siemens 840D Users Guide

Download

User's Guide 11/2002 Edition

Measuring Cycles SINUMERIK 840D/840Di/810D

Part 1: User's Guide

SINUMERIK 840D/840Di/810D

Measuring Cycles

User's Guide

Introduction

Description of Parameters

Measuring Cycle Auxiliary

Programs

Measuring in JOG

Measuring Cycles for

Milling and Machining

Centers

Valid for

Control Software version

SINUMERIK 840D 6 SINUMERIK 840DE (export version) 6 SINUMERIK 840D powerline 6 SINUMERIK 840DE powerline 6 SINUMERIK 840Di 2 SINUMERIK 840DiE (export version) 2 SINUMERIK 810D 3 SINUMERIK 810DE (export version) 3 SINUMERIK 810D powerline 6 SINUMERIK 810DE powerline 6

Measuring Cycles for

Turning Machines

Miscellaneous Functions

Part 2: Description of

Functions

Hardware, Software and

Installation

Supplementary

Conditions

Data Description

Examples

11.02 Edition

Data Fields, Lists

Appendix

Contents 11.02

SINUMERIK® Documentation

Printing history

Brief details of this edition and previous editions are listed below.

The status of each edition is shown by the code in the "Remarks" column.

Status code in the "Remarks" column:

A .... New documentation.

B .... Unrevised edition with new Order No.

C .... Revised edition with new status.

If factual changes have been made on the page since the last edition, this is indicated by a new edition coding in the header on that page.

Edition Order No. Remarks

09.95

03.96

6FC5298-3AA01-0BP0 6FC5298-3AA70-0BP1

A C

12.97 6FC5298-4AA70-0BP0 C

12.98 6FC5298-5AA70-0BP0 C

08.99 6FC5298-5AA70-0BP1 C

06.00 6FC5298-5AA70-0BP2 C

10.00 6FC5298-6AA70-0BP0 C

09.01 6FC5298-6AA70-0BP1 C

11.02 6FC5298-6AA70-0BP2 C

This manual is included in the documentation available on CD ROM (DOCONCD) Edition Order No. Remarks

11.02 6FC5 298-6CA00-0BG3 C

Trademarks

SIMATIC POSMO be trademarks which, if used by third parties, could infringe the rights of their owners.

Further information is available on the Internet under: http:/www.ad.siemens.de/sinumeri k

This publications was produced with WinW ord V 8.0 and Designer V 7.0. The reproduction, transmission or use of this document or its contents 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 or design, are reserved.

, SIMATIC HMI®, SIMATIC NET®, SIROTEC®, SINUMERIK®, SIMODRIVE® and SIMODRIVE

are registered trademarks of Siemens AG. Other product names used in this documentation may

Other functions not described in this documentation might be executable in the control. This does not, however, represent an obligation to supply such functions with a new control or when servicing.

We have checked that the contents of this document correspond to the hardware and software described. Nonetheless, differences might exist and therefore we cannot guarantee that they are completely identical. The information contained in this document is, however, reviewed regularly and any necessary changes will be included in the next edition. We welcome suggestions for improvement.

Subject to change without prior notice

Order No. 6FC5298-6AA70-0BP2 Printed in Germany

Siemens Aktiengesellschaft

11.02 Contents

Contents

Part 1: User's Guide

Introduction 1-15

1.1 Basics.............................................................................................................................. 1-16

1.2 General preconditions ..................................................................................................... 1-17

1.3 Plane definition................................................................................................................ 1-19

1.4 Suitable probes ............................................................................................................... 1-20

1.5 Workpiece probe, calibration tool in TO memory............................................................ 1-22

1.5.1 Workpiece probe in TO memory for milling machines and machining centers ........ 1-22

1.5.2 Workpiece probe, calibration tool in TO memory on turning machines .................... 1-23

1.6 Measuring principle ......................................................................................................... 1-25

1.7 Measuring strategy and compensation value calculation for tools with automatic

tool offset......................................................................................................................... 1-28

1.8 Parameters for checking the dimension deviation and compensation............................ 1-31

1.9 Effect of empirical value, mean value and tolerance parameters ................................... 1-37

1.10 Reference points on the machine and workpiece ........................................................... 1-38

1.11 Measurement variants for milling machines & machining centers .................................. 1-39

1.11.1 Workpiece measurement for milling machines......................................................... 1-39

1.11.2 Measurement variants for fast measurement at a single point ................................. 1-40

1.11.3 Measurement variants for workpiece measurement paraxial ................................... 1-40

1.11.4 Measurement variants for workpiece measurement at random angles .................... 1-42

1.11.5 Measuring a surface at a random angle ................................................................... 1-43

1.12 Measurement variants for lathes.................................................................................... 1-44

1.12.1 Tool measurement for lathes .................................................................................... 1-44

1.12.2 Workpiece measurement for turning machines: Single-point measurement............ 1-45

1.12.3 Workpiece measurement for turning machines: Two-point measurement ............... 1-47

1.13 Measuring cycles interface............................................................................................. 1-48

1.13.1 Displaying measuring result screens ........................................................................ 1-48

1.13.2 Setting parameters.................................................................................................... 1-50

Description of Parameters 2-53

2.1. Parameter concept for measuring cycles........................................................................ 2-54

2.2 Parameter overview ........................................................................................................2-56

2.2.1 Input parameters ....................................................................................................... 2-56

2.2.2 Result parameters..................................................................................................... 2-57

Contents 11.02

2.3 Description of the most important defining parameters...................................................2-58

2.3.1 Measurement variant: _MVAR ..................................................................................2-58

2.3.2 Number of measuring axis: _MA............................................................................... 2-61

2.3.3 Tool number and tool name: _TNUM and _TNAME .................................................2-62

2.3.4 Offset number _KNUM.............................................................................................. 2-63

2.3.5 Offset number _KNUM with flat D number structure................................................. 2-65

2.3.6 Variable measuring speed: _VMS............................................................................. 2-66

2.3.7 Compensation angle position for monodirectional probe: _CORA............................ 2-66

2.3.8 Tolerance parameters: _TZL, _TMV, _TUL, _TLL, _TDIF and _TSA....................... 2-67

2.3.9 Multiplication factor for measurement path 2a: _FA..................................................2-68

2.3.10 Probe type/Probe number: _PRNUM ........................................................................2-69

2.3.11 Empirical value/mean value: _EVNUM ..................................................................... 2-70

2.3.12 Multiple measurement at the same location: _NMSP ...............................................2-71

2.3.13 Weighting factor k for averaging: _K .........................................................................2-71

2.4. Description of output parameters ...................................................................................2-72

2.4.1 Measuring cycle results in _OVR ..............................................................................2-72

2.4.2 Measuring cycle results in _OVI ................................................................................2-73

Measuring Cycle Auxiliary Programs 3-75

3.1 Package structure of measuring cycles.......................................................................... 3-76

3.2 Measuring cycle subroutines ..........................................................................................3-77

3.2.1 CYCLE103: Parameter definition for measuring cycles ............................................3-78

3.2.2 CYCLE116: Calculation of center point and radius of a circle................................... 3-79

3.3 Measuring cycle user programs .....................................................................................3-81

3.3.1 CYCLE198: User program prior to calling measuring cycle ......................................3-81

3.3.2 CYCLE199: User program at the end of a measuring cycle .....................................3-82

3.4 Subpackages..................................................................................................................3-83

Measuring in JOG 4-85

4.1 General preconditions .................................................................................................... 4-86

4.2 Workpiece measurement ............................................................................................... 4-89

4.2.1 Operation and function sequence of workpiece measurement .................................4-90

4.2.2 Measuring an edge.................................................................................................... 4-91

4.2.3 Measuring a corner ................................................................................................... 4-92

4.2.4 Measuring a hole .......................................................................................................4-94

4.2.5 Measuring a spigot .................................................................................................... 4-95

4.2.6 Calibrating the measuring probe ...............................................................................4-96

4.3 Tool measurement .........................................................................................................4-99

4.3.1 Operation and function sequence of tool measurement ...........................................4-99

4.3.2 Tool measurement ..................................................................................................4-100

4.3.3 Calibrating the tool measuring probe ...................................................................... 4-101

0-6 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

11.02 Contents

Measuring Cycles for Milling and Machining Centers 5-103

5.1 General preconditions ................................................................................................... 5-104

5.2 CYCLE971 Tool measuring for milling tools ................................................................. 5-106

5.2.1 CYCLE971 Measuring strategy............................................................................... 5-108

5.2.2 CYCLE971 Calibrate tool probe .............................................................................. 5-110

5.2.3 CYCLE971 Measure tool......................................................................................... 5-114

5.3 CYCLE976 Calibrate workpiece probe.......................................................................... 5-119

5.3.1 CYCLE976 Calibrate workpiece probe in any hole (plane) with known

hole center .............................................................................................................. 5-122

5.3.2 CYCLE976 Calibrate workpiece probe in any hole (plane) with unknown hole

center (measuring cycles SW 4.4 and higher) ........................................................ 5-124

5.3.3 CYCLE976 Calibrate workpiece probe on a random surface ................................. 5-126

5.3.4 Calibrate workpiece probe in applicate with calculation of probe length

(measuring cycles SW 4.4. and higher) .................................................................. 5-128

5.4 CYCLE977 Workpiece measurement: Hole/shaft/groove/web/rectangle (paraxial) ..... 5-130

5.4.1 CYCLE977 Measure hole, shaft, groove, web, rectangle ....................................... 5-134

5.4.2 CYCLE977 ZO calculation in hole, shaft, groove, web, rectangle .......................... 5-140

5.5 CYCLE978 Workpiece measurement: Surface ............................................................ 5-146

5.5.1 CYCLE978 ZO calculation on a surface (single point measuring cycle)................. 5-149

5.5.2 CYCLE978 Single-point measurement ................................................................... 5-152

5.6 CYCLE979 Workpiece measurement: Hole/shaft/groove/web (at a random angle)..... 5-156

5.6.1 CYCLE979 Measure hole, shaft, groove, web ........................................................ 5-159

5.6.2 CYCLE979 ZO calculation in hole, shaft, groove, web ........................................... 5-164

5.7 CYCLE998 Angular measurement (ZO calculation) ..................................................... 5-169

5.8 CYCLE961 Automatic setup of inside and outside corner ............................................ 5-180

5.8.1 Automatic setup of corner with distances and angles specified.............................. 5-180

5.8.2 Automatic setup of corner by defining 4 points (measuring cycles ≥ SW 4.5) ........ 5-185

Measuring Cycles for Turning Machines 6-189

6.1 General preconditions .................................................................................................. 6-190

6.2 CYCLE972 Tool measurement ....................................................................................6-192

6.2.1 CYCLE972 Calibrating the tool probe ..................................................................... 6-194

6.2.2 CYCLE972 Determine dimensions of calibration tools ........................................... 6-197

6.2.3 CYCLE972 Measure tool......................................................................................... 6-198

6.3 CYCLE982 Tool measurement (SW 5.3 and higher)................................................... 6-203

6.3.1 CYCLE982 Calibrate tool measuring probe ............................................................ 6-208

6.3.2 CYCLE982 Measure tool......................................................................................... 6-210

6.3.3 CYCLE982 Automatic tool measurement ............................................................... 6-221

6.3.4 Incremental calibration (SW 6.2 and higher)........................................................... 6-228

Contents 11.02

6.3.5 Incremental measurement (SW 6.2 and higher) .....................................................6-231

6.3.6 Milling tool: suppression of starting angle positioning with _STA1 (≥ SW 6.2)........6-237

6.4 CYCLE973 Calibrate workpiece probe .........................................................................6-238

6.4.1 CYCLE973 Calibrate in the reference groove (plane) .............................................6-240

6.4.2 CYCLE973 Calibrate on a random surface .............................................................6-242

6.5 CYCLE974 Workpiece measurement ..........................................................................6-244

6.5.1 CYCLE974 Single-point measurement ZO calculation ...........................................6-246

6.5.2 CYCLE974 Single-point measurement ...................................................................6-249

6.5.3 CYCLE974 Single-point measurement with reversal ..............................................6-253

6.6 CYCLE994 Two-point measurement............................................................................ 6-257

6.7 Complex example for workpiece measurement ...........................................................6-262

Miscellaneous Functions 7-265

7.1 Logging of measuring results .......................................................................................7-266

7.1.1 Storing the log .........................................................................................................7-266

7.1.2 Handling of log cycles.............................................................................................. 7-267

7.1.3 Selecting the log contents .......................................................................................7-269

7.1.4 Log format ...............................................................................................................7-271

7.1.5 Log header ..............................................................................................................7-272

7.1.6 Variable for logging.................................................................................................. 7-273

7.1.7 Example of measuring result log .............................................................................7-274

7.2 Cycle support for measuring cycles..............................................................................7-276

7.2.1 Files for cycle support.............................................................................................. 7-277

7.2.2 Loading the cycle support........................................................................................ 7-277

7.2.3 Assignment of calls and measuring cycles.............................................................. 7-278

7.2.4 Description of parameterization cycles.................................................................... 7-279

7.3 Measuring cycle support in the program editor (≥ SW 6.2) ..........................................7-290

7.3.1 Menus, cycle explanation ........................................................................................ 7-290

7.3.2 New functions of the input forms .............................................................................7-291

7.3.3 GUD variables for adaptation of measuring cycle support ......................................7-297

Part 2: Description of Functions

Hardware, Software and Installation 8-301

8.1 Overview....................................................................................................................... 8-302

8.2 Hardware requirements ................................................................................................8-303

8.2.1 General hardware requirements.............................................................................. 8-303

8.2.2 Probe connection..................................................................................................... 8-303

8.2.3 Measuring in JOG ................................................................................................... 8-303

8.3 Software requirements .................................................................................................8-308

8.3.1 General measuring cycles.......................................................................................8-308

0-8 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

11.02 Contents

8.3.2 Measuring in JOG ................................................................................................... 8-309

8.4 Function check .............................................................................................................8-310

8.5 Start-up sequences ......................................................................................................8-312

8.5.1 Start-up flowchart for measuring cycles and probe circuit ...................................... 8-312

8.5.2 Starting up the measuring cycle interface for the MMC 102 ...................................8-315

Supplementary Conditions 9-317

Data Description 10-319

10.1 Machine data for machine cycle runs......................................................................... 10-320

10.2 Cycle data................................................................................................................... 10-323

10.2.1 Data concept for measuring cycles ....................................................................... 10-323

10.2.2 Data blocks for measuring cycles: GUD5.DEF and GUD6.DEF........................... 10-324

10.2.3 Central values .......................................................................................................10-328

10.2.4 Central bits ............................................................................................................ 10-333

10.2.5 Central strings ....................................................................................................... 10-336

10.2.6 Channel-oriented values ....................................................................................... 10-337

10.2.7 Channel-oriented bits ............................................................................................ 10-339

10.3 Data for measuring in JOG ........................................................................................ 10-344

10.3.1 Machine data for ensuring ability to function ......................................................... 10-344

10.3.2 Modifying the GUD7 data block ............................................................................ 10-346

10.3.3 Settings in data block GUD6 ................................................................................. 10-349

10.3.4 Loading files for measuring in JOG....................................................................... 10-351

Examples 11-353

11.1 Determining the repeat accuracy ............................................................................... 11-354

11.2 Adapting the data for a particular machine ................................................................ 11-355

Data Fields, Lists 12-359

12.1 Machine data.............................................................................................................. 12-360

12.2 Measuring cycle data ................................................................................................. 12-360

12.3 Alarms ........................................................................................................................ 12-361

Appendix A-369

A Overview of measuring cycle parameters ....................................................................A-371

B Abbreviations................................................................................................................A-405

C Terms ...........................................................................................................................A-407

D References...................................................................................................................A-415

E Index.............................................................................................................................A-429

F Identifiers......................................................................................................................A-434

Preface 11.02

Structure of the manual

840 D NCU 571

840 D NCU 572 NCU 573

810 D 840 Di

Preface

Organization of documentation

The SINUMERIK documentation is organized on 3 different levels:

• General Documentation

• User Documentation

• Manufacturer/Service Documentation

Target group

This manual is aimed at machine tool users. It provides detailed information for operating the SINUMERIK 840D, 810D.

Standard scope

This Operator's Guide describes only the functionality of the standard scope. A description of add-on features or modifications made by the machine builder are not included in this guide.

For more detailed information on SINUMERIK 840D, 810D publications and other publications covering all SINUMERIK controls (e.g. universal interface, measuring cycles...), please contact your local Siemens office.

Other functions not described in this documentation might be executable in the control. This does not, however, represent an obligation to supply such functions with a new control or when servicing.

Validity

This User's Guide is valid for the following controls: SINUMERIK 810D, 840D, 840Di, MMC 100 and MMC 102/103. Software versions stated in the User's Guide refer to the 840D and their 810D equivalent, e.g. SW 6 (840D) corresponds to SW 3 (810D).

SINUMERIK 840D powerline From 09.2001

• SINUMERIK 840D powerline and

• SINUMERIK 840DE powerline

are available, with improved performance. A list of the available powerline modules can be found in the hardware description /PHD/ in Section 1.1

SINUMERIK 810D powerline From 12.2001

• SINUMERIK 810D powerline and

• SINUMERIK 810DE powerline

are available, with improved performance. A list of the available powerline modules can be found in the hardware description /PHC/ in Section 1.1

0-10 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

11.02 Preface

Structure of the manual

840 D NCU 571

Hotline

Internet address

840 D NCU 572 NCU 573

810 D 840 Di

Explanation of symbols

Procedure

Please address any questions to the following hotline: A&D Technical Support Phone: ++49-(0)180-5050-222

Fax: ++49-(0)180-5050-223 Email: adsupport@siemens.com

If you have any questions (suggestions, corrections) concerning the documentation, please fax or e-mail them to the following address:

Fax: ++49-(0)0131-98-2176 Email: motioncontrol.docu@erlf.siemens.de

Fax form: See answer form at the end of the document.

http://www.ad.siemens.de/sinumerik

Ordering option

Explanation

Function

Parameters

Programming example

Programming

Further notes

Cross-reference to other documentation, chapters, sections, or subsections

Notes and indication of danger

Additional notes or background information

Preface 11.02

Use as intended

840 D NCU 571

Warnings

The following warnings are used with graded severity.

840 D NCU 572 NCU 573

810 D 840 Di

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 the safety alert symbol indicates a potentially hazardous situation which, if not avoided, may result in minor or moderate injury or in property damage.

Caution

Used without safety alert symbol indicates a potentially hazardous situation which, if not avoided, may result in property damage.

Notice

Used without the safety alert symbol indicates a potential situation which, if not avoided, may result in an undesirable result or state.

0-12 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

11.02 Preface

Use as intended

840 D NCU 571

Basis

Your SIEMENS SINUMERIK 840D, 804Di, 810D is state of the art and is manufactured in accordance with recognized safety regulations, standards and specifications.

Add-on equipment

Using special add-on equipment and expanded configurations from SIEMENS, SIEMENS controls can be adapted to suit your specific application.

Personnel Only authorized and reliable personnel with the relevant training must be allowed to handle the

control. Nobody without the necessary training must be allowed to work on the control, not even for a short time.

840 D NCU 572 NCU 573

810 D 840 Di

The responsibilities of the personnel employed for setting, operating and maintenance must be clearly

defined and supervised.

Behavior Before the control is started up, it must be ensured

that the Operator's Guide has been read and understood by the personnel responsible. The operating company is also responsible for constantly monitoring the overall technical state of the control (faults and damage apparent from the outside and changes in response).

Preface 11.02

Use as intended

840 D NCU 571

Service

Repairs must only be carried out in accordance with the information given in the Service and Maintenance Guide by personnel trained and qualified in the relevant field. The relevant safety regulations must be observed.

Note The following is contrary to the intended purpose and exonerates the manufacturer from any liability:

Any use whatsoever beyond or deviating from the

application stated in the above points.

If the control is not in perfect technical condition, or is operated without awareness for safety or the dangers involved or without observing the instructions given in the instruction manual.

840 D NCU 572 NCU 573

810 D 840 Di

If faults that can reduce safety are not remedied before the control is started up.

Any modification, overriding or deactivation of equipment on the control used for the perfect functioning, unrestricted use or active and passive safety.

This can result in unforeseen dangers for:

• the health and life of people,

• the control, machine and other property of the

operating company and user.

0-14 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

09.01

Introduction

1.1 Basics.............................................................................................................................. 1-16

1.2 General preconditions ..................................................................................................... 1-17

1.3 Plane definition................................................................................................................ 1-19

1.4 Suitable probes ............................................................................................................... 1-20

1.5 Workpiece probe, calibration tool in TO memory............................................................ 1-22

1.5.1 Workpiece probe in TO memory for milling machines and machining centers ....... 1-22

1.5.2 Workpiece probe, calibration tool in TO memory on turning machines ................... 1-23

1.6 Measuring principle ......................................................................................................... 1-25

1.7 Measuring strategy and compensation value calculation for tools with automatic

tool offset......................................................................................................................... 1-28

1.8 Parameters for checking the dimension deviation and compensation............................ 1-31

1.9 Effect of empirical value, mean value and tolerance parameters ................................... 1-37

1.10 Reference points on the machine and workpiece ........................................................... 1-38

1.11 Measurement variants for milling machines & machining centers .................................. 1-39

1.11.1 Workpiece measurement for milling machines........................................................ 1-39

1.11.2 Measurement variants for fast measurement at a single point................................ 1-40

1.11.3 Measurement variants for workpiece measurement paraxial .................................. 1-40

1.11.4 Measurement variants for workpiece measurement at random angles................... 1-42

1.11.5 Measuring a surface at a random angle .................................................................. 1-43

1.12 Measurement variants for lathes ..................................................................................... 1-44

1.12.1 Tool measurement for lathes ................................................................................... 1-44

1.12.2 Workpiece measurement for turning machines: Single-point measurement........... 1-45

1.12.3 Workpiece measurement for turning machines: Two-point measurement.............. 1-47

1.13 Measuring cycles interface.............................................................................................. 1-48

1.13.1 Displaying measuring result screens ....................................................................... 1-48

1.13.2 Setting parameters................................................................................................... 1-50

Introduction 12.97

1.1 Basics

08.99

840 D

NCU 571

1.1 Basics

Measuring cycles are general subroutines designed to solve specific measurement tasks. They can be suitably adapted to the problem at hand by means of parameter settings.

With regard to measurement applications, a distinction

must generally be made between tool measurement

and workpiece measurement.

Workpiece measurement

For workpiece measurement, a measuring probe is moved up to the clamped workpiece in the same way as a tool. The flexibility of the measuring cycles makes it possible to perform nearly all measurements which may need to be taken on a milling machine. An automatic tool offset or an additive ZO can be applied to the result of the tool measurement. The measurement variants which can be implemented with the measuring cycles available in this configuration are described on the following pages.

840 D

NCU 572

NCU 573

810 D 840Di

Tool measurement

To perform tool measurement, the changed tool, which in the case of a lathe is usually located in the turret, is moved up to the probe which is either permanently fixed or swiveled into the working range. The automatically derived tool geometry is entered in the relevant tool offset data record.

1-16 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

11.02

1.2 General preconditions

840 D

NCU 571

840 D

NCU 572

NCU 573

1.2 General preconditions

Certain preconditions need to be fulfilled before measuring cycles can be used.

These conditions are described in greater detail in Part 2 Description of Functions (from Chapter 8 onwards).

The following checklist is useful in determining whether all such preconditions are fulfilled:

Machine

• All machine axes are designed in accordance with

DIN 66217

Availability of cycles

• The data blocks:

GUD5.DEF and

GUD6.DEF have been loaded into the control ("Definitions" directory in file system) and

• the measuring cycles have been loaded into the

standard cycle directory of the control followed by a power ON operation.

Initial position

• The reference points have been approached.

• All axes are positioned prior to the cycle call in such

a way that the setpoint position can be approached without a change in direction.

• The start position can be reached without collisions

by means of linear interpolation.

Displaying measuring result screens

It is only possible to display measurement result screens with an MMC/PCU.

810 D 840Di

Introduction 12.97

1.2 General preconditions

09.01

840 D

NCU 571

Programming

• The inch/metric units system selected in the

• The milling radius compensation and the

• All parameters for the cycle call have been defined

• The cycle is called no later than at the 5th program

• Neither of the operating modes "Block search" or

• The specified default setting of the supplied data

• With measuring cycles SW 4.4 and higher,

840 D

NCU 572

NCU 573

machine data for the basic setting is active.

programmable frame are deselected prior to the cycle call.

beforehand.

level.

"Dry run" is active since these are automatically skipped by the measuring cycles.

blocks is required to ensure that all example programs run correctly.

measurement in a programmed measurement system that differs from the basic system is possible, i.e. in a metric basic system with active G70 and in an inch basic system with active G71.

measurement in a programmed measurement system that differs from the basic system is possible with technology data switched over. This means in a metric basic system with active G700 and in an inch basic system with active G710.

810 D 840Di

Software status ID

In the delivery status of the measuring cycles, the current software status of the control is entered in parameter _SI[1] in the GUD6 block, i. e. 5 for SW 5. This parameter must be changed to match the measuring cycles to older software releases. Example: When using measuring cycles status 5.x.x on a control with SW 4, à_SI[1] = 4 Precondition: In order to use the measuring cycles, the software

status of the control must be ≥ 3.

1-18 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

1.3 Plane definition

840 D

NCU 571

1.3 Plane definition

Tool radius compensation planes G17, G18 or G19 can

be selected. Lengths 1, 2 and 3 are assigned as follows to the axes depending on the tool type used:

G17 plane

Tool type 100 Length 1 applies to Z Length 2 applies to Y Length 3 applies to X

840 D

NCU 572

NCU 573

810 D 840Di

Y Ordinate

Abscissa X

Z Applicate

G18 plane

Tool type 100 Length 1 applies to Y Length 2 applies to X Length 3 applies to Z

G19 plane

Tool type 100 Length 1 applies to X Length 2 applies to Z Length 3 applies to Y

X Ordinate

Abscissa Z

Y Applicate

Z Ordinate

Abscissa Y

X Applicate

Introduction 12.97

1.4 Suitable probes

840 D

NCU 571

1.4 Suitable probes

Function

In order to measure tool and workpiece dimensions, a touch-trigger probe is required that supplies a constant signal (rather than a pulse) when deflected.

The probe must be capable of virtually bounce-free switching. This is normally achieved by adjusting the probe mechanically.

The probe type is defined in the measuring cycles in a parameter.

Various types of probes made by different manufacturers are available on the market. Probes are classified in three groups according to the number of directions in which they can be deflected.

Classification of probe types

Probe type Turning machines Milling mach. and mach. centers

Multidirectional

Bidirectional

Monodirectional

While a bidirectional probe can be used for turning machines, with milling machines and machining centers it is also possible to use a mono probe for workpiece measuring.

The probe is defined in the measuring cycles in a parameter.

840 D

NCU 572

NCU 573

Tool measurement Workpiece measurement Workpiece measurement

X X X

- X X

- - X

810 D 840Di

1-20 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

1.4 Suitable probes

840 D

NCU 571

Multidirectional probe (3D)

With this type, measuring cycles for workpiece measurement can be used without limitation.

Bidirectional probe

This probe type is used for workpiece measurement on milling machines and machining centers.

This probe type is treated in the same way as a monodirectional probe for workpiece measurement on milling machines and machining centers.

840 D

NCU 572

NCU 573

810 D 840Di

Monodirectional probe

This probe type can only be used for workpiece measurement on milling machines and machining centers with slight limitations; reference is made to this in the cycles concerned. In order to be able to use this type of probe on milling machines and machining centers, it must be possible to position the spindle with the NC function SPOS and to transmit the switching signal of the probe through 360° to the receiving station (at the machine column).

Introduction 12.97

1.5 Workpiece probe, calibration tool in TO memor

840 D

NCU 571

The probe must be mechanically aligned in the spindle in

such a way that measurements can be taken in the following directions at the 0 degree position of the spindle.

X-Y plane G17 positive X direction

Z-X plane G18 positive Z direction

Y-Z plane G19 positive Y direction

The measurement will take longer when using a

1.5 Workpiece probe, calibration tool in TO memory

1.5.1 Workpiece probe in TO memory for milling machines and machining centers

monodirectional probe since the spindle must be positioned in the cycle several times by means of SPOS.

Workpiece probe

On milling machines and machining centers, the probe is classified as tool type 1x0 and must therefore be entered as such in the TO memory. In SW 4 and higher, tool type 710 (3D probe) can also be used.

Entry in TO memory

840 D

NCU 572

NCU 573

810 D 840Di

P1 710 Tool type P3 L1 Geometr P6 r Geometry P21 L1 Tool base dimension

_CBIT[14]=1

_CBIT[14]=0

1-22 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

11.02

1.5 Workpiece probe, calibration tool in TO memor

840 D

NCU 571

1.5.2 Workpiece probe, calibration tool in TO memory on turning machines

840 D

NCU 572

NCU 573

810 D 840Di

On turning machines, the probes are treated as tool

type 500 with the permissible tool edge positions 5 to 8 and must therefore be entered like this in the TO memory. Measuring cycle SW 6.2 and higher also allows you to enter probe type 580 with tool edge positions 5 to 8. Due to their spatial positions, the probes are divided into the following types:

Workpiece probe SL 5

Entry in TO memory

P1 500 Tool type P2 5 Tool edge position P3 L1 Geometry

P4 L2 Geometry P6 r Geometry P12 L1 Wear P13 L2 Wear

P15 r Wear P21 L1 Tool base dimension P22 L2 Tool base dimension

Workpiece probe SL 6 (8)

(data in brackets is in front of turning center) Entry in TO memory

P1 500 Tool type P2 6 (8) Tool edge position P3 L1 Geometry P4 L2 Geometry P6 r Geometry

P12 L1 Wear P13 L2 Wear P15 r Wear P21 L1 Tool base dimension P22 L2 Tool base dimension

Introduction 12.97

1.5 Workpiece probe, calibration tool in TO memor

840 D

NCU 571

Workpiece probe SL 7

Entry in TO memory

840 D

NCU 572

NCU 573

810 D 840Di

P1 500 Tool type P2 7 Tool edge position P3 L1 Geometry

P4 L2 Geometry P6 r Geometry P12 L1 Wear

P13 L2 Wear P15 r Wear P21 L1 Tool base dimension P22 L2 Tool base dimension

Workpiece probe SL 8 (6)

(data in brackets is in front of turning center) Entry in TO memory

P1 500 Tool type P2 8 (6) Tool edge position P3 L1 Geometry

P4 L2 Geometry P6 r Geometry

P12 L1 Wear P13 L2 Wear P15 r Wear P21 L1 Tool base dimension P22 L2 Tool base dimension

Calibration tool

On turning machines, the calibration tool is classified as a tool with tool edge position 3 and must therefore be entered as such in the TO memory. Entry in TO memory

P1 500 Tool type P2 3 Tool edge position

P3 L1 Geometry P4 L2 Geometry P6 r Geometry

P12 L1 Wear P13 L2 Wear P15 r Wear P21 L1 Tool base dimension P22 L2 Tool base dimension

1-24 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

1.6 Measuring principle

840 D

NCU 571

1.6 Measuring principle

840 D

NCU 572

NCU 573

810 D 840Di

Two inputs for the connection of touch trigger probes

are provided on the I/O device interface of the SINUMERIK 840D and the FM-NC control systems.

Function

Evaluation of the measuring probe signal If a measuring point is to be approached, a traverse command is transmitted to the position control loop and the probe is moved towards the measuring point. A point behind the expected measuring point is defined as setpoint position. As soon as the probe makes contact, the actual axis value at the time the switching position is reached is measured and the drive is stopped. The remaining "distance-to-go" is deleted.

Meas. cycle

Delete distanceto-go

Act. val. acquis.

Position control

Actual value

"On-the-fly" measurement

The principle of "on-the-fly" measurement is implemented in the control. The advantage of this method is that the probe signal is processed directly in the NC.

Set position

Meas. dist. a

Delete dist.-to-go

-V

=Traversing path by signal processing

=Following error

1) Actual value loaded with probe signal

Meas. dist. a

Act. position

Probe switching point

Start position = End position

Introduction 12.97

1.6 Measuring principle

840 D

NCU 571

Start position/setpoint position

In the measuring procedure used, a position is specified as setpoint value for the cycle at which the signal of the touch-trigger probe is expected.

Since it is unlikely that the probe will respond at precisely this point, the start position is approached by the control in rapid traverse mode or at a defined positioning velocity. The set position is then approached at the feedrate specified in the parameter for measurement speed. The switching signal is then anticipated over a distance of a maximum length of 2a from the start position.

Load actual value/delete distance-to-go

At the instant the switching signal is output by the probe, the current position is stored internally "on-thefly" as the actual value followed by execution of the "Delete distance-to-go" function.

Measuring path a/measuring speed

The path increment a is normally 1 mm, but can be increased with a parameter when measuring cycles are called.

The approach speed automatically increases from 150 mm/min to 300 mm/min if the value for a is defined as greater than 1.

The maximum approach speed (measurement speed) is thus dependent upon

• the permissible deflection path of the probe used

• the delay until "delete distance to go" is executed

• the deceleration behavior of the axis.

and

840 D

NCU 572

NCU 573

810 D 840Di

1-26 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

11.02

1.6 Measuring principle

840 D

NCU 571

Calculation of the deceleration path

840 D

NCU 572

NCU 573

810 D 840Di

Since an optimal measurement speed can be set for measuring cycles via a parameter, it must be ensured that safe deceleration can take place within the deflection path of the probe. The required deceleration path can be calculated as follows:

sb = v t +

Deceleration path in m

∆

+ ∆s

∆

v Approach speed in m/s t Delay in s b Deceleration in m/s

s Following error in m

Measuring accuracy

The repeat accuracy of the 840D and FM-NC controls for "on-the-fly measurement" is ±1 µm.

The measuring accuracy which can be obtained is thus dependent on the following factors:

• Repeat accuracy of the machine

• Repeat accuracy of the probe

• Resolution of the measuring system

Example: Path-time diagram

s [mm]

Deceleration

b = 1m/s

(11 mm)

(1.66 mm)

The deflection of the probe up to zero spee d of the axis is approximately 12.6 mm with an approach speed of 6 m/min and a delay of 1 m/s

Kv-Factor

1m/min

min

Zero speed

1 m/min

(16 ms) Delay until distance-to-go is deleted

6 m/min Approach speed v

4 m/min

10 10

Axis zero speed

Zero speed

t [ms]

Introduction 12.97

1.7 Measuring strategy and compensation value calculation for tools

08.99

840 D

NCU 571

1.7 Measuring strategy and compensation value calculation for tools with automatic tool

840 D

NCU 572

NCU 573

810 D 840Di

offset

The actual workpiece dimensions must be measured

exactly in order to be able to determine and compensate the actual dimensional deviations on the workpiece.

Function

When taking measurements on the machine, the actual dimensions are derived from the path measuring systems of the position-controlled feed axes. For each dimensional deviation determined from the set and actual workpiece dimensions there are many causes which essentially can be classified in 3 categories:

• Dimensional deviations with causes that are

n o t subject to a particular trend,

scatter of the feedforward axes or differences in measurement between the internal measurement (measuring probe) and the external measuring device (micrometer, measuring equipment, etc.).

In this case, it is possible to apply so-called

empirical values, which are stored in separate

memories. The set/actual difference determined is automatically compensated by the empirical value.

• Dimensional deviations with causes that a r e

subject to a particular trend

thermal expansion of the leadscrew.

These deviations are compensated by specifying fixed threshold values.

• Accidental dimensional deviations, e.g. due to

temperature fluctuations, coolant or slightly soiled measuring points.

, e.g. tool wear or

e.g. positioning

1-28 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

1.7 Measuring strategy and compensation value calculation for tools

840 D

NCU 571

840 D

NCU 572

NCU 573

810 D 840Di

Assuming the ideal case, only those dimensional

deviations which are subject to a trend can be taken into account for compensation value calculation. Since, however, it is hardly ever known to what extent and in which direction accidental dimensional deviations influence the measurement result, a strategy (floating average value generation) is needed which derives a compensation value from the actual/set difference measured.

Mean value calculation

Mean value calculation in combination with a higherorder measurement weighting has proved a suitable means to do this.

The formula of the mean value generation chosen is:

Mv D

−

Mv Mv

=−

new old

old i

Mv Mv

Mean value new = amount of compensation

new

Mean value prior to last measurement

old

k Weighting factor for average value calculation D

Actual/set difference measured

(minus empirical value, if any)

The mean value calculation takes account of the trend

of the dimensional deviations of a machining series,

weighting factor k from which the mean value is

where derived is selectable.

A new measurement result affected by accidental dimensional deviations only influences the new tool offset to some extent, depending on the weighting factor.

Introduction 12.97

1.7 Measuring strategy and compensation value calculation for tools

08.99

840 D NCU 571

Computational characteristic of the mean value

840 D NCU 572 NCU 573

810 D 840Di

with different weightings k (effects)

• The greater the value of k, the slower the formula

will respond when major deviations occur in computation or counter compensation. At the same time, however, accidental scatter will be reduced as k increases.

• The lower the value of k, the faster the formula will

react when major deviations occur in computation or counter compensation. However, the effect of accidental variations will be that much greater.

• The mean value Mv is calculated starting at 0 over

the number of workpieces i, until the calculated average value exceeds the range of "zero compensation". From this limit on, the calculated average value is applied for compensation.

Example of mean value generation

Lower limit = 40 µm

[µm]

Mean value

k=3

[µm]

Mean value

k=2

[µm]

1st measurement 30 10 15

2nd measurement 50 23.3 32.5

3rd measurement 60 35.5 46.2



4th measurement 20 30.3 10 5th measurement 40 32.6 25 6th measurement 50 38.4 37.5 7th measurement 50 42.3



43.75



8th measurement 30 10 15 9th measurement 70 30 42.5

10th measurement 70 43.3





Set/actual difference

Mean value calculated

Setpoint

1234 560

Characteristic of mean values with two different weighting factors k

12345678910

k=2

k=3

Lower limit = "Zero offset"

k=1

k=2

k=3

Number of averaging operations (workpieces)

Mean value calculated

k=10

Set/actual difference

Zero compensation

1-30 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

08.99

1.8 Parameters for checking the dim. deviation and compensation

840 D NCU 571

1.8 Parameters for checking the dim. deviation and compensation

Explanation

For constant deviations not subject to a trend the dimensional deviation measured can be compensated by an empirical value for certain measurement variants. For other compensations resulting from dimensional deviations, symmetrical tolerance bands are assigned to the set dimension which result in different responses.

Empirical value _EVNUM

The empirical values are used to suppress dimensional

deviations

The empirical values are stored in the GUD field

_EV empirical value.

_EVNUM specifies the number of the empirical value memory. The actual/set difference determined by the

measuring cycle is corrected by this value further correction measures are taken. This is the case

• for workpiece measurement with automatic tool

• for tool measurement

• for single-point measurement with automatic

The tolerance bands (range of permissible dimensional tolerance) and the responses derived from them have been specified as follows:

840 D NCU 572 NCU 573

that are not subject to a trend.

offset

ZO compensation

810 D 840Di

before any

Introduction 12.97

1.8 Parameters for checking the dim. deviation and compensation

05.98

840 D NCU 571

•

840 D NCU 572 NCU 573

810 D 840Di

For workpiece measurement with automatic

tool offset

_TSA

_TDIF

_TLL, _TUL

_TMV

_TZL

Safe area

Dimensional difference check

Workpiece tolerance

2/3 workpiece tolerance

Zero compensation (lower limit)

Setpoint

Alarm: "Safe area overrun"

Alarm: "Permissible dimensional difference overrrun"

Compensation of current deviation Alarm: "Oversize", "Undersize"

Compensation of current deviation

Averaging (_EVNUM, _K) and compensation by mean value

Averaging is stored

The workpiece set dimension is placed in the center

of the permissible ± tolerance limit applied.

For tool measurement

•

_TSA

_TDIF

_TZL

Safe area

Dimensional difference check

Zero compensation (lower limit)

Setpoint = Tool data

Alarm: "Safe area overrun"

Alarm: "Permissible dimensional difference overrun"

Tool memory is compensated

Tool memory unchanged

1-32 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

05.98

1.8 Parameters for checking the dim. deviation and compensation

840 D NCU 571

•

840 D NCU 572 NCU 573

810 D 840Di

For workpiece measurement with zero offset

_TSA

Safe area

Setpoint

For workpiece probe calibration

•

_TSA

Safe area

Alarm: "Safe area overrun"

Compensation of ZO memory

Alarm: "Safe area overrun"

_TZL

Zero compensation (lower limit)

Setpoint =_WP[]-data

For tool probe calibration

•

_TSA

_TZL

Safe area

Zero compensation (lower limit)

Setpoint=_TP[]-data

_WP[] data is compensated

_WP[] data unchanged

Alarm: "Safe area overrun"

_TP[] data is compensated

_TP[] data unchanged

Introduction 12.97

1.8 Parameters for checking the dim. deviation and compensation

08.99

840 D NCU 571

Safe area _TSA

The safe area is active for all measurement variants and does not affect the offset value; it is used for diagnosis. If this value is reached,

• a defect in the probe,

• an incorrect setpoint position or

• an illegal deviation from the setpoint position

may be the cause.

AUTOMATIC operation is interrupted and the program

cannot continue. An alarm text appears to warn the user.

Dimensional difference control _TDIF

_TDIF is active only for workpiece measurement with automatic tool offset and for tool measurement. This limit has no effect on generation of the compensation value either. When it is reached, the tool is probably worn and needs to be replaced.

840 D NCU 572 NCU 573

810 D 840Di

An alarm text is displayed to warn the operator and the

This tolerance limit is generally used by the PLC for tool

program can be continued by means of an NC start.

management purposes (twin tools, wear monitoring).

Tolerance of the workpiece _TLL, _TUL Both parameters are active only for tool measurement with automatic tool offset. When measuring a dimensional deviation ranging

between "2 difference control", this is regarded 100% as tool compensation. The previous average value is erased. It is therefore possible to effect fast counteraction if major dimensional deviations occur.

/3 tolerance of workpiece" and "Dimensional

1-34 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

08.99

1.8 Parameters for checking the dim. deviation and compensation

840 D NCU 571

840 D NCU 572 NCU 573

810 D 840Di

AUTOMATIC operation is interrupted when the tolerance

limit of the workpiece is exceeded. "Oversize" or "undersize" is displayed to the operator depending on the tolerance zone position. Machining can be continued by means of NC start.

2/3 workpiece tolerance _TMV

_TMV is active only for workpiece measurement with automatic tool offset.

Within the range of "Lower limit" and "2

/3 workpiece

tolerance" the mean value is calculated according to the formula described in Section "Measuring strategy".

• If Mv

is compared with the zero compensation range:

new

is greater than this range, compensation is

new corrected by Mv

and the associated mean value

new

memory is cleared.

• If Mv

is less than this range, no compensation is

new carried out to prevent excessively abrupt compensations from being made.

Mean value_EVNUM

_EVNUM is active only for workpiece measurement with automatic tool offset. When calculating the mean value in a series of machining operations, the mean value determined by the measurement at the same measurement location on the previous workpiece can be taken into account (_CHBIT[4]=1).

The mean values are stored in the GUD field

values

. _EVNUM also specifies the number of the mean

value memory in this GUD field.

Weighting factor for mean value calculation _K

_K is active only workpiece measurement with automatic tool offset. The weighting factor k can be applied to allow different weighting to be given to an individual measurement.

A new measurement result thus has only a limited effect on the new tool offset as a function of _K.

_MV mean

Introduction 12.97

1.8 Parameters for checking the dim. deviation and compensation

840 D NCU 571

Bottom limit (zero compensation area) _TZL

_TZL active for

• Workpiece measurement with automatic tool offset

• Tool measurement and calibration for milling tools

This tolerance range corresponds to the amount of maximum accidental dimensional deviations. It has to be determined for each machine. No tool compensation is made within these limits.

However, the average value of this measuring point is updated and re-stored with the actual/set difference measured for workpiece measurement with automatic tool offset, compensated by an empirical value if necessary.

840 D NCU 572 NCU 573

and tool probes

810 D 840Di

1-36 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

05.98

1.9 Effect of empirical value, mean value and tolerance parameters

840 D NCU 571

1.9 Effect of empirical value, mean value and tolerance parameters

840 D NCU 572 NCU 573

810 D 840Di

The following flowchart shows the effect of empirical

value, mean value and tolerance parameters by way of a workpiece measurement with automatic tool offset.

Measuring cycle

Measure

Calculate act/set difference

Difference minus empirical value

Difference > safe area _TSA

Yes

Compensation strategy

Calculate mean value considering weighting factor _K

Mean value > lower limit _TZL

Store mean value (only for _CHBIT[4]=1)

Difference > workpiece tol. _TUL/_TLL

Difference > 2/3 workpiece tol. _TMV

Smoothed

YesNo

compensation

Compensation by mean value

Delete mean value

Difference > dimensional diff. control _TDIF

Yes

Display: Oversize or undersize

100 % compens.

YesNo

Delete mean value

Compensation by difference

Yes

Display: Permiss. Dimensional difference exceeded

Repeat measurement

Alarm 61303

Alarm: Safe area exceeded

Display: Safe area exceeded

Yes

End

Introduction 12.97

1.10 Reference points on the machine and workpiece

840 D NCU 571

840 D NCU 572 NCU 573

810 D 840Di

1.10 Reference points on the machine and workpiece

Function

The actual axis values of different actual value systems must be measured depending on the measuring process applied. While, for example, the machine actual value can be used to advantage to calculate the tool length, the workpiece zero is important for measuring workpiece dimensions and calculating the tool wear compensation. The machine actual value is the dimension between the machine zero and the tool reference point.

M = Machine zero M' = Machine zero offset by DRF C = Control zero resulting from PRESET offset W = Workpiece zero F = Tool reference point

Spindle chuck

MM'C W

Workpiece

1-38 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

1.11 Measurement variants for milling machines & machining centers

840 D NCU 571

1.11 Measurement variants for milling machines & machining centers

840 D NCU 572 NCU 573

810 D 840Di

The measurement variants which can be implemented

with measuring cycles for milling machines and machining centers are illustrated in diagrams below.

1.11.1 Workpiece measurement for milling machines

Tool probe calibration

Result: Probe switching point with reference to machine zero

Calibration tool

Measuring the tool

Result: Tool length

Length

Drill

Tool radius

Radius

Mill

Introduction 12.97

1.11 Measurement variants for milling machines & machining centers

840 D NCU 571

1.11.2 Measurement variants for fast measurement at a single point

Function

CYCLE978 makes it easy to take a measurement at one point of a surface.

The measuring point is approached paraxially.

Depending on the measurement variant, the result may influence the selected tool offset or zero offset.

Workpiece measurement, blank measurement

Result: Position, deviation, Zero offset

840 D NCU 572 NCU 573

810 D 840Di

Workpiece measurement, single-point

1.11.3 Measurement variants for workpiece measurement paraxial

measurement

Result: Actual dimension, deviation, tool offset

Function

The following measurement variants are provided for the paraxial measurement of a hole, shaft, groove or web. They are executed by the cycle CYCLE977.

1-40 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

1.11 Measurement variants for milling machines & machining centers

840 D NCU 571

Workpiece measurement, measuring the hole

Result: Actual dimension (diameter), deviation, center point, tool offset, zero offset

Workpiece measurement, measuring the shaft

Result: Actual dimension (diameter), deviation, center point, tool offset, zero offset

Workpiece measurement, measuring the

groove

840 D NCU 572 NCU 573

810 D 840Di

Result: Actual dimension (groove width), deviation, groove center, tool offset, zero offset

Workpiece measurement, measuring the web

Result: Actual dimension (web width), deviation, web center, tool offset, zero offset

Workpiece measurement, measuring the

inside rectangle

Result: Actual value rectangle length and width, actual dimension rectangle center, deviation rectangle length and width, deviation rectangle center, tool offset, zero offset

Introduction 12.97

1.11 Measurement variants for milling machines & machining centers

840 D NCU 571

Workpiece measurement, measuring the

1.11.4 Measurement variants for workpiece measurement at random angles

outside rectangle

Result: Actual value rectangle length and width, actual dimension rectangle center, deviation rectangle length and width, deviation rectangle center, tool offset, zero offset

Function

840 D NCU 572 NCU 573

810 D 840Di

The following measurement variants are provided for the measurement of a bore, shaft, groove or web at random angles. They are executed by CYCLE979.

Triple-point (quadruple-point) measurement at

random angles

Result: Actual dimension (diameter), deviation, center point, tool offset, zero offset

Hole, shaft, circle segment

1-42 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

1.11 Measurement variants for milling machines & machining centers

840 D NCU 571

Two-point measurement at random angles

Result: Actual dimension (groove width, web width), deviation, groove center, web center, zero offset

840 D NCU 572 NCU 573

810 D 840Di

Groove, web

1.11.5 Measuring a surface at a random angle

Function

The zero offset can be compensated after measurement of a surface at a random angle by means of CYCLE998.

Workpiece measurement, angular

measurement

Result: Actual dimension (angle), deviation, zero offset

Angle measurement

Introduction 12.97

1.12 Measurement variants for lathes

840 D NCU 571

1.12 Measurement variants for lathes

1.12.1 Tool measurement for lathes

Tool probe calibration

Result: Probe switching point with reference to machine zero

840 D NCU 572 NCU 573

810 D 840Di

Calibration tool

Measuring the tool

Result: Tool length (length1, length2)

1-44 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

05.98

1.12 Measurement variants for lathes

840 D NCU 571

1.12.2 Workpiece measurement for turning machines: Single-point measurement

840 D NCU 572 NCU 573

810 D 840Di

Single-point measurement outside

Result: Actual dimension (diameter, length), deviation, tool offset, zero offset

Single-point measurement inside

Calibrate

Measure

Result: Actual dimension (diameter, length), deviation, tool offset,

Calibrate

zero offset

Measure

Introduction 12.97

1.12 Measurement variants for lathes

05.98

840 D NCU 571

Single-point measurement outside with 180°°°°

reversal spindle

840 D NCU 572 NCU 573

810 D 840Di

Result: Actual dimension (diameter, length), deviation,

Calibrate

tool offset

Measure

Single-point measurement inside with 180°°°°

reversal spindle

Result: Actual dimension (diameter, length), deviation, tool offset

Calibrate

Measure

1-46 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

05.98

1.12 Measurement variants for lathes

840 D NCU 571

1.12.3 Workpiece measurement for turning machines: Two-point measurement

Two-point measurement on outside diameter

Result: Actual dimension (diameter), deviation, tool offset

840 D NCU 572 NCU 573

810 D 840Di

Two-point measurement on inside diameter

Result: Actual dimension (diameter), deviation, tool offset

Introduction 12.97

1.13 Measuring cycles interface

840 D NCU 571

1.13 Measuring cycles interface

The measuring cycles provide an interactive function for

defining input and output parameters.

Values can be assigned to the input parameters via a help cycle in an input dialog.

The results of measurement can be displayed automatically via another help cycle.

1.13.1 Displaying measuring result screens

Function

840 D NCU 572 NCU 573

810 D 840Di

Depending on the configuration

Measuring results can be displayed automatically while a measuring cycle is running.

Activation of this function depends on the configuration

of the measuring cycle interface in the MMC and the settings in the measuring cycle data.

Observe the specifications of the machine

manufacturer.

• the measuring result displays are automatically

deselected at the end of a measuring cycle

• the measuring result displays must be

acknowledged with the NC Start key;

In this case, the measuring cycle outputs the message:

"Please acknowledge measuring result display with

NC Start"

1-48 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

1.13 Measuring cycles interface

840 D NCU 571

Explanation

The measuring cycles can display different measuring result screens depending on the measurement variant:

• Tool probe calibration

• Tool measurement

• Workpiece probe calibration

• Workpiece measurement

The result displays contain the following data:

Calibrating the tool probe

− Measuring cycle and measurement variant

− Probe ball diameter and difference

− Trigger values of axis directions and differences

− Positional deviation during calibration on the plane

− Probe number

− Safe area

Tool measurement

− Measuring cycle and measurement variant

− Actual values and differences for tool offsets

− T number and D number

Calibrate tool probe

− Measuring cycle and measurement variant

− Trigger values of axis directions and differences

− Positional deviation during calibration on the plane

− Probe number

− Safe area and permissible dimensional difference

Workpiece measurement

− Measuring cycle and measurement variant

− Setpoints, actual values and their differences

− Upper and lower tolerance limits

− Offset value

− Probe number

− Safe area and permissible dimensional difference

− T number and D number or ZO memory for

840 D NCU 572 NCU 573

automatic offset

810 D 840Di

Introduction 12.97

1.13 Measuring cycles interface

840 D NCU 571

1.13.2 Setting parameters

Function

Values can be assigned to measuring cycle parameters with CYCLE103.

Activation of this function depends on the configuration

of the measuring cycle interface in the MMC.

Observe the specifications of the machine

manufacturer.

Explanation

When CYCLE103 is selected and started, an input dialog for setting parameters for the measuring cycles is opened. During the course of this dialog, a series of input screen forms are opened one after the other on top of the current display. Once the values have been entered each display must be concluded by pressing the OK key in the vertical softkey bar. At the end of the dialog, the message "Input dialog successfully completed" is displayed in the dialog line of the control and the display before dialog mode was activated is reconstructed.

It is immediately possible to select and start the last measuring cycle assigned parameters.

840 D NCU 572 NCU 573

810 D 840Di

1-50 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Introduction

1.13 Measuring cycles interface

840 D NCU 571

Explanation

The sequence of the dialog for assigning parameters is as follows:

• Selection of the measuring cycle to which

• Selection of the measurement variant;

• Assignment of parameters for the measurement

• Input and confirmation of generally applicable

The input values for selecting the measuring cycle and the measurement variant are subjected to a plausibility check and the input screen forms are repeated if necessary.

840 D NCU 572 NCU 573

parameters are to be assigned;

variant chosen, this could involve several input screen forms depending on the measuring cycle;

measuring cycle data which do not usually change.

810 D 840Di

If the operating area is switched over during the course of the input dialog, the dialog can be selected again at a later stage with "Cycles" softkey in the extended menu.

Introduction 12.97

1.13 Measuring cycles interface

Notes

840 D NCU 571

840 D NCU 572 NCU 573

810 D 840Di

1-52 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Description of Parameters

09.01

Description of Parameters

2.1. Parameter concept for measuring cycles........................................................................ 2-54

2.2 Parameter overview ........................................................................................................ 2-56

2.2.1 Input parameters ....................................................................................................... 2-56

2.2.2 Result parameters..................................................................................................... 2-57

2.3 Description of the most important defining parameters .................................................. 2-58

2.3.1 Measurement variant: _MVAR .................................................................................. 2-58

2.3.2 Number of measuring axis: _MA............................................................................... 2-61

2.3.3 Tool number and tool name: _TNUM and _TNAME ................................................. 2-62

2.3.4 Offset number _KNUM.............................................................................................. 2-63

2.3.5 Offset number _KNUM with flat D number structure ................................................ 2-65

2.3.6 Variable measuring speed: _VMS............................................................................. 2-66

2.3.7 Compensation angle position for monodirectional probe: _CORA ........................... 2-66

2.3.8 Tolerance parameters: _TZL, _TMV, _TUL, _TLL, _TDIF and _TSA ...................... 2-67

2.3.9 Multiplication factor for measurement path 2a: _FA ................................................. 2-68

2.3.10 Probe type/Probe number: _PRNUM........................................................................ 2-69

2.3.11 Empirical value/mean value: _EVNUM ..................................................................... 2-70

2.3.12 Multiple measurement at the same location: _NMSP ............................................... 2-71

2.3.13 Weighting factor k for averaging: _K......................................................................... 2-71

2.4. Description of output parameters .................................................................................... 2-72

2.4.1 Measuring cycle results in _OVR .............................................................................. 2-72

2.4.2 Measuring cycle results in _OVI................................................................................ 2-73

Description of Parameters 12.97

2.1. Parameter concept for measuring cycles

840 D NCU 571

840 D NCU 572 NCU 573

810 D 840Di

2.1. Parameter concept for measuring cycles

Function

As explained at the beginning, measuring cycles are general subroutines designed to solve specific measuring tasks. They can be adapted for this purpose by means of so-called defining parameters.

They also return data such as measurement results. They are stored in result parameters.

Furthermore, the measuring cycles also require

internal parameters for calculations.

Defining parameters

The defining parameters of the measuring cycles are defined as Global User Data (abbreviated to GUDs).

They are stored in the nonvolatile storage area of the control such that their setting values remain stored even when the control is switched off and on.

These data are contained in the data definition blocks

• GUD5.DEF and

• GUD6.DEF

which are supplied together with the measuring cycles.

Further notes

Many of the defining parameters have preset values. See Section 2.2

2-54 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Description of Parameters

2.1. Parameter concept for measuring cycles

840 D

NCU 571

840 D

NCU 572 NCU 573

810 D 840Di

These blocks must be loaded into the control during

start-up. They must then be adapted by the machine manufacturer according to the characteristics of the relevant machine (see Part 2 Description of Functions, from Chapter 8 onwards).

Values can be assigned to these GUDs in the program

or by means of keyboard inputs.

Result parameters

The results are also stored in specific GUDs.

Internal parameters

Local User Data (abbreviated to LUDs) are used in the measuring cycles as internal arithmetic parameters.

These are set up in the cycle and thus exist only for the duration of the run-time.

Description of Parameters 12.97

2.2 Parameter overview

840 D

NCU 571

840 D

NCU 572 NCU 573

2.2 Parameter overview

2.2.1 Input parameters

Explanation

810 D 840Di

12.98

The defining parameters of the measuring cycles can be classified as follows:

• Mandatory parameters

• Additional parameters

Mandatory parameters are parameters that have to be adapted to the measuring task at hand (for example, setpoint axis, measuring axis, etc.) before each measuring cycle call. Additional parameters can generally be assigned once on a machine. They are then valid for each measuring cycle call until they are modified by programming or operation.

All parameters with dimensions (see overview below),

except for those marked 1), must be programmed in the unit of measurement of the basic system. The parameters marked 1) must be programmed in the unit of the active system of units. Mandatory parameters

Parameters Type Validity Default: Meaning

_SETVAL

_SETV[3]

_ID

_CPA

_CPO

_SZA

_SZO

_STA1

_INCA

_MVAR

_MA

_MD

_TNUM

_TNAME

REAL CHAN - Setpoint

REAL CHAN - Measure setpoint values on rectangle REAL CHAN - Incremental infeed depth/offset REAL CHAN - Center point abscissa for measuring at angle REAL CHAN - Center point ordinate for measuring at angle REAL CHAN - Protection zone in abscissa REAL CHAN - Protection zone in ordinate REAL CHAN 0 Initial angle REAL CHAN - Indexing angle INT CHAN - Measurement variant INT CHAN - Measuring axis INT CHAN - Measuring direction INT CHAN - T number STRING[32] CHAN - Tool name (alternative to _TNUM in tool

management)

_KNUM

_RA

INT CHAN 0 Correction number (D No. or ZO No.) INT CHAN - Number of rotary axis at angle measurement

2-56 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Description of Parameters

12.98

2.2 Parameter overview

840 D

NCU 571

840 D

NCU 572 NCU 573

810 D 840Di

Auxiliary parameters

Parameters Type Validity Default Meaning

_VMS

_RF

_CORA

_TZL

_TMV

_TUL

_TLL

_TDIF

_TSA

_FA

_CM[8]

_PRNUM

_EVNUM

_CALNUM

_NMSP

REAL CHAN 0 Variable measuring velocity REAL CHAN 1000 Feedrate at circular-path programming REAL CHAN 0 Compensation angle for mono probe REAL CHAN 0.001 Zero offset area REAL CHAN 0.7 Mean value generation with compensation REAL CHAN 1.0 Upper tolerance limit REAL CHAN -1.0 Lower tolerance limit REAL CHAN 1.2 Dimensions difference check REAL CHAN 2 Safe area REAL CHAN 2 Measuring path multiplication factor REAL NCK 90, 2000, 1, 0,

0.005, 50, 4, 10

Monitoring parameters at tool measurement

with rotating spindle INT CHAN 1 Probe number INT CHAN 0 Empirical value memory number INT CHAN 0 Calibration block number INT CHAN 1 Number of measurements at the same

location

INT CHAN 1 Weighting factor for mean value derivation

Parameters for logging only

Parameters Type Validity Meaning

_PROTNAME[2]

STRING[32] NCK [0]: Name of main program the log is from

[1]: Name of log file

_HEADLINE[6]

_PROTFORM[6]

_PROTSYM[2]

_PROTVAL[13]

STRING[80] NCK 6 strings for protocol headers INT NCK Formatting for protocol CHAR NCK Separator in the protocol STRING[100] NCK [0, 1]: Protocol header line

[2-5]: Specification of the values to be logged [6-12]: Internal

_DIGIT

INT NCK Number of decimal places

2.2.2 Result parameters

Parameters Type Validity Meaning

_OVR[32]

REAL CHAN Result parameters: Setpoint values, actual values,

differences, offset values and others

_OVI[11]

INT CHAN Result parameter, integer

Description of Parameters 12.97

2.3 Descri

840 D

NCU 571

2.3 Description of the most important defining parameters

2.3.1 Measurement variant: _MVAR

Function

840 D

NCU 572 NCU 573

tion of the most important defining parameters

810 D 840Di

08.99

The measurement variant of the individual cycles is defined in parameter _MVAR.

Parameters

Values of _MVAR The parameter can assume certain positive integers for each measuring cycle which are listed individually below.

The setting of parameter _MVAR is subjected to a

plausibility check by the cycle. If it does not have a defined value, the following alarm message is output:

"Measurement variant incorrectly defined".

The cycle must be interrupted by an NC RESET.

Measurement and calibration variants for workpiece measurement on milling machines

Possible values of _MVAR

CYCLE976 0

CYCLE977 1 Measure hole

and 2

CYCLE979 3

CYCLE977

1...112101 Calibrate in random hole (plane)

8...10108 Calibrate workpiece probe in any hole (plane) with

101

102

103

104 ZO calculation on web

5 Measure rectangle inside

6 Measure rectangle outside

105 ZO calculation in rectangle inside

106 ZO calculation in rectangle outside

Calibration on any surface (applicate)

unknown position of the hole center

Measure shaft

Measure groove

Measure web

ZO calculation in hole

ZO calculation in shaft

ZO calculation in groove

Measurement variants

2-58 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Description of Parameters

08.99

2.3 Description of the most important defining parameters

840 D

NCU 571

840 D

NCU 572 NCU 573

810 D 840Di

CYCLE977

1001 Measure hole with travel around a protection zone

1002 Measure shaft while accounting for a protection zone

1003

1004

Measure hole with contouring of a protection zone

Measure web by including for a protection zone

1005 Measure rectangle inside with protection zone

1006 Measure rectangle outside with protection zone

1101 ZO calculation hole with travel around a protection zone

1102 ZO calculation of shaft while accounting for a protection

zone

1103

ZO calculation in groove with contouring of a protection zone

CYCLE978

CYCLE998

1104

ZO calculation at web by including a protection zone

1105 ZO calculation in rectangle inside with protection zone

1106 ZO calculation in rectangle outside with protection zone

100

1000

1100

105

1105

Measure surface

ZO calculation on surface

Measure surface with differential measurement

ZO calculation on surface with differential measurement

Angular measurement, ZO calculation

Angular measurement with differential measurement, ZO calculation

Measurement and calibration variants for tool

measurement on milling machines

Possible values of _MVAR Measurement variants

CYCLE971 1

Measure tool with motionless spindle (Length or radius)

2 Measure tool with rotating spindle

(Length or radius)

0 Calibration of the tool probe

10000 Incremental calibration of the tool probe

Further notes

1) Measuring cycles SW 4.5 and higher

Description of Parameters 12.97

2.3 Descri

tion of the most important defining parameters

840 D

NCU 571

840 D

NCU 572 NCU 573

810 D 840Di

Measurement and calibration variants for workpiece measurement on lathes

Possible values of _MVAR Measurement variants

CYCLE973 0

CYCLE974

CYCLE994

13...12113 Calibration in reference groove (plane)

100

1000

Calibration on any surface (applicate)

Single-point measurement

Single-point measurement ZO calculation

Single-point measurement with reversal

Two-point measurement with protection zone (for inside measurement only)

Two-point measurement with programmed protection zone (for inside measurement without protection zone)

Measurement and calibration variants for tool

measurement on lathes

Possible values of _MVAR Measurement variants

CYCLE972 0

CYCLE982

1 Tool measurement

Tool probe calibration

(measuring cycle SW 5.3 and higher)

1 Measuring turning and milling tools

2 Automatic measurement

2-60 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Description of Parameters

2.3 Description of the most important defining parameters

840 D

NCU 571

840 D

NCU 572 NCU 573

810 D 840Di

2.3.2 Number of measuring axis: _MA

Function

The axis number (1...3) for the measuring axis in the coordinate system must be specified via _MA (not the hardware axis number).

Parameters

Values of _MA

G17 plane

Measuring axis abscissa _MA = 1 Measuring axis ordinate _MA = 2 Measuring axis applicate _MA = 3

_MA must be defined with offset axis /measuring axis for certain measurement variants; in such cases, the first two digits contain the code for the offset axis and the second two digits the code for the measuring axis.

Example: _MA = 102 Þ Offset axis: 1 (abscissa) Þ Measuring axis: 2 (ordinate)

Axis definition in acc. to DIN 66217

_MA=2

_MA=1

Description of Parameters 12.97

2.3 Descri

840 D

NCU 571

2.3.3 Tool number and tool name: _TNUM and _TNAME

Function

840 D

NCU 572 NCU 573

tion of the most important defining parameters

810 D 840Di

08.99

The tool to be offset is entered during workpiece measurement in the parameters _TNUM and _TNAME.

The parameter _TNAME is only relevant if tool

management is active.

Parameters

The parameter _TNUM contains the tool number of the tool to be automatically offset during workpiece measurement. If tool management is active, the name of the tool can be entered in parameter _TNAME as an alternative.

Example:

• without tool management:

_TNUM = 12 _TNAME = " " Þ is not assigned;

• with tool management:

_TNUM = 0 _TNAME = "DRILL"

Þ the tool with the name

"DRILL" is offset or _TNUM = 13 _TNAME = " " or _TNAME="DRILL"

Þ the tool with the internal

T number 13 is offset

In SW 4 and higher with spare tools the one is offset which was last used (was in the spindle). However, the requirement is that only one tool in a group is "active" at on time. Otherwise, the internal tool number of the tool used must be determined and assigned to _TNUM when machining via the system variable $P_TOOLNO.

2-62 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Description of Parameters

11.02

2.3 Description of the most important defining parameters

840 D

NCU 571

840 D

NCU 572 NCU 573

2.3.4 Offset number _KNUM

Parameters

The parameter _KNUM contains the tool offset memory number for workpiece measurement or the specification of the zero offset to be compensated for ZO calculation.

_KNUM setting values

_KNUM can accept integers with up to 6 digits, or 8 digits with flat D number structures. These digits have the following significance:

1. Specification for tool offset: Structure of tool offset parameter _KNUM

810 D 840Di

654321

D number Currently not assigned, i. e. = 0 0/1...Length compensation

2...Radius compensation Normal/inverted offset

0...Normal

1...Inverted Offset acc. to 4th digit

1...Offset of L1

2...Offset of L2

3...Offset of L3

4...Radius compensation

In SW 5 and higher the last 3 digits are evaluated as a D number for a value of this MD from 10...999 depending on MD 18102: MM_TYPE_OF_CUTTING_EDGE = 0 and MD 18105: MM_MAX_CUTTING_EDGE_NO. If the

value is ≥1000, _KNUM is evaluated as for a flat D number

structure.

Example:

_KNUM = 12003

Þ D3 is corrected, Þ calculated as radius offset Þ inverted correction

Description of Parameters 12.97

2.3 Descri

840 D

NCU 571

2. Specification for zero offset:

840 D

NCU 572 NCU 573

_KNUM=1 ... 99 Automatic inclusion of ZO in ZO G54 ... G57 and G505...G599

In measuring cycle SW 4.4 and higher: _KNUM=1000 automatic ZO in basic frame G500 (offset always in the last channel-specific basic frame if there are more than one).

In measuring cycle SW 6.2 and higher:

- KNUM=1011...1026 automatic ZO in 1st to 16th basic frame (channel) ($P_CHBFR[0]...$P_CHBFR[15])

- KNUM=1051...1066 automatic ZO in 1st to 16th basic frame (global) ($P_NCBFR[0]...$P_NCBFR[15]) Note: The remaining active frame chain must be retained. With NCU-global frames, correction for rotation is not possible.

- _KNUM=2000 automatic ZO in the system frame (scratch system frame $P_SETFR)

- _KNUM=9999 automatic ZO in the active frame: settable frame G54...G57, G505...G599, or G500 in the last active basic frame according to $P_CHBFRMASK (most significant bit). Note: Only here does a changed frame become active in the

tion of the most important defining parameters

810 D 840Di

cycle immediately, otherwise it is activated by the user writing G500, G54...G5xy.

11.02

The following must be set for start-up: MD 28082: MM_SYSTEM_FRAME_MASK, Bit 0=1 and Bit 5=1 (system frames for scratching and cycles)

With a _KNUM setting of 0, the automatic tool offset and ZO are deactivated.

In measuring cycle SW 6.2 and higher, CYCLE115 is introduced for the ZO. CYCLE114 is only responsible for the tool offset.

If a fine offset is active (MD 18600: MM_FRAME_FINE_TRANS), the additive ZO will be implemented in it (all measuring cycles with ZO except CYCLE961), otherwise it is implemented in the coarse offset. ZO with CYCLE961 is always in the coarse offset and any fine offset there may be is reset.

2-64 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Description of Parameters

09.01

2.3 Description of the most important defining parameters

840 D NCU 571

840 D NCU 572 NCU 573

810 D

2.3.5 Offset number _KNUM with flat D number structure

Parameters

The flat D number functionality is implemented in SW 4 and higher. Which type of D number management is valid is defined in MD 18102: MM_TYPE_OF_CUTTING_EDGE.

References: /FB/, W1, "Tool offset"

MD 18102: 0: as previously (default setting) 1: flat D number direct programming

With activation of flat D numbers, a five-digit D number is assumed in _KNUM.

876543

D number

0/1...Length compensation

2...Radius compensation Normal / inverted offset

0...Normal

1...Inverted Offset acc. to 6th digit

1...Offset of L1

2...Offset of L2

3...Offset of L3

4...Radius compensation

Description of Parameters 12.97

2.3 Descri

840 D

NCU 571

840 D

NCU 572 NCU 573

tion of the most important defining parameters

810 D 840Di

2.3.6 Variable measuring speed: _VMS

Parameters

The measuring speed can be freely selected by means

_VMS. It is specified in mm/min or inch/min

of depending on the basic system.

The maximum measuring speed must be selected such that safe deceleration within the probe deflecting path is ensured.

12.98

When _VMS = 0, then the feedrate is preset as standard to 150 mm increased to 300 mm (_FA > 1 ) is altered via _FA. If the basic system is in inches, 5.9055 inch/min or

11.811 inch/min takes effect.

/min. This value is automatically

/min if the measuring path a

2.3.7 Compensation angle position for monodirectional probe: _CORA

Function

When using a monodirectional probe, it may be necessary for machine-specific reasons (e.g. horizontal probe to be able to carry out the measurement.

/vertical millhead) to correct the position of the

Parameters

The incorrect position can be corrected by means of parameter to 90° or a multiple thereof. If the direction of rotation is altered as a result of swiveling the milling head, then _CORA must be preset to –360° (normally 0°).

_CORA. Generally speaking, _CORA is set

2-66 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Description of Parameters

2.3 Description of the most important defining parameters

840 D NCU 571

840 D NCU 572 NCU 573

810 D 840Di

2.3.8 Tolerance parameters: _TZL, _TMV, _TUL, _TLL, _TDIF and _TSA

Some information about the tolerance parameters applied in conjunction with measuring cycles is already given in Section 1.8.

Parameters

These parameters contain the following variables:

_TZL

_TMV

_TUL/_TLL

_TDIF

_TSA

Zero offset Average-value generation with compensation Workpiece tolerance Dimension difference check Safe area

1) for workpiece measurement with automatic tool offset only

2) also for tool measurement

1)2)

Value range

All of these parameters are capable of assuming any value. However, only values increasing from _TZL to _TSA are meaningful. Parameters _TUL/_TLL are specified in mm or inches depending on the active dimension system. All other parameters are programmed in the basic system.

Description of Parameters 12.97

2.3 Descri

tion of the most important defining parameters

840 D

NCU 571

840 D

NCU 572 NCU 573

810 D 840Di

2.3.9 Multiplication factor for measurement path 2a: _FA

Parameters

Path increment a is 1 mm irrespective of the dimension system, but can be increased with parameter the measuring cycles are called and defines the distance from the expected position at which the probe is triggered. The maximum value for _FA is calculated as follows:

_FA

Axis traversing path

max

The measuring cycles automatically generate a

measurement path of 2

a · _FA, which is traversed at

_FA when

10.00

the measuring feedrate, i.e. at a distance of

a · _FA in

front of the specified setpoint position at which the probe is actuated under ideal conditions, up to

a · _FA after the anticipated setpoint position.

If the probe is triggered during this measurement path the movement is aborted with delete distance-to-go.

Example:_FA=5

à Irrespective of the system of units, a measurement

path of 10 mm is generated, starting at 5 mm before and ending 5 mm after the specified setpoint position.

2-68 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Description of Parameters

08.99

2.3 Description of the most important defining parameters

840 D NCU 571

840 D NCU 572 NCU 573

810 D 840Di

2.3.10 Probe type/Probe number: _PRNUM

Function

The data relating to the workpiece probes are stored in GUD field the tool probes are stored in GUD field

probe

The data fields _WP and _TP are configured by the machine manufacturer during start-up. _PRNUM specifies the number of the selected data field within these fields and the probe type.

_WP Workpiece probe, the data relating to

_TP Tool

Parameters

Values of _PRNUM

PRNUM can assume integers of three digits. In this case, the first digit represents the probe type, i.e.

• 0 = Multidirectional probe

• 1 = Monodirectional probe.

The other two digits contain the code for the probe number.

Digit Meaning

- - Probe number (two digits) 0 Multiprobe probe 1 Mono probe

3 2 1

Example of workpiece measurement:

_PRNUM = 102

Further notes

Þ Probe type: Monodirectional

Þ Data field number: 2

probe

The associated field index in _WP = 1, i. e. the data of the _WP[1,0...9] field are considered by the measuring cycle in the calculation of the measuring results.

Description of Parameters 12.97

2.3 Descri

840 D

NCU 571

2.3.11 Empirical value/mean value: _EVNUM

Function

840 D

NCU 572 NCU 573

tion of the most important defining parameters

810 D 840Di

12.98

The empirical values are used to suppress dimensional deviations that are

The empirical and mean values themselves are stored in GUD fields

values

_EVNUM specifies the number of the empirical value memory. The number of the mean value memory is defined at the same time via _EVNUM. The number of empirical and mean values is specified in the GUD field

_EVMVNUM. The unit of measurement is mm in the

metric basic system and inch in the inch basic system, irrespective of the active system of units.

Parameters

Values of _EVNUM The following values can be set:

• = 0 Without empirical value, without mean value

• > 0 Empirical value memory number = mean

If _EVNUM is defined as < 9999, the first 4 digits of

_EVNUM are interpreted as the mean value memory number and the second 4 digits as the empirical value memory number.

Example:

_EVNUM = 90012

memory

value memory number

not subject to a trend.

_EV Empirical value and _MV Mean

Further notes

2-70 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

The corresponding field index in field _EV = 11 and in field _MV = 8.

Þ EV memory: 12

Þ MV memory: 9

12.97 Description of Parameters

2.3 Description of the most important defining parameters

840 D NCU 571

840 D NCU 572 NCU 573

810 D 840Di

2.3.12 Multiple measurement at the same location: _NMSP

Parameters

Parameter _NMSP can be used to determine the number of measurements at the same location.

The actual/setpoint value difference D is determined arithmetically.

SS S

n...number of measurements

...

2.3.13 Weighting factor k for averaging: _K

Function

A detailed description is given in Section 1.7 "Measuring

The weighting factor k can be applied to allow different weighting to be given to an individual measurement.

A new measurement result thus has only a limited effect on the new tool offset as a function of _K.

strategy and compensation value definition".

Description of Parameters 12.97

2.4. Descri

840 D

NCU 571

2.4. Description of output parameters

Function

840 D

NCU 572 NCU 573

tion of output parameters

810 D 840Di

2.4.1 Measuring cycle results in _OVR

In the same way as their defining parameters, the measuring cycle results are Global User Data of the module GUD5.

In this case, the results are not stored as individual data, but in two fields of the

INTEGER (_OVI) types.

Function

The field _OVR[32] contains the following values:

• Setpoints and actual values for abscissa, ordinate

and applicate

• Lower and upper tolerance limits for the three axes

• Setpoint/actual value differences in abscissa,

ordinate and applicate

• Safe area

• Dimensional difference

• Empirical value.

The results are described individually with the relevant

measuring cycles or measurement variants.

REAL (_OVR) and

2-72 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Description of Parameters

05.98

2.4. Description of output parameters

840 D NCU 571

2.4.2 Measuring cycle results in _OVI

Function

The field _OVI[10] contains the following values:

• D or ZO number

• Machining plane

• Measuring cycle number

• Measurement variants

• Weighting factor

• Probe number

• Mean value memory number

• Empirical value memory number

• Tool number

• Alarm number.

840 D NCU 572 NCU 573

810 D 840Di

The results are described individually with the measuring cycles.

Notes

Description of Parameters 12.97

2.4. Descri

840 D

NCU 571

840 D

NCU 572 NCU 573

tion of output parameters

810 D 840Di

2-74 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Measuring Cycle Auxiliary Programs

Measuring Cycle Auxiliary Programs

3.1 Package structure of measuring cycles .......................................................................... 3-76

3.2 Measuring cycle subroutines........................................................................................... 3-77

3.2.1 CYCLE103: Parameter definition for measuring cycles........................................... 3-78

3.2.2 CYCLE116: Calculation of center point and radius of a circle ................................. 3-79

3.3 Measuring cycle user programs ...................................................................................... 3-81

3.3.1 CYCLE198: User program prior to calling measuring cycle..................................... 3-81

3.3.2 CYCLE199: User program at the end of a measuring cycle .................................... 3-82

3.4 Subpackages ..................................................................................................................3-83

Measuring Cycle Auxiliary Programs 12.97

3.1 Package structure of measuring cycles

840 D

NCU 571

840 D

NCU 572

NCU 573

FM-NC 810 D 840Di

3.1 Package structure of measuring cycles

The machine data configuration and the software package version determine which programs can be used. It is also possible to partially define these programs in the global cycle data during start-up.

(Please refer to data supplied by the machine manufacturer and Installation and Start-up Guide.)

Function

The measuring cycle package supplied consists of:

• Data blocks for defining the global measuring cycle

data,

• measuring cycles,

• measuring cycle subroutines and

• easy-to-use functions.

To ensure that the measuring cycles can be executed in the control, the data blocks must have been loaded into directory "Definitions" and the measuring cycles and measuring cycle subroutines must be stored in the part program memory.

Please note that the control always requires a Power ON between loading and execution of the measuring cycles!

3-76 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Measuring Cycle Auxiliary Programs

11.02

3.2 Measuring cycle subroutines

840 D

NCU 571

840 D

NCU 572

NCU 573

FM-NC 810 D 840Di

3.2 Measuring cycle subroutines

Function

These measuring cycle subroutines are called directly by the cycles. With the exception of CYCLE116, these subroutines cannot be executed through a direct call.

Programming

Cycle

CYCLE100

CYCLE101

CYCLE102

CYCLE103

CYCLE104

CYCLE105

CYCLE106

CYCLE107

CYCLE108

CYCLE109

CYCLE110

CYCLE111

CYCLE112

CYCLE113

CYCLE114

CYCLE115

CYCLE116

Function As from

Activate logging X

Deactivate logging X

Measured result display

Parameter setting in interactive mode

Internal subroutine: measuring cycle interface

Internal subroutine: logging X

Output of measuring cycle messages

Output of measuring cycle alarms

Internal subroutine: data transfer X

Internal subroutine: plausibility checks

Internal subroutine: measuring functions

Internal subroutine: logging X

Internal subroutine: load ZO memory, load WCS wear

Internal subroutine: Load WCS wear X

Internal subroutine: Load ZO memory X

Calculation of the center point and radius on a circle

SW 4

As from SW 4.5

In SW 6.2 and higher

CYCLE117

CYCLE118

Internal subroutine: measuring functions

Internal subroutine: logging X

Measuring Cycle Auxiliary Programs 12.97

3.2 Measuring cycle subroutines

840 D

NCU 571

840 D

NCU 572

NCU 573

FM-NC 810 D 840Di

3.2.1 CYCLE103: Parameter definition for measuring cycles

Explanation

This auxiliary cycle controls an input dialog for assigning parameters for the measuring cycles.

It can be either directly selected and started or written in the program before the actual measuring cycle is called.

Several input screen forms are displayed one after the other during the course of this dialog. After entering the values, each display must be concluded with the OK key.

The input values for selecting the measuring cycle and the measurement variant are checked for plausibility. As of measuring cycles SW 4.5, CYCLE103 is no longer supported or developed further. Instead, use the cycle support for measuring cycles to supply the parameter data. Please refer to Chapter 7.2 for a detailed description.

Programming

CYCLE103

Programming example

Calibrate tool probe

CALIBRATION_IN_X_Y

N10 G54 G17 G0 X100 Y80

N15 T9 D1 Z10

N20 CYCLE103

N25 CYCLE976

N50 M30

Position probe at the center of the hole and select ZO

Select tool length compensation, position probe in the hole

The operator can assign the parameters for calibration cycle CYCLE976 in interactive mode

Measuring cycle call for calibr. in X-Y plane

End of program

3-78 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Measuring Cycle Auxiliary Programs

06.00

3.2 Measuring cycle subroutines

840 D

NCU 571

840 D

NCU 572

NCU 573

FM-NC 810 D 840Di

3.2.2 CYCLE116: Calculation of center point and radius of a circle

Explanation

This cycle calculates from three or four points positioned on one plane the circle they inscribe with center point and radius.

To allow this cycle to be used as universally as possible, its data are transferred via a parameter list.

A field of REAL variables of length 13 must be transferred as the parameter.

Calculation of circle data from 3 points

Radius

Programming

CYCLE116 (_DATE, _ALM)

Parameters

Input data

_DATE [0]

_DATE [1]

_DATE [2]

_DATE [3]

_DATE [4]

_DATE [5]

_DATE [6]

_DATE [7]

_DATE [8]

Number of points for calculation (3 or 4)

Abscissa of first point

Ordinate of first point

Abscissa of second point

Ordinate of second point

Abscissa of third point

Ordinate of third point

Abscissa of fourth point

Ordinate of fourth point

Measuring Cycle Auxiliary Programs 12.97

3.2 Measuring cycle subroutines

840 D

NCU 571

Output data

The results of the calculation are stored in the last four elements of the same field:

_DATE [9]

_DATE [10]

_DATE [11]

_DATE [12]

_ALM

This cycle is called as a subroutine by measuring cycle CYCLE979.

Example:

Circle.MPF

DEF INT _ALM DEF REAL _DATE[13]= (3,0,10,-10,0,0,-10,

0,0,0,0,0,0)

CYCLE116(_DATE, _ALM) M0 STOPRE M30

840 D

NCU 572

NCU 573

FM-NC 810 D 840Di

Abscissa of circle center point

Ordinate of circle center point

Circle radius

Status for calculation 0 Calculation in progress 1 Error occurred

Error number ( 61316 or 61317 possible)

; 3 points specified P1:0,10

P2: -10,0 P3: 0,-10

; Result _DATE[9]=0

_DATE[10]=0 _DATE[11]=10 _DATE[12]=0 _ALM=0

3-80 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Measuring Cycle Auxiliary Programs

09.01

3.3 Measuring cycle user programs

840 D

NCU 571

840 D

NCU 572

NCU 573

FM-NC 810 D 840Di

3.3 Measuring cycle user programs

Function

These measuring cycle user programs are called directly by the measuring cycles and can be used to program necessary adaptations before or after a measurement.

3.3.1 CYCLE198: User program prior to calling measuring cycle

Explanation

This cycle is called at the start of each measuring cycle. It can be used to program necessary adaptations prior to starting measurement (e. g. activate probe, position spindle). As delivered, this cycle contains only one CASE instruction for a jump to a marker that corresponds to the measuring cycle called, followed by command M17.

e. g.: _M977: prior to call CYCLE977

M17 End of cycle

The user can program the necessary machine adaptations here.

Measuring Cycle Auxiliary Programs 12.97

3.3 Measuring cycle user programs

09.01

840 D

NCU 571

840 D

NCU 572

NCU 573

FM-NC 810 D 840Di

3.3.2 CYCLE199: User program at the end of a measuring cycle

Explanation

This cycle is called at the end of each measuring cycle. It can be used to program necessary actions following completion of a measurement (e. g. deactivate probe). As delivered, this cycle (just like CYCLE198) contains only one CASE instruction for a jump to a marker that corresponds to the measuring cycle called, followed by command M17.

e. g.: _M971: at the end of the CYCLE971

M17 End of cycle

The user can program the necessary machine adaptations here.

3-82 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

12.97 Measuring Cycle Auxiliary Programs

09.01

3.4 Subpackages

840 D

NCU 571

840 D

NCU 572

NCU 573

3.4 Subpackages

Explanation

In many application cases not all the measuring cycles are used on one machine, instead part packages are used. The following overview shows which part packages are advisable and executable. This allows you to save memory capacity.

Milling measuring cycles

Calibrate tool probe + measure tool

CYCLE971

CYCLE107 CYCLE108 CYCLE109 CYCLE110 CYCLE111 CYCLE198 CYCLE199

Turning measuring cycles

Measure tool + calibrate tool probe

FM-NC 810 D 840Di

Basic package

Calibrate workpiece probe + measure tool + write ZO or TC

CYCLE961 CYCLE976

CYCLE977 CYCLE978 CYCLE979 CYCLE998

Basic package

Calibrate workpiece probe + measure workpiece + write ZO or TC

CYCLE107 CYCLE108 CYCLE109 CYCLE110 CYCLE111 CYCLE112 CYCLE114 CYCLE116 CYCLE198 CYCLE199

Additional package Measuring at milling machine in JOG mode

Semi-automatic calibration of tool probe + measure tool

E_MS_CAL E_MS_CAN E_MS_HOL

Additional package Operator interface

Measurement result display selection

Activation: _CHBIT[10]=1

CYCLE102 CYCLE104

Input dialog

Activation:

CYCLE103 CYCLE104

E_MS_PIN E_MT_CAL E_MT_LEN E_MT_RAD

Call in user NC program

Semi-automatic calibration of tool probe, calculation and setting of reference points

CYC_JM CYC_JMC

Additional package Operator interface

Precondition: SW 4.3 in NCK

Activation: CYCLE100

CYCLE100 CYCLE101 CYCLE105 CYCLE106 CYCLE113 CYCLE118

CYCLE972 CYCLE982 CYCLE107 CYCLE108 CYCLE109 CYCLE110 CYCLE111 CYCLE198 CYCLE199

CYCLE973

CYCLE974 CYCLE994

CYCLE107 CYCLE108 CYCLE109 CYCLE110 CYCLE111 CYCLE114 CYCLE117 CYCLE198 CYCLE199

Measuring Cycle Auxiliary Programs 12.97

3.4 Subpackages

Notes

840 D

NCU 571

840 D

NCU 572

NCU 573

FM-NC 810 D 840Di

3-84 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

06.00 Measuring in JOG

Measuring in JOG

4.1 General preconditions ............................................................................................... 4-86

4.2 Workpiece measurement .......................................................................................... 4-89

4.2.1 Operation and function sequence of workpiece measurement ................................ 4-90

4.2.2 Measuring an edge ................................................................................................... 4-91

4.2.3 Measuring a corner ................................................................................................... 4-92

4.2.4 Measuring a hole....................................................................................................... 4-94

4.2.5 Measuring a spigot.................................................................................................... 4-95

4.2.6 Calibrating the measuring probe ............................................................................... 4-96

4.3 Tool measurement .................................................................................................... 4-99

4.3.1 Operation and function sequence of tool measurement ........................................... 4-99

4.3.2 Tool measurement .................................................................................................... 4-99

4.3.3 Calibrating the tool measuring probe ...................................................................... 4-101

Measuring in JOG 06.00

4.1 General preconditions

09.01

840 D NCU 572 NCU 573

4.1 General preconditions

Certain preconditions must be fulfilled before measuring in JOG can be used. These conditions are described in greater detail in Part 2 Description of Functions (from Chapter 8 onwards).

The following checklist is useful in determining whether all such preconditions are fulfilled:

Machine

• All machine axes are designed in accordance

with DIN 66217.

• A touch-trigger probe (3D) is provided for acquiring

workpiece dimensions, and a touch-trigger tool probe for acquiring tool dimensions. (see also Section 1.4 Suitable probe types)

• The reference points have been approached.

810D 840Di

Control

• 840D as of NCU 572 with SW 5.3 and higher,

810D SW 3.3 and higher MMC103 SW 5.3 and higher

Machine data for running machine cycles:

• All machine data listed in Section 10.1 meet the

minimum requirements for running measuring cycles.

Machine data for measuring in JOG

• Machine data

– MD 11602: ASUB_START_MASK – MD 11604: ASUB_START_PRIO_LEVEL – MD 20110: RESET_MODE_MASK – MD 20112: START_MODE_MASK are set as specified in the detailed function description (see Subsection 10.3.1).

Notice: Interrupt number 8 is used to start the

ASUBs for measuring in JOG and must therefore not be used by the user.

4-86 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

06.00 Measuring in JOG

Availability of measuring cycles

• The data blocks:

GUD5.DEF and

GUD6.DEF in directory DEFINE on diskette 1 have been loaded in the control (directory "Definitions" in the file system) and

• the measuring cycles in directory CYCLES on

diskette 1 have been loaded into the standard cycle directory of the control and then a power-on executed.

Availability of JOG measuring files

• All files in directory JOG_MESS on diskette 2 have

been loaded into the control via "Data in" and a power-on then executed.

Adaptation of data block GUD7.DEF: Data block GUD7.DEF has been adapted to the requirements of measuring in JOG as specified in the detailed function description (see Subsection 10.3.1).

4.1 General preconditions

Function

MEASURING IN JOG comprises the following functions:

• Semi-automatic calculation of tool lengths and storage in tool offset

memory.

• Semi-automatic calculation and setting of reference points and storage

in zero offset memory.

The functions are operated with softkeys and input displays. The measuring operation is canceled with RESET.

Notice

Make sure that you select the correct channel, as the function MEASURING IN JOG operates channel dependently. Selecting the wrong channel when the measuring operation is active could destroy the measuring probe.

The measuring function is selected via the softkey bar in the JOG basic display.

Measuring in JOG 06.00

4.1 General preconditions

840 D NCU 572 NCU 573

810D 840Di

Measure workpiece

For calculating and setting reference points.

Measure tool

For measuring milling and drilling tools.

4-88 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

06.00 Measuring in JOG

09.01

4.2 Workpiece measurement

840 D NCU 572 NCU 573

810D 840Di

4.2 Workpiece measurement

Function

With this function you can set reference points on the workpiece using a workpiece probe on the machine.

You call a measuring cycle to set up a workpiece that is clamped on the table. This measuring cycle automatically generates the measurement paths and intermediate positions as a function of the specified setpoints. While the measuring cycle is running, the basic offset defined via GUD6 or a settable ZO, as well as a further working plane G17...G19 set in GUD6 data are effective. The GUD6 data also specifies which data field is assigned to the measuring probe in the spindle and the measuring probe type (multiprobe or monoprobe) (the parameters for switching behavior found by calibrating the measuring probe are also stored in this data field). All the measuring points required for the measurement task are approached. Prepositioning can either be performed manually or in a program.

When measurement is complete, the result (corner, center point of hole/spigot, edge) is automatically calculated in the measuring cycle according to the type of measurement, and the reference point is set with reference to the basic frame or a settable zero offset according to the selection made by correcting the zero offset memory in question. If "Off" is selected, no correction is made.

Precondition

• The workpiece probe is located in the spindle and

has been calibrated.

Measuring in JOG 06.00

4.2 Workpiece measurement

09.01

840 D NCU 572 NCU 573

810D 840Di

4.2.1 Operation and function sequence of workpiece measurement

Procedure

1. The workpiece is clamped, the probe is positioned in the spindle and calibrated.

2. When you press softkey "Measure workpiece", the following softkey bar is displayed for selection:

Edge >

Corner >

Hole >

Spigot >

Calibrate probe

<< back

• Select zero offset to which the defined setpoint position

refers and for which the offset is to apply: – Basic frame – Settable zero offset G54...

• Enter setpoints if necessary (e.g. approx. diameter of

hole/spigot).

• Select the setpoint position in the measuring axis (for

edge), the center point (for hole/spigot) or the corner point.

• Select axis and axis direction for edge/corner.

4. On "NC Start", the measuring operation is performed with a measuring feedrate set in the measuring cycle data (GUD6). The measuring probe is triggered. When a corner or edge is measured, the probe is automatically retracted in rapid traverse to its starting position for the measuring point in question. When a hole or spigot is measured, all four points are automatically scanned one after the other. The translation offset and also an offset for the rotation around the infeed axis in relation to the corner defined for the selected zero offset is determined on the basis of the measuring results and the specified setpoint position. When the basic frame is selected, the last channel-specific basic frame is always taken if more than one is available.

4-90 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

06.00 Measuring in JOG

11.02

4.2 Workpiece measurement

840 D NCU 572 NCU 573

4.2.2 Measuring an edge

Function

If "Measure edge" is selected, a reference point can be set in any axis of the working plane (G17...G19) defined in a GUD6 data.

810D 840Di

Sequence of operations

Precondition

The measuring probe is located in the spindle and has been calibrated.

Approach the workpiece

Position the probe in the required axis direction in front of the workpiece, e.g. in the +X direction.

Select the function with softkey

Measure workpiece

Enter details in input form

• Select the zero offset to which the specified setpoint

position refers and for which the offset is to apply: – Basic frame – or zero offset taken from the list of zero offsets

• Direction: Set the sampling direction of the selected axis

for which the reference point has been set, e.g. +X.

• Enter set position of the reference point (edge).

Set the feedrate override switch to the same value as for calibration!

Edge

...

Measuring in JOG 06.00

4.2 Workpiece measurement

11.02

840 D NCU 572 NCU 573

On "NC Start", the measuring operation is automatically performed with a measuring feedrate set via GUD data.

• The measuring probe is triggered.

• Automatic retraction to starting position in rapid traverse.

• The translation offset for the selected zero offset is

determined on the basis of the measuring results and the specified setpoint position. On selection of the basic frame the offset is always implemented in the last channel-specific basic frame, if there are more than one. The offset is implemented in the coarse offset and any fine offset there may be is reset.

4.2.3 Measuring a corner

810D 840Di

Function

With the selection "Corner", the corner of a workpiece can be measured as the reference point. The probe is positioned at a selected corner of the workpiece.

Sequence of operations

Precondition

The measuring probe is located in the spindle and has been calibrated.

Approach the workpiece

Position the probe at a selected corner of the workpiece.

4-92 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

06.00 Measuring in JOG

11.02

4.2 Workpiece measurement

840 D NCU 572 NCU 573

810D 840Di

Select the function with softkey

Measure workpiece

Corner

Enter details in input form

• Select the zero offset to which the specified

setpoint position for the corner refers and for which the offset is to apply: – Basic frame – or zero offset taken from the list of zero offsets

• Position: Set the corner to be used as the reference

point.

• Enter set position of the reference point (corner).

Approach sampling point

Position the probe at the first sampling point P1 of the

workpiece edge.

Set the feedrate override switch to the same value as for calibration!

On "NC Start", the measuring operation is automatically performed with a measuring feedrate set via GUD data.

• The measuring probe is triggered.

• Automatic retraction to starting position in rapid

traverse.

Store the position values of sampling point P1 by

pressing softkey "Save P1". Repeat the procedure "approach sampling points" for sampling points P2...P4 in

the same way.

Calculate corner

Press softkey "Calculate corner" to calculate the translation offset and the rotational offset around the infeed axis for the selected zero offset. On selection of the basic frame the offset is always implemented in the last channel-specific basic frame, if there are more than one. The offset is implemented in the coarse offset and any fine offset there may be is reset.

• The order in which sampling points P1...P4 are

approached must be maintained. On a rectangular workpiece, three sampling points are sufficient for the calculation.

Measuring in JOG 06.00

4.2 Workpiece measurement

09.01

840 D NCU 572 NCU 573

4.2.4 Measuring a hole

Function

With "Hole", you can set the center of a hole as the reference point. The probe is approximately positioned at the center of the hole and measuring depth.

810D 840Di

Sequence of operations

Precondition

The measuring probe is located in the spindle and has been calibrated.

Approach the workpiece

Position the probe approximately in the center of the hole.

Select the function with softkey

Measure workpiece

Enter details in input form

• Select the zero offset to which the specified setpoint

position for the center of the hole refers and for which the offset is to apply: – Basic frame – or zero offset taken from the list of zero offsets

• Diameter: Enter approximate diameter of the hole.

If no diameter is entered, sampling is started from the starting point at measurement feedrate.

• Enter set position of the hole center.

Hole

4-94 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

06.00 Measuring in JOG

11.02

4.2 Workpiece measurement

840 D NCU 572 NCU 573

Set the feedrate override switch to the same value as for calibration!

Measurement is performed automatically as soon as you press "NC Start". One after the other, the probe samples four points on the inner surface of the hole.

Once the measurement is complete, the translation offset is determined for the selected zero offset. On selection of the basic frame the offset is always implemented in the last channel-specific basic frame, if there are more than one. The offset is implemented in the coarse offset and any fine offset there may be is reset.

810D 840Di

4.2.5 Measuring a spigot

Function

With "Spigot", you can set the center of a spigot (shaft) as the reference point. The probe is approximately positioned above the center of the spigot.

Sequence of operations

Precondition

The measuring probe is located in the spindle and has been calibrated.

Approach the workpiece

Position the probe approximately above the center of the spigot.

Select the function with softkey

Measure workpiece

Spigot

Measuring in JOG 06.00

4.2 Workpiece measurement

11.02

840 D NCU 572 NCU 573

Enter details in input form

• Select the zero offset to which the specified setpoint

position for the center of the spigot refers and for which the offset is to apply: – Basic frame – or zero offset taken from the list of zero offsets

• Diameter: Specify the approximate spigot diameter

(check diameter>0, safety clearance, include probe offsets).

• Specify set position of the center of the spigot.

• Enter measurement infeed.

Set the feedrate override switch to the same value as for calibration!

Measurement is performed automatically as soon as you press "NC Start". One after the other, the probe samples four points on the outside of the spigot.

810D 840Di

4.2.6 Calibrating the measuring probe

Function

With milling machines and machining centers, the probe is usually loaded into the spindle from a tool magazine. This may result in errors when further measurements are taken on account of probe clamping tolerances in the spindle. In addition, the trigger point must be precisely determined in relation to the spindle center. This is performed by the calibration cycle with which it is possible to calibrate the measuring probe either in any hole or on a surface. The type of calibration is selected with softkeys "Length" and "Radius".

4-96 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

06.00 Measuring in JOG

4.2 Workpiece measurement

840 D NCU 572 NCU 573

810D 840Di

Calibrating the workpiece probe in any hole (radius)

With this cycle, the probe can be calibrated in any hole of a reference part, e.g. on a workpiece or in an adjustment ring. The resulting trigger points are automatically loaded in the corresponding data storage area of the GUD6 block.

Sequence of operations

Precondition

The measuring probe is located in the spindle. The precise radius of the probe ball must be entered in the tool offset block. An adjustment ring with a known radius, for example, is used for calibration.

Approaching the reference part

The probe is approximately positioned at the center of and at the calibration depth of the hole.

Select the function with softkey

Measure workpiece

Enter details in input form

Enter diameter ∅ of the reference part (here:

adjustment ring).

Calibration is performed automatically as soon as you press "NC Start". First, the precise position of the center of the adjustment ring is calculated. Then, four trigger points inside the adjustment ring are sampled one after the other.

Calibrate probe >

Radius

Measuring in JOG 06.00

4.2 Workpiece measurement

09.01

840 D NCU 572 NCU 573

810D 840Di

Calibrating a workpiece probe on any surface

With this measuring cycle you can calibrate the probe on a random surface, e.g. on the workpiece, to determine the length.

Sequence of operations

Precondition

The measuring probe is located in the spindle. The precise radius of the probe ball must be entered in the tool offset block.

Approach the workpiece

The probe must be positioned opposite the calibration surface of the workpiece.

Select the function with softkey

Measure workpiece

Enter details in input form

Known reference Z the active zero offset set by GUD6 during measurement.

Calibration is performed automatically as soon as you press "NC Start". The measuring probe is triggered.

The calculated length of the probe is written to the tool offset data block.

Calibrate probe >

Length

of the machine table relative to

4-98 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

06.00 Measuring in JOG

4.3 Tool measurement

840 D NCU 572 NCU 573

4.3 Tool measurement

Function

Tools can be measured in the machine with this function. The tool lengths are automatically written to a tool offset memory and are therefore immediately available for workpiece machining directly after measurement.

General preconditions

• The reference points have been approached.

• The tool measuring probe is swung in or

inserted.

• The tool probe has been calibrated.

• The tool to be measured is located in the spindle.

• The tool geometry data (length and radius) have

been entered in the tool offset data block as

approximate values.

• The tool must be prepositioned in such a way that

collision-free approach to the tool measuring probe

is possible.

810D 840Di

4.3.1 Operation and function sequence of tool measurement

Procedure

1. The tool is replaced or inserted manually.

2. When you press softkey "Measure tool", the following

selection appears on the softkey bar:

Length >

3. Enter the measurement type and enter the

values in the input form.

4. Position the tool near the tool measuring probe with

the JOG direction keys.

5. Start the measuring procedure with "NC-Start".

Diameter >

Calibrate probe

<< back

Measuring in JOG 06.00

4.3 Tool measurement

840 D NCU 572 NCU 573

4.3.2 Tool measurement

Function

In tool measurement with a tool measuring probe (table probe system) either the radius or the length of a tool can be measured.

Sequence of operations

Precondition

• The tool probe is calibrated.

• The tool geometry data (length and radius/diameter)

have been entered in the tool offset data block of the tool list as approximate values.

• The tool to be measured is located in the spindle.

• The data of the tool measuring probe (active

width/diameter for length/radius measurement, distance between tool lower edge and tool probe upper edge, permissible axis directions) must be entered in the relevant GUD7 data.

810D 840Di

Approaching the tool measurement probe

Position the tool near the measuring surface of the tool probe. Select whether the radius/diameter or the length of the tool is to be measured.

Select the function with softkey

Measure tool

Radius/diameter Length

Diameter

Length

4-100 SINUMERIK 840D/840Di/810D User's Guide Measuring Cycles (BNM) – 11.02 Edition

siemens 840D Users Guide

Specifications and Main Features

Frequently Asked Questions

User Manual