Renishaw NC1 Operating instructions

H-2000-6199-02-A
NC1 non-contact
tool setting system
Programming Guide
(Siemens 810D / 840D and FMNC)
=>?@D
R25=y
12
R11=h
R25=y
R26=z

© 2001 Renishaw. All rights reserved.
Renishaw® is a registered trademark of Renishaw plc.
This document may not be copied or reproduced in whole or in
part, or transferred to any other media or language, by any means
without the written prior permission of Renishaw.
The publication of material within this document does not imply
freedom from the patent rights of Renishaw plc.
Disclaimer
Considerable effort has been made to ensure that the contents of
this document are free from inaccuracies and omissions.
However, Renishaw makes no warranties with respect to the
contents of this document and specifically disclaims any implied
warranties. Renishaw reserves the right to make changes to this
document and to the product described herein without obligation
to notify any person of such changes.
Trademarks
All brand names and product names used in this document are
trade names, service marks, trademarks, or registered trademarks
of their respective owners.
Renishaw part no: H-2000-6199-02-A
Issued – February 2001

1
NC1 non-contact
tool setting system
Programming Guide
(Siemens 810D / 840D and FMNC controls)
=>?@D
Renishaw plc
New Mills, Wotton-under-Edge,
Gloucestershire, GL12 8JR, UK
Tel: [phone] [07000 RENISHAW]
Fax: [phone]
email: [e-mail]
www.renishaw.com

2
Caution – Laser safety
The laser used in the Renishaw NC1 non-contact tool
setting system emits visible red light at a wavelength of
670nm and has a maximum power output of less than
1mW. It is a Class 2 product as defined by European and
American laser safety standards (EN60825-1:1994 and US Code of
Federal Regulations 21CFR1040).
When using the NC1 system:
n Do not stare directly into the laser beam. The beam may be
viewed safely from the side.
n Ensure that the laser beam is not reflected into the eyes of
another person via a mirror or other reflective surface.
n Do not expose skin to the laser beam for longer than is absolutely
essential.
n When the system is not being used, cover the laser beam
aperture with the sliding cover.
Caution – Software safety
The software you have purchased is used to control the
movements of a machine tool. It has been designed to
cause the machine to operate in a specified manner under
operator control, and has been configured for a particular
combination of machine tool hardware and controller.
Renishaw has no control over the exact program configuration of the
controller with which the software is to be used, nor of the
!
Cautions

3
mechanical layout of the machine. Therefore, it is the responsibility of
the person putting the software into operation to:
n ensure that all machine safety guards are in position and are
correctly working before commencement of operation;
n ensure that any manual overrides are disabled before
commencement of operation;
n verify that the program steps invoked by this software are
compatible with the controller for which they are intended;
n ensure that any moves which the machine will be instructed to
make under program control would not cause the machine to
inflict damage upon itself or upon any person in the vicinity;
n be thoroughly familiar with the machine tool and its controller and
know the location of all emergency stop switches.
Related publications
When using the Beam alignment cycle (subroutine L9860) you will
also need to refer to the following Renishaw publication. This contains
instructions on how to physically align the beam at the NC1
transmitter unit.
NC1 Installation Guide and Parts List
(Renishaw Part No. H-2000-5048)
Cautions

4
Contents
Renishaw NC1 tool setting system ..................................................... 6
Features of the NC1 system software ................................................ 7
Measuring subroutine features .................................................... 7
Calibration subroutine features .................................................... 7
Service subroutine features ......................................................... 8
Software memory requirements ......................................................... 9
Machine tool controllers supported .................................................... 9
Tool-offset types supported .............................................................. 10
Positive tool-offset applications .................................................. 10
Negative tool-offset applications ................................................ 10
Relative to a master tool with zero (0) tool-offset value. ........... 11
Measurement values used in this guide ........................................... 11
Installing the software ....................................................................... 12
Subroutine parameters ..................................................................... 12
Parameter store for calibration data ........................................... 12
Setting-data subroutine L9760 ................................................... 13
Common parameters ................................................................. 19
Customising the subroutines ............................................................ 20
Editing the measure move subroutine L9762 ............................ 20
Orientation of the NC1 system ......................................................... 21
Beam-find and measuring moves ..................................................... 22
Scatter tolerance checking ............................................................... 23
Beam alignment (subroutine L9860) ................................................ 24
Calibrating the NC1 (subroutine L9861) ........................................... 32
Tool length setting (subroutine L9862) ............................................. 38
Contents

5
Tool radius/diameter setting (subroutine L9862) .............................. 43
Tool length and radius setting (subroutine L9862) ........................... 49
Cutting edge checking (subroutine L9862) ...................................... 55
Broken tool detection – plunge checking (subroutine L9863) .......... 60
Broken tool detection – radial checking (subroutine L9864) ............ 65
Cutter radius and linear profile checking (subroutine L9865) .......... 70
Temperature compensation tracking (subroutine L9861) ................. 79
Error messages and alarms ............................................................. 85
Contents

6
Renishaw NC1 system
Renishaw NC1 tool setting system
This guide describes how to use the Renishaw NC1 non-contact tool
setting system software.
The Renishaw NC1 is a laser-based non-contact tool setting system
that provides high-speed/high-precision measurement of cutting tools
on a machining centre under normal operating conditions.
As a tool is moved through the laser beam, the system detects when
the beam is broken. Output signals sent to the controller allow the
presence of a tool and the position of the tip, a tooth, or a cutting
edge to be established.
The NC1 allows the following parameters to be established:
n Length and diameter of the cutting tool. Tools as small as 0.2 mm
(0.008 in) diameter can be accurately measured.
n Detection of a broken tool.
n Detection of a broken tip or cutting edge, or excessive runout of a
tool.
n Compensation for thermal changes in the machine tool.

7
Features of the NC1 system software
NC1 system software provides the following measuring and
calibration features:
Measuring subroutine features
Four measuring subroutines provide the following features:
n L9862 – used for measuring the length and diameter of the
cutting tool and for cutting edge checking.
n L9863 – used for broken tool detection by plunge measurement.
This is intended for use on vertical machining centres.
n L9864 – used for broken tool detection by radial measurement.
This is intended for use on horizontal machining centres.
n L9865 – used for checking the radii and linear profile of the cutter.
Calibration subroutine features
Two calibration subroutines provide the following features:
n L9860 – used for aligning the laser beam, setting the provisional
positions of the beam in the spindle and radial-measuring axes,
and setting the measuring position along the beam.
n L9861 – used for calibrating the positions of the laser beam in the
spindle and radial-measuring axes, and for temperature
compensation of the spindle and radial-measuring axes.
Software features

8
Service subroutine features
The measuring and calibration subroutines are supported by the
service subroutines listed below.
n L9760 – used for the settings data.
n L9761 – used for startup functions.
n L9762 – used for the measuring routine.
n L9763 – used for the G31 routine.
n L9764 – used for the G0/G1 routine.
n L9765 – used for the G2/G3 routine.
n L9766 – used for the search routine.
n L9769 – used for error messages.
n L9800 – clears global ‘R’ parameters used for subroutine input
data.
NOTE: L9800 Clear global ‘R’ parameters.
The subroutine L9800 is called at the end of every measuring and
calibration subroutine (9800-series) to reset the global ‘R’
parameters, used as inputs, to a default value.
If global ‘R’ parameters R00 to R26 are used for other
programming purposes outside of this tool setting package, it is
recommended that L9800 is called prior to setting them for the
next tool setting routine. All examples in this programming guide
show this being done.
Software features

9
Software memory requirements
NC1 system software requires approximately 28.0Kb (70 metres) of
part-program memory.
If your controller is short of memory, there is no need to load any of
the subroutines listed below if you do not intend using them:
n L9862 (tool setting routine) 4.0 Kb (10 metres) of memory.
n L9863 (broken tool – plunge check) 1.2 Kb (3 metres) of
memory.
n L9864 (broken tool – radial check) 1 Kb (2.5 metres) of memory.
n L9865 (checking cutter radii and linear profiles) 4.0 Kb
(10 metres) of memory.
You may also remove the following subroutine after you have finished
running the Beam alignment cycle:
n L9860 (laser beam alignment routine) 1.5 Kb (3.8 metres) of
memory
Machine tool controllers supported
NC1 system software is suitable for use on the following machine tool
controllers:
n Siemens 810D
n Siemens 840D
n Siemens FMNC
Software memory requirements

10
Tool-offset types supported
Positive tool-offset applications
The NC1 software is ideally suited to setting tools using positive tool-
offset values that represent the physical length of the tool.
Throughout this programming guide, descriptions refer to positive
tool-offset applications.
The software can also be used in applications where negative tool-
offset values are used or where all tool-offset values are entered as ±
values relative to a master tool. These applications are described
below.
Negative tool-offset applications
The offset value entered is the distance the tool tip must be moved
from the home position to reach the zero (0) position of the part
program (air-gap method), rather than the physical length of the tool.
Example
Home position, to the zero (0) position of the part
program = –1000 mm.
A master calibration tool of 150 mm is used (offset register
value = –850 mm).
The longest tool for the machine is 200 mm long.
The shortest tool for the machine is 50 mm long.
Parameters RENC[10] and RENC[11] must be set in the Setting-data
subroutine (L9760). Set them as follows:
Tool-offset types supported

11
RENC[10] = –800.0 Maximum length tool
RENC[11]= –950.0 Minimum length tool
Relative to a master tool with zero (0) tool-
offset value.
The master tool-offset register is set to zero (0) and all other tool-
offset registers are set as ± values relative to the master tool.
Example
Home position, to the zero (0) position of the part
program = –1000 mm (but this is not important)
A master calibration tool of 150 mm is used (offset register
value = 0).
The longest tool for the machine is 200 mm long.
The shortest tool for the machine is 50 mm long.
Parameters RENC[10] and RENC[11] must be set in the Setting-data
subroutine (L9760). Set them as follows:
RENC[10] = 50.0 Maximum length tool
RENC[11] = -100.0 Minimum length tool
Measurement values used in this guide
Throughout this guide, metric units of measurement, i.e. millimetres,
are used in the examples. The equivalent imperial measurements, i.e.
inches, are shown in brackets.
Tool-offset types supported

12
Installing the software
Before installing the NC1 software, read the guidelines contained in
the Readme file on the software floppy disk.
Subroutine parameters
The following parameters are used by the NC1 system software:
n ‘RENT’ global parameters – used for the calibration data and
settings data.
n Global parameters RENC[0] to RENC[49] – used for the settings
data.
n Local parameters RENL[1] to RENL[32] – used for locally defined
data.
n Global parameters R01 to R26 – used for subroutine inputs.
Parameter store for calibration data
The following parameters are set automatically during the calibration
cycles.
RENT[20] Z-axis position of the beam, when measured from the
positive side of the beam.
RENT[21] (Reserved)
RENT[22] X or Y-axis position of the beam, when measured from
the negative side of the beam.
RENT[23] X or Y-axis position of the beam, when measured from
the positive side of the beam.
Installing the software

13
RENT[24] Position along the beam at which measurements are
made.
RENT[26] Spindle (length-measuring) axis temperature
compensation zero offset.
RENT[27] Radial-measuring axis temperature compensation zero
offset.
Setting-data subroutine L9760
Read the following parameter descriptions then edit subroutine L9760
as described.
RENC[5] False trigger retries.
If probe status checking is deactivated (see RENT[5]
parameter), the software defaults to one (1) retry.
Default: 1
RENC[6] Safe return position (in ‘machine’ co-ordinates).
RENC[7] The unit used for setting data in subroutine L9760.
1 = mm, 0.04 = inch
Default: 1 (mm)
RENC[9] Setting for tool offset type, either radius or diameter.
1 = Radius, 2 = Diameter
Default: 1
RENC[10] Maximum length of the tool. This defines the rapid
approach height of the spindle nose above the laser
beam.
Parameter store for calibration data

14
RENC[11] Minimum length of the tool. This defines the lowest
measuring height of the spindle nose above the laser
beam.
RENC[12] Maximum diameter of the tool. This value is dependent
on the machine tool.
RENC[13] Radial-measuring axis options.
1 = measure from positive side of the beam,
–1 = measure from negative side of the beam,
2 = measure from both sides of the beam.
Default: 2
RENC[14] Radial calibration options.
1 = measure from positive side of the beam,
–1 = measure from negative side of the beam,
2 = measure from both sides of the beam.
Default: 2.
RENC[15] Hardware signal pulse time.
The time that the trigger signal is held on. This is
hardware-dependent. The value is specified when the
NC1 system is ordered.
Check the status LED sequence on power up (for
details, see “NC1 Installation Guide and Parts List ”).
RENC[17] Default overtravel distance and radial clearance.
Overtravel is the distance through the beam that the
tool is permitted to move before a BEAM NOT CUT
alarm is initiated.
Radial clearance is the distance between the tool and
Setting-data subroutine

15
the beam when moving down the side of the beam.
Default: 5 mm (0.197 in)
RENC[18] Default measurement resolution (feedrate-per-rev.).
Typically 0.001 mm (0.0001 in) feed per revolution.
The larger the value, the less accurate measurements
will be.
Default: 0.002 mm (0.0001 in)
RENC[19] Default spindle speed.
Measurement cycles are optimised for a spindle speed
of 3150 rev/min.
Some tools, e.g. those that are unbalanced or large,
must be run at speeds less than 3150 rev/min. This is
the responsibility of the user. Use the R19= input to set
speed.
Measurement cycle times increase with slower speeds.
The minimum speed is 800 rev/min.
Default value: 3150 rev/min
RENC[21] Beam axis.
n If the laser beam is parallel to the X-axis, select 1.
n If the laser beam is parallel to the Y-axis, select 2.
n If the laser beam is parallel to the Z-axis, select 3.
RENC[22] Axis used for radial measurement.
n If the X-axis is to be used for radial measurement,
select 1.
n If the Y-axis is to be used for radial measurement,
select 2.
Setting-data subroutine

16
n If the Z-axis is to be used for radial measurement,
select 3.
Default: 2
RENC[23] Axis used for length measurement, i.e. the spindle axis.
n If the X-axis is to be used for length measurement,
select 1.
n If the Y-axis is to be used for length measurement,
select 2.
n If the Z-axis is to be used for length measurement,
select 3.
Default: 3
NOTE: RENC[23] must always define the spindle axis
and the direction in which the tool offset is applied. If
the spindle is in the negative direction, the value
entered must also be negative (–1 = –X axis, –2 = –Y
axis, –3 = –Z axis).
RENC[24] Scatter tolerance value.
For a description of this feature, see the figure in
“Scatter tolerance checking” on page 23.
Default: 0.010 mm (0.0004 in)
RENC[25] Tolerance value for tool runout or cutting edge.
Default: 0.025 mm (0.001 in)
RENC[26] Sample size for scatter.
The number of measurement samples to be taken.
The number of retry attempts is twice this value.
Setting-data subroutine

17
For a description of this feature, see the figure in
“Scatter tolerance checking” on page 23.
Default: 3
RENC[27] Rapid traverse feedrate.
Default: 5000 mm/min
RENC[28] Select language.
1 = English, 2 = German, 3 = French, 4 = Italian
RENT[5] Number of the digital input for monitoring the probe
status signal. This can be used only if the machine tool
builder (MTB) has provided the input.
From Siemens 840D version 4 software or 810D
version 2 software, a Probe Status flag is available.
This is used as the default.
Default: 0 (Siemens Probe Status flag)
RENT[7] Measuring input used on I/O interface connector X121.
RENT[7] = 1 Configured for N/O input on MEPUS 0
RENT[7] = -1 Configured for N/C input on MEPUS 0
RENT[7] = 2 Configured for N/O input on MEPUS 1
RENT[7] = -2 Configured for N/C input on MEPUS 1
RENT[9] Tool management system in use.
RENT[9] = n, where ‘n’ is the location number, usually
1, in the tool buffer. This is decided by the MTB during
machine commissioning.
Default: 0 (i.e. disabled)
Setting-data subroutine

18
RENT[28] M code number to disable the latch mode. If the latch
mode feature is not to be used, enter 9 to select M9
coolant off (or similar).
RENT[29] M code number to enable the latch mode. If the latch
mode feature is not to be used, enter 9 to select M9
coolant off (or similar).
Editing subroutine L9760
Before running the cycles, edit the settings data between block
numbers LN1 and LN2 .
First, enter the metric/inch units factor (1. or .04) in parameter
RENC[7]. Next, enter data in the other parameters using the same
units.
Sample of subroutine L9760
LN1:
RENC[5]=1; RETRIES
RENC[6]=-1.; SAFE RETURN POSITION
RENC[7]=1; UNITS FOR DATA 1MM .04INCH
RENC[9]=1; OFFSET-RADIUS 1/DIAMETER 2
RENC[10]=200.; MAX TOOL LENGTH (8.0 in)
RENC[11]=70.; MIN TOOL LENGTH (2.75 in)
RENC[12]=80.; MAX CUTTER DIAMETER (3.15 in)
RENC[13]=2; TL SET RADIUS MEAS DIR
RENC[14]=2; CALIB RADIUS MEAS DIR
RENC[15]=.10; NC1-DELAY IN SECS
RENC[17]=5.; DEFAULT OVERTRAVEL (0.197 in)
RENC[18]=.002; MEASURE RESOLUTION (0.0001 in)
Setting-data subroutine