heidenhain TNC 430 User Manual
Touch Probe Cycles
TNC 426
TNC 430
NC Software
280 472-xx
280 473-xx
280 474-xx
280 475-xx
280 476-xx
280 477-xx
User’s Manual
English (en)
6/2003
TNC Model, Software and Features
This manual describes functions and features provided by TNCs as of
the following NC software numbers.
TNC model NC software number
TNC 426, TNC 430 280 472-10
TNC 426, TNC 430 280 474-13
TNC 426, TNC 430 280 476-04
The suffixes E and F indicate the export versions of the TNC The
export versions of the TNC have the following limitations:
n Linear movement is possible in no more than 4 axes simultaneously.
The machine tool builder adapts the useable features of the TNC to his
machine by setting machine parameters. Some of the functions
described in this manual may not be among the features provided by
your machine tool.
TNC functions that may not be available on your machine include:
n Digitizing option
n Tool Measurement with the TT
Please contact your machine tool builder to become familiar with the
features of your machine.
Many machine manufacturers, as well as HEIDENHAIN, offer
programming courses for the TNCs. We recommend these courses as
an effective way of improving your programming skill and sharing
information and ideas with other TNC users.
User’s Manual:
All TNC functions that have no connection with touch
probes are described in the User's Manual of the
respective control. Please contact HEIDENHAIN if you
need a copy of this User’s Manual.
Location of use
The TNC complies with the limits for a Class A device in accordance
with the specifications in EN 55022, and is intended for use primarily
in industrially-zoned areas.
HEIDENHAIN TNC 426, TNC 430 I
New features of the NC software 280 476-xx
n Management of an arbitrary number of calibration data with the TS
triggering touch probe (see “Managing more than one block of
calibrating data (as of NC software 280 476-xx)” on page 15)
n Cycles for automatic tool measurement with the TT 130 according
to ISO (see “Overview” on page 112)
n Cycle for measuring the thermal behavior of a machine (see
“MEASURE AXIS SHIFT (touch probe cycle 440, ISO: G440,
available as of NC software 280 476-xx)” on page 106)
Changed features of the NC software 280 476-xx
n All cycles for the automatic datum setting can now also be run
during an active basic rotation (see “Characteristics common to all
touch probe cycles for datum setting” on page 43).
n Cycle 431 find the angular values needed for tilting the working
plane with a spatial angle (see “MEASURE PLANE (touch probe
cycle 431, ISO: G431)” on page 97).
II
Contents
Introduction
Touch Probe Cycles in the Manual and
Electronic Handwheel Modes
Touch Probe Cycles for Automatic
Workpiece Inspection
Touch Probe Cycles for Automatic Tool
Measurement
1
2
3
4
Digitizing
5
HEIDENHAIN TNC 426, TNC 430 III
1 Introduction ..... 1
1.1 General Information on Touch Probe Cycles ..... 2
Function ..... 2
Touch Probe Cycles in the Manual and Electronic Handwheel Modes ..... 3
Touch probe cycles for automatic operation ..... 3
1.2 Before You Start Working with Touch Probe Cycles! ..... 5
Maximum traverse to touch point: MP6130 ..... 5
Safety clearance to touch point: MP6140 ..... 5
Orient the infrared touch probe to the programmed probe direction: MP6165 (as of 280 476-10) ..... 5
Multiple measurement: MP6170 ..... 5
Confidence interval for multiple measurement: MP6171 ..... 5
Touch trigger probe, probing feed rate: MP6120 ..... 6
Touch trigger probe, rapid traverse for pre-positioning: MP6150 ..... 6
Measuring touch probe, probing feed rate: MP6360 ..... 6
Measuring touch probe, rapid traverse for pre-positioning: MP6361 ..... 6
Running touch probe cycles ..... 7
HEIDENHAIN TNC 426, TNC 430 V
2 Touch Probe Cycles in the Manual and Electronic Handwheel Modes ..... 9
2.1 Introduction ..... 10
Overview ..... 10
Selecting probe cycles ..... 10
Recording Measured Values from the Probe Cycles ..... 11
Writing the measured values from probe cycles in datum tables ..... 12
2.2 Calibrating a Touch Trigger Probe ..... 13
Introduction ..... 13
Calibrating the effective length ..... 13
Calibrating the effective radius and compensating center misalignment ..... 14
Displaying calibration values ..... 15
Managing more than one block of calibrating data (as of NC software 280 476-xx) ..... 15
2.3 Calibrating a Measuring Touch Probe ..... 16
Introduction ..... 16
Course of actions ..... 16
Displaying calibration values ..... 17
2.4 Compensating Workpiece Misalignment ..... 18
Introduction ..... 18
Measuring the basic rotation ..... 18
Displaying a basic rotation ..... 19
Cancel a basic rotation ..... 19
2.5 Setting the Datum with a 3-D Touch Probe ..... 20
Introduction ..... 20
To set the datum in any axis (see figure at right) ..... 20
Corner as datum—using points that were already probed for a basic rotation (see figure at right) ..... 21
Corner as datum—without using points that were already probed for a basic rotation ..... 21
Circle center as datum ..... 22
Setting datum points using holes/cylindrical studs ..... 23
2.6 Measuring Workpieces with a 3-D Touch Probe ..... 24
Introduction ..... 24
To find the coordinate of a position on an aligned workpiece: ..... 24
Finding the coordinates of a corner in the working plane ..... 24
Measuring workpiece dimensions ..... 25
To find the angle between the angle reference axis and a side of the workpiece ..... 26
VI
3 Touch Probe Cycles for Automatic Workpiece Inspection ..... 27
3.1 Measuring Workpiece Misalignment ..... 28
Overview ..... 28
Characteristics common to all touch probe cycles for measuring workpiece misalignment ..... 28
BASIC ROTATION (touch probe cycle 400, ISO: G400) ..... 29
BASIC ROTATION from two holes (touch probe cycle 401, ISO: G401) ..... 31
BASIC ROTATION over two studs (touch probe cycle 402, ISO: G402) ..... 33
BASIC ROTATION compensation via rotary axis (touch probe cycle 403, ISO: G403) ..... 35
SET BASIC ROTATION (touch probe cycle 404, ISO: G404, available as of NC software 280 474-xx) ..... 37
Compensating workpiece misalignment by rotating the C axis (touch probe cycle 405, ISO: G405, available as of
NC software 280 474-xx) ..... 38
3.2 Automatic Datum Setting ..... 42
Overview ..... 42
Characteristics common to all touch probe cycles for datum setting ..... 43
DATUM FROM INSIDE OF RECTANGLE (touch probe cycle 410, ISO: G410) ..... 44
DATUM FROM OUTSIDE OF RECTANGLE (touch probe cycle 411, ISO: G411) ..... 46
DATUM FROM INSIDE OF CIRCLE (touch probe cycle 412, ISO: G412) ..... 48
DATUM FROM OUTSIDE OF CIRCLE (touch probe cycle 413, ISO: G413) ..... 50
DATUM FROM OUTSIDE OF CORNER (touch probe cycle 414, ISO: G414) ..... 52
DATUM FROM INSIDE OF CORNER (touch probe cycle 415, ISO: G415) ..... 55
DATUM CIRCLE CENTER (touch probe cycle 416, ISO: G416) ..... 58
DATUM IN TOUCH PROBE AXIS (touch probe cycle 417, ISO: G417) ..... 60
DATUM AT CENTER BETWEEN 4 HOLES (touch probe cycle 418, ISO: G418) ..... 61
HEIDENHAIN TNC 426, TNC 430 VII
3.3 Automatic Workpiece Measurement ..... 68
Overview ..... 68
Recording the results of measurement ..... 69
Measurement results in Q parameters ..... 70
Classification of results ..... 70
Tolerance monitoring ..... 70
Tool monitoring ..... 71
Reference system for measurement results ..... 71
REFERENCE PLANE (touch probe cycle 0, ISO: G55) ..... 72
DATUM PLANE (touch probe cycle 1) ..... 73
MEASURE ANGLE (touch probe cycle 420, ISO: G420) ..... 74
MEASURE HOLE (touch probe cycle 421, ISO: G421) ..... 76
MEASURE CIRCLE OUTSIDE (touch probe cycle 422, ISO: G422) ..... 79
MEASURE RECTANGLE FROM INSIDE (touch probe cycle 423, ISO: G423) ..... 82
MEASURE RECTANGLE FROM OUTSIDE (touch probe cycle 424, ISO: G424) ..... 85
MEASURE INSIDE WIDTH (touch probe cycle 425, ISO: G425) ..... 88
MEASURE RIDGE WIDTH (touch probe cycle 426, ISO: G426) ..... 90
MEASURE COORDINATE (touch probe cycle 427, ISO: G427) ..... 92
MEASURE BOLT HOLE CIRCLE (touch probe cycle 430, ISO: G430) ..... 94
MEASURE PLANE (touch probe cycle 431, ISO: G431) ..... 97
3.4 Special Cycles ..... 103
Overview ..... 103
CALIBRATE TS (touch probe cycle 2) ..... 104
MEASURING (touch probe cycle 3, available as of NC software 280 474-xx) ..... 105
MEASURE AXIS SHIFT (touch probe cycle 440, ISO: G440, available as of NC software 280 476-xx) ..... 106
VIII
4 Touch Probe Cycles for Automatic Tool Measurement ..... 109
4.1 Tool Measurement with the TT Tool Touch Probe ..... 110
Overview ..... 110
Setting the machine parameters ..... 110
Display the results of measurement ..... 111
4.2 Available Cycles ..... 112
Overview ..... 112
Differences between Cycles 31 to 33 and Cycles 481 to 483 ..... 112
Calibrating the TT ..... 113
Measuring the tool length ..... 114
Measuring the tool radius ..... 116
Measuring tool length and radius ..... 118
5 Digitizing ..... 121
5.1 Digitizing with Triggering or Measuring Touch Probe (Option) ..... 122
Overview ..... 122
Function ..... 123
5.2 Programming Digitizing Cycles ..... 124
Selecting digitizing cycles ..... 124
Defining the digitizing range ..... 124
Point Tables ..... 126
5.3 Types of Digitizing ..... 129
Meander digitizing ..... 129
Contour line digitizing ..... 131
Unidirectional line digitizing ..... 133
Digitizing with rotary axes ..... 136
5.4 Using Digitized Data in a Part Program ..... 140
Resulting NC blocks of a file containing data that were digitized with the CONTOUR LINES cycle. ..... 140
HEIDENHAIN TNC 426, TNC 430 IX
X
Introduction
1
1.1 General Information on Touch
Probe Cycles
The TNC must be specially prepared by the machine tool
builder for the use of a 3-D touch probe.
If you are carrying out measurements during program run,
be sure that the tool data (length, radius) can be used from
the calibrated data or from the last TOOL CALL block
(selected with MP7411).
If you are working alternately with a triggering and a
measuring touch probe, be sure that
n You have selected the correct touch probe in MP 6200.
n The measuring and triggering touch probes are never
connected to the control at the same time.
The TNC cannot detect which probe is actually in the
spindle.
Function
Whenever the TNC runs a touch probe cycle, the 3-D touch probe
approaches the workpiece in one linear axis. This is also true during an
active basic rotation or with a tilted working plane. The machine tool
builder determines the probing feed rate in a machine parameter (see
“Before You Start Working with Touch Probe Cycles” later in this
chapter).
When the probe stylus contacts the workpiece,
1.1 General Information on Touch Probe Cycles
n the 3-D touch probe transmits a signal to the TNC: the coordinates
of the probed position are stored,
n the touch probe stops moving, and
n returns to its starting position in rapid traverse.
If the stylus is not deflected within a distance defined in MP 6130), the
TNC displays an error message.
Z
Y
F
F MAX
X
2 1 Introduction
Touch Probe Cycles in the Manual and Electronic Handwheel Modes
In the Manual and Electronic Handwheel operating modes, the TNC
provides touch probe cycles that allow you to:
n Calibrate the touch probe
n Compensate workpiece misalignment
n Datum setting
Touch probe cycles for automatic operation
Besides the touch probe cycles, which you can use in the Manual and
Electronic handwheel operating modes, the TNC provides numerous
cycles for a wide variety of applications in automatic operation:
n Calibrating the touch probe (Chapter 3)
n Compensating workpiece misalignment (Chapter 3)
n Setting datums (Chapter 3)
n Automatic workpiece inspection (Chapter 3)
n Automatic workpiece measurement (Chapter 4)
Digitizing with triggering or measuring touch probe (Option, Chapter 5)
n
You can program the touch probe cycles in the Programming and
Editing operating mode via the TOUCH PROBE key. Like the most
recent fixed cycles, touch probe cycles use Q parameters with
numbers of 400 and above as transfer parameters. Parameters with
the same function that the TNC requires in several cycles always have
the same number: For example, Q260 is always assigned the
clearance height, Q261 the measuring height, etc.
To simplify programming, the TNC shows an illustration during cycle
definition. In the illustration, the parameter that needs to be entered is
highlighted (see figure at right).
1.1 General Information on Touch Probe Cycles
To improve clarity, the help illustrations sometimes omit
certain parameters.
HEIDENHAIN TNC 426, TNC 430 3
Defining the touch probe cycle in the Programming and Editing
operation mode
UUUU The soft-key row shows all available touch probe
functions divided into groups.
UUUU Select the desired probe cycle, for example datum
setting. Digitizing cycles and cycles for automatic tool
measurement are available only if your machine has
been prepared for them.
UUUU Select a cycle, e.g. datum setting at pocket. The TNC
initiates the programming dialog and asks all required
input values. At the same time a graphic of the input
parameters is displayed in the right screen window.
The parameter that is asked for in the dialog prompt
is highlighted.
UUUU Enter all parameters requested by the TNC and
conclude each entry with the ENT key.
UUUU The TNC ends the dialog when all required data has
been entered.
Group of measuring cycles Soft key
Cycles for automatic measurement and compensation
of workpiece misalignment
Cycles for automatic datum setting
Example: NC blocks
5 TCH PROBE 410 DATUM INSIDE RECTAN.
Q321=+50 ;CENTER IN 1ST AXIS
Q322=+50 ;CENTER IN 2ND AXIS
Q323=60 ;1ST SIDE LENGTH
Q323=60 ;1ST SIDE LENGTH
Q324=20 ;2ND SIDE LENGTH
Q261=-5 ;MEASURING HEIGHT
Q320=0 ;SET-UP CLEARANCE
Q260=+20 ;CLEARANCE HEIGHT
Q301=0 ;TRAVERSE TO CLEAR HEIGHT
Q305=10 ;NO. IN TABLE
Q331=+0 ;DATUM
Q332=+0 ;DATUM
Cycles for automatic workpiece inspection
Automatic calibration cycle
1.1 General Information on Touch Probe Cycles
Cycles for digitizing with measuring touch probe
(option, not available for ISO)
Cycles for digitizing with measuring touch probe
(option, not available for ISO)
Cycles for automatic tool measurement (enabled by
the machine tool builder, not ISO)
4 1 Introduction
1.2 Before You Start Working with
Touch Probe Cycles!
To make it possible to cover the widest possible range of applications,
machine parameters enable you to determine the behavior common
to all touch probe cycles:
Maximum traverse to touch point: MP6130
If the stylus is not deflected within the path defined in MP6130, the
TNC outputs an error message.
Safety clearance to touch point: MP6140
In MP6140 you define how far from the defined (or calculated) touch
point the TNC is to pre-position the touch probe. The smaller the value
you enter, the more exactly must you define the touch point position.
In many touch probe cycles you can also define a setup clearance in
addition that is added to machine parameter 6140.
Orient the infrared touch probe to the
programmed probe direction: MP6165 (as
of 280 476-10)
To increase measuring accuracy, you can use MP 6165 = 1 to have an
infrared touch probe oriented in the programmed probe direction
before every probe process. In this way the stylus is always deflected
in the same direction.
Multiple measurement: MP6170
To increase measuring certainty, the TNC can run each probing
process up to three times in sequence. If the measured position
values differ too greatly, the TNC outputs an error message (the limit
value is defined in MP6171). With multiple measurement it is possible
to detect random errors, e.g., from contamination.
If the measured values lie within the confidence interval, the TNC
saves the mean value of the measured positions.
Confidence interval for multiple measurement: MP6171
In MP6171 you store the value by which the results may differ when
you make multiple measurements. If the difference in the measured
values exceeds the value in MP6171, the TNC outputs an error
message.
HEIDENHAIN TNC 426, TNC 430 5
1.2 Before You Start Working with Touch Probe Cycles!
Touch trigger probe, probing feed rate: MP6120
In MP6120 you define the feed rate at which the TNC is to probe the
workpiece.
Touch trigger probe, rapid traverse for prepositioning: MP6150
In MP6150 you define the feed rate at which the TNC pre-positions the
touch probe, or positions it between measuring points.
Measuring touch probe, probing feed rate: MP6360
In MP6360 you define the feed rate at which the TNC is to probe the
workpiece.
Measuring touch probe, rapid traverse for prepositioning: MP6361
In MP6361 you define the feed rate at which the TNC pre-positions the
touch probe, or positions it between measuring points.
1.2 Before You Start Working with Touch Probe Cycles!
6 1 Introduction
Running touch probe cycles
All touch probe cycles are DEF active. This means that the TNC runs
the cycle automatically as soon as the TNC executes the cycle
definition in the program run.
Make sure that at the beginning of the cycle the
compensation data (length, radius) from the calibrated
data or from the last TOOL CALL block are active
(selection via MP7411, see the User's Manual of the
respective control, “General User Parameters”).
NC software 280.476-xx
You can also run the touch probe cycles 410 to 418 during
an active basic rotation. Make sure, however, that the
basic rotation angle does not change when you use cycle
7 “zero shift from datum table” after the measuring cycle.
Touch probe cycles with a number greater than 400 position the touch
probe according to a positioning logic:
n If the current coordinate of the south pole of the stylus is less than
the coordinate of the clearance height (defined in the cycle), the TNC
retracts the touch probe in the probe axis to the clearance height
and then positions it in the working plane to the first starting
position.
n If the current coordinate of the south pole of the stylus is greater
than the coordinate of the clearance height, the TNC first positions
the probe in the working plane to the first starting position and then
moves it immediately to the measuring height in the touch probe
axis.
HEIDENHAIN TNC 426, TNC 430 7
1.2 Before You Start Working with Touch Probe Cycles!
2
Touch Probe Cycles in the Manual and Electronic Handwheel Modes
2.1 Introduction
Overview
The following touch probe cycles are available in the manual mode:
Function Soft key
Calibrate the effective length
2.1 Introduction
Calibrate the effective radius
Measure a basic rotation using a line
Datum setting in any axis
Set the datum at a corner
Set the datum at a circle center
Measure a basic rotation using two holes/cylindrical
studs
Set the datum using four holes/cylindrical studs
Set the circle center using three holes/cylindrical studs
Selecting probe cycles
UUUU Select the Manual Operation or Electronic Handwheel mode of
operation.
UUUU To choose the touch probe functions, press the
TOUCH PROBE soft key. The TNC displays additional
soft keys—see table at right.
UUUU To select the probe cycle: press the appropriate soft
key, for example PROBING ROT, and the TNC
displays the associated menu.
10 2 Touch Probe Cycles in the Manual and Electronic Handwheel Modes
Recording Measured Values from the Probe Cycles
The TNC must be specially prepared by the machine tool
builder for use of this function. The machine tool manual
provides further information.
After executing any selected probe cycle, the TNC displays the soft
key PRINT. If you press this soft key, the TNC will record the current
values determined in the active probe cycle. You can then use the
PRINT function in the menu for setting the data interface (see the
User's Manual Chapter 12, “MOD Functions, Setting the Data
Interfaces”) to define whether the TNC is to
n print the measuring result,
n store the measuring results on the TNC’s hard disk, or
n store the measuring results on a PC.
If you store the measuring results, the TNC creates the ASCII file
%TCHPRNT.A. Unless you define a specific path and interface in the
interface configuration menu, the TNC will store the %TCHPRNT file
in the main directory TNC:\.
When you press the PRINT soft key, the %TCHPRNT.A
file must not be
active in the Programming and Editing mode of operation.
The TNC will otherwise display an error message.
The TNC stores the measured data in the %TCHPRNT.A
file only. If you execute several probe cycles in succession
and want to store the resulting measured data, you must
make a backup of the contents stored in %TCHPRNT.A
between the individual cycles by copying or renaming the
file.
Format and contents of the %TCHPRNT file are preset by
the machine tool builder.
2.1 Introduction
HEIDENHAIN TNC 426, TNC 430 11
Writing the measured values from probe cycles in datum tables
This function is active only if you have datum tables active
on your TNC (bit 3 in machine parameter 7224.0 =0).
With the ENTER IN DATUM TABLE soft key, the TNC can write the
values measured during a probe cycle in a datum table:
UUUU Select any probe function.
2.1 Introduction
UUUU Enter the desired coordinates of the datum in the appropriate input
fields (depends on the touch probe cycle being run).
UUUU Enter the datum number in the datum number = input box.
UUUU Enter the name of the datum table (complete path) in the datum
table input box.
UUUU Press the soft key ENTER IN DATUM TABLE. The TNC displays
whether the data are to be transferred to the indicated datum table
as actual values or reference values.
If, in addition to the desired coordinate of the datum, you wish to enter
an incremental distance in the table, switch the soft key DISTANCE to
ON. The TNC then displays an additional input box for each axis, in
which you can enter the desired distance. The TNC then writes the
sum of the desired datum and its assigned distance into the table.
If immediately after probing you have used the probing
menu to reset the datum, do not write the probe values to
a datum table. The probe values saved by the TNC are
always based on the datum that was active at the time of
probing. Writing the probe values to a datum table would
result in incorrect entries.
12 2 Touch Probe Cycles in the Manual and Electronic Handwheel Modes
2.2 Calibrating a Touch Trigger
Probe
Introduction
The touch probe must be calibrated in the following cases:
n Commissioning
n Stylus breakage
n Stylus exchange
n Change in the probe feed rate
n Irregularities caused, for example, when the machine heats up
During calibration, the TNC finds the “effective” length of the stylus
and the “effective” radius of the ball tip. To calibrate the touch probe,
clamp a ring gauge of known height and known internal radius to the
machine table.
Calibrating the effective length
UUUU Set the datum in the spindle axis such that for the machine tool table
Z=0.
UUUU To select the calibration function for the touch probe
length, press the TOUCH PROBE and CAL L soft
keys. The TNC then displays a menu window with
four input fields.
UUUU Enter the tool axis (with the axis key).
UUUU Datum: Enter the height of the ring gauge.
UUUU The menu items Effective ball radius and Effective
length do not require input.
UUUU Move the touch probe to a position just above the ring
gauge.
UUUU To change the traverse direction (if necessary) press a
soft key or an arrow key.
UUUU To probe the upper surface of the ring gauge, press
the machine START button.
Z
2.2 Calibrating a Touch Trigger Probe
Y
5
X
HEIDENHAIN TNC 426, TNC 430 13
Calibrating the effective radius and compensating center misalignment
After the touch probe is inserted it normally needs to be aligned
exactly with the spindle axis. The misalignment is measured with this
calibration function and compensated electronically.
For this operation the TNC rotates the 3-D touch probe by 180°. The
rotation is initiated by a miscellaneous function that is set by the
machine tool builder in machine parameter 6160.
The center misalignment is measured after the effective ball tip radius
is calibrated.
UUUU In the Manual Operation mode, position the ball tip in the bore of the
ring gauge.
UUUU To select the calibration function for the ball-tip radius
and the touch probe center misalignment, press the
CAL R soft key.
UUUU Select the tool axis and enter the radius of the ring
gauge.
UUUU To probe the workpiece, press the machine START
button four times. The touch probe contacts a
position on the bore in each axis direction and
calculates the effective ball-tip radius.
2.2 Calibrating a Touch Trigger Probe
UUUU If you want to terminate the calibration function at this
point, press the ENDE soft key.
Z
Y
X
10
In order to be able to determine ball-tip center
misalignment, the TNC needs to be specially prepared by
the machine manufacturer. The machine tool manual
provides further information.
UUUU If you want to determine the ball-tip center
misalignment, press the180° soft key. The TNC
rotates the touch probe by 180°.
UUUU To probe the workpiece, press the machine START
button four times. The touch probe contacts a
position on the bore in each axis direction and
calculates the ball-tip center misalignment.
14 2 Touch Probe Cycles in the Manual and Electronic Handwheel Modes
Displaying calibration values
The TNC stores the effective length and radius, as well as the center
misalignment, for use when the touch probe is needed again. You can
display the values on the screen with the soft keys CAL L and CAL R.
Storing calibration values in the TOOL.T tool table
This function is only available if bit 0 in machine parameter
7411 = 1 is set (activate touch probe data with TOOL CALL),
and tool table TOOL.T is active (machine parameter 7260
not equal to 0).
If you conduct measurements during program run, the compensation
data for the touch probe can be activated from the tool table via a TOOL
CALL. To store the calibration data in the TOOL.T tool table, enter the
tool number in the calibration menu (confirm with ENT) and then press
the ENTER R IN TOOL TABLE or the ENTER L IN TOOL TABLE soft
key.
Managing more than one block of calibrating data (as of NC software 280 476-xx)
To be able to use more than one block of calibration data, you must set
bit one in machine parameter 7411. The calibration data (length,
radius, center misalignment, and spindle angle) are then always saved
by the TNC in the tool table TOOL.T under a tool number that can be
selected in the calibration menu (see also User's Manual, section 5.2,
“Tool Data”).
2.2 Calibrating a Touch Trigger Probe
If you use this function, you must first activate the
corresponding tool number with a tool call before
executing a touch probe cycle, regardless of whether you
wish to run the touch probe cycle in automatic mode or
manual mode.
You can view and edit the calibration data in the calibration menu, but
you must make sure to write the changes back into the tool table by
pressing the ENTER R IN TOOL TABLE or ENTER L IN TOOL TABLE
soft key. The TNC does not write the calibration values into the table
automatically!
HEIDENHAIN TNC 426, TNC 430 15
2.3 Calibrating a Measuring Touch
Probe
Introduction
If the TNC displays the error message "Stylus already in
contact," select the 3-D calibration menu and press the
RESET 3D soft key.
The measuring touch probe must be calibrated whenever
the machine parameters for 3-D touch probes are changed.
The effective length is calibrated in the same way as with
triggering touch probes. You must also enter tool radius R2
(corner radius).
With MP6321 you can define whether the TNC should
probe to find the stylus center.
The 3-D calibration cycle for measuring touch probes enables you to
measure a standard ring gauge fully automatically. (The standard ring
gauge is available from HEIDENHAIN). Fix the standard ring gauge to
the machine table with fixing clamps.
From the data measured during calibration, the TNC calculates the
spring rate of the touch probe, the stylus deflection and the stylus
center misalignment. At the end of the calibration cycle, the TNC
automatically stores these values in the input menu.
2.3 Calibrating a Measuring Touch Probe
Course of actions
UUUU In the Manual Operation mode, position the touch probe to a
position approximately in the center of the standard ring gauge and
set it to 180°.
UUUU To select the 3-D calibration cycle, press the 3D CAL
soft key
UUUU Enter the values for stylus radius 1 and stylus radius 2.
Enter the same value for stylus radius 1 and 2 if you
are using a stylus with ball tip. Enter different values
for stylus radius 1 and 2 if you are using a stylus with
a corner radius.
UUUU Diameter ring gauge: The diameter is engraved on the
standard ring gauge.
UUUU
To start the calibration cycle, press the machine START
button: The touch probe measures the standard ring
gauge in a programmed sequence of steps.
UUUU Rotate the touch probe to 0° as soon as the TNC asks
you to.
UUUU To start the calibration cycle once again to determine
center misalignment, press the machine START
button. The touch probe again measures the standard
ring gauge in a programmed sequence of steps.
16 2 Touch Probe Cycles in the Manual and Electronic Handwheel Modes
Displaying calibration values
The compensation factors and force ratios are stored in the TNC for
later use whenever the measuring touch probe is needed.
You can display the stored values on the screen by pressing the 3D
CAL soft key.
Storing calibration values in the TOOL.T tool table
This function is only available if machine parameter 7411
= 1 is set (activate touch probe data with TOOL CALL), and
tool table TOOL.T is active (machine parameter 7260 not
equal to 0).
If you conduct measurements during program run, the compensation
data for the touch probe can be activated from the tool table via a TOOL
CALL. To store the calibration data in the TOOL.T tool table, enter the
tool number in the calibration menu (confirm with ENT) and then press
the ENTER R IN TOOL TABLE soft key.
The TNC stores the stylus radius 1 in the R column, and the stylus
radius 2 in the R2 column.
2.3 Calibrating a Measuring Touch Probe
HEIDENHAIN TNC 426, TNC 430 17
2.4 Compensating Workpiece
Misalignment
Introduction
The TNC electronically compensates workpiece misalignment by
computing a “basic rotation.”
For this purpose, the TNC sets the rotation angle to the desired angle
with respect to the reference axis in the working plane. See figure at
right.
Select the probe direction perpendicular to the angle
reference axis when measuring workpiece misalignment.
To ensure that the basic rotation is calculated correctly
during program run, program both coordinates of the
working plane in the first positioning block.
Measuring the basic rotation
UUUU Select the probing function by pressing the PROBING
ROT soft key.
2.4 Compensating Workpiece Misalignment
The TNC saves the basic rotation in non-volatile memory. The basic
rotation is effective for all subsequent program runs and graphic
simulation.
UUUU Position the ball tip at a starting position near the first
touch point.
UUUU Select the probe direction perpendicular to the angle
reference axis: Select the axis by soft key.
UUUU To probe the workpiece, press the machine START
button.
UUUU Position the ball tip at a starting position near the
second touch point.
UUUU To probe the workpiece, press the machine START
button.
Y
PA
Y
X
A B
X
18 2 Touch Probe Cycles in the Manual and Electronic Handwheel Modes
Loading...