heidenhain iTNC 530 User Manual

Touch Probe Cycles iTNC 530

NC Software 340 420-xx 340 421-xx

User’s Manual

English (en)

4/2002

TNC Models, Software and Features

This manual describes functions and features provided by the TNCs as of the following NC software numbers.

TNC Model	NC Software No.
iTNC 530	340 420-01
iTNC 530 E	340 421-01

The suffix E indicates the export version of the TNC. The export version of the TNC has the following limitations:

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:

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

iTNC 530. 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 iTNC 530

I

II

Contents	Introduction	1
		2
	Touch Probe Cycles in the Manual and
	Electronic Handwheel Modes	3
	Touch Probe Cycles for Automatic
	Workpiece Inspection	4
	Touch Probe Cycles for Automatic Tool
	Measurement

HEIDENHAIN iTNC 530	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 .....										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
Running touch probe cycles .....			7

Contents

HEIDENHAIN iTNC 530

V

Contents

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
To calibrate 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 .....							15
2.3 Compensating workpiece misalignment				.....	16
Introduction .....	16
Measuring the basic rotation .....			16
Displaying a basic rotation		.....	17
To cancel a basic rotation: .....			17
2.4 Setting the Datum with a 3-D Touch Probe .....					18
Introduction .....	18
To set the datum in any axis (see figure at right)						.....	18
Corner as datum—using points that were already probed for a basic rotation (see figure at right) .....													19
Corner as datum—without using points that were already probed for a basic rotation .....												19
Circle center as datum .....		20
Setting datum points over holes/cylindrical studs .....							21
2.5 Measuring Workpieces with a 3-D Touch Probe .....						22
Introduction .....	22
To find the coordinate of a position on an aligned workpiece: .....									22
Finding the coordinates of a corner in the working plane .....								22
Measuring workpiece dimensions .....				23
To find the angle between the angle reference axis and a side of the workpiece .....											24

VI

Inhalt

3 Touch Probe Cycles for Automatic Workpiece Inspection			..... 25
3.1 Measuring Workpiece Misalignment 26.....
Overview .....	26
Characteristics common to all touch probe cycles for measuring workpiece misalignment ..... 26
BASIC ROTATION (touch probe cycle 400, ISO: G400) .....		27
BASIC ROTATION from two holes (touch probe cycle 401, ISO: G401) .....						29
BASIC ROTATION over two studs (touch probe cycle 402, ISO: G402) .....						31
BASIC ROTATION compensation via rotary axis (touch probe cycle 403, ISO: G403) ..... 33
BASIC ROTATION (touch probe cycle 404, ISO: G404) .....		36
Compensating workpiece misalignment by rotating the C axis (touch probe cycle 405, ISO: G405) ..... 37
3.2 Automatic Datum Setting ..... 41
Overview .....	41
Characteristics common to all touch probe cycles for datum setting .....				42
DATUM FROM INSIDE OF RECTANGLE (touch probe cycle 410, ISO: G410) .....							43
DATUM FROM OUTSIDE OF RECTANGLE (touch probe cycle 411, ISO: G411) .....							45
DATUM FROM INSIDE OF CIRCLE (touch probe cycle 412, ISO: G412)				.....		47
DATUM FROM OUTSIDE OF CIRCLE (touch probe cycle 413, ISO: G413)						..... 50
DATUM FROM OUTSIDE OF CORNER (touch probe cycle 414, ISO: G414) .....							53
DATUM FROM INSIDE OF CORNER (touch probe cycle 415, ISO: G415) .....						56
DATUM CIRCLE CENTER (touch probe cycle 416, ISO: G416) .....			59
DATUM IN TOUCH PROBE AXIS (touch probe cycle 417, ISO: G417) .....				61
DATUM AT CENTER BETWEEN 4 HOLES (touch probe cycle 418, ISO: G418) .....							62

Contents

HEIDENHAIN iTNC 530

VII

Contents

3.3 Automatic Workpiece Measurement ..... 69
Overview .....	69
Recording the results of measurement			..... 70
Measurement results in Q parameters .....			71
Classification of results		..... 71
Tolerance monitoring .....		71
Tool monitoring ..... 72
Reference system for measurement results ..... 72
REFERENCE PLANE (touch probe cycle 0, ISO: G55) .....				73
DATUM PLANE (touch probe cycle 1) .....			74
MEASURE ANGLE (touch probe cycle 420, ISO: G420) .....				75
MEASURE HOLE (touch probe cycle 421, ISO: G421) .....				77
MEASURE CIRCLE OUTSIDE (touch probe cycle 422, ISO: G422)					..... 80
MEASURE RECTANGLE FROM INSIDE (touch probe cycle 423, ISO: G423) .....						83
MEASURE RECTANGLE FROM OUTSIDE (touch probe cycle 424, ISO: G424) .....						86
MEASURE INSIDE WIDTH (touch probe cycle 425, ISO: G425) .....					89
MEASURE RIDGE WIDTH (touch probe cycle 426, ISO: G426) .....					91
MEASURE COORDINATE (touch probe cycle 427, ISO: G427) .....					93
MEASURE BOLT HOLE CIRCLE (touch probe cycle 430, ISO: G430) ..... 95
MEASURE PLANE (touch probe cycles 431, ISO: G431) .....				98
3.4 Special Cycles .....	104
Overview .....	104
CALIBRATE TS (touch probe cycle 2) .....			105
MEASURING (touch probe cycle 3) .....			106
MEASURE AXIS OFFSET (touch probe cycle 440, ISO: G440) .....					107

VIII

Inhalt

.....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 (touch probe cycle 30 or 480, ISO: G480) .....				113
Measuring the tool length (touch probe cycle 31 or 481, ISO: G481) .....					114
Measuring the tool radius (touch probe cycle 32 or 482, ISO: G482) .....					116
Measuring the tool radius (touch probe cycle 33 or 483, ISO: G483) .....					118

Contents

HEIDENHAIN iTNC 530

IX

1

Introduction

1.1 General Information on Touch Probe Cycles

1.1General 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).

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 Z chapter).

Y

When the probe stylus contacts the workpiece,

The 3-D touch probe transmits a signal to the TNC: the coordinates of the probed position are stored,

The touch probe stops moving, and

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.

X

F

F MAX

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:

Calibrate the touch probe

Compensate workpiece misalignment

Set datums

Touch probe cycles for automatic operation

Besides the touch probe cycles, which you can use in the Manual and Electronic handwheel operating modes, several cycles are available for a wide variety of applications in automatic operation:

Calibrating the touch probe (Chapter 3)

Compensating workpiece misalignment (Chapter 3)

Setting datums (Chapter 3)

Automatic workpiece inspection (Chapter 3)

Automatic workpiece measurement (Chapter 4)

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 specific functions that are required 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

HEIDENHAIN iTNC 530

3

1.1 General Information on Touch Probe Cycles

Defining the touch probe cycle in the Programming and Editing operation mode

The soft-key row shows all available touch probe functions divided into groups.

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.

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

Enter all parameters requested by the TNC and conclude each entry with the ENT key.

The TNC terminates the dialog when all required data have been entered

Group of measuring cycles

Soft key

Cycles for automatic measurement and compensation of workpiece misalignment

Cycles for automatic datum setting

Cycles for automatic workpiece inspection

Automatic calibration cycle

Cycles for automatic tool measurement (enabled by the machine tool builder)

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 CLEARANCE HEIGHT
Q305=10	;NO. IN TABLE
Q331=+0	;DATUM
Q332=+0	;DATUM
Q303=+1	;MEAS. VALUE TRANSFER

4	1 Introduction

1.2Before 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

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.

1.2 Before You Start Working with Touch Probe Cycles!

HEIDENHAIN iTNC 530

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.

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 iTNC 530, “General User Parameters”).

You may 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:

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.

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.

1.2 Before You Start Working with Touch Probe Cycles!

HEIDENHAIN iTNC 530

7

2

Touch Probe Cycles in the

Manual and Electronic

Handwheel Modes

2.1 Introduction

2.1 Introduction

Overview

The following touch probe cycles are available in the manual mode:

Function

Soft key

Calibrate the effective length

Calibrate the effective radius

Measuring a basic rotation using a line

Datum setting in any axis

Set the datum at a corner

Set the datum at a circle center

Measuring a basic rotation using two holes/cylindrical studs

Set the datum using four holes/cylindrical studs

Setting the circle center using three holes/cylindrical studs

Selecting probe cycles

Select the Manual Operation or Electronic Handwheel mode of operation.

To choose the touch probe functions, press the TOUCH PROBE soft key. The TNC displays additional soft keys—see table at right.

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

print the measuring result,

store the measuring results on the TNC’s hard disk, or

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 iTNC 530

11

2.1 Introduction

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:

Select any probe function.

Enter the desired coordinates of the datum in the appropriate input fields (depends on the touch probe cycle being run).

Enter the datum number in the input field datum number =.

Enter the name of the datum table (complete path) in the "datum table" input field.

Press the soft key ENTER IN DATUM TABLE. The TNC saves the datum into the indicated datum table under the entered number.

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 field 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 datum 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

2.2Calibrating a Touch Trigger Probe

Introduction

The touch probe must be calibrated in the following cases:

Commissioning

Stylus breakage

Stylus exchange

Change in the probe feed rate

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.

To calibrate the effective length:

Set the datum in the spindle axis such that for the machine tool table Z=0.

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.

Enter the tool axis (with the axis key).

Datum: Enter the height of the ring gauge.

The menu items Effective ball radius and Effective length do not require input.

Move the touch probe to a position just above the ring gauge.

To change the traverse direction (if necessary) press a soft key or an arrow key.

To probe the upper surface of the ring gauge, press the machine START button.

Z

Y

5

2.2 Calibrating a Touch Trigger Probe

X

HEIDENHAIN iTNC 530

13

2.2 Calibrating a Touch Trigger Probe

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 the machine parameter 6160.

The center misalignment is measured after the effective ball tip radius is calibrated.

In the Manual Operation mode, position the ball tip in the bore of the ring gauge.

To select the calibration function for the ball-tip radius and the touch probe center misalignment, press the CAL R soft key.

Select the tool axis and enter the radius of the ring gauge.

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.

If you want to terminate the calibration function at this point, press the ENDE soft key.

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.

If you want to determine the ball-tip center misalignment, press the180° soft key. The TNC rotates the touch probe by 180°.

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.

Z

Y

X

10

14	2 Touch Probe Cycles in the Manual and Electronic Handwheel Modes

Displaying calibration values

The TNC stores the effective length and radius, and 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

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”).

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!

2.2 Calibrating a Touch Trigger Probe

HEIDENHAIN iTNC 530

15

2.3 Compensating workpiece misalignment

2.3Compensating 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.

Y	Y
PA
X		X
	A	B

Measuring the basic rotation

Select the probing function by pressing the PROBING ROT soft key.

Position the ball tip at a starting position near the first touch point.

Select the probe direction perpendicular to the angle reference axis: Select the axis by soft key.

To probe the workpiece, press the machine START button.

Position the ball tip at a starting position near the second touch point.

To probe the workpiece, press the machine START button.

The TNC saves the basic rotation in non-volatile memory. The basic rotation is effective for all subsequent program runs and graphic simulation.

16	2 Touch Probe Cycles in the Manual and Electronic Handwheel Modes

Displaying a basic rotation

The angle of the basic rotation appears after ROTATION ANGLE whenever PROBING ROT is selected. The TNC also displays the rotation angle in the additional status display (STATUS POS.)

In the status display a symbol is shown for a basic rotation whenever the TNC is moving the axes according to a basic rotation.

To cancel a basic rotation:

Select the probing function by pressing the PROBING ROT soft key.

Enter a rotation angle of zero and confirm with the ENT key.

To terminate the probe function, press the END key.

2.3 Compensating workpiece misalignment

HEIDENHAIN iTNC 530

17

2.4 Setting the Datum with a 3-D Touch Probe

2.4Setting the Datum with a 3-D Touch Probe

Introduction

The following functions are available for setting the datum on an aligned workpiece:

Datum setting in any axis with PROBING POS

Defining a corner as datum with PROBING P

Setting the datum at a circle center with PROBING CC

To set the datum in any axis (see figure at right)

Select the probing function by pressing the PROBING POS soft key.

Move the touch probe to a starting position near the touch point.

Select the probe axis and direction in which you wish to set the datum, such as Z in direction Z–. Selection is made via soft keys.

To probe the workpiece, press the machine START button.

Datum: Enter the nominal coordinate and confirm your entry with ENT, or write the value to the table (see “Writing the measured values from probe cycles in datum tables” on page 12).

Z

Y

X

18	2 Touch Probe Cycles in the Manual and Electronic Handwheel Modes