.

With swarf removal selected:

Retract for swarf removal to reference plane shifted forward by an

amount corresponding to the safety clearance with G0 for swarf removal,

executing the dwell time at starting point (parameter R106), approach

last drilling depth minus clearance distance calculated in the cycle using

G0.

3. Traverse to next drilling depth with G1 and the programmed feed; this

motional sequence is continued as long as the final drilling depth is

reached.

4. Retract to retract plane with G0.

Cycles

SINUMERIK 801 9-9

Operation and Program ming

—

Turning

Example: Deep-hole drilling

1455 1

1002020

Fig. 9-4 Example drawing

;This program executes the cycle LCYC83 at position X0.

N100 G0 G18 G90 T4 S500 M3 ;Define technology values

N110 Z155

N120 X0 ;Approach first drilling position

N125 G17

R101=155 R102=1 R103=150

R104=5 R105=0 R109=0 R110=100 ;Parameter assignment

R111=20 R107=500 R127 =1 R108=400

N140 LCYC83 ;1st call of cycle

N199 M2

Cycles

9-10 SINUMERIK 801

Operation and Program ming

—

Turning

9.4 Tapping with compensating chuck – LCYC840

Notice:

This cycle function can be active only when a servo spindle is used.

Function The tool drills with the programmed spindle speed and direction of rotation

down to the entered thread depth. The feed of the drilling axis results from the

spindle speed. This cycle can be used for tapping with compensating chuck

and spindle actual-value encoder. The direction of rotation is automatically

reversed in the cycle. The retract can be carried out at a separate speed. M5

acts after the cycle has been executed (spindle stop).

Call LCYC840

Fig.9-5

Precondition This cycle can only be used with a speed-controlled spindle with position

encoder. The cycle does not check whether the actual-value encoder for the

spindle really exists.

The spindle speed and the direction of rotation must be defined in the

higher-level program.

The drilling position must be approached before calling the cycle in the

higher-level program.

The required tool with tool of fset must be sele cted before calling the cycle.

G17 must be active.

Parameters Parameter Meaning, Value Range

R101 Retract plane (absolute)

R102 Safety clearance

R103 Reference plane (ab solute )

R104 Final drilling depth (ab solu t e)

R106 Thread lead as value

value range: 0.001 .... 2000.000 mm

R126 Direction of rot ation of spindle for tapping

G33

R101

R103

R103+R102

R104

Cycles

SINUMERIK 801 9-11

Operation and Program ming

—

Turning

Value range: 3 (for M3), 4 (for M4)

Cycles

9-12 SINUMERIK 801

Operation and Program ming

—

Turning

Information

R101 -R104 See LCYC84

R106 Thread lead as value

R126 The tapping block is executed with the direction of rotation of spindle

programmed under R126. The direction of rotation is automatically reversed in

the cycle.

Motional sequence Position reached prior to beginning of cycle:

- last position in the higher-level program (drilling position)

The cycle produces the following motional seq uence:

1. Approach reference plane shifted forward by an amount corresponding

to the safety clearance using G0

2. Tapping down to final drilling depth with G33

3. Retract to reference plane shifted forward by an amount corresponding

to the safety clearance with G33

4. Retract to retract plane with G0

Example This program is used for tapping on the position X0; the Z axis is the drilling

axis. The parameter for the direction of rotation R126 must be parameterized.

A compensating chuck must be used for machining. The spindle speed is

defined in the higher-level program.

Fig.9-6 Example drawing

N10 G0 G17 G90 S300 M3 D1 T1 ; Define technology values

N20 X0 Z60 ; Approach drilling position

G17

N30 R101=60 R102=2 R103=56 R104=15 ; Parameter assi gnment

N40 R106=0.5 R126=3 ; Parameter assignment

N40 LCYC840 ; Cycle call

N50 M2 ; End of program

Cycles

SINUMERIK 801 9-13

Operation and Program ming

—

Turning

9.5 Boring – LCYC85

Function The tool drills with the spindle speed and feedrate programmed down to the

entered final drilling depth. When the final drilling depth is reached, a dwell

time can be programmed. The approach and retract movements are carried

out with the feedrates programmed u nder the respective parameters.

Call LCYC85

Fig.9-7 Motional sequence and p arameters of the cycle

Precondition The spindle speed and the direction of rotation must be defined in the

higher-level program.

The drilling position must be approached before calling the cycle in the

higher-level program.

Before calling the cycle, the respective tool with tool offset must be selected.

Parameters Parameter Meaning, Value Range

R101 Retract plane (absolute)

R102 Safety clearance

R103 Reference plane (ab solute )

R104 Final drilling depth (ab solu t e)

R105 Dwell time at drilling depth in seconds

R107 Feed for drilling

R108 Feed when retracting from drill hole

Information

Parameters R101 - R105 see LCYC82

R107 The feed value defined here acts for drilling.

R108 The feed value entered under R108 acts for retracting from the drill

hole.

R104

R101

R103+R102

R103

Cycles

9-14 SINUMERIK 801

Operation and Program ming

—

Turning

Motional sequence Position reached prior to beginning of cycle:

last position in the higher-level program (drilling positi on)

The cycle produces the following motional seq uence:

1. Approach reference plane shifted forward by an amount corresponding

to the safety clearance using G0

2. Traverse to final drilling depth with G1 and the feed programmed under

parameter R 106.

3. Execute dwell time at final drilling depth.

4. Retract to reference plane shifted forward by an amount corresponding

to the safety clearance with G1 and the retract feed programmed under

R108.

Example The cycle LCYC85 is called in X0 in G17 plane. The Z axis is the drilling axis.

No dwell time is programmed. The workpiece upper edge is at Z=102.

102

Fig.9-8 Example drawing

N10 G0 G90 G17 F1000 S500 M3 T1 D1 ; Define technology values

N20 Z102 X0 ; Approach drilling position

N30 R101=105 R102=2 R103=102 R104=77 ; Define parameters

N35 R105=0 R107=200 R108=400 ; Define parameters

N40 LCYC85 ; Call drilling cycle

N50 M2 ; End of program

Cycles

SINUMERIK 801 9-15

Operation and Program ming

—

Turning

9.6 Recess cycle – LCYC93

Fuction The recess cycle is designed to produce symmetrical recesses for longitudinal

and face machining on cylindrical contour elements. The cycle is suitable for

machining internal and external recesses.

Call LCYC93

R101

R108

R116

R114 R118

R116 R115 R100

R117

Fig.9-9 Parameters in the recess cycle in longitudinal machining

Precondition The recess cycle can only be called if G23 (diameter programming) is active.

The tool offset of the tool whose tool nose width has been programmed with

R107 must be activated before the recess cycle is called. The zero position of

the tool nose faces machine zero.

Parameters Table 9–3 Parameters for LCYC93 cycle

Parameter Meaning, Value Range

R100 Starting point in facing axis

R101 Starting point in longitudinal axis

R105 Machining method,

Value range 1 ... 8

R106 Finishing allowance, without sign

R107 Tool nose width, without sign

R108 Infeed depth , without sign

R114 Recess width , without sign

R115 Recess width , without sign

R116 Flank angle, without sign,

between 0 <= R116 < = 89.999 degrees

R117 Chamfer on rim of recess

R118 Chamfer on recess base

R119 Dwell time on recess base

Information

R100 The recess diameter in X is specified in parameter R100.

Cycles

9-16 SINUMERIK 801

Operation and Program ming

—

Turning

R101 R101 determines the point at which the recess starts in the Z axis.

R105 R105 defines the recess variant:

Table 9–4 Recess variants

Value Longitudinal/Facing External/Internal Starting Point Position

1 L A Left

2 P A Left

3 L I Left

4 P I Left

5 L A Right

6 P A Right

7 L I Right

8 P I Right

If the parameter is set to any other value, the cycle is aborted with the alarm

61002 “Machining type incorrectly programmed”.

R106 Parameter R106 determines the finishing allowance for roughing of the

recess.

R107 Parameter R107 determines the tool nose width of the recessing tool. This

value must correspond to the width of the tool actu ally used.

If the tool nose of the active tool is wider, the contour of the programmed

recess will be violated. Such violations are not monitored by the cycle.

If the programmed tool nose width is wider than the recess width at the base,

the cycle is aborted with the alarm

G1602 “Tool width incorrectly defined”.

R108 By programming an infeed depth in R108, it is possible to divide the

axis-parallel recessing process into several infeed depths. After each infeed,

the tool is retracted by 1 mm for chip breakage.

Recess form Parameters R114 ... R118 determine the form of the recess. The cycle always

bases its calculation on the point programmed un der R100, R101.

R114 The recess width programmed in parameter R114 is measured on the base.

The chamfers are not included in the measu rem ent.

R115 Parameter R115 determines the depth of the recess.

R116 The value of parameter R116 determines the angle of the flanks of the recess.

When it is set to “0”, a recess with axis-parallel flanks (i.e. rectangular form) is

machined.

R117 R117 defines the chamfers on the recess rim.

R118 R118 defines the chamfers on the recess base.

Cycles

SINUMERIK 801 9-17

Operation and Program ming

—

Turning

If the values programmed for chamfers do not produce a meaningful recess

contour, then the cycle is aborted with the alarm

61603 “Recess form incorrectly defined”.

R119 The dwell time on the recess base to be entered in R119 must be selected

such that at least one spindle revolution can take place during the dwell period.

It is programmed to comply with an F word (in seconds).

Motional Sequence Position reached prior to beginning of the cycle:

z Any position from which each recess can be approached without risk of

collision.

The cycle produces the following motional seq uence:

z Approach with G0 st arting point cacluated internally in the cycle.

z Execute depth infeeds:

Roughing in parallel axes down to base, taking finishing allowance into

account. Tool travels clear for chip breakage af ter each infeed.

z Execute widt h infeeds:

Width infeeds are executed perpendicular to the depth infeed with G0,

the roughing process for machining the depth is repeated.

The infeeds both for depth and width are distributed evenly with the highest

possible value.

z Rough the flanks. Infeed along the recess width is executed in several

steps if necessary.

z Finish-machine the whole contour, starting at both rims and working

towards center of recess base, at the feedrate programmed before the

cycle call.

Example

Chamfers 2mm

Starting point (95, 60)

R108=10

20°20°

25 mm

Fig.9-10 Example diagram

;A recess is machined that st arts at point (95.60), 47mm in depth

;and 30 mm in width.

;Two chamfers of 2 mm in length are programmed on the base.

;The finishing allowance is 1 mm.

Cycles

9-18 SINUMERIK 801

Operation and Program ming

—

Turning

N10 G0 G90 Z100 X100 T 2 D1 S300 M3 G23 ;Select start position

N20 G95 F0.3 ;and technology values

R100=60 R101=95 R105=5 R106=1 R107=12 ;Parameters for cycle call

R108=10 R114=30 R115=47 R116=20

R117=0 R118-2 R119=1

N60 LCYC93 ;Call recess cycle

N70 G90 G0 Z100 X50 ;Next position

N100 M2

Note on example The tool offset of the recessing tool must be stored in D1 of tool T2. The tool

nose width m ust be 12 mm.

Cycles

SINUMERIK 801 9-19

Operation and Program ming

—

Turning

9.7 Undercut cycle – LCYC94

Function This cycle machines undercuts of forms E and F in compliance with DIN 509

for normal stressing on finished pa rt diameters > 3 mm.

A tool offset must be activated before the cycle is called.

Call LCYC94

FORM E FORM F

For workpieces with

one machining

surface

For workpieces with

two mutually

perpendicular

machining surfaces

R101

R100

Fig.9-11 Undercut forms E and F

Condition G23 (diameter programming) must be active for this cycle.

Parameters Table 9–5 Parameters for LCYC94 cycle

Parameter Meaning, Value Range

R100 Starting poi nt in facing axis, without sign

R101 Starting poi nt in longitudinal axis

R105 Definition of form:

Value 55 for form E

Value 56 for form F

R107 Definition of tool point direction:

Values 1...4 for directions 1...4

Information

R100 The finished part diameter for the undercut is specified in p arameter R100.

If the value programmed for R100 corresponds to a final diameter of <= 3 mm,

then the cycle is aborted with the alarm

61601 “Finished part diame t er too small”.

R101 R101 determines the finished part dimension in the longitudinal axis.

R105 Forms E and F are defined in DIN509 and must be selected using one of

these parameters.

Cycles

9-20 SINUMERIK 801

Operation and Program ming

—

Turning

If parameter R105 is set to a value other than 55 or 56, then the cycle is

aborted and generates the alarm

61609 “Form incorrectly defined”.

R107 This parameter defines the tool point direction and thus the undercut position.

The value set here must correspond to the actual point direction of the tool

selected prior t o cycle call.

SL 3

Tool nose

radius

Theoretical

nose tip

SL 4

SL 2

SL 1

Fig.9-12 Tool point directions 1…4

If the parameter is set to any other value, the alarm

61608 “Incorrect tool point direction programmed” is output and the cycle is

aborted.

Motional sequence Position reached prior to beginning of cycle:

z Any position from which undercut can be approached without risk of

collission.

The cycle produces the following motional seq uence:

z Approach with G0 st arting point calculated internally in the cycle.

z Select tool nose radius compensation in accordance with active tool

nose direction and traverse undercut contour at feedrate programmed

prior to cycle call.

z Return to starting point with G0 and deselect tool nose radius

compensation with G40.

Example ;This program machines an undercut of form E.

N50 G0 G90 G23 Z100 X50 T25 D3 S300 M3 ;Select starting positio n

N55 G95 F0.3 ;and enter technology values

R100=20 R101=60 R105=55 R107 =3 ;Parameters for cycle call

N60 LCYC94 ;Call undercut for cycle

N70 G90 G0 Z100 X50 ;Next position

N99 M02

Cycles

SINUMERIK 801 9-21

Operation and Program ming

—

Turning

9.8 Stock removal cycle – LCYC95

Function This cycle can machine a contour, which is programmed in a subroutine, in a

longitudinal or face machining process, externally or internally, through

axis-parallel stock removal.

The technology (roughing/finishing/complete machining) can be selected. The

cycle can be called from any cho sen collision-free position.

A tool offset must have been activated in the pro gram with the cycle call.

Call LCYC95

Contour shifted by

finishing allowance

Original contour

Infeed

1 Infeed

2 Roughing

3 Cut residual

corners

4 Lift

5 Return

Fig.9-13 Motional sequence with LCYC 95 cycle

Condition

z The cycle requires an a ctive G23 (diame ter programming).

z The file SGUD.DEF, which is supplied on the cycles diskette, must be

available in the control system.

z The stock removal cycle can be called to the 3rd program level.

Parameters Table 9–6 Parameters for the LCYC95 cycle

Parameter Meaning, Value Range

R105 Machining type,

value range 1 ... 12

R106 Finishing allowance, without sign

R108 Infeed depth, without sign

R109 Infeed angle for roughing, it should be zero at face

machining.

R110 Contour clea rance distance for roughing

R111 Feedrate for roughing

R112 Feedrate for fi nishing

Cycles

9-22 SINUMERIK 801

Operation and Program ming

—

Turning

Information

R105 The machining types:

z longitudinal/facing

z internal/external

z roughing/finishing/complete machining

are defined by the parameter determini ng the type of machining.

When longitudinal machining is selected, the infeed always takes place in the

facing axis, and vice versa.

Table 9–7 Variants of stoc k removal

Value Longitudinal/Facing

(P) External/Internal

(A/I) Roughing/Finishing/

Complete Machining

1 L A Roughing

2 P A Roughing

3 L I Roughing

4 P I Roughing

5 L A Finishing

6 P A Finishing

7 L I Finishing

8 P I Finishing

9 L A Complete

10 P A Complete

11 L I Complete

12 P I Complete

If any other value is programmed for the parameter, the cycle is aborted and

the following alarm output

61002 “Machining type incorrectly programmed”.

R106 A finishing allowance can be programm ed in parameter R106.

The workpiece is always rough-machined down to this finishing allowance. In

this case, the residual corner produced in the course of each axis-parallel

roughing process is immediately cut away in parallel with the contour at the

same time. If no finishing allowance is programmed, the workpiece is

rough-machined right down to the final contour.

R108 The maximum possible infeed depth for the roughing process is entered under

parameter R108. However, the cycle itself calculates the current infeed depth

that is applied in rough-machining o perations.

R109 The infeed motion for roughing can be executed at an angle which can be

programmed in parameter R109. In the face machining process a slanting

immerse is not possible, R109 must be programmed to ZERO.

R110 Parameter R110 specifies the distance by which the tool is lifted from the

contour in both axes after each roughing operation so that it can be retracted

by G0.

Cycles

SINUMERIK 801 9-23

Operation and Program ming

—

Turning

R111 The feedrate programmed under R111 applies to all paths on which stock is

removed during roughing operations.

If finishing is the only machining type selected, then this parameter has no

meaning at all.

R112 The feedrate programmed under R112 is applied for finishing operations. If

roughing is the only machining type selected, then this parameter has no

meaning at all.

Contour definition The contour to be machined by stock removal is programmed in a subroutine.

The name of the subroutine is transferred to the cycle via the _CNAME

variable.

The contour may consist of straight lines and circle segments; radii and

chamfers can be inserted. The programmed circle sections can be quarter

circles as a maximum.

Undercuts may not be contained in the contour. If an undercut element is

detected, the cycle is aborted, and the alarm

61605 “Contour incorrectly defined” is output.

The contour must always be programmed in the direction that is traversed

when finishing according to the selected machining direction.

Example of contour programming

P8(35,120)

P0 = program m ed starting point of contour

P8 = program m ed end point

P0(100,40)

P1(85,40)

P2(85,54)

P3(77,70)

P4(67,70)

P5(62,80)

P6(62,96)

P7(50,120)

Fig.9-14 Example of contour programming

With the coordinates given in the program, the contour must be programmed

for longitudinal external machining as follows:

N10 G1 Z100 X40 ;Starting point

N20 Z85 ;P1

N30 X54 ;P2

N40 Z77 X70 ;P3

Cycles

9-24 SINUMERIK 801

Operation and Program ming

—

Turning

N50 Z67 ;P4

N60 G2 Z62 X80 CR=5 ;P5

N70 G1 Z62 X96 ;P6

N80 G3 Z50 X120 CR=12 ;P7

N90 G1 Z35 ;P8

For external facing, the contour must be programmed starting at P8 (35,120)

and finishing at P0 (100,40).

Motional sequence Position reached prior to beginning of cycle:

z Any position from which the contour starting point can be approached

without risk of collision.

The cycle produces the following motional seq uence

Roughing

z Approach cycle starting point (calculated internally) with G0 in both axes

simultaneously.

z Perform depth infeed with the angle programmed under R109 to the next

roughing depth.

z Approach roughing cut point in parallel axes with G1 and at a feedrate

programmed in R111.

z Travel in parallel with contour along contour + finishing allowance up to

the last roughing cut point with G1/G2/G3 and at feed rate R111.

z Lift in each axis by the clearance (in mm) programmed in R110 and

retract with G0.

z Repeat this sequence until the final roughing depth is reached.

Finishing

z Approach the cycle starting point in individual axes with G0

z Approach the contour starting point in both axes simultaneously with G0.

z Finish-machine along the contour with G1/G2/G3 and at the feedrate

programmed in R112.

z Retract to cycle starting point in both axes with G0.

When finishing is selected, the tool radius compensation is automatically

activated internally in the cycle.

Starting point The cycle automatically calculates the point at which machining must start.

The starting point is always approached in both axes simultaneously for

roughing and in individual axes for finishing. In this case, the infeed axis

approaches the starting point first.

When complete machining is selected, the tool does not return to the internally

calculated starting point after the la st roughing cut.

Cycles

SINUMERIK 801 9-25

Operation and Program ming

—

Turning

Example The cycle requires the follo wing two programs:

z program with cycle call

z contour subroutine (TESTK1.MPF)

;The contour shown in the example must be machined externally

;in a complete machining operation in the longitudinal axis.

;The maximum infeed is 5 mm, the finishing allowance is 1.2 mm,

;and the infeed angle is 7 degrees.

N10 T1 D1 G0 G23 G95 S500 M3 F0.4 ;Definition of technology values

N20 Z125 X162 ;Collision-free approach position

prior to the call

_CNAME= “TESTK1” ;Name of contour subroutine

R105=9 R106=1.2 R108=5 R109=7 ;Set further parameters for

R110=1.5 R111=0.4 R112=0.25 ;cycle call

N60 LCYC95 ;Cycle call

N70 G0 G90 X162 Z125 ;Re-approach starting position of

X162 Z125 by different axes

N99 M2

Subroutine “TESTK1”

N10 G1 Z100 X40 ;Starting point

N20 Z85 ;P1

N30 X54 ;P2

N40 Z77 X70 ;P3

N50 Z67 ;P4

N60 G2 Z62 X80 CR=5 ;P5

N70 G1 Z62 X96 ;P6

N80 G3 Z50 X120 CR=12 ;P7

N90 G1 Z35 ;P8

Cycles

9-26 SINUMERIK 801

Operation and Program ming

—

Turning

9.9 Thread cutting – LCYC97

Function The thread cutting cycle is suitable for cutting external and internal,

single-start or multiple-start threads on cylindrical and tapered bodies in the

facing or longitudinal axis. Depth infeed is an automatic function.

Whether a right-hand or left-hand thread is produced is determined by the

direction of rotation of the spindle, which must be programmed before calling

the cycle. Feed and spindle override are not effective in the traversing blocks

containing thread cutting operations.

Call LCYC97

Fig.9-15 Schematic diagram of para meters for thread cutting

Parameters Table 9–8 Parameters for LCYC97 cycle

Parameter Meaning, Value Range

R100 Diameter of thread at starting point

R101 Thread starting point in longitudinal axis

R102 Diameter at end point

R103 Thread end point in longitudinal axis

R104 Thread lead as value, without sign

R105 Definition of thread cutting method:

Value range: 1, 2

R106 Finishing allowance, without sign

R109 Approach path, without sign

R110 Run-out path, without sign

R111 Thre ad depth, without sign

R112 Starting point offset, withou t sign

R113 Number of rough cuts, without sign

R114 Number of threads, without sign

R103 R101

R109

R110

R111 R100 = R102

External thread cutting

Effect of parameters for lead,

infeed angle and f i nishing

allowance

R104 R106

Cycles

SINUMERIK 801 9-27

Operation and Program ming

—

Turning

Information

R100, R101 These parameters define the thread st arting point in X and Z.

R102, R103 The thread end point is programmed under R102 and R103. In the case of

cylindrical threads, one of these parameters has the same value as R100 or

R101.

R104 The thread lead is an axis-pa rallel valu e and is specified without sign.

R105 Parameter R105 defines whether the thread is machined internally or

externally.

R105 = 1: External thread

R105 = 2: Internal thread

If the parameter is set to any other value, the cycle is aborted with the alarm

61002 “Machining type incorrectly programmed”.

R106 The programmed finishing allowance is subtracted from the specified thread

depth. The remainder is divided into rough cuts.

The finishing allowance is removed in one cut after roughing.

R109, R110 Parameters R109 and R110 specifiy the internally calculated thread approach

and run-out paths. The cycle shifts the programmed starting point forward by

the approach distance. The run-out path extends the length of the thread

beyond the programmed end point.

R111 Parameter R111 defines the total depth of the thread.

R112 An angle value can be programmed in this parameter. This value defines the

point at which the first thread cut starts on the circumference of the turned part,

i.e. it is a starting point offset.

Possible values for this parameter are between 0.0001 ... + 359.9999

degrees.

If no starting point offset is specified, the first thread automatically starts at the

zero-degree marking.

R113 Parameter R113 determines the number of roughing cuts for thread cutting

operations. The cycle independently calculates the individual, current infeed

depths as a function of the settings in R105 and R111.

R114 This parameter specifies the number of threads. These are arranged

symmetrically around the circumference of the turned part.

Longitudinal or The cycle itself decides whether a thread must be machined in the longitudinal

face thread or facing axis. If the angle on the taper is less than or equal to 45 degrees,

then the thread is machined as a longitudinal thread, otherwise as a face

thread.

Cycles

9-28 SINUMERIK 801

Operation and Program ming

—

Turning

Motional sequence Position reached prior to beginning of cycle:

z Any position from which the programmed thread starting point +

approach path can be approached without risk of collision.

The cycle produces the following motional seq uence:

z Approach starting point at the beginning of the approach path (calculated

internally in the cycle) to cut first thread with G0.

z Infeed for rough cutting according to the infeed method defined under

R105.

z Repeat thread cuts according to the programmed number of rough cuts.

z Remove the finishing allowance with G33.

z Repeat the whole sequence for every further threa d.

Example

M42×2

Fig.9-16 Example diagram

;A two-start thread, M42x2, must be machined.

N10 G23 G95 F0.3 G90 T1 D1 S1000 M4 ;Define technology values

N20 G0 Z100 X120 ;Program start position

R100=42 R101=80 R102=42 R103=45 R104=4 ;Parameters for cycle call

R105=1 R106=1 R109=12 R110=6

R111=1.083 R112=0 R113=3 R114=2

N50 LCYC97 ;Cycle call

N100 G0 Z100 X60 ;Position after cycle end

N110 M2

Cycles

SINUMERIK 801 9-29

Operation and Program ming

—

Turning

SINUMERIK 801

Operation and Programming –

Turning

Usual Manual

Order No.: A5E00702070

Edition: 11. 2005

A5E00702070