Biesse OSAI 10 User Manual

SOFTWARE USER’S MANUAL

Software

Biesse Applications

for Numerical
Control OSAI 10
Series CNC

5804A0062 ENGLISH
Issue.Revision: 1.4

Serial number

481/96

Information on this publication

Information on this publication

Code: Issue: Revision: Approval number:

5804A0062 1 0 (11/2001) 2001/037

1 (03/2002) 01/0957M

2 (04/2002) 02/0199M

3 (05/2002) 03/0105M

4 (11/2003) 03/0026M

List of changes

Revision: Additions: Deletions: Changes:

0 new document

1 chapter

5, 6

paragraph

1.1, 2.1.3, 2.3, 3.1, 3.2.2,

3.4, 3.5

2 paragraph

2.2

3 appendix

B

4 paragraph

3.7

paragraph

2.1.5, 3.2.2, 3.4

paragraph

3.2.2, 3.4, C.1

paragraph

3.2, 3.6, C.11

This manual has been prepared for use by clients only and it contains information protected by
copyright. It must not be photocopied or reproduced in any form, either fully or in part, without the
prior written consent of BIESSE. The manual is supplied together with the machine, and must be
kept in a safe place in order to have it always to hand for consultation.

The manual must only be used by personnel who have been adequately trained to operate the
machine. BIESSE cannot be considered responsible or liable for damage resulting from incorrect
or improper use of the documentation provided. In order to avoid incorrect manoeuvres that might
result in danger to the operator or to third parties, it is essential to read and fully understand all the
documentation supplied with the machine.

BIESSE S.p.A. ©
(5804a0062.fm-181103)

3

Information on this publication

4

BIESSE S.p.A. ©

(5804a0062.fm-181103)

Table of contents

Introduction

Field of application and limits of the manual . . . . . . . . . -9

Documents supplied with the machine . . . . . . . . . . . . . -9

Warning signs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . -9

Warnings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . -9

Chapter 1. User interface

1.1 Menus and softkeys . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-1

User softkeys . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-2

Table of contents

Chapter 2. Notes on tooling

2.1 Management of the magazine and tools. . . . . . . . . . . . . . . 2-1

2.1.1 Displaying the table editor. . . . . . . . . . . . . . . . . . . . . . . 2-2

2.1.2 Listing magazines . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-3

2.1.3 Listing the tools in the magazine . . . . . . . . . . . . . . . . . . 2-5

Tool characteristics . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-8

2.1.4 Listing tools in the Data Base Table . . . . . . . . . . . . . . . 2-9

2.1.5 Management of tools distributed over a number of

magazines (for TC machines) . . . . . . . . . . . . . . . . . . . . 2-10

2.2 Saving a table . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-10

2.3 Work table management. . . . . . . . . . . . . . . . . . . . . . . . . . . 2-11

2.4 Tool presetting . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-12

For EP machines with patented electronic axis . . . . . . . 2-12

For pneumatic EP machines . . . . . . . . . . . . . . . . . . . . . 2-12

For pneumatic TC machines . . . . . . . . . . . . . . . . . . . . . 2-12

For TC or TCR machines with patented electronic axis. 2-13

Chapter 3. Notes on programming

3.1 Tool change . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-1

Automatic tool change . . . . . . . . . . . . . . . . . . . . . . . . . . 3-1

Manual tool change . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-2

3.2 Programming functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-5

Brief notes on S, T, F, G functions. . . . . . . . . . . . . . . . . 3-5

3.2.1 M functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-6

Modal and non modal M functions . . . . . . . . . . . . . . . . . 3-7

Prelude and postlude M functions . . . . . . . . . . . . . . . . . 3-7

3.2.2 List of M functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-7

“M” FUNCTIONS TABLE . . . . . . . . . . . . . . . . . . . . . . . . 3-9

Using the M codes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-13

Types of “M” functions . . . . . . . . . . . . . . . . . . . . . . . . . . 3-16

Description of code M0 . . . . . . . . . . . . . . . . . . . . . . . . . 3-16

Description of code M33 . . . . . . . . . . . . . . . . . . . . . . . . 3-17

3.3 Notes on the use of revolving axes. . . . . . . . . . . . . . . . . . . 3-18

BIESSE S.p.A. ©
(5804a0062TOC.fm-181103)

5

Table of contents

Tilting axis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-19

3.4 Control variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-19

3.5 Dedicated programming variables. . . . . . . . . . . . . . . . . . . . 3-21

3.6 Default conditions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-25

3.7 Programming machining operations using the electronic copier3-27

Examples:. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-28

3.8 Treatment of machine parameters . . . . . . . . . . . . . . . . . . . 3-29

3.8.1 Dynamic parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-30

3.8.2 Dynamic limits . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-32

3.8.3 Program SET-UP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-33

Chapter 4. Notes on machining

4.1 Updating tool tables. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-1

4.2 Machining operations in dual mode. . . . . . . . . . . . . . . . . . . 4-2

Chapter 5. Bar code reader control

5.1 Installing the reader . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5-1

Checking operation of the reader and connection . . . . . 5-1

5.2 Using the brcman program . . . . . . . . . . . . . . . . . . . . . . . . . 5-2

Using the three cycles . . . . . . . . . . . . . . . . . . . . . . . . . . 5-3

Appendix A. Laser projector for electrospindles

A.1 Installation and wiring . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-1

A.2 Using the software associated with the projector . . . . . . . . A-1

Appendix B. Renishaw NC1 tool adjustment system

B.1 Memory requirements for the software . . . . . . . . . . . . . . . . B-1

B.2 Software installation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-2

B.3 Types of tool correction supported . . . . . . . . . . . . . . . . . . . B-2

B.4 Software functions of the NC1 system . . . . . . . . . . . . . . . . B-2

Macro functions for measuring . . . . . . . . . . . . . . . . . . . . B-2

Macro functions for calibration . . . . . . . . . . . . . . . . . . . . B-2

Macro functions for service . . . . . . . . . . . . . . . . . . . . . . B-3

B.5 Use of the macros . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-3

B.6 Macro variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-4

Macro variables for the calibration data . . . . . . . . . . . . . B-4

Macro variables for adjustment data . . . . . . . . . . . . . . . B-5

B.7 NC1 system orientation . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-9

B.8 Beam detection and measuring movements . . . . . . . . . . . . B-10

B.9 Dispersion tolerance check . . . . . . . . . . . . . . . . . . . . . . . . . B-10

B.10 MAIN macro execution . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-11

B.11 Using the individual macros. . . . . . . . . . . . . . . . . . . . . . . . . B-18

B.12 Laser beam alignment. . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-18

Calibration tool required . . . . . . . . . . . . . . . . . . . . . . . . . B-19

Adjustment data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-19

Macro inputs. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-19

Output. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-20

B.13 NC1 system calibration . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-21

Calibration tool required . . . . . . . . . . . . . . . . . . . . . . . . . B-22

Macro inputs. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-22

Output. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-22

Alarms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-22

6

(5804a0062TOC.fm-181103)

BIESSE S.p.A. ©

B.14 Tool length adjustment . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-23

Macro inputs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-24

Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-24

Alarms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-25

B.15 Tool diameter and length adjustment . . . . . . . . . . . . . . . . . B-26

Macro inputs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-26

Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-27

Alarms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-27

B.16 Tool breakage detection . . . . . . . . . . . . . . . . . . . . . . . . . . . B-28

Macro inputs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-29

Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-29

Alarms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-30

B.17 Error messages and alarms . . . . . . . . . . . . . . . . . . . . . . . . B-31

Appendix C. PLC Messages

C.1 Logic messages . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . C-1

C.1.1 Error messages . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . C-2

C.2 Semantic checks effected by the PLC . . . . . . . . . . . . . . . . C-24

C.2.1 M code semantic checks . . . . . . . . . . . . . . . . . . . . . . . . C-25

C.2.2 S code semantic checks . . . . . . . . . . . . . . . . . . . . . . . . C-26

C.2.3 T code semantic checks . . . . . . . . . . . . . . . . . . . . . . . . C-27

C.2.4 PSEUDOAXES semantic checks (NC stops) . . . . . . . . C-28

Table of contents

BIESSE S.p.A. ©
(5804a0062TOC.fm-181103)

7

Table of contents

8

(5804a0062TOC.fm-181103)

BIESSE S.p.A. ©

Introduction

Introduction

Field of application and limits of the manual

This manual is aimed at the operator, and is an integration of the “Machining Centre” Software
user’s manual. As the present manual alone is not sufficient to allow use of the software, the
above mentioned Software user’s manual must also be read thoroughly.
In order to become familiar with the machine and its use you are also recommended to read the
Machine User’s Manual and relative Enclosures.

Documents supplied with the machine

A list of these documents is provided in the Machine User’s Manual.

Warning signs

Paragraphs that should not be overlooked are highlighted and preceded by the symbols described
and illustrated below:

DANGER

Paragraphs marked with this symbol indicate an imminent danger, and the contents must
therefore be taken into careful account in order to prevent a serious accident.

CAUTION

Paragraphs marked with this symbol indicate procedures to be used and actions to be
taken to avoid any damage to goods and property.

INFORMATION

This symbol is used to indicate points of particular importance that must not be overlooked.

Warnings

Before using the machine, read the safety information provided in the MACHINE USER’S
MANUAL.

BIESSE S.p.A. ©
(a202h005.fm-181103)

9

Introduction

10

BIESSE S.p.A. ©

(a202h005.fm-181103)

1

-

Chapter 1. User interface

All the basic information in the user interface is described in detail in the “Machining Centre”
Software user’s manual. The following paragraph gives a brief description of how to use the
softkeys and menus.

1.1 Menus and softkeys

The menu is made up of three lines and 15 labels (ref. A) each one of which contains an item on
the menu. The softkeys are the 5 function keys (ref. B), located at the top of the keyboard, used to
select a label item from the menu and to enter commands directly.

The following figure shows the main menu, with the relative lines and labels, and the softkeys:

A

POS DISPLAY

AUTO

MACHINE SET-UP

F5 F6 F7 F8 F9

B

When a line is displayed or enabled it is shown in cyan, and the menu items are displayed in white.

NEXT DISPLAY

MANUAL

TABLES

SELECT PROCESS

PART PROGRAM

DIAGNOSTICS

ENLARGE

VARIABLES

HELP

OEM

UTILITY

BIESSE S.p.A. ©
(a203h009.fm-181103)

1 - 1

Chapter 1.
User interface

User softkeys

The softkeys described below have been customised by BIESSE and are displayed by pressing
softkey A.

A

→•←

BCD E

B: used to perform a general reset of the machine.

C: used to perform the manual lubrication cycle.

D: used to reset the incremental counter to zero working hours.

E: used to modify the automatic lubrication time and to reset the hour counter.

¡¡¡

000000

¡¡¡

δ

1 - 2

BIESSE S.p.A. ©

(a203h009.fm-181103)

2

-

Chapter 2. Notes on tooling

Tooling is the phase during which the machine is set up to carry out machining operations. For
correct NC tooling, proceed as indicated below, with reference also to the “Machine user’s
manual”.

 Select the set of tools and aggregates to be used with the machine.

 Fit the tools in the magazine tool holders;

 Enter the characteristics of the tools selected, in the data lists (see par. 2.1 “Management of

the magazine and tools” on page 2 - 1).

 Enter the tools that are already installed in the automatic tool change magazine tool holders,

in the Magazine Table (see par. 2.1.2 “Listing magazines” on page 2 - 3).

 Enter the type of table and tool the latter (see par. 2.3 “Work table management” on page 2 -

11).

 Carry out presetting of tools (see par. 2.4 “Tool presetting” on page 2 - 12).

2.1 Management of the magazine and tools

Management of the magazine and of the tools is carried out using an Editor program, known as
Table Editor. Before reading this chapter, it is important that the operator acquire a detailed
working knowledge of all the procedures necessary to open, save and modify the CNC tables, all
of which are described in the “Machining Centre” Software User’s manual.

The editor makes it possible to manage, in the form of tables, a while series of data items, which
are grouped together in four different environments (Tables):

 The tool environment (Tool Table), in which all the tools are listed.

 The magazines environment (Magazine Table), in which all the magazines present in the

machine are listed.

 The tool data base environment (Tool Data Base Table): the data base containing all the data

regarding tool characteristics.

 The correctors environment (Correctors Table), in which it is possible to enter variations to the

positions set previously, so as to avoid having to modify the part program (machining
program) or other parameters of fundamental importance for the machining operation.

BIESSE S.p.A. ©
(a207h004.fm-181103)

2 - 1

Chapter 2.
Notes on tooling

All the “tables” created are normally saved in the system memory (current tables), which will store
them even after the NC has been switched off, and which can be accessed by selecting the file
“MEMORY”. “Tables” in the same family (for example for different machining operations) can be
saved to the hard disk in the form of files, the names of which are displayed on screen when
access to a table is requested.

INFORMATION

In TC machines equipped with a number of milling units, management of tools is based on a
single tool table, in which all the tools present in the magazines are listed.

INFORMATION

When managing the tables, the control will always refer to the current tables, that is to say the
ones in the file “MEMORY”.

INFORMATION

Always exit the table manager environment before running a part program.

2.1.1 Displaying the table editor.

To access the Table Editor, from the main menu, press the softkey corresponding to the menu item
TABLES. The main Editor environment is displayed (see figure below), from which it is possible to
open the four environments described above.

2 - 2

BIESSE S.p.A. ©

(a207h004.fm-181103)

Chapter 2.

Notes on tooling

The menus that allow the four environments to be displayed are:

 TOOL: tool table.

 MAGAZINE: magazine table.

 OFFSET: correction table (offset).

 TOOL DATA BASE: tool data base table.

2.1.2 Listing magazines

Listing of the magazines consists in recording all the characteristics of magazines present in the
machine, dividing them according to type. This list is managed by a single Magazine Table; to
view it, follow the procedure described below:

 from the main menu, press the softkey for the TABLES menu. The Tables Editor is displayed;

 press the softkey for the menu item MAGAZINE;

 using the arrow keys on the keyboard, select the file MEMORY; press Enter to confirm the

operation. A table will appear containing the following fields:

Magazine magazine number;

Maga type magazine type;

Pockets total number of tool holders in the magazine;

First Pocket number for the first physical tool holder in the magazine.

INFORMATION

To use the machine properly the operator must manage one magazine table only. This is the one
pre-set by BIESSE, which must always be active (selected).

To display the characteristics of the various tool holders, move onto the table and select the
magazine required, scrolling through the various lines in the columns. Press the softkey for the

BIESSE S.p.A. ©
(a207h004.fm-181103)

2 - 3

Chapter 2.
Notes on tooling

POCKET menu item to display the environment shown in the figure below

(*)

which illustrates a

magazine with 12 tool holders (known as pockets).

The 12 boxes depicting the tool holders in the magazine (pockets) use the following conventions:

 black box with white number: pocket free;

 green box with white number: master type pocket;

 green box with black number: overlap type pocket;

 red box with black number: incongruence in the definition.

The operator can modify the characteristics of the pocket (known as “reservation”) but not the
structure of the magazine. It is possible to make a “reservation” for single pockets or groups of
pockets, using the parameters in the input box shown below:

Start pocket :0
End pocket :0

Pocket type :0
Pocket mode :0

To display the input box, press the softkey for the menu item INIT POCKET. The fields in this box
have the following meanings:

(*). If the POCKET softkey is disabled you must
return to the Table Editor screen, press the softkey
for the menu item MAGAZIN, select the file MAGAZ.MAG
(using the LOAD softkey), exit (press EXIT) and then
access the magazine editor once more.

2 - 4

BIESSE S.p.A. ©

(a207h004.fm-181103)

Chapter 2.

Notes on tooling

 Start pocket and End pocket: set the number of the tool holder that starts and ends a group

of pockets that is to form part of a type of tool holder. For example: from pocket 1 (Start
pocket= 1) to 5 (End pocket= 5) the tool holders are of the master type (Pocket type=1). Start
pocket is the number of the first tool holder (pocket) occupied by the tool (master or overlap).

 Pocket type: set the type of tool holder to be assigned to a group of pockets, defined in the

preceding Start and End pocket fields. The following choices are available:

0. free pocket

1. master pocket

2. master pocket with overlap to the left

3. master pocket with overlap to the right

4. master pocket with overlap to left and right

 Pocket mode: set the pocket characteristics:

0 = tool holder destined for “random” type tools (i.e. with variable position);

1 = tool holder destined for “non random” type tools (i.e. with fixed position).

If any pockets have been reserved previously, before creating a new configuration for the
magazine it will be necessary to cancel all the existing reservations, setting the Input window as
follows:
in the field start pocket, the value corresponding to the first tool holder in the magazine;
in the field end pocket, the value corresponding to the last tool holder in the magazine;
in the field pocket type, the value 0 (free pocket).

2.1.3 Listing the tools in the magazine

Listing consists in recording the characteristics of the tools to be used with the machine. Tools, like
magazines, are managed using a single table (known as the Tool Table) in which the operator
enters all the data for the tools present in the machine.

To access the Tool Table, follow the procedure described below:

 from the main menu (main screen), press the softkey for the TABLES menu. The Tables

Editor is displayed;

 press the softkey for the menu item TOOL;

 using the arrow keys on the keyboard, select the file MEMORY; press Enter to confirm the

operation. A table will appear containing the following fields:

Code tool number;

Pocket number of the physical location of the tool in the magazine;

BIESSE S.p.A. ©
(a207h004.fm-181103)

2 - 5

Chapter 2.
Notes on tooling

Class class of tools (indicate whether the tool is of the “random” or “non random”

class);

Position position of the tool (indicate whether the tool is inside or outside the

magazine);

Spindle number of the electrospindle in which the tool is fitted.

The columns in the table only contain the principal parameters.

Once the table has been displayed, if the parameters for a tool are to be modified, use the arrow
keys to move the selection bar onto the record (line) required, and press the softkey for the menu
item EDIT. Another table is displayed, in which all the physical and geometrical characteristics of
the tools are indicated. The following fields are shown:

Tool code: 12 figure number, without sign, identifying the tool. Some of the figures in the code can

be used to indicate the family to which the tool belongs.

Tool Pocket: number between 1 and 12, identifying the position of the tool in the magazine.

Tool Class: number representing both the class of tool in the magazine, and the type of tool (1, 2

or 3 position). The class serves to specify whether a tool is “random”, that is to say it can be
housed in any pocket, or whether it is “non random”, that is to say it cannot be housed in any
pocket, but only in a set pocket.

The following values can be set in this field:

0 tool is of the “non random” type;

1 tool is of the “non random” type and occupies the location indicated in the Tool Pocket

field;

2 tool is of the “non random” type and occupies two locations (the one indicated in the

Tool Pocket field and the preceding one);

3 tool is of the “non random” type and occupies two locations (the one indicated in the

Tool Pocket field and the following one);

4 tool is of the “non random” type and occupies three locations (the one indicated in the

Tool Pocket field, the preceding one and the following one);

5 tool is of the “random” type and occupies the location indicated in the Tool Pocket

field;

6 tool is of the “random” type and occupies two locations (the one indicated in the Tool

Pocket field and the preceding one);

7 tool is of the “random” type and occupies two locations (the one indicated in the Tool

Pocket field and the following one);

8 tool is of the “random” type and occupies three locations (the one indicated in the Tool

Pocket field, the preceding one and the following one).

2 - 6

BIESSE S.p.A. ©

(a207h004.fm-181103)

Chapter 2.

Notes on tooling

INFORMATION

Remember that if a tool belongs to a certain class it must be housed in the pocket with which it is
compatible, which is set in the Magazine Table in the field Pocket mode.

Tool Status: number identifying the current status of the tool:

0 tool not ready.

1 tool ready.

If a tool is declared “not ready” this means it will be excluded from use. Requesting a tool that
is “not ready” will generate the error message “BAD TOOL CODE”. On the other hand, a tool
that is “ready” can always be used.

The status field can also be used to store a number of tools with the same code in the
magazine, with the tool to be used being marked “ready”.

Too l Position: number indicating the current position of the tool with respect to the magazine. A

value of 1 indicates that the tool is present in the magazine.

Offset Number: number between 1 and 300 that automatically defines the correction factor

associated with the tool, when the latter is not specified using the “T” programming function. If
this field is given the value 0, no correction factor is associated with the tool.

Position in Spindle: number identifying the electrospindle on which the tool is fitted. The value 0

indicates that the tool is in the magazine and not on the electrospindle.

Tool difference 2-1: (for TC machines only) number expressed in millimetres, between -5 and

+5, determining a correction along the Z

(*)

axis for the tool in electrospindle number 2.
Basically speaking, this number serves to compensate the difference in length between the
tool in electrospindle N° 2 and the one in electrospindle N° 1, when parallel machine
operations are to be carried out.

Tool difference 3-1: as above, applied to electrospindle number 3.

Max RPM Tool (for Excel RBM machine only): numerical value identifying the maximum number

of rpm for the tool; an invalid value will generate an error code.

(*). In actual fact the correction is applied to the electrospindle electronic setting axis.

BIESSE S.p.A. ©
(a207h004.fm-181103)

2 - 7

Chapter 2.
Notes on tooling

The drawing below illustrates the situation in a machining operation using three electrospindles in
parallel. In this case, the family of tools used is represented by a single data item in the Correctors
Table (offset). The data fields Tool difference 2-1 and Tool difference 3-1 (found in the Tool
Table) are used to indicate the “differences in length” between the tools that have been fitted in the
three electrospindles (TC machines only).

“U” axis setting 1(or pneumatic)“V” axis setting 2“W” axis setting 3

2

1

3

Z carriage

C

114

B

110

107

A

Ta bl e

A110, is the length of the tool in electrospindle 1.

B 107-110 = - 3, is the “difference in length” between the tool in electrospindle 3 and the one in

electrospindle 1.

C114-110 = 4, is the “difference in length” between the tool in electrospindle 2 and the one in

electrospindle 1.

INFORMATION

The values entered in the remaining fields in the Tool Table are automatically copied into the
Correctors Table (offset) to which they are connected. See paragraph “Tool characteristics” on
page 2 - 8 for a description of this.

Tool characteristics

The physical characteristics of the tools are described in the Correctors Table (offset). For any
clarification that may be required, please consult the “Machining Centre” software user’s manual.

The following are a few indications on how to use certain fields in the Correctors Table:

2 - 8

BIESSE S.p.A. ©

(a207h004.fm-181103)

Chapter 2.

Notes on tooling

Length 1; rated tool length value. By default, this corrector is associated with the Z axis when the

machine is turned on or after a reset. This means that when the offset is enabled this value
will be added to the programmed Z position.

Length 2; this has the same meaning and characteristics as length 1, but is associated by default

with the X axis.

Diameter; rated tool diameter value.

Different associations between Length 1, Length 2 and the coordinated axes can be obtained in
ISO programming using the AXO triliteral (consult the “Machining Centre” software user’s manual).

2.1.4 Listing tools in the Data Base Table

The characteristics of tools are stored in a table, the Data Base Table, in which it is possible to list
up to 500 tools.
In this environment it is possible to load, delete or modify tools and transfer data to the Tool Table.

To display the tool data base, proceed as follows:

 from the main menu (main screen), press the softkey for the TABLES menu;

 press the softkey for the menu item TOOL DATA BASE;

 using the arrow keys on the keyboard, select the file MEMORY; press Enter to confirm the

operation. A table will appear containing the following fields:

Description tool name;

Tool Code tool code;

Length 1 tool length 1;

Length 2 tool length 2;

Diameter tool diameter.

 once the table has been displayed, to access the specific characteristics of a tool, use the

arrow keys to move the selection bar onto the record (line) required, and press the softkey for
the menu item EDIT.

BIESSE S.p.A. ©
(a207h004.fm-181103)

2 - 9

Chapter 2.
Notes on tooling

2.1.5 Management of tools distributed over a number of magazines (for TC machines)

In the machines equipped with a number of electrospindles, management of the tools in the
magazines is based on a single Tool Table. The fact that there is only one table considerably
facilitates parallel machining operations which, in general, are the most common. In this case, all
the electrospindles taking part in the machining operation are tooled up with the same tools, each
one from its own magazine.

In special machining operations, in which it is necessary to use tools that, due to their number
and/or size, cannot be tooled up in a single magazine, it is necessary to resort to special tooling
and ISO programming operations. It is only possible to use a part of the configured tools,
according to the electrospindle selected. For example:

set electrospindle N° 1 (using function M501) to call up one of the tools inserted in pockets 1
to 18 (for TC machines), 1 to 12 (for TC machines) or 1 to 10 (for TCR machines);

set electrospindle N° 2 (using function M502) to call up one of the tools inserted in pockets 19
to 36 (for TC machines), 13 to 24 (for TC machines) or 11 to 20 (for TCR machines);

set electrospindle N° 3 (using function M503) to call up one of the tools inserted in pockets
pocket 37 to 54 (for TC machines), 26 to 39 (for TC machines) or 21 to 30 (for TCR
machines).

2.2 Saving a table

To save a table in the default directory “E:\TBL” from the “dual port” memory, proceed as follows:

1. Press the softkey corresponding to the menu item TOOL and select the file “MEMORY” to

open the table you require.

2. Press the softkey corresponding to the menu item SAVE MEMORY to display the directory

input window.

3. Create a copy of the file with another name, or call up the file and overwrite it. Press Enter to

confirm.

4. If you wish to overwrite the file, the system will request confirmation (Y= the table will be

saved; N= the table will not be saved).

INFORMATION

Files saved in the directory “E:\TBL” will be given the extension TOL, and it is possible to carry out
a backup of these files to floppy-disk using DOS SHELL.

INFORMATION

This procedure makes it possible to create a file that can be used by the Post processor
(Alphacam for Excel and Arrow machines) for management of tool change operations in “masked
time” (please see the Post processor manual for further details).

2 - 10

BIESSE S.p.A. ©

(a207h004.fm-181103)

Chapter 2.

Notes on tooling

2.3 Work table management

The operator can manage two types of work table:

 Normal: In this case the two tables are separate. The right hand one corresponds to the Y

axis, the left hand one to the W axis. In this way, the tables are independent axes and it is
possible to carry out pendular machining operations.

 Gantry: In this case the right and left hand table form a single axis, the Y axis. If a movement

of the Y axis is programmed the result will be a “synchronised” movement of both tables. In
this way, a machine with a single work table made up of two tables is obtained.

How to select the tables

1. From the main menu, access the AMP (machine parameters environment) directory list by
pressing the softkey for the item UTILITY and the softkey for the item AMP. An environment
containing the following fields is displayed:

RUNNING AMP; (top right hand box) represents the current configuration.

ACTIVATED AMP; (top central box) represents the active configuration. This will become
the current one the next time the system is turned on.

AMP DIRECTORY LIST; (large central box) represents the list of configurations that can
be used.

2. Inside the central box, scroll the selection bar down the list (using the arrow keys on the
keyboard) until it reaches the configuration you require. The configurations are indicated with
symbolic names and short comments; regardless of the name, they are presented in the
following order:

0 - normal.

1 - gantry.

(*)

2 - service.

3. Activate the configuration selected as above by pressing the softkey for the item ACTIVATE.
If the operation is successful, the symbolic name for the configuration selected will be
displayed in the top central box.

4. To make the configuration the current one (and therefore the one displayed in the top right
hand box), turn the control off and then on again.

For information on tooling-up of the work table, please consult the machine user’s manual.

(*). Item “1” in an AMP installed in a single table machine is empty, as gantry mode is not applicable
on this type of machine.

BIESSE S.p.A. ©
(a207h004.fm-181103)

2 - 11

Chapter 2.
Notes on tooling

2.4 Tool presetting

Tool presetting is the procedure by which, before carrying out the machining operation, the
dimensions of the tools and the positions of the electrospindles are adjusted. The dimensions of
the tools can be determined using the “pre-set”, an electronic device designed to carry out tool
registration and control operations.

For EP machines with patented electronic axis

The following describes how to adjust the tool along the Z axis, with respect to the piece to be
machined. This adjustment will affect the field length 1 in the Correctors Table (offset).

For single machining operations: the tool can be locked in the electrospindle without worrying

about its length (protrusion of the tool from the nose of the spindle).
For each tool involved in the machining operation it will be sufficient to measure the length
and enter it in the field length 1 in the Correctors Table.

For parallel machining operations: tools in the same family (perfectly identical tools fitted to

more than one electrospindle) may have minimum differences in length. To compensate for
these differences during machining operations it is necessary to enter the length of each tool
in the magazines and in the electrospindles in the field length 1 on the Correction table
(offset) and to insert the values for the “difference in length” of the tools in the “USER” variable
called “!DIFF.LR”.

enter the values for the length of tools in the magazine or in electrospindle N° 1 in the
“USER” variable “!DIFF.LR”.

INFORMATION

For information on how to use the variable “USER”, “!DIFF” please see Chapter 3. “Notes on

programming” on page 3 - 1.

For pneumatic EP machines

For parallel machining operations: Tools in the same family (perfectly identical tools fitted on
more than one electrospindle) may have minimum differences in length. The differences in length
from one tool to another may be compensated for by manual adjustment of the mechanical jacks
on each electrospindle.

For pneumatic TC machines

The following describes how to adjust the tool along the Z axis, with respect to the piece to be
machined. The length is the value in the field length 1 in the Correctors Table (offset).

The presetting operation varies according to whether the machining operations are single or in
parallel. This difference derives from the fact that, whereas in single machining operations each

2 - 12

BIESSE S.p.A. ©

(a207h004.fm-181103)

Chapter 2.

Notes on tooling

tool is able to intervene using its own length, in parallel operations this is not possible, as the tools
are grouped together and represented by one offset.

For TC or TCR machines with patented electronic axis

For parallel machining operations that use the same tool and a number of electrospindles, the
parameter Tool difference 2-1, Tool difference 3-1 and Tool difference 4-1, described in
paragraph 2.1.3 “Listing the tools in the magazine” on page 2 - 5, must be entered in the Tool
Table.

BIESSE S.p.A. ©
(a207h004.fm-181103)

2 - 13

Chapter 2.
Notes on tooling

2 - 14

BIESSE S.p.A. ©

(a207h004.fm-181103)

3

-

Chapter 3. Notes on programming

A thorough knowledge of standard ISO programming procedures is necessary when reading this
chapter. In this regard it is recommended that you read all the parts of the “Machining Centre”
Software user’s manual that deal with the basic instructions for creation of a program.

3.1 Tool change

The following paragraphs show various examples of how to carry out a tool change operation
within a machining program, or by means of manual data input (using the MDI command).

Automatic tool change

Within a program, to change the tool being used for machining operations it is necessary to:

1. set function T to call up the new tool.

2. set function M7 and the associated offset, or the offset specified with function M6, to enable
tool change.

Examples:

MDI Programming

Line

T1 M6 M7 loads tool 1 and enables the connected offset

T1.3 M6 M7 loads tool 1 and enables the specified offset 3

Description of Programming Line

T.2 M6, T0.2 M6 enables offset 2 without changing the working tool

T0 M6 M7, T0.0 M6 M7 removes the tool (without changing it with others) and disables

the offset

T.0 M6 disables the offset and keeps the tool

T1.0 M6 M7 loads tool 1 and disables the offset

BIESSE S.p.A. ©
(a210h003.fm-181103)

3 - 1

Chapter 3.
Notes on programming

Useful tips:

 It is possible to carry out a tool change operation even if the machine is carrying out another

operation (for example while the boring unit is working).

 In certain cases, the working conditions of the machine and the size of the tools fitted in the

tool change device might, during tool change operations, result in a collision between it and
the unit carrying out machining operations. It is the job of the operator to program the function
M7 in such a way as to make it coherent with the functions being carried out by the machine.

 If function M7 is entered in a program in which a tool change operation is requested, it will

temporarily block performance of subsequent functions M3, M4, M5, M7, M10, M11 M20,
M30,M32, M91, M92, M93, M94 and of the requests for movement of axes A, B, C, D (if they
belong to the electrospindles involved in the tool change).

INFORMATION

Consult paragraph ( C.2 “Semantic checks effected by the PLC” in Appendix C. “PLC Messages”)
for further clarification on the use of these functions.

INFORMATION

For the Excel RBM machine the code M7 blocks performance of subsequent functions until the
machine has completed the tool change.

Manual tool change

DANGER

This operation must only be carried out by the operator to deal with blockage of the
machine, and in any case not before reading the paragraphs relating to the controls,
management of the electrospindle and the tool magazine, and the tool change sequence.
The operator is the only person responsible for any damage to the machine that may result
from incorrect performance of this operation.

DANGER

Manual tool change operations will not modify or update the tool table.

In automatic management of tool change operations various controls and synchronisation
operations take place, aimed at proper completion of the tool change operation itself. For example,
the control carries out the following operations:
unlocking of the tools from the electrospindle only after locking them in the tool change device,
which in the meantime has picked them up;
unlocking of the tools in the automatic tool change device only after locking them in the magazine
tool holder;
restarting of the tool change device and returning it to the start position.

On the other hand, for manual management of tool change operations, control of the above
operations is extremely limited.
Then again, manual operations must be carried out using the tooling button pad and not the

3 - 2

BIESSE S.p.A. ©

(a210h003.fm-181103)

Chapter 3.

Notes on programming

control, so as to ensure that an error on the part of the latter will not prejudice the ability to restore
tooling operations manually.

INFORMATION

When training staff it is recommended that a number of test tool change operations be carried out
on an empty machine, without installing tools in the magazine. This makes it possible to check
movement of the automatic tool change device and control actions.

To carry out manual tool change operations, the machine must be made to repeat the exact
sequence of operations described in the Machine user’s manual, following the procedure given
below:

 For TC machines:

1. Turn the selector provided (see Machine user’s manual), located on the Pilot Panel, to
MANUAL mode.

2. Select the electrospindle on which the tool change operation is to be carried out.

3. Completely raise the boring unit and the suction box.

4. Turn the automatic tool change device, so that it can pick up the tools in the pocket
required and in the electrospindle.

5. Command unlocking of the pocket required and of the electrospindle.

6. Turn the selector provided (see Machine user’s manual) so that the tool change device
lowers to extract the tools, rotates by 180° to change the positions of tools, rises again
to insert the tools in their housings.

7. Command locking of the current pocket and of the electrospindle.

8. Turn the selector (see Machine user’s manual) to return the tool change device to the
parked position.

 For TCR machines:

1. Turn the selector provided (see Machine user’s manual), located on the Pilot Panel, to
MANUAL mode.

2. Select the electrospindle on which the tool change operation is to be carried out.

3. Completely raise the boring unit and the suction box.

4. Turn the selector (see Machine user’s manual) to insert the revolver tool magazine tool
holder in the electrospindle.

5. Command unlocking of the electrospindle.

6. Turn the selector (see Machine user’s manual) to extract the tool from the
electrospindle.

7. Turn the selector (see Machine user’s manual) to turn the revolver tool magazine to the
position required.

8. Turn the selector (see Machine user’s manual) to insert the tool in the electrospindle.

BIESSE S.p.A. ©
(a210h003.fm-181103)

3 - 3

Chapter 3.
Notes on programming

9. Turn the selector (see Machine user’s manual) to lock the tool in the electrospindle.

10. Turn the selector (see Machine user’s manual) to extract the revolver tool magazine
tool holder from the electrospindle.

 For the Excel RBM machine:

The Excel RBM machine uses two auxiliary tool magazines, located at the two ends of the X
carriage, which can each contain one aggregate for circular blade tool with HSK63 type
coupling only.
In the case of automatic tool change the NC is able to distinguish both the pocket to which the
aggregate belongs and the auxiliary magazine housing it. The tools in the magazines must be
of the “non random” type, as once they have been picked up they must be returned to the
same tool holder.
If, during loading/unloading of the tool from the auxiliary magazine, there is an interruption in
the tool change operation, correct positioning of the two auxiliary magazines must be restored
using the “Tooling button pad".

In the Excel RBM it is not possible to carry out manual tool change operations. The only
manual operation possible is resetting of the tool change operation when an emergency stop
is triggered in the machine during an automatic machining cycle. This operation is carried out
in full safety using the “Tooling button pad”. To carry out manual operations, follow the
instructions provided below:

1. Press the emergency button and turn the key selector to the manual position, to enable
the “Tooling button pad".

2. Turn the MODE selector on the Pilot Panel to manual.

INFORMATION

All the “Tooling button pad” and Pilot Panel functions are described in the Machine user’s
manual.

DANGER

Blockage of the tool change operation, due to triggering of an emergency button and
subsequent shutdown of the machine, will not modify or update the tool table.

3 - 4

BIESSE S.p.A. ©

(a210h003.fm-181103)

Chapter 3.

Notes on programming

3.2 Programming functions

Programming is carried out in a software environment that is described in detail in the "Machining
Centre" Software user’s manual. In this environment it is possible to create a part program by
drawing up “blocks” containing the functions required to make the machine carry out certain
commands, written in standard ISO language.

INFORMATION

For further clarification of the meaning and use of these “blocks”, please see the "Machining
Centre" Software user’s manual.

The functions examined and explained in detail are the “M” functions; a short paragraph is
dedicated to the S, T, F and G functions (for further information, consult the “Machining Centre”
Software user’s manual).

INFORMATION

For a correct interpretation of the direction of axes, please see the "Machining Centre" Software
user’s manual

DANGER

Do not attempt to modify the machine management programs and the control
configurations. BIESSE will not be held responsible for any damage to persons or property
deriving from modifications made without prior approval.

Brief notes on S, T, F, G functions

S function: this function specifies the electrospindle rotation speed. It is set by typing the

character “S”, followed by a positive whole number, which must be higher than or equal to 100
and lower than or equal to 18000.
This function can be entered manually, with the command MDI, or set from within the program
before the electrospindle rotation function (M3 - M4). If, in the program, function M3 (or M4) is
not preceded by an S function, an error is triggered.

T function: this function defines the tool and the corrector required for the machining operation. It

must be followed by two values separated by a dot, e.g. T X.Y.
Values X and Y must be a positive whole number higher than or equal to 300. These values
identify an offset, contained in a special table (see "Machining Centre" Software user’s
manual). An Offset value set previously can be cancelled using the function T.0.
After setting a T function it is necessary to insert the function M7, which enables the tool
change, and M6 which enables the offset identified by the function T. If, in the program, the
function M6 or M7 is not preceded by a T function, an error is triggered.

INFORMATION

For proper management of the correctors, please refer to the contents of paragraph “Tool

characteristics” on page 2 - 8.

BIESSE S.p.A. ©
(a210h003.fm-181103)

3 - 5

Chapter 3.
Notes on programming

F function: this function defines the speed of advance of the axes. It can be programmed within

the interval +0.00001 - +99999.99999. However, if the programmed speed is higher than the
maximum speed of the axis, the control will display the speed that has been programmed, but
will work at the maximum speed allowed.

To interpret the function "F" additional codes, called "G", are used. These are:

 G70 programming in inches;

 G71 programming in millimetres;

 G93 time required by the axes to reach a specific point. For example, if the following program

block is entered
X100 Y200 F1
the axes will advance at a speed of 1 mm per minute.
Whereas by entering
G93
X100 Y200 F1
the axes will reach the programmed position in 1 second.
Function G93 is used to change the speed of advance "F1", which is expressed in millimetres

per minute, into the time required to advance, expressed in sec

-1

.

 G94 speed of advance in millimetres/minute or in inches/minute;

 G95 speed of advance in millimetres/turn or in inches/turn.

It is also possible to use a value “t”. This function automatically calculates the time required by the
axes to carry out a certain movement towards a specific position. It is only valid within the block in
which it is programmed (example: G1 X 1000 t10 = t function is active; G1 Y -500 = t function is not
active).

3.2.1 M functions

M functions are used to enable various machine operations. This command is set by inserting the
character M in a program line, followed by a number code, which can be between 0 and 999.

It is not possible to insert more than 4 M functions in one program line.

INFORMATION

In the "Machining Centre" Software user’s manual there is a chapter describing certain M
functions: it is important to remember that these descriptions merely serve as an example.

CAUTION

Not all M functions can be enabled with the machine in hold (HOLD).

The M functions can be “modal”, “non modal”, “prelude” or “postlude”.

3 - 6

BIESSE S.p.A. ©

(a210h003.fm-181103)

Chapter 3.

Notes on programming

Modal and non modal M functions

A modal M function is a function that requires the presence of another function of the same
category in order to be cancelled (example: a 501 requires the presence of a 502). Non modal M
functions, on the other hand, are cancelled immediately after they are carried out. Thus, whereas
the “modal” M function remains active and is displayed on the numerical control monitor until
another function in the same category is read, which will then take its place, “non modal” M
functions will disappear from the screen once they have been carried out.

There are also “modal” M functions that behave differently. For example, the function M5 (stop
electrospindles) is modal and in the same category as M3 or M4 (clockwise and anticlockwise
rotation of electrospindles) but, after being read and carried out, it will only be displayed on the
monitor for a few seconds before disappearing.

Prelude and postlude M functions

The “prelude” M function is a function that, regardless of its position within a program line, is
activated by the NC before movement of the axes.
Vice versa, the “postlude” M function is a function that, regardless of its position within a program
line, is activated by the NC after movement of the axes.

3.2.2 List of M functions

As the M functions are created and managed exclusively by BIESSE, always use the information
provided in this chapter when consulting and using them.

CAUTION

The references made to these functions in the "Machining Centre" Software user’s manual
are for explanatory purposes only. The table provided in this paragraph, with the relative
notes, is therefore the only source officially recognised by BIESSE. It also contains a
description of certain M functions that relate to functions or devices not present on all
machines. These functions must be interpreted taking into account the following points.

The machines manufactured by BIESSE differ from one another in size, devices and functions.

As the table of “M” functions provided here takes into account all the functions available in
standard BIESSE machines, it is necessary to note one or two points when reading and
interpreting the descriptions:

 The electrospindle selection codes only act on the ones that are actually present in the

machine; thus if, for example, the function M 535 (select electrospindles 1, 3, 5 and 7) is
programmed in a machine whose configuration includes only one electrospindle, only
electrospindle N° 1 will be used.

 For the axis identification codes, please refer to the Machine user’s manual.

BIESSE S.p.A. ©
(a210h003.fm-181103)

3 - 7

Chapter 3.
Notes on programming

 Some elements (for example the boring unit or certain types of stop) may not be present in

your machine, and the operator should ignore the M functions that relate to these elements.

INFORMATION

Remember that programming of a code dedicated to a function or to control of a device not
present on the machine will not generate any part program interpretation error, and will merely be
ignored by the machine logic.

3 - 8

BIESSE S.p.A. ©

(a210h003.fm-181103)

Chapter 3.

Notes on programming

“M” FUNCTIONS TABLE

Description of the columns in the table:

 M: list of M codes.

 PRELUDE: indicates whether a function is a prelude or a postlude; YES = prelude; NO =

postlude.

 HOLD: indicates whether or not a function can be enabled when the machine is in hold; YES

= function can be enabled; NO = function cannot be enabled.

 DESCRIPTION: description of the function

M Prelude Hold Description

M0 NO NO Program suspensions

M3 YES NO Clockwise rotation of the electrospindles or optionals

M4 YES NO Anticlockwise rotation of the electrospindles or optionals

M5 NO NO Stop rotation of the electrospindles or optionals

M6 NO NO Activate a new offset

M7 YES NO Change tools

M8 YES NO Turn boring units on

M9 NO NO Turn boring units off

M10 YES NO Lower electrospindles or optionals

M11 YES NO Lower electrospindles in floating mode

M12 YES YES Lower boring units

M13 YES YES Negative inclination of optional

M14 YES YES Positive inclination of optional

M15 NO YES Enable optional bistable electrovalve 1 (right table)

M16 NO YES Enable optional bistable electrovalve 2 (right table)

M17 NO YES Enable optional bistable electrovalve 3 (right table)

M18 NO YES Enable optional bistable electrovalve 4 (right table)

M19 YES YES Enables lowering of the mechanical presser.

M20 NO YES Raise electrospindles or optionals

M22 NO YES Raise boring units

M23 NO YES Reset tilting in rest position

M25 YES YES Disable optional bistable electrovalve 1 (right table)

M26 YES YES Disable optional bistable electrovalve 2 (right table)

BIESSE S.p.A. ©
(a210h003.fm-181103)

3 - 9

Chapter 3.
Notes on programming

M Prelude Hold Description

M27 YES YES Disable optional bistable electrovalve 3 (right table)

M28 YES YES Disable optional bistable electrovalve 4 (right table)

M29 YES YES Enables raising of the mechanical presser.

M30 NO NO End of program reset

M31 YES YES Couple locking selectors

M32 YES YES Start blower

M33 YES YES Enable composition of electrospindle selection codes

M35 NO NO Enable optional bistable electrovalve 1 (left table)

M36 NO NO Enable optional bistable electrovalve 2 (left table)

M37 NO NO Enable optional bistable electrovalve 3 (left table)

M38 NO NO Enable optional bistable electrovalve 4 (left table)

M39 NO YES Optional milling unit with blade in X direction

M40 YES YES Optional milling unit with blade in Y direction

M41 NO YES Uncouple locking selectors

M42 NO YES Stop blower

M43 YES YES Disable composition of electrospindle selection codes

M45 NO NO Disable optional bistable electrovalve 1 (left table)

M46 NO NO Disable optional bistable electrovalve 2 (left table)

M47 NO NO Disable optional bistable electrovalve 3 (left table)

M48 NO NO Disable optional bistable electrovalve 4 (left table)

M52 YES YES Enable mechanical copier blower

M54 NO YES Stop out on left and right table

M55 NO YES Stop out on right table

M56 NO YES Stop out on left table

M57 NO YES Right table pallet outfeed

M58 NO YES Left table pallet outfeed

M62 YES YES Disable mechanical copier blower

M64 YES YES Stop in on left and right table

M65 YES YES Stop in on right table

M66 YES YES Stop in on left table

M67 YES YES Right table pallet return

M68 YES YES Left table pallet return

3 - 10

BIESSE S.p.A. ©

(a210h003.fm-181103)

M Prelude Hold Description

M70 YES NO Lock vacuum on right table

M71 YES NO Lock vacuum on left table

M72 YES NO Lock vacuum on left - right table

M78 YES NO Select supplementary vacuum areas

M80 NO NO Unlock vacuum on right table

M81 NO NO Unlock vacuum on left table

M82 NO NO Unlock vacuum on left - right table

M90 YES YES Select level for supplementary box 6-10

M91 YES YES Suction box at level 1

M92 YES YES Suction box at level 2

M93 YES YES Suction box at level 3

Chapter 3.

Notes on programming

M94 YES YES Suction box at level 4

M95 YES NO Suction box at level 5

M96 YES NO Right and left NC stops in parked position

M97 YES NO Right NC stops in parked position

M98 YES NO Left NC stops in parked position

M99 YES YES Lower suction boxes down for cleaning

M100 NO YES Raise boring and milling unit tools

M101 YES YES Select vertical bit 1 in the boring unit

M102 YES YES Select vertical bit 2 in the boring unit

M103 YES YES Select vertical bit 3 in the boring unit

M104 YES YES Select vertical bit 4 in the boring unit

M105 YES YES Select vertical bit 5 in the boring unit

M106 YES YES Select vertical bit 6 in the boring unit

M107 YES YES Select vertical bit 7 in the boring unit

M108 YES YES Select vertical bit 8 in the boring unit

M109 YES YES Select vertical bit 9 in the boring unit

M110 YES YES Select vertical bit 10 in the boring unit

M111 YES YES Select vertical bit 11 in the boring unit

M112 YES YES Select vertical bit 12 in the boring unit

M113 YES YES Select vertical bit 13 in the boring unit

M114 YES YES Select vertical bit 14 in the boring unit

BIESSE S.p.A. ©
(a210h003.fm-181103)

3 - 11

Chapter 3.
Notes on programming

M Prelude Hold Description

M115 YES YES Select vertical bit 15 in the boring unit

M116 YES YES Select vertical bit 16 in the boring unit

M117 YES YES Select vertical bit 17 in the boring unit

M118 YES YES Select vertical bit 18 in the boring unit

M119 YES YES Select vertical bit 19 in the boring unit

M120 YES YES Select vertical bit 20 in the boring unit

M121 YES YES Select vertical bit 21 in the boring unit

M122 YES YES Select vertical bit 22 in the boring unit

M123 YES YES Select vertical bit 23 in the boring unit

M124 YES YES Select vertical bit 24 in the boring unit

M125 YES YES Select vertical bit 25 in the boring unit

M126 YES YES Select vertical bit 26 in the boring unit

M127 YES YES Select vertical bit 27 in the boring unit

M128 YES YES Select vertical bit 28 in the boring unit

M129 YES YES Select vertical bit 29 in the boring unit

M199 YES YES Lower selected boring and milling unit tools

M201 YES YES Select horizontal bit 1 in the boring unit

M202 YES YES Select horizontal bit 2 in the boring unit

M203 YES YES Select horizontal bit 3 in the boring unit

M204 YES YES Select horizontal bit 4 in the boring unit

M205 YES YES Select horizontal bit 5 in the boring unit

M206 YES YES Select horizontal bit 6 in the boring unit

M207 YES YES Select horizontal bit 7 in the boring unit

M250 NO NO 5-axis milling unit enable

M260 NO NO 5-axis milling unit disable

M296 YES NO Right and left NC stop multipositioning

M297 YES NO Right NC stop multipositioning

M298 YES NO Left NC stop multipositioning

M301 YES YES Select blade 1 in the boring and milling unit

M500 YES YES Select all electrospindles

M501 YES YES Select electrospindle 1

M502 YES YES Select electrospindle 2

3 - 12

BIESSE S.p.A. ©

(a210h003.fm-181103)

M Prelude Hold Description

M503 YES YES Select electrospindle 3

M504 YES YES Select electrospindle 4

M505 YES YES Select electrospindle 5

M506 YES YES Select electrospindle 6

M507 YES YES Select electrospindle 7

M508 YES YES Select electrospindle 8

M509 YES YES Select electrospindle 9

M517 YES YES Select electrospindles 1, 4 and 7

M519 YES YES Select electrospindles 1, 3, 5, 7 and 9

M528 YES YES Select electrospindles 2, 5 and 8

M535 YES YES Select electrospindles 1, 3, 5 and 7

Chapter 3.

Notes on programming

M539 YES YES Select electrospindles 3, 6 and 9

M546 YES YES Select electrospindles 2, 4, 6 and 8

M600 YES YES Select all optionals

M601 YES YES Select optional 1

M602 YES YES Select optional 2

M603 YES YES Select optional 3

M604 YES YES Select optional 4

M700 YES YES Select all boring units

M701 YES YES Select boring unit 1

M702 YES YES Select boring unit 2

M703 YES YES Select boring unit 3

M704 YES YES Select boring unit 4

Using the M codes

M3, M4: these functions are only accepted if:

- an electrospindle selection is active;

- the electrospindles are stopped;

- a speed greater than or equal to 100 rpm and lower than or equal to 18000 rpm has been
programmed;

- a collet spindle is inserted in each of the electrospindles selected;

BIESSE S.p.A. ©
(a210h003.fm-181103)

3 - 13

Chapter 3.
Notes on programming

- the electrospindles are enabled using the special key selector, and are in the working
position (down).

Z

M4

M3

Y

X

M3 - M4

M6, M7: if a T function has not been programmed beforehand, the logic does not have enough

data to carry out the operation, and the function M6 or M7 is therefore refused (“M function
not allowed”). If a T function involving a tool change has been programmed, the function M7 is
accepted if the electrospindles are stopped and selected (for example M501) and the
revolving axes (if present) are at 0. For further clarification on programming of the tool change
operation, please read paragraph 3.2 “Programming functions”.
Should it be necessary to carry out an automatic tool change, the electrospindle and the
suction box will be made to rise automatically.

WARNING: consult paragraph 3.1 “Tool change”.

M8: accepted if a selection is active in the boring unit.

M11: if an electrospindle is down, it can be made to float (by selecting an electrospindle, for

example M501, and then setting the function M11) without first making it rise. However it is
not possible to do the reverse: to pass from floating electrospindle to electrospindle down it is
first necessary to raise the electrospindle.

M13; M14; M23: the horizontal milling unit can tilt in 2 directions: positive and negative. Before

changing the inclination, select the function M23 to position the milling unit parallel to the work
table.

M23

M23

M14

M13

M15 to M18; M25 to M28; M35 to M38; M45 to M48: these functions activate the optional

electrovalves to which special devices (supplied by BIESSE or by the client) can be
connected.

M30: equivalent to pressing the RESET button.

3 - 14

BIESSE S.p.A. ©

(a210h003.fm-181103)

Chapter 3.

Notes on programming

M31; M41: when simultaneous vacuum in areas 1, 2 or 3, 4 of each table is required, the function

M 31 makes it possible to use a single blocking selector (1, 2 and 3, 4) instead of all the
corresponding ones. Function M 41 is used to disable this option.

M32; M42: these functions enable and disable the blower on the electrospindle selected by the

relative M code only (M500. M502).

M33; M43: M33 enables selection of active electrospindles. See paragraph “Description of code

M33” on page 3 - 17.

M54; M55; M56; M64; M65; M66: these must be inserted in a program to raise and lower the side

stops. Always lower the stops before running a program.
The stops are lowered automatically by the PLC when functions M70, M71 or M72 (vacuum
area enabling/disabling) are inserted.

M57; M58: these functions can be inserted in the program to move the Pallets towards the loading

position, called "Pallet out". The pallets are only moved if the tables are in position 0 (zero). If
this is not the case an error message will be displayed. In Gantry mode it is sufficient to use
just one of these two codes to move the pallet out.

M67; M68: these functions can be inserted in the program to move the Pallets towards the working

position, called "Pallet in", after loading the piece. In Gantry mode it is sufficient to use just
one of these two codes to move the pallet in.

M78: if this function precedes one of the piece locking or unlocking commands, the auxiliary

vacuum area is associated with the vacuum areas selected previously. M78 is disabled by a
subsequent piece locking or unlocking command or by M30 (reset).

M91 to M94: these functions command movement of the suction box to the levels required for

proper suction during machining operations. For proper use, and to avoid rapid deterioration
of the bristles A and the bellows B, make sure that the box is not too close to the piece during
machining operations. The following figure indicates the minimum distance that must be left
between the bottom edge of the box and the surface of the piece.

B

min 40 mm

A

PANEL

M96 to M98: these functions return the NC rear stops to the bottom of the work table (position 0).

M250 and M260: These functions allow enabling or disabling the machining operation with RB

milling unit. Both codes require use of the code M501 or M502 to be able to select the
operating section to which the RB milling unit belongs (M501 for the first, M502 for the
second). Failed omission of one of these two codes before code M250 and/or M260 causes
the machine to lock.

BIESSE S.p.A. ©
(a210h003.fm-181103)

3 - 15

Chapter 3.
Notes on programming

M500 to M549: these functions select the electrospindles. The functions inserted in the program

after functions M5XX (for example M3 or M4) will only have an effect on the selected
electrospindles.

M700 to M734: these functions have the same purposes as codes M5xx, but they operate on the

boring units.

Types of “M” functions

The M functions can be divided into three different types:

1. Functions in which a specific action is required on a certain subject. Example: function M35
specifies the action (enabling) and the subject (optional bistable electrovalve 1).

2. Functions in which one or more subjects are identified. Example: function M501 (select
electrospindle 1) identifies a subject, electrospindle 1.

3. Functions that require actions. Example: function M3 (clockwise rotation of electrospindles)
requires an action, rotation of the electrospindles.

The third type of function require, during the programming procedure, the identification of a subject
on which to carry out the action. Thus, if electrospindle n° 2 is to be lowered, it will be necessary to
program the subject, electrospindle 2 (M502) and the action, lower electrospindles (M10), using
the following sequence:

..........

M502

..........

M10

..........

If an action is requested using a function of the third type, without specifying the subject, the logic
will display an error message (for example “electrospindles not selected”).

Description of code M0

Code M0 makes it possible to carry out suspensions of the part program. This means that, when
inserted in a program “block”, it causes temporary interruption of the program at the line
immediately following the code M0.

 To resume the program after suspension, press the START CYCLE button, located on the

Pilot panel or on the supplementary button pad.

 To bypass a code M0 press the START CYCLE button on the Pilot panel. This operation is

only valid for the first code M0 carried out by the program after the START CYCLE button has
been pressed.

 To bypass the end of machining code M0 press the START CYCLE button on the

supplementary button pad. This operation is known as “start reservation”. It is useful when

3 - 16

BIESSE S.p.A. ©

(a210h003.fm-181103)

Chapter 3.

Notes on programming

carrying out pendular machining operations, and serves to reserve machining operations on
one table in advance, while the machine is still working on the other table. The part program
will bypass the code M0, thus allowing the machine not to stop when the machining operation
has been completed, but to move directly to the other table. Reservation is indicated by
flashing of the green start button indicator on the supplementary button pad. Pressing the
START CYCLE button again during reservation will cancel the reservation, and the machine
will proceed as though that reservation had never been requested.

Description of code M33

Code M33 (enable composition of electrospindle selection codes) allows the operator to create
“temporary” program blocks using a number of electrospindles which cannot be programmed
merely using the functions M5XX, because they are not included in the list of M functions.

For example:

 For a machine with 9 electrospindles in line, to select electrospindles N° 1, 4 and 7, lower

them and make them turn simultaneously, simply set the following functions:

[...]
M 517
M 10
M 3
[...]

in which codes M10 (lower electrospindles) and M3 (clockwise rotation of electrospindles) act
on the last modal code entered, M 517 (electrospindles n° 1, 4 and 7).

 Let us suppose that (again for a machine with 9 electrospindles in line) the operation

described above is to be carried out by electrospindles n° 3 and 4 (not included in a single
M5XX function). If the functions are set as follows:
[...]
M 503
M 504
M 10
M 3
[...]
only electrospindle n° 4 will be lowered and turned (M 504, because codes M 10 and M 3 only
act on the last modal

code entered (M504). Furthermore, the M 5XX codes are exclusive, so
that M 504 excludes M 503.
This problem is solved by inserting, before and after the two modal, exclusive functions (M
503, M 504), the function M33 and the function M43. The sequence of blocks to be inserted in
the control is as follows:
[...]
M33
M503
M504
M43
M10
M3
[...]
where M 33 and M 43, which represent enabling and disabling of electrospindle selection
code composition, respectively, must open and close the sequence of blocks, so as to make it

BIESSE S.p.A. ©
(a210h003.fm-181103)

3 - 17

Chapter 3.
Notes on programming

modal. In this way, codes M503 and M504 are “added together”. The codes that follow (M10
and M3) act on the whole sequence of blocks; thus M10 will command lowering of
electrospindles n° 3 and 4, and M3 will make the electrospindles turn. The selection
preceding M33 is cancelled by M33 itself.

Functions M33 - M43 have the same effect on all types of electrospindle. Code M33 cancels
all active electrospindle selections.

3.3 Notes on the use of revolving axes

Due to overlap, when the milling unit is up (with reference to the pneumatic disconnection point for
the unit) a tool fitted in the electrospindle cannot be tilted to all positions; this is because the tool
might hit the Z carriage or the automatic tool change device.

To limit the risk of collision, the machine logic sets the following restrictions:

 If the position of the revolving axis is not 0, the electrospindle manual raising function is

disabled, and programming of functions M20 and M7 is refused (“M function not allowed”).

 The revolving axis of an electrospindle in the “forced up” position is locked. This state is

indicated by a letter “L” alongside the axis position; programming of a locked axis will not
result in any movement or generate any error message.

DANGER

When an electrospindle is in the up position but not in the “forced up” position, the
revolving axis is not locked, so that any programmed movement of the axis will be carried
out normally; in this situation there is a risk of collision.

DANGER

When resetting the revolving axis of an electrospindle in the up position, make sure that it
is not fitted with any angled tool or aggregate.

When the machine reverts to emergency mode, the axes move slightly from their position: this
change in position will cause the revolving axis, which is set to position zero, to introduce the
restrictions described above.

INFORMATION

When an angled aggregate previously mounted on another electrospindle is used, its reference
dowel must be re-adjusted, to avoid unsafe locking or excessive play.

3 - 18

BIESSE S.p.A. ©

(a210h003.fm-181103)

Chapter 3.

Notes on programming

Tilting axis

The rotating axis C, when fitted in the electrospindle that is also fitted with the Tilting axis, cannot
be moved when the electrospindle is in the up position.

INFORMATION

After turning the machine on it is recommended that you lower the electrospindle and reset the
axes before moving the Tilting axis.

DANGER

If, during automatic execution of a program, the tilting axis is moved with the electrospindle
up an emergency will be triggered in the machine. Restore the machine to normal operation
manually. Using the selector provided (see machine user’s manual), lower the
electrospindles to the working position and re-position the tilting axis at Ø.

DANGER

Before turning the machine off, remove the aggregates fitted on the electrospindle using
the automatic NC procedure in MDI mode: M500 TØ M7; press ENTER and then START
CYCLE.

3.4 Control variables

The control variables are user variables that can be used as a logic interface between machine ­operator/program to enable or disable the controls carried out while the part program is running.
The value of these variables can be defined in two ways:
within the part program, as an MDI instruction;
in an “input box”, which is displayed by pressing the softkey for the item VARIABLES and the
softkey for the item PLUS VARIABLES.

Performing a reset will bring all the user variables back to their default values.

The following paragraphs illustrate and describe some of the variables present in the “input box”.

1 - Vacuum area unlocking control variable

@HOLD: the value 0 is set as the default value; in this condition, if a piece is unlocked during

a machining cycle an emergency is triggered in the machine.
On the contrary, when the value set is 1, if a piece is unlocked during a machining cycle the
machine will revert to hold.

:

After requesting and obtaining, or confirming locking of a vacuum area using an M function,
the machine logic controls the status of the vacuometer for the area selected. If the vacuum
level drops below the one set on the vacuometer for the selected area there is the prospect of
a potential danger: expulsion of the piece due to the thrust exerted on it by the tool and the
axes. To prevent this danger situation, the logic forces stoppage of the machine in the mode
selected by the operator using the variable @HOLD.

BIESSE S.p.A. ©
(a210h003.fm-181103)

3 - 19

Chapter 3.
Notes on programming

Stoppage of the machine in emergency (default condition) is preferable to stoppage in hold,
as it is quicker and leaves the machine with all power actuators deactivated.

Stoppage in hold may be necessary in particular circumstances when, during the initial stage
of locking, the vacuum value is not stationary and may generate situations difficult for the
logic to interpret correctly. In this case hold mode does not prevent machining operations from
being continued.

DANGER

Management of unlocking operations in hold must only be used if it is not possible to
adjust the vacuometer in a suitable manner.

2 - Rapid movements control variable

@ASYNC: value 0 is the default value; the machine PLC waits until the current electrospindle

and/or boring unit have risen before carrying out rapid movements (G00) of the X, Y and W
axes. The only rapid movement that does not generate this wait is raising of the Z axis.

By setting the value 1 the machine PLC does not wait until the current electrospindle and/or
boring unit have finished rising before moving the axes. Thus, the operator can only activate
this control variable if he is certain that the Z axis has first been made to rise to a “safe”
position. This is to prevent axes X, Y and W from hitting the lowered Z axis while performing
rapid movements.
The value of this variable remains unchanged until it is programmed again; resetting the NC
returns it to the default value.

3 - Pallet movement control variable

(for Arrow machines only)

@UDAPALLET: 0 is the default value.

If the value is set to 1, the two pallets will connect mechanically before carrying out the
movement, and will disconnect again after the movement has been completed.

The value of the variable will remain unchanged until it is programmed again; if the NC is
reset, the variable will return to the default value.

4 - Control variable to check any collisions between the NC stops and the machine parts

@COLLISION: the value 1 is the default condition.

Setting the value 1, the controls are enabled to prevent that the rear NC stops collide with
some parts of the machine. During stop positioning (multipositioning and programmed
position) if the tables are not loaded it is prohibited to call the NC stops. If the NC stops are
not moved to the rest position, this operation is carried out automatically by the PLC.
Setting the value 0, the controls are disabled to prevent collisions.

To reset the default conditions, press the RESET key.
When programming, always check that the stops do not collide with other parts of the
machine. It is recommended to use this variable to prevent possible dangerous conditions
due to forgetfulness.

3 - 20

(a210h003.fm-181103)

BIESSE S.p.A. ©

Chapter 3.

Notes on programming

3.5 Dedicated programming variables

The dedicated programming variables are user variables which can be used as machine ­operator/program interface logic, and they are used in place of the parameters so as to make the
program more easy to understand.

To display the programming variables “input box”, from the main menu press the softkey for the
item VARIABLES and the softkey for the item USER VARIABLES.

1 - Description of the multipositioning variables for the NC rear stops

!PPOS(n); “n”th position of the NC stop “p”

!QPOS(n); “n”th position of the NC stop “q”

Multipositioning for the NC rear stops “p” and/or “q” consists in the ability to move these stops
to a series of positions (maximum 10) while the machine is working on the other table, i.e.
without having to insert in the part program a series of successive positions separated by the
code M0 (which would have the effect of not allowing machining on the other table during
loading of this one).

Program syntax:

!PPOS1=1234.56789 !PPOS: name of the stop, i.e. "p"

1: number of the position (from 0 to 9)
1234: positioning level of the stop in millimetres (whole numbers)
56789: positioning level of the stop in millimetres (figures after the
decimal point)

After assigning the positions for stops, it is necessary to enter the M code for the stop/s for
which this mode is to be enabled.

When the function is enabled, the start buttons on the supplementary button pads will flash,
and each time they are pressed the stop (or stops) will move to the position indicated in the
next vector in the series.
For simultaneous positioning of the stops (code M296) the positions in a single vector (for
example !PPOS(n), or both vectors are read: !PPOS(n), for stop P (code M297); !QPOS(n),
for stop Q (code M298). Positioning finishes at the tenth position, or at the first
unprogrammed position in the series.
In hold, multipositioning is suspended (not stopped) until the NC is no longer in this state;
reset obviously aborts the operation in progress.

EXAMPLES

- Program generated by the operator

:

!PPOS (Ø)=500 first positioning operation.

!PPOS (1)=1000 second positioning operation.

!PPOS (2)=1200 third positioning operation.

BIESSE S.p.A. ©
(a210h003.fm-181103)

3 - 21

Chapter 3.
Notes on programming

!PPOS (3)=Ø end of positioning operation.

M297 code requesting positioning of the stops on the right table by

pressing the right table START button.

CAUTION

Do not use the START button on the Pilot Panel,
because pressing it causes immediate stoppage of the
procedure and start of the machining operation.

M70 code requesting enabling of the right table vacuum areas,

with subsequent stoppage of the program.

MØ stop code, which must only be inserted in the program if

code M70 has not been entered.

M96 code allowing the stops to return to the parked position.

start machining

- Program generated directly by the Post processor:

!PPOS (Ø)=500 first positioning operation.

!PPOS (1)=1000 second positioning operation.

!PPOS (2)=2860 the stops move to the parked position, which is stored in the

Post Processor configuration file.

M297 code requesting positioning of the stops on the right table

by pressing the right table START button.

CAUTION

Do not use the START button on the Pilot Panel,
because pressing it causes immediate stoppage of the
procedure and start of the machining operation.

M70 code requesting enabling of the right table vacuum areas,

with subsequent stoppage of the program.

MØ program stop code.

start machining

When the multipositioning phase has been completed, make sure that the stops are in the
parked position and press the START CYCLE button for the table in question, or the START
CYCLE button on the Pilot Panel, to start machining operations.

CAUTION

The START button on the Pilot Panel must only be pressed at the end of the
multipositioning phase.

3 - 22

BIESSE S.p.A. ©

(a210h003.fm-181103)

Chapter 3.

Notes on programming

2 - Description of the difference in tool length variable for EP machine

! DIFF(n); “n”th tool length value, expressed in mm.

After activating this variable, a data input box is displayed (see figure below), in which it is
necessary to enter the various “differences in length” for the tools in electrospindles N°: 2, 3,
4, 5, 6, 7, 8, 9, with respect to electrospindle N° 1.

INDEX

01
02
03
04
05
06
07
08
09
10

VALUE

0000.00000

0000.00000

0000.00000

0000.00000

0000.00000

0000.00000

0000.00000

0000.00000

0000.00000

0000.00000

The value of INDEX 01 corresponds to the difference obtained by measuring the length of the
tool in electrospindle N° 1 and the length of electrospindle N ° 2 (see “difference in tool length”
2-1 in the figure); this measurement must be repeated on all the electrospindles up to N° 9.
The drawing below illustrates how to measure this “difference in length” on tools fitted in three
electrospindles, when parallel machining operations are to be carried out:

“U” axis setting 1(or pneumatic)“V” axis setting 2“W” axis setting 3

2

3

C

114

B

107

A

A110, is the length of the tool in electrospindle 1.

BIESSE S.p.A. ©
(a210h003.fm-181103)

Z carriage

1

110

Ta bl e

3 - 23

Chapter 3.
Notes on programming

B 107-110 = - 3, is the “difference in length” between the tool in electrospindle 3 and the one in

electrospindle 1.

C114-110 = 4, is the “difference in length” between the tool in electrospindle 2 and the one in

electrospindle 1.

3 - Selecting the vacuum areas

To select the vacuum areas, it is necessary to use the variable @VC.
During creation of the program, after entering the vacuum area you require, you must also
enter the M code for the table on which the vacuum is to be provided (M70 for the right table;
M71 for the left table; M72 for the right - left table).
Example:

@VC = 123
M72

vacuum reservation for areas 1, 2 and 3
on the right table

The variable can have the following values:
1, to select area number 1;
2, to select area number 2;
3, to select area number 3;
4, to select area number 4;
12, to select area number 1 and 2;
34, to select area number 3 and 4;
123, to select area number 1, 2 and 3;
1234, to select area number 1, 2, 3 and 4.

3 - 24

BIESSE S.p.A. ©

(a210h003.fm-181103)

Chapter 3.

Notes on programming

3.6 Default conditions

The following list shows the default conditions of the machine. These conditions are imposed
automatically each time a RESET is performed.

Axis movement

G0 Rapid axis positioning

CET = 0.01 Precision tolerance within which the difference between the initial radius and

the final radius of the circle must stay;

FCT = 0.001 Threshold of the complete circle expressed in millimetres;

ARM = 0 Definition of the arc normalising mode;

CRT = 10 Threshold radius for the automatic reduction of the speed in the arcs;

CRK = 1 Automatic reduction factor in the arcs;

G27 Continuous operation with automatic reduction of speed at corners of piece.

DLA = 1 “Look Ahead” deceleration in dynamic mode G27;

MDA = 90 maximum angular offset of the axis in dynamic mode G27;

VEF = 0.8 factor used to perfect the calculation of the speed at the corners in dynamic

mode G27;

ODH = 1 checks the existence of continuous mode movements G28 in the part

program with excessive programmed profile speeds;

IPB = 0.02 axis positioning tolerance;

VFF = 0 “Velocity Feed Forward” control of speed and position;

MOV = 2 non-linear acceleration and deceleration ramps;

JERK = 1.875 Machining time with non linear ramps.

Origins and control of the co-ordinates

G17

Circular interpolation and profile correction on the XY plane (1

st

and 2nd axis);

G71 Programming in mm;

G90 Absolute programming;

G94 Feed speed in mm/min or inches/min;

BIESSE S.p.A. ©
(a210h003.fm-181103)

3 - 25

Chapter 3.
Notes on programming

Modification of axis reference system

(SCF) Scale factor de-activated on all axes;

(MIR) Specular inversion of the figure disabled on all axes;

(ROT,0) Interpolation plane rotation disabled;

(UAO,0) Axes referred to machine zero (home);

Limit switches and protected areas

SOL Reset limit switch software specified in AMP;

(PAD,n) Disable protected areas without eliminating definitions (PAD,n).

Virtualising

All virtualising (UPR, UVP, UVC, TCP) is disabled.

Tool programming

T.0 Tool corrector de-activated;

(AXO,-Z,-X) The first axis is Z, the second axis is X;

Tool diameter compensation

TPO = 1 Activated route optimisation at corners.

TPT = 0.1 Threshold of offset from corner with TPO = 1;

Electrospindle functions

G97 Electrospindle rotation speed in rpm.

Auxiliary M functions

All selections made using the M function are annulled.

3 - 26

BIESSE S.p.A. ©

(a210h003.fm-181103)

Notes on programming

Modification of the program execution sequence

DSB = 0 The barred blocks are executed;

Multi-process management commands

(GTA,X1,Y2,...,Z4,.../-Z,-X) Restores the normal configuration (contained in AMP);

(RDV,A) Releases access to drive A:

Control Variables

@COLLISION = 1 Anticollosion control enabled.

@GANTRY = 0 Disables mechanical union of tables (for Arrow only).

@UDAPALLET = 0 Disables synchronised movement of tables (for Arrow only).

Chapter 3.

@TPP = 0 Disables Teach pendent pocket.

@ASYNC = 0 Fast movement is only permitted with working units in the up position.

3.7 Programming machining operations using the electronic copier

To program machining with the electronic copier, it is necessary to use the variable @WRK_Z and
the following functions: M11, M52, M62. The M functions must always be inserted in front of the
program row specifying the machining depth.

Code M11= allows lowering of the electrospindles in floating mode.

Code M52= allows enabling of the copier blower.

Code M62= allows disabling of the copier blower. This function must be inserted at the end of the
program.

variable @WRK_Z= allows definition of copier positioning. To enable the system to establish the
position of the copier, associate this variable with the positive tool working depth value (see
examples on page 3 - 28).

BIESSE S.p.A. ©
(a210h003.fm-181103)

@WRK_Z

3 - 27

Chapter 3.
Notes on programming

To use the copier as a suction hood, install the curtain guards and use the programming functions
and commands normally used for this type of device.

The copier axes are associated with the setting axes. For this reason, errors appearing in the
software that relate to movement of the copiers will indicate the name of the setting axis to which
each copier is associated (see table below).

Copier axis Associated

Setting axis

Copier 1 Setting 5

Copier 2 Setting 6

Copier 3 Setting 7

Copier 4 Setting 8

Examples:

Example 1:

…
T1.01 M6 M7
ME46

M11 (lower the electrospindle in floating mode)
M52 (enable blower)

S18000 M3
(UAO,E40)
(UTO,E40, XE43, YE42, ZE44)
(AXO,-Z)
G0 Z45
X-9 Y263 Z45
G1 Z25 F2000

@WRK_Z=20 (copier positioning)

G41 X0 Y290 Z-20 (machining depth)
Y570 F8000
G2 X10 Y580 R10
G1 X415
G2 X490 Y505 R75
…

Example 2:

…
T1.01 M6 M7
ME46

@WRK_Z=20 (copier positioning)
M11 (lower the electrospindle in floating mode)
M52 (enable blower)

S18000 M3
(UAO,E40)

3 - 28

BIESSE S.p.A. ©

(a210h003.fm-181103)

Chapter 3.

Notes on programming

(UTO,E40, XE43, YE42, ZE44)
(AXO,-Z)
G0 Z45
X-9 Y263 Z45
G1 Z25 F2000
G41 X0 Y290 Z-20 (machining depth)
Y570 F8000
G2 X10 Y580 R10
G1 X415
G2 X490 Y505 R75
…

3.8 Treatment of machine parameters

The system is provided with a series of parameters, known as machine parameters, which modify
its function according to preset values.
The parameters that can be modified by the user are:

 VFF (Velocity Feed Forward) which defines behaviour of the system at machining corners.

 Dynamic limits. These are three parameters that relate to:

- automatic deceleration at corners along the trajectory (DLA);

- maximum angle of deviation (MDA) in G27;

- speed factor (VEF) in G27 at corners along the trajectory.

 Electrospindle speed limits.

 Percentage return speed in G84.

 Thickness tracer parameters.

 Axis references.

 Precision in circular interpolation.

 Wait time for G04.

 Date and time.

To access these parameters from the main menu, press the softkey for the menu item MACHINE
SET-UP. The following submenu is displayed:

POS DISPLAY

DINAMIC PARAM

REF

BIESSE S.p.A. ©
(a210h003.fm-181103)

NEXT DISPLAY

DINAMIC LIMITS

SET ACCURACY

SELECT PROCESS

PROGRAM SET-UP

ENLARGE

BLOCK RETRACE

HELP

PROBE SET-UP

TIME/DATE SET

3 - 29

Chapter 3.
Notes on programming

The following paragraphs give a description of the parameters and the procedures to be applied to
modify their functions and values.

3.8.1 Dynamic parameters

The softkey for the menu item DYNAMIC PARAM opens an “input box” similar to the one shown
below:

DYNAMIC PARAMETERS

ENABLE VFF (Y/N):
G04 DWELL TIME:

SPINDLE LIMIT (RMP):

% TAP RETRACT FEED (G84):

The meaning of the fields is as follows:

1- ENABLE VFF (Y/N)

Can have the following values:

Y. Enables VFF when running a part program. With VFF enabled and a constant axis speed,
the error threshold when running a part program is close to zero.

N. Disables VFF when running a part program. With VFF disabled the axis, during movement,
causes a certain error threshold proportional to the speed of the axis itself and the ring gain
(which can be configured in AMP). Thus, a constant speed corresponds to a constant error
threshold.

The parameter VFF (Velocity Feed Forward) modifies the value of this error. The error is displayed
in the axis data area by pressing the softkey for the item POS DISPLAY and selecting the option
ERROR.

When a part program is active and the movements are carried out without deceleration at corners
(G28), the path followed by the axes changes according to whether VFF is enabled or disabled,
and a number of shape errors may occur at the corners of the profile:

 Machining with VFF enabled causes trajectory errors, as the corner is passed.

 Machining with VFF disabled causes trajectory errors, as the corner is cut.

3 - 30

BIESSE S.p.A. ©

(a210h003.fm-181103)

The following figures illustrate four examples of VFF application.

trajectory

traiettoria

trajectory

traiettoria

Raw outside without VFF

GREZZO ESTERNO SENZA VFF GREZZO INTERNO SENZA VFF

Raw inside without VFF

Chapter 3.

Notes on programming

trajectory

trajectory

traiettoria

Raw outside with VFF

Raw inside with VFF

GREZZO INTERNO CON VFFGREZZO ESTERNO CON VFF

traiettoria

2- G04 DWELL TIME

Defines the rest time at the end of a block (G04).

This time is used in G04 and in the following fixed cycle blocks:

 In G94; dwell time expressed in seconds.

 In G95; dwell time expressed in number of turns.

For more detailed information on this parameter, pleas consult the "Machining Centre" Software
user’s manual.

To save any operations carried out in the “input box”, press ENTER or the DYNAMIC PARAM
softkey. To close the box without saving modifications, press ESC.

BIESSE S.p.A. ©
(a210h003.fm-181103)

3 - 31

Chapter 3.
Notes on programming

3.8.2 Dynamic limits

The softkey for the menu item DYNAMIC LIMITS opens the following “input box”:

Description of the fields in the box:

ENABLE LOOK-AHEAD (Y/N) Automatic deceleration at corners. Can have the following

values:

Y Enables automatic deceleration at corners when running

a part program.

N Disables automatic deceleration at corners when

running a part program.

If N is selected, all DLA instructions in the current part
program will be ignored.

3 - 32

BIESSE S.p.A. ©

(a210h003.fm-181103)

Chapter 3.

Notes on programming

MAXIMUM DEVIATION
ANGLE

MDA (Maximum Deviation Angle) is the maximum angular
deviation of the axis in which G27 is active. The selected
angle represents the working limits for G27.

An angle of deviation higher than the one indicated is carried
out in G29 mode, point by point.

The value allowed varies from 0 to 180 degrees. The default
value is 90 degrees.

VELOCITY FACTOR The velocity factor (VEF) is a parameter used to regulate the

speed at corners in G27 mode. Small VEF values will cause
great reductions in speed. The value allowed varies from 0 to

999999999999. The default value is 8.

To save any operations carried out in the “input box”, press ENTER or the DYNAMIC LIMITS
softkey. To close the box without saving modifications, press ESC.

For more detailed information on DLA, MDA and VEF, please consult the "Machining Centre"
Software user’s manual.

3.8.3 Program SET-UP

The softkey for the menu item PROGRAM SET-UP opens an “input box” that allows configuration
of certain parameters that condition the way in which the part programs are run:

- Delete block;

- Optional stop;

- Feed rate bypass;

- Control rapid speed;

- Rotation;

- Stock allowance;

For each of the axes present it is possible to configure the following parameters:

- Stand still mode (stand still);

- Mirror mode (mirror);

- Scale;

- Scale factors.

BIESSE S.p.A. ©
(a210h003.fm-181103)

3 - 33

Chapter 3.
Notes on programming

To save any operations carried out in the “input box”, press ENTER. To close the box without
saving modifications, press ESC.

For further information, please consult the NC on-line Help.

3 - 34

BIESSE S.p.A. ©

(a210h003.fm-181103)

4

-

Chapter 4. Notes on machining

4.1 Updating tool tables

During machining operations, each tool change operation corresponds to an update of the Tool
Table, which always takes place when the cycle has almost finished, immediately after detecting
locking of the tools.

This information becomes extremely important when the operator, in the face of a tool change
operation that has not been completed successfully (for example due to interruption), has to
decide how to intervene manually. There are various options:

 the cycle stopped before locking of the tools in the electrospindle or in the magazine. In this

case, as the table has not yet been updated, the operator must carry out manual tool change
operations so as to restore the conditions existing prior to the unsuccessful tool change
operation;

 the cycle stopped after locking of the tools in the electrospindle or in the magazine. In this

case the operator must carry out the manual tool change operations required to park the tool
change device. It is, however, recommended that he also check the tool position data in the
table, to ensure they correspond with the actual position of tools in the magazine.

For TC machines
tool change cycles the position of that tool in the magazine will generally speaking no longer be the
initial one (the one in which it was fitted during tooling). It is therefore necessary to make sure the
data in the table and the actual tooling of the machine are coherent.

The following example shows how a table is updated at each tool change (for the meanings of the
fields, please see the chapter Chapter 2. “Notes on tooling” at paragraph 2.1.3 “Listing the tools in

the magazine”):

a. Let us suppose that tool n° 2 is fitted in an electrospindle and that it is to be replaced by tool

n° 8, which is in the magazine. The situation before the tool change operation is as follows:

(with chain type tool change), if a tool is managed in "random" mode, after a few

Code Pocket Position Spindle Offset

... ... ... … ...

2 4 out 1 1

... .... ... … ...

8 5 magaz. 0 1

BIESSE S.p.A. ©
(a269h001.fm-181103)

4 - 1

Chapter 4.
Notes on machining

b. After the tool change operation the table is updated as follows:

Code Pocket Position Spindle Offset

... ... ... … ...

25magaz.01

... .... ... … ...

85out11

It can be seen that, whereas all the fields for the tool that has returned to the magazine are
updated, the tool fitted in the electrospindle, although it is indicated as being positioned outside the
magazine (Position= out) still maintains its previous location in the tool holder (pocket= 5).
It must therefore be underlined that all manual operations have to be carried out with the maximum
care and attention.

During the tooling phase there is nothing to stop different pockets being associated with the same
tool number. This characteristic is useful when working materials other than wood, but it can create
problems in management of the magazine.

For the above reasons, during tooling or manual intervention it is not recommended that you:

associate the same tool number with different pockets;

tool up the magazine with a tool that is already in the electrospindle.

4.2 Machining operations in dual mode

When a work table wider than a single table is required, both the tables can be used and moved as
if they were a single axis. In this case the machining operations are carried out in what is known as
dual mode. To machine in this way it is possible to use two different methods:

1. Configure the machine normally and use the code UDA in the part program. For the syntax
and a description of this code, please see the “Machining Centre” Software user’s manual.

2. Configure the machine in gantry mode. When in gantry mode, as described in paragraph 2.3

“Work table management” on page 2 - 11, the two tables are united to form a single work

table. This work table is considered by the programmer as the Y axis.

For machining operations in dual mode, gantry configuration of the machine guarantees greater
precision in alignment of the tables. Carry out test runs on the piece to determine whether or not,
for a certain machining operation, it is sufficient to use the UDA code with normal configuration.

4 - 2

BIESSE S.p.A. ©

(a269h001.fm-181103)

5

-

Chapter 5. Bar code reader control

The optional “Bar code reader” includes:

 a complete power supply reading system;

 set-up of a serial port for connection of the feeder;

 a reading system test program and a device control program. The

programs are on disk generatable from the self-extracting file
Brcman_v1.exe found on the machine CD in the BIESSE
Applications directory, English or Italian (see figure on the right);

 the installation and user manual.

5.1 Installing the reader

A socket connector for the bar code reader feeder, and a jack for connection of the other end of the
feeder are provided inside the machining carriage. Thus the power supply unit can be inserted in
the carriage and the reader connected to the serial port located on the left-hand side (or front,
depending on the type of commander) of the carriage.

To carry out a machining operation using the reader it is necessary to install the program that
manages the reader itself, copying the two files Brcman and Kgdv from the floppy disk to the
same directory on the NC.

Checking operation of the reader and connection

The operation described below serves to check proper functioning of all the electrical connections
after installation of the bar code reader.

 Copy the BRCTEST program to the directory F:\ using the softkeys U

C

OPY and insert in Entry From: A:\BRCTEST; To : F:\ .

 Exit from D

OS SHELL using the softkey Exit.

TILITY, DOS SHELL and

 Press the softkey Part Program and select the copied program (if it does not appear in the

list, write the name in the command field called Program Name). Activate the program with
the softkey Activate.

BIESSE S.p.A. ©
(a218h003.fm-181103)

5 - 1

Chapter 5.
Bar code reader control

 Press the RUN button to make the machine run the program: a dialogue box will be displayed

in which you are requested to specify which serial line the reader is connected to (usually
COM1). Make your choice and press ENTER.

 SERIAL LINE CONNECTED SUCCESSFULLY appears on the screen above the first

program line. If the dialogue box does not appear, this means that the NC has not been
enabled.

 Read, as an example, one of the bar codes on the appliance user manual. The indications

that appear under the code itself should be displayed on screen, if not, check the connections
and contact the Biesse service department if necessary.

5.2 Using the brcman program

To use the reader, the client has a single program (Brcman) containing three different types of
machining cycle. Operation of these three cycles, called Twojob (1), Pend (2) and Free (3), is
divided into two parts:

 During the first part, which relates to the user interface, the NC looks for the INIT file which, if

present, must be in the directory F:\ and which can be used by the client to move all the
elements present on the machine (e.g. pallet outfeed, axis parking, etc.).

 If this file does not exist, the control asks, through a dialogue window, whether it should

anyway proceed with reading and execution of the program.

 If you decide to continue, a second dialogue window is displayed asking you to specify the

path where the working programs are stored, whose names will be read through the bar code
reader.

INFORMATION

The file name can have a maximum length of 30 characters, and must not contain the
character “.”, which is already used as a separator for information contained in the bar code
and might therefore cause the program to malfunction (e.g. Test is correct, Test.txt is
incorrect). On the other hand, the path string can contain up to 50 characters and must end
with the character “\” (e.g. A:\Barcode\).
The machining programs can be stored both in disks E and F of the NC, and in drive A and
the remote disk (drive K).

 If no path is defined, the NC will search for the file in the folders specified during the software

installation and configuration phase. The bar codes may contain a name and 9 parameters
and the elements must be separated from each other by a dot (e.g.: Pippo.23.456.12).

 Finally, two dialogue boxes will be displayed, the first of which is used to indicate the serial

port to be used, and the second to indicate the type of cycle to be enabled.

5 - 2

BIESSE S.p.A. ©

(a218h003.fm-181103)

Chapter 5.

Bar code reader control

Using the three cycles

On completing the first stage of data input, the operator can select the cycle to be used. For the
correct procedure, follow the instructions given below according to the cycle selected.

Using the Twojob cycle

If the operator selects this cycle, the following operations can be executed:

 The control brings both the tables and the pallets into the loading position, enables the

pneumatic stops (if there are any), makes a reservation for activation of the vacuum and then
waits for the first bar code to be read.

 Subsequently, with the START CYCLE command (green flashing button on the relevant table)

machining on the right table starts, as defined in the program created by the user.

 As soon as this machining phase starts, the operator can read a new code that will be kept in

memory by the reader until the next machining operation.
When machining on the right table has been completed, the Brcman program moves this
table and the relevant pallet to the loading position, releases the piece, activates the
pneumatic stops and presets vacuum activation for the next piece.

 In the meantime, if the START CYCLE button has also been pressed after locking the piece

on the second table, machining will start on that table.

This cycle allows pendular machining on the two tables of programs that change each time.
T

WOJOB itself enables the correct table and origin, using the commands DAN and UAO; the user

thus only has to program the Y axis (never the W axis), and must not use either the command
DAN or UAO. Also, if the user program contains a UTO to assign the local origin, this must refer to
the correct global origin enabled at that moment. To avoid errors, the program Brcman provides
the user with details of the origin enabled, in the global variable SN12. In this way, when writing a
UTO (SN12,…) the operator is certain that it will refer to the correct global origin.

The following page shows a diagram for operation of the program described above.

BIESSE S.p.A. ©
(a218h003.fm-181103)

5 - 3

Chapter 5.
Bar code reader control

Star t

Search INIT file

Exists Does not exist

INIT execution Do you want to continue anyway?

yes

Do you want to specify a path?

no

yes

Write path

Select serial port used

Select cycle to execute

Tables in loading position, pneumatic stop

activation, vacuum preset

Bar code reading: e.g. Pippo.300.400.20.50

- Activation of tables (DAN) and origin 1
(UAO) ­CYCLE

no

5 - 4

(CLS, Pippo)

Piece unloading and preparation of next

loading operation: vacuum preset

-Exchange of tables (DAN) and
activation of origin 2 (UAO)

- CYCLE

Bar code reading: e.g. Pluto.500.200.40.80

(CLS, Pluto)

Piece unloading and preparation of next

loading operation: vacuum preset

End

BIESSE S.p.A. ©

(a218h003.fm-181103)

Chapter 5.

Bar code reader control

The following gives a brief example of how to use the program Brcman via the TWOJOB cycle.

1. Activation and START of Brcman program.

2. Selection of Twojob cycle.

3. Reading of the bar code PZDX.panel thickness.jig thickness (e.g. PZDX.20.50).

4. Piece locking on the right table and pressing of the flashing START CYCLE button on the
relevant table.

5. After machining has started, reading of the bar code PZSX.panel thickness.jig thickness
(e.g. PZSX.20.50).

6. Piece locking on the left table and pressing of the flashing START CYCLE button on the
relevant table.

7. Repetition of the procedure describe above from point 3 to point 6.

INFORMATION

The program PZDX forms a square, PZSX forms a triangle: neither of them uses the command
UAO or the command DAN.

Using the Pend cycle

Pend is the abbreviation for Pendulum and indicates that the cycle in reference carries out
pendular machining of a number of pieces:

 The control moves both the tables and the pallets to the loading position, activates the

pneumatic stops (if present), presets vacuum activation and waits for reading of the bar code
where the name of the program to be executed is specified.

 The machining operation contained in the program is executed first on the right table and then

on the left and so forth until complete interruption.

 At the end of each machining operation, the program moves the table and the relevant pallet

to the loading position, releases the piece, activates the pneumatic stops and presets vacuum
activation for the next piece.

As the command M0 is also used after each vacuum reservation in the Pend cycle, at the end of
each locking operation it will be necessary to press the START CYCLE button, which will flash
(green button on the corresponding table). As the Pend cycle itself enables both the table on which
it is carrying out machining operations and the reference origin, the machining program that is
open and running must not contain DAN and/or UAO instructions, and only the Y axis must be set
(not the W axis. Furthermore, if a UTO is present in the user program for assignment of the local
origin, this must refer to the correct global origin (activated in that moment). To prevent errors, the
Brcman program makes the activated origin available to the user in the global variable SN12.
Therefore, when writing UTO (SN12,…) you are sure that you are referring to the correct global
origin.

BIESSE S.p.A. ©
(a218h003.fm-181103)

5 - 5

Chapter 5.
Bar code reader control

To better understand functioning of the program just described, consult the following diagram:

Start

Search INIT file

Exists Does not exist

INIT execution Do you want to continue anyway?

yes

Do you want to specify a path?

no

yes

Write path

Select serial port used

Select cycle to execute

Tables in loading position, pneumatic stop

activation, vacuum preset.

Bar code reading: e.g. Pippo.300.400.20.50

- Activation of tables (DAN) and origin 1
(UAO)

- CYCLE

no

5 - 6

(CLS, Pippo)

Piece unloading and preparation of next

loading operation: vacuum preset

-Exchange of tables (DAN) and
activation of origin 2 (UAO)

- CYCLE

(CLS, Pippo)

Piece unloading and preparation of next

loading operation: vacuum preset

End

BIESSE S.p.A. ©

(a218h003.fm-181103)

Chapter 5.

Bar code reader control

The following gives a brief example of how to use the program Brcman via the PEND cycle.

1. Activation and START of the Brcman program;

2. Selection of P

END cycle;

3. Reading of the bar code PZDX.panel thickenss.jig thickness (e.g. PZDX.20.50);

4. Piece locking on the right table and pressing of the flashing START CYCLE button on the
relevant table;

5. The NC executes the machining operation defined in PZDX on the right table;

6. Piece locking on the left table and pressing of the flashing START CYCLE button on the
relevant table;

7. The NC executes the machining operation defined in PZDX on the left table;

8. Repetition of the procedure describe above from point 3 to point 6.

INFORMATION

The program PZDX forms a square, PZSX forms a triangle: neither of them uses the command
UAO or the command DAN.

Using the Free cycle

If the operator selects this cycle, the following operations can be executed:

 The NC waits for reading of the first bar code and immediately starts machining, after which

the new code can be read.

 In this case, unlike the T

WOJOB cycle, the program Brcman will do nothing further, and it will

be up to the current machining program to prepare loading/unloading, enable the pneumatic
stops if there are any, make a reservation for the vacuum, define both the table on which
machining operations are to be carried out and the origin to be used.

 The F

REE is also repetitive, that is to say it calls up the program indicated in the bar code and

performs it once. After this it prepares to read a second bar code. This cycle is useful when
working in Gantry mode or when the CAD used automatically inserts information relating to
the table, origin, vacuum, piece loading and unloading, directly in the programs. If the same
machining operation is to be carried out in Gantry mode, the cycle must be incorporated in the
program required, otherwise it will be necessary to re-read the same bar code repeatedly.

BIESSE S.p.A. ©
(a218h003.fm-181103)

5 - 7

Chapter 5.
Bar code reader control

A flow diagram of functioning of the program just described is shown below:

Start

Search INIT file

Exists Does not exist

INIT execution Do you want to continue anyway?

Do you want to specify a path?

Write path

Select serial port used

Select cycle to execute

Bar code reading: e.g. Pippo.300.400.20.50

(CLS; Pippo)

End

The following gives a brief example of how to use the program Brcman via the F

REE cycle.

1. Activation and START of the Brcman program;

2. Selection of F

REE cycle;

3. Reading of the bar code Pendulum;

4. Start of machining operations; the operator can proceed to read the next bar code.

INFORMATION

The program PENDULUM performs a pendular machining operation without using any EPP
instructions, simply by repeating the code for the machining operation.

5 - 8

BIESSE S.p.A. ©

(a218h003.fm-181103)

Chapter 5.

Bar code reader control

CAUTION

Always comply with the following restrictions to guarantee proper operation of the program
Brcman:

 In the machining operations called through bar code reading, the M30 command

must absolutely not appear, since it launches a machine RESET and hence stops
any program being executed including the handler of the Brcman bar code reader.

 In the programs called the EPP command cannot be used, since it does not

recognise the labels.

 The first 51 characters in the global variable SC (character type) are used by the

program Brcman and must therefore be considered occupied. This is also true for
the first 12 variables SN (SN1...SN12).

 The Kgdv file is used to activate program reading from a possible remote drive

(connected to the NC via Ethernet) which must be set on the control with the
identification K.

 If when running the program BRCMAN, or even after you have finished using this

program, there is any difficulty in accessing drive A or the remote unit (drive K:), it
will be necessary to enable MDI mode, type the string (RDV,A) or (RDV,K) in the
command line, and then press ENTER and the green START CYCLE button.

BIESSE S.p.A. ©
(a218h003.fm-181103)

5 - 9

Chapter 5.
Bar code reader control

5 - 10

BIESSE S.p.A. ©

(a218h003.fm-181103)

A

-

Appendix A. Laser projector for

electrospindles

The laser projector, which is supplied by Biesse as an optional, can be used to project the profile of
the piece and the position of suction cups on the tables, thus allowing them to be positioned
correctly. The machine is equipped with a specific software and an electric system that allows it to
interact perfectly with the laser device.

A.1 Installation and wiring

The projector is equipped with a power supply connector, three serial connectors (9 pin, 25 pin and
RJ10) for communication with the control device, a cable type RJ10 for connection to the machine,
and a power supply cable. To operate correctly, the projector must be connected to the electrical
power supply, using a suitable cable, and to the RJ10 type socket on the side of the cabinet, using
the cable provided.

A.2 Using the software associated with the projector

The laser projector is supplied complete with a software for serial cable data transmission, a
number of utility programs and some explanatory programs. The files supplied are as follows:

Ssend; this transmits the data contained in a file resident in the NC (including the path and

extension) to the projector, via the serial port. The string for this file, named SCO0.31, must
not exceed a length of 31 characters (e.g.: SCO0.31=”F:\PROVAPD.PLT”). The file Ssend is
installed in the directory E:\PP, it must contain the commands for the projector and it must be
in HPGL format.
It also allows the projector to be managed through the Alphacam software post-processor,
which can be purchased from BIESSE as an optional.

Zero; in combination with Zero.plt, this launches the laser projector reset procedure. To ensure

that this program operates correctly, copy the file Zero.plt to directory F:.

Sltest; together with Ssend, laserpd.plt and laserps.plt, this provides an example of how the

projector and the software supplied with it can be used. To ensure that the program operates
correctly, copy the files laserpd.plt and laserps.plt to directory F:.

INFORMATION

This software, which is supplied along with the laser projector, is an application developed by
BIESSE in ASSET, and is therefore open to further developments aimed at improving
communication between the NC and the laser projector.

BIESSE S.p.A. ©
(a270h001.fm-181103)

A - 1

Appendix A.
Laser projector for electrospindles

EXAMPLE OF A PROGRAM:

The following is a brief example of how to use the management programs supplied with the laser
projector. The lines highlighted in bold type represent the lines containing codes of interest.

codes description

[...]

M500 M5 M20

M700 M22

M100

SC0.31=”F:PROVAD.PLT” vacuum module program call-up

(CLS,SSED)

M0

E60=-1000; x value for right positioning

E61=-3000; x value for left positioning

E63=-800; y/w positioning value

E10=2; right table

G0 G79 Z0

G79 Y0

M100

E42= 0; y origin

“INIZ”

E41= 0; x origin

E44= 20;E45= 0; panel thickness

E45= 0 sub-panel thickness

E46= 501; selected electrospindle

E47= 701; selected boring unit

G16XY

SC0.31=”F:PROVAD.PLT” piece profile projection file call-up

(CLS,SSED)

G0 G79 XE60 Y0 Z0

M70

M0

E1=TIM

E40=1; work table: 1=right 2=left

(UAO,E40)

E44 = E44 + E45

G0 G79 Z0

A - 2

BIESSE S.p.A. ©

(a270h001.fm-181103)

B

-

Appendix B. Renishaw NC1 tool adjustment

system

INFORMATION

Metric units of measure are used (millimetres) for the examples described in the chapter. The
Anglo-Saxon units of measure (inches) are shown in brackets.

This chapter contains the instructions for use of the software of the Renishaw NC1 non-contact
tool adjustment system. The NC1 non-contact tool adjustment system functions with the aid of a
laser. In normal conditions of use, it allows measuring the cutting tools with maximum accuracy
and maximum execution speed. During movement of the tool in the laser beam, the system
detects if the tool is broken and from the pulses transmitted to the controller can determine the
presence of the tool and the position of the bit, a tooth and a cutting edge.

With the NC1 system the following parameters can be set:

 Cutting tool length and diameter. Accurate measurement of tools with a diameter of 0.2 mm

(0.008 in).

 Tool breakage detection.

Machine tool controllers supported

The NC1 system software can be used on the controllers of the OSAI series 10 machine tools.

B.1 Memory requirements for the software

The NC1 system software requires about 45.00 KB part-program memory.

If the controller has only a small memory, the MEASURE macro and the BRKTL macro do not
have to be loaded if you do not intend using them.

 MEASURE; macro (tool adjustment procedure) 5.0 KB memory.

 BRKTL; macro (tool breakage - plunge control) 4 KB memory.

After completing the beam alignment cycle, the ALIGN macro can be removed (laser beam
alignment procedure macro; 7.0 KB memory).

BIESSE S.p.A. ©
(a732h0001.fm-181103)

B - 1

Appendix B.
Renishaw NC1 tool adjustment system

B.2 Software installation

Before installing the NC1 software, read the guidelines contained in the ReadMe file on the
software disk.
All the tracing macros must reside in the directory F:\PROBE\ of the CNC.
To load the macro the DOSHELL utility of the CNC can be used.

B.3 Types of tool correction supported

Applications for positive tool correction

The NC1 software is suitable for adjusting tools with positive tool correction values which
represent the physical length of the tool.
The descriptions given in the chapter refer to the applications for positive tool correction.

B.4 Software functions of the NC1 system

The NC1 system software offers the following measuring and calibration functions:

 Macro functions for measuring;

 Macro functions for calibration;

 Macro functions for service.

Macro functions for measuring

The following macros are provided for measuring:

 MEASURE macro; Allows measuring the length and diameter of the cutting tool and

controlling the cutting edge.

 BRKTL macro; To detect breakage of a tool by plunge measurement. This macro has been

created for use on vertical processing centres.

Macro functions for calibration

The following macros are provided for calibration:

 ALIGN macro; Allows aligning the laser beam, adjusting the provisional positions of the beam

in the spindle and in the radial measuring axes, and calibrating the measuring position along
the beam.

B - 2

BIESSE S.p.A. ©

(a732h0001.fm-181103)

Appendix B.

Renishaw NC1 tool adjustment system

 CALIB macro; Allows calibrating the laser beam positions in the spindle and in the radial

measuring axes.

Macro functions for service

The macros for measuring and calibration are supported by the service macros listed below.

SETUP macro; Allows adjusting the data.

CLRVAR macro; Allows performing the start functions.

PRBX macro; Allows performing the measuring procedures.

PRBXM macro; Allows performing the measuring procedures.

PRBY macro; Allows performing the measuring procedures.

PRBYM macro; Allows performing the measuring procedures.

PRBZ macro; Allows performing the measuring procedures.

SETVAR macro; Allows loading the data used for tool length/diameter acquisition.

SETVAR1 macro; Allows loading the data used for the tool integrity check.

B.5 Use of the macros

To use the macros observe one of the following methods:

 Call the macros individually.

 Use the MAIN program within which all the macros are integrated and can be executed.

The following macros can be called from the MAIN program:

 ALIGN; To align the laser beam.

 CALIB; To calibrate the laser beam.

 MEASURE; To requalify the tool length/diameter.

 BRKTL; To check tool integrity.

 PR_DIFF; To requalify alignment of the electrospindle boring heads.

INFORMATION

The MAIN program allows simplifying programming.

BIESSE S.p.A. ©
(a732h0001.fm-181103)

B - 3

Appendix B.
Renishaw NC1 tool adjustment system

B.6 Macro variables

Below follows a list of the macro variables used:

 USER variables; For the calibration and adjustment data.

 E variables; For the adjustment data and the data defined locally.

The default base number is L140.

Macro variables for the calibration data

During the calibration cycles the following variables are automatically set (used for the laser beam
origins of the NC1 probe):

 L140; X position of the beam (data automatically acquired and written in the USER table of

the CNC).

 L141; Y position of the beam (data automatically acquired and written in the USER table of

the CNC).

 L142; Z position of the beam (data automatically acquired and written in the USER table of

the CNC).

 L143; Beam thickness (not used for calibration and measuring on a single side).

 L145; Internal support variable.

These variables are viewable through the User Table together with the machine configuration data.
The table may be protected by a password entered directly by the machine manufacturer to
prevent that incorrect data is entered manually, which could preclude good functioning of the
machine.

In any event, the variables used by the macros are automatically loaded by the CALIB and ALIGN
macros.

B - 4

BIESSE S.p.A. ©

(a732h0001.fm-181103)

Appendix B.

Renishaw NC1 tool adjustment system

Macro variables for adjustment data

The macro variables for the adjustment data are type E and go from variable E0 to variable E130.
Read the description of all the variables and then modify the SETUP macro according to the
method described.

Machine setting variables of the manufacturer (not to be modified if not necessary)

E102 Magazine number

1 = one magazine present;
2 = two magazines present;
3 = three magazines present;
4 = four magazines present

E103 Pocket number for each magazine

10 = revolver magazine;
12 = chain magazine;
18 = chain magazine

E104 Distance between centres of the electrospindle boring heads

E104 = xxx.yyy.

E105 X-axis position with the calibration tool referenced to the probe centre

E105 = xxxx.yyyy.

E106 Y-axis position with the calibration tool referenced to the laser beam centre

E106 = xxxx.yyyy.

E107 Z-axis position with the sample tool at 10 mm from the laser centre

E107 = xxx.yyyy

E108 Corrector length of the sample tool

E108 = xxx.yyyy.

E109 Corrector diameter of the sample tool

E109 = xxx.yyyy.

The parameters E108 - E109 refer to the dimensions of the sample tool used for the alignment and
calibration phase of the NC1 probe.
The data is loaded in the OFFSET table record 300.

Configurable variables:

E1 Beam axis.

1= if the laser beam is parallel to the X-axis.
0= if the laser beam is parallel to the Y-axis.

E2 Options for radial measuring axes.

1 = measuring on the positive side of the beam,

-1 = measuring on the negative side of the beam,
0 = measuring on both sides of the beam.
Default Value: 0

E7 M code number to disable the "latch" mode.

If the "latch" mode is not used, do not modify the data entered except when adjustment

BIESSE S.p.A. ©
(a732h0001.fm-181103)

B - 5

Appendix B.
Renishaw NC1 tool adjustment system

causes problems. If problems occur, use the coolant M9 (or a similar product) not used in
these cycles.

E8 M code number to enable the "latch" mode.

If the "latch" mode is not used, do not modify the data entered except when adjustment
causes problems. If problems occur, use the coolant M9 (or a similar product) not used in
these cycles.
Radial calibration options
1 = measuring on the positive side of the beam;

-1 = measuring on the negative side of the beam;
0 = measuring on both sides of the beam.
Default Value: 0

E11 First backing distance after tracing.

Default Value: 2.5

E12 Second backing distance after tracing.

Default Value: 0.25

E13 Attempts for tool breakage check.

Number of measuring cycles executed during the BRKTL macro necessary to eliminate the
effects of the coolant.
Default Value: 15

E14 Default measurement resolution (feed speed per revolution).

In general, the feed speed per revolution is 0.002 mm (0.0001 in). The greater the value the
less accurate the measurement.
Default Value: 0.002 mm (0.0001 in)

E15 Approach distance.

Tool distance above the laser beam before starting the measurement.
Default Value: 10

E16 Approach method.

1 = no tool data required in correction tables;
0 = tool dimensions ±5 mm known (not used);
With E16 = 0, the tool bit goes to fast forward speed towards the approach distance (E15)
above the beam.
Default Value: 1

E18 Sample dimensions for dispersion.

Number of measuring samples to be executed.
The repeat attempts are twice this value:
Ex: E18=2 four tracing operations are carried out of which the mean value is calculated on the
last two.
For a description of the function, consult the figure shown in the paragraph B.9 “Dispersion

tolerance check” on Page B - 10.

Default Value: 1

E19 Forward movement towards the beam.

Initial forward speed towards the measuring position.
Default Value: 3000 mm/min

B - 6

BIESSE S.p.A. ©

(a732h0001.fm-181103)

Appendix B.

Renishaw NC1 tool adjustment system

E19 Fast transversal feed speed.

Default Value: 3000 mm/min

E20 Initial safety position.

Z position which allows providing the safety distance, above any obstructions, with the
longest tool of the spindle. This position must be set during installation.
Default Value: None

E24 Maximum tool length.

Determines the fast approach height of the spindle bit above the laser beam.

E25 Minimum tool length.

Determines the minimum measuring height of the spindle bit above the laser beam.

E26 Maximum tool diameter.

The value depends on the machine tool.

E27 Dispersion tolerance value.

For a description of the function, consult the figure shown in the paragraph B.9 “Dispersion

tolerance check”, on page B - 10.

Default Value: 0.010 mm (0.0004 in)

E28 Hardware signal pulse duration.

Time interval during which the activation signal remains on. This interval depends on the
hardware.
The value is specified at the time of ordering the NC1 system.
Check the sequence of the status LED at the time of switching on (for further information,
consult the publication "Guide to installation and NC1 component List").
Default Value: 100

E29 Set the alarm or the tool breakage indicator E100.

0 = Indicator (the tool is not declared broken);
1 = Alarm (the tool is declared broken in the table, the spindle is no longer reloaded if
requested by the program).
Default Value: 1

E30 Rotation of tools with dimensions greater than this value.

The tools exceeding the dimensions defined with this variable automatically rotate during the
adjustment.
Default Value: 10

E55 Spindle speed at which calibration or measuring occurs.

Default Value: 3000 rpm

BIESSE S.p.A. ©
(a732h0001.fm-181103)

B - 7

Appendix B.
Renishaw NC1 tool adjustment system

E70 Default spindle speed.

The measuring cycles are optimised for a spindle speed of 1000 rpm.
Machining of some tools among which, for example, unbalanced or large tools, must occur at
a speed lower than 3000 rpm. Machining speed control is one of the responsibilities of the
user. Use the input E55 to adjust the speed.
The measuring cycle times increase at lower speeds. The minimum speed is 800 rpm.

Default Value: 1000 rpm

Macro modification for the adjustment data (SETUP)

Before executing the cycles, modify the adjustment data in order to adapt the application and the
machine setting. Enter the data in the units of measure with which the machine must perform the
measurement, for example, in millimetres or inches.

Be careful with the variables E24, E25 and E20.

CAUTION

Before executing any cycle, enter the valid data relating to the machine tool in the variables
E24, E25 (the maximum and minimum tool lengths) and E20 (the safety position in the
machine coordinates). If these values are incorrect, there is a risk that the tool collides with
the NC1 unit.

Example of SETUP macro

N1
E102 = 3
E103 = 10
E104 = 780.0
E105 = -xxxx.yyyy (X-axis)
E106 = -xxxx.yyyy (Y-axis)
E107 = -xxxx.yyyy (Z-axis)
E108 = xxx.yyyy (sample tool corrector length)
E109 = xxx.yyyy (sample tool corrector diameter)
E1 = 1
E2 = 0
E7 = #0
E8 = #0
E9 = 0
E11 = 2.5
E12 = 0.5
E13 = 15
E14 = 0.002
E15 = 10
E16 = 1
E18 = 2
E19 = 3000
E19 = 3000
E20 = -5
E24 = 280
E25 = 80
E26 = 120
E27 =.050
E28 = 100

B - 8

BIESSE S.p.A. ©

(a732h0001.fm-181103)

Appendix B.

Renishaw NC1 tool adjustment system

E29 = 1
E30 = 10
E70 = 3000

B.7 NC1 system orientation

The indications listed are based on the assumption that the NC1 system is installed with the laser
beam parallel to the X-axis. The length measurements are carried out from the Z-axis, while the
radial ones are carried out from the Y-axis.
If the system has been installed with a different orientation, the necessary adjustments must be
made to the axes used for the length and the radial measurements (for further information, consult
the variables E1, E2 and E9 set manually).
For the Biesse type machines the system is oriented with the beam along the X-axis.

Z

Y

X

Beam parallel to X-axis: E1 = 1

Beam parallel to Y-axis: E1 = 0

BIESSE S.p.A. ©
(a732h0001.fm-181103)

B - 9

Appendix B.
Renishaw NC1 tool adjustment system

B.8 Beam detection and measuring movements

The beam detection and measuring movements are all carried out by moving the tool inside the
laser beam (see following figure). The measuring movements are carried out by rotating the tool.

Measure

feed

Fast
feed

Reduced

feed

Sample

measurements

B.9 Dispersion tolerance check

In the following example the adjustment value of the dimensions of the predefined sample is used
(E18=3). The number of attempts is set automatically to twice the sample dimensions; the number
written is six (6).

The sample is measured until the maximum number of permitted attempts has been reached, thus
setting off an alarm, or until the sample falls within the limits. In the latter case, the mean value is
measured and the measurement is complete.

Maximum

Scatter
tolerance

Minimum

B - 10

BIESSE S.p.A. ©

(a732h0001.fm-181103)

Appendix B.

Renishaw NC1 tool adjustment system

B.10 MAIN macro execution

Execution of the MAIN macro requires knowing the meanings of the variables to be entered in the
pull-down menus when requested, which exactly determine the cycle to be executed. The
structure of the Main program is listed below showing the procedure to follow.

MAIN

Running laser alignment? (Y/N)

Y

Data Entry:
Enter calibration tool number

ALIGN macro execution

Y

Running new laser alignment? (Y/N)

N

Laser CALIB macro execution

Requalify Tool offset? (Y/N):(Y/N):

Y

Data Entry:
Insert Tool Number:

N

N

Enter

Data Entry:
Enter the parameters requested:

BIESSE S.p.A. ©
(a732h0001.fm-181103)

Enter

MEASURE macro execution

B - 11

Appendix B.
Renishaw NC1 tool adjustment system

BRKTL

Broken Tool Detection? (Y/N)

Y

Data Entry:
Insert Tool Number:

BRKTL macro execution

PR_DIFF

Requalify Setting axes? (Y/N)

Y

Data Entry:
Enter the data requested in the pull-down menu

PR_DIFF macro execution

Enter

N

N

Exit

Check the values entered in the variables requested in the pull-down menu, since they might
cause incorrect positioning of the tool.
Before proceeding with execution of the MAIN macro, move the sample tool, already installed on
the electrospindle, to the position used for tool adjustment; generally in the middle of the beam and
at about 10 mm (0.394 in) on Z above the centre of the beam.
The positioning value must be written in the parameters E105, E106, E107 and in the SETUP file.

The first request of the MAIN macro is to run the alignment cycle of the NC1 probe.

 ALIGN macro:

Running Beam Alignment? (Y/N): Y

B - 12

BIESSE S.p.A. ©

(a732h0001.fm-181103)

Appendix B.

Renishaw NC1 tool adjustment system

 Confirm by pressing the <ENTER> key.

 Entering the letter Y, you are requested to enter the number of the sample tool, previously

entered in magazine 1, whose length and diameter data should already have been entered in
the variable E108 (length), E109 (diameter) and in the SETUP file. As the degree of precision
of the NC1 probe alignment depends on these data, it is recommended to always enter them
and to be as accurate as possible.
In the window below a test tool (1) has been used. The sample tool must always be loaded in
magazine 1, regardless of whether it is a revolver magazine with 10 tool holders or a chain
magazine with 12 tool holders.

Insert Tool number calibrated : 1.000

 Confirm by pressing the <ENTER> key.

 The alignment phase is executed automatically. At the end of the alignment cycle the program

highlights the misalignment of the NC1 device on the Z-axis. Pressing the START CYCLE
button on the pilot panel, the program highlights the misalignment on the X-axis.

 Make the mechanical correction of the +/- error of the X-axis by loosening the support plate,

making small movements along the Y-axis and then tightening the support plate.

P2

P1

Y+

+error

X+

 Make the mechanical correction of the +/- error of the Z-axis by turning the adjusting

lockscrew with a No. 4 wrench.

P2

P1

Z+

+error

X+
Y+

 If the tolerance exceeds +/- 0.03 hundredths for both the Z and the X axis, the alignment

macro must be executed again, confirming the new request with Y:

Running new cycle alignment? (Y/N): Y

BIESSE S.p.A. ©
(a732h0001.fm-181103)

B - 13

Appendix B.
Renishaw NC1 tool adjustment system

 Confirm by pressing the <ENTER> key.

 Entering the letter Y, the cycle is again executed until the misalignment positions fall within the

required tolerances.

 Entering the letter N, the CALIB macro is executed, which determines the origins of the centre

of the laser tracer. These origins are subsequently used as fundamental reference for the
"Requalify Tool" and "Tool integrity check" macros. This procedure must be carried out
periodically as the device is fitted on the Y-axis work table since subject to continuous
vibration and movements.

 At the end of the calibration phase the next request is "Requalify tool".

 MEASURE macro:

Riqualify Tool offset? (Y/N): Y

 Confirm by pressing the <ENTER> key.

 Entering the letter Y, you are requested to enter the number of the tool to be requalified:

Insert tool number: 2.000

 Confirm by pressing the <ENTER> key.

 After the tool has been activated (loading on the spindle) the requalify data is requested.

E6 = 0 tool length
E6 = 2 tool diameter

 Data requested by DATA ENTRY for tool requalification:

Measuring height of tool
Radial step over for lenght setting
Overtrav. Dist. And radial clarence
Spindle rotation

E4 : 0.0000
E5 : 0.0000
E15 : 10.000
E55 : 3000.0

 Confirm by pressing the <ENTER> key.

 The data requested in the previous pull-down menu determines the acquisition mode of the

length and diameter of the tool; the variables below assume the following meaning:

B - 14

BIESSE S.p.A. ©

(a732h0001.fm-181103)

Renishaw NC1 tool adjustment system

The following figure regards acquisition of the
length only. The variable requested is E5, which
determines at what point with respect to the
centre the tool measures its length. It is
normally used for tools that have cutting edges
on the mill edge and non-rotating tools. By
default the parameter is set to 0, since in most
cases tracing is done in the centre of the tool
with the mill rotating.

The following figure illustrates acquisition of the
tool length and diameter. The variables in this
case assume the following meaning:
E4; is the position of the Z-axis on the side of
the tool on which the measurement is carried
out.
E5; As above.
E15; is the distance of the tool above the beam
before the start of measuring.
E55; is the tool rotation speed during
measuring.

Length setting
with no ES
input

E5

21

E15

Appendix B.

E5

3

Length setting
with ES input

21

E15

E4

 The cycle is executed automatically. At the end of requalification the tool is deposited in the

magazine and the data is loaded in the OFFSET table of the NC.

 To repeat the cycle with a new tool, enter the letter Y. To continue with a new request, enter

the letter N.

Riqualify Tool offset? (Y/N): N

 Confirm by pressing the <ENTER> key.

 Entering the letter N, the BRKTL macro appears for the "Tool integrity check".

Broken Tool detection? (Y/N): Y

BIESSE S.p.A. ©
(a732h0001.fm-181103)

B - 15

Appendix B.
Renishaw NC1 tool adjustment system

 Entering the letter Y, you are requested to enter the "tool number" to check for any breakage.

Insert Tool number? : 1.000

 Confirm by pressing the <ENTER> key.

 The following request regards the broken tool detection cycle with the BRKTL macro. This

cycle uses a plunge control which moves the tool inside and outside the laser beam on the
axis used for length adjustment. The cycle checks if there are any long tools due to possible
extraction of the tool during machining.

 The data requested requires the following variables which assume the following meaning:

Radial step over distance
Value that define,when the tool BRK
Spindle rotation (default 3000 rpm)

E5 : 0.00000
E10 : -0.25
E55 : 3000.00

Z

E10

E5

 Confirm by pressing the <ENTER> key.

E5; Correction along the laser beam at which measuring of the tool length occurs. 0 is the
default value.
E10; Tolerance value which determines tool breakage. The negative value (E10-) checks
both the presence of a possible broken tool and the presence of long tools. -0.25 is the default
value.
E55; Spindle speed at which the tool breakage check is carried out (see SETUP macro).

 To repeat the cycle with a new tool, enter the letter Y. To continue with a new request, enter

the letter N.

Broken Tool detection? (Y/N): N

 Confirm by pressing the <ENTER> key.

 Entering the letter N, "requalify working unit positions" with the PR_DIFF macro is requested.

Riqualify Setting axis? (Y/N): Y

 Confirm by pressing the <ENTER> key.

B - 16

BIESSE S.p.A. ©

(a732h0001.fm-181103)

Appendix B.

Renishaw NC1 tool adjustment system

 The PR_DIFF macro allows performing automatic alignment of the working units when tools

of the same family are used and when performing simultaneous machining operations of
several identical workpieces. Since inserting the tool in the HSK cone or the ISO30 cone does
not guarantee the same position for each tool of the same family, this macro allows
determining their length. The differences found on each tool are automatically loaded in the
TOOL table of the NC and are activated during descent of the working units. This allows
machining with the working units perfectly aligned.

This macro can be used on the working units with Electronic Setting axis controlled by
the NC.

The following figure shows some tools with different lengths, but perfectly aligned.

Z

Y

X

T21 T11 T1

 The cycle is executed automatically. After requalification of the working units, the data is

loaded in the TOOL table in EDITOR mode after having selected the tool. Example: tool 1
Field:
Tool Difference 2_1; (difference in tool length of working unit 2 - compared to working unit 1)
Tool Difference 3_1; (difference in tool length of working unit 3 - compared to working unit 1)
Tool Difference 4_1; (difference in tool length of working unit 4 - compared to working unit 1)

 Repeat the cycle, as requested, entering the letter Y.

Riqualify Setting axis? (Y/N): Y

 Confirm by pressing the <ENTER> key.

 To terminate the MAIN program, enter the letter N. The machine goes into reset state. Launch

the program.

CAUTION

For good functioning of the machine, the meaning of the variables to be used in the macros
must be known in detail.

BIESSE S.p.A. ©
(a732h0001.fm-181103)

B - 17

Appendix B.
Renishaw NC1 tool adjustment system

B.11 Using the individual macros

This chapter explains the use of the individual macros to be used instead of the MAIN macro.

CLRVAR macro execution

Before executing any cycle, always run the CLRVAR macro which resets all the E variables (E0
through E150). This operation is important, since the values stored in the E variables are not
automatically deleted after execution of the program. Any optional input in the subsequent macros
hence remains active until it is deleted.

B.12 Laser beam alignment

INFORMATION

At the time of installation and setup of the system, the beam alignment macro must be executed
before using the CALIB macro to calibrate the system.

To align the laser beam, to be done during installation of the NC1 system, the ALIGN macro is
used. The use of the beam alignment cycle allows carrying out the following operations:

 Checking that the alignment with the machine axis is correct.

 Measuring the provisional position of the laser beam on the Z-axis.

 Measuring the provisional position of the beam on the X-axis and the Y-axis. The

measurements must be made on the positive and/or negative sides of the beam.

 Adjusting the measuring point along the beam axis on which the tool is measured. The

provisional values are updated during execution of the calibration cycle. Even though the
beam alignment macro is used mainly during installation of the NC1 system, it can also be
used to check ordinary alignment.

ALIGN macro approach position on X/Y/Z
with respect to the machine origin

at starting point

R(+/-)Jog or handwheel

Z

Y

X

INFORMATION

E3

When using the beam alignment macro, consult the guide to installation and List of components of
the Renishaw NC1 non-contact tool adjustment system (Art. Renishaw H-2000-5129) containing

the instructions for physical alignment of the beam with the transmitter.

B - 18

BIESSE S.p.A. ©

(a732h0001.fm-181103)

Appendix B.

Renishaw NC1 tool adjustment system

Calibration tool required

The cycle requires a calibration tool to be installed on the spindle. The ideal solution is a
cylindrical-type, robust, flat-bottomed tool with minimal eccentricity. The exact adjustment length
and diameter of the tool must be known.

 Install the calibration tool on the spindle.

 Move the tool to the position used for tool adjustment, generally in the middle of the beam and

at about 10 mm (0.394 in) above the centre of the beam (see figure in paragraph B.12 “Laser

beam alignment”), using JOG mode. The cycle, after having measured the beam, returns to

the central position and terminates on a program stop M00.

 After carrying out the beam alignment adjustments, the cycle must be restarted in order to

identify the new alignment errors.

Adjustment data

Before proceeding, check that the SETUP macro settings are correct.
For further information consult the paragraph “Macro variables for adjustment data” on page B -

5.

Format

T.x M6 (sample tool corrector activation)
(CLS, CLRVAR) (variable reset)
E3 = 100
[E4 = 5.]
(CLS, ALIGN) (ALIGN macro call)
where [ ] indicates the optional inputs

Macro inputs

The following inputs are used with the ALIGN macro:

 E3; Distance between the reference measuring points.

For greatest accuracy, the distance value must be as high as possible, compatible with the
space between the transmitter and the receiver of the NC1 system and the dimensions of the
calibration tool.

 E4; Incremental measuring depth.

The value determines the depth on the calibration tool at which calibration is carried out.
Default Value: 15 mm (0.38 in).

Input E3: When the value of the input E3 is specified, make sure that the tool holder does not
collide with the NC1 tool adjustment system. If the default input Z is used for the incremental
measuring depth, the calibration tool projection must be at least 35 mm (1.38 in).

BIESSE S.p.A. ©
(a732h0001.fm-181103)

B - 19

Appendix B.
Renishaw NC1 tool adjustment system

Output

After execution of the cycle, the following outputs are displayed:

 E52; Beam alignment error relating to the X-axis on the distance measured.

(empty if the X-axis is the beam axis)

P2

P1

Y+

+error

X+

 E52; Beam alignment error relating to the Y-axis on the distance measured.

(empty if the Y-axis is the beam axis)

+error

P2

P1

Y+

X+

 E47; Beam alignment error relating to the Z-axis on the distance measured.

(empty if the Z-axis is the beam axis)

P2

P1

Z+

+error

X+
Y+

Example:

Beam alignment and adjustment of provisional beam
Position

"N1"
G0 G79 Z-5

G1 Z......

G1 X..... Y......

(CLS ,CLRVAR)
G0

B - 20

BIESSE S.p.A. ©

(a732h0001.fm-181103)

Appendix B.

Renishaw NC1 tool adjustment system

T. 1M 6
E3 = 10 (Axial distance between the measurements)
E4 = 10 (Search distance)
(CLS, ALIGN)
G0
M0 (programmed cycle stop)
(GTO,N1) (macro repeat)

B.13 NC1 system calibration

The CALIB macro is used to carry out normal calibration of the NC1 system. It must also be used
after beam alignment by means of the beam alignment cycle. The calibration cycle is used to
accurately calibrate the beam positions on the X, Y and Z axes.

Before executing this or other cycles (except for the ALIGN macro for beam alignment) load the
nominal calibration data.
The data can be entered automatically using the ALIGN macro for beam alignment. Alternatively,
the indicative data can be entered manually (for further information, consult the paragraph “Macro

variables for adjustment data” on Page B - 5).

Install the calibration tool on the machine spindle and activate the tool number (T) before
executing the cycle.
The beam position on the Z-axis and the beam centre are calibrated on both the X and the Y axis
during tool rotation. The beam width is calibrated by means of the static balance of the tool. This
allows eliminating the eccentricity errors which may be introduced by the tool.

21

3

E5

E4E4

Format

(CLS, CALIB)
T.2 M 6
(CLS, CLRVAR)
[E4=5.]

BIESSE S.p.A. ©
(a732h0001.fm-181103)

B - 21

Appendix B.
Renishaw NC1 tool adjustment system

(CLS, CALIB)
where [ ] indicates the optional inputs

Calibration tool required

The cycle requires a calibration tool to be installed on the machine spindle. Moreover, the tool
number (T) must be active.
The ideal solution is a cylindrical-type, robust, flat-bottomed tool with minimal eccentricity. The
exact adjustment length and diameter of the tool must be known.

Macro inputs

The following inputs are used with the CALIB macro:

E4; Adjustment height on the tool.
Determines the height of the beam on the tool at which diameter calibration occurs. The default
value is 5 mm (0.197 in).

E5; Radial step-over for length calibration.
Determines the correction along the beam at which measuring occurs. The tool always first goes
down on the centre line of the beam. Default Value: on centre.

E55; Spindle speed at which calibration occurs
For further information consult the paragraph “Macro variables for adjustment data” on Page B -

5). Default Value: 3000 rpm (E70).

Output

After execution of the cycle, the following outputs are set or updated:

L140; Central position relative to the X-axis of the beam.
L141; Central position relative to the Y-axis of the beam.
L142; position relative to the Z-axis of the beam.
L143; Beam thickness when the measurement is made on both sides.

Alarms

After execution of the cycle, the following alarms may be activated:

BEAM LOCKED
CALIBRATION INPUT (E9) ABSENT
PROBE PARAMETERS NOT SPECIFIED
CHECK VIA PROBE NOT EXECUTED

B - 22

BIESSE S.p.A. ©

(a732h0001.fm-181103)

Appendix B.

Renishaw NC1 tool adjustment system

For further clarification on the meaning of the alarms, consult the paragraph B.17 “Error

messages and alarms” on Page B - 31.

Example:

Calibration with tool T1 88.0 mm (3.46 in) in length and 6.0 mm (0.236 in) in diameter.

“N1”
G0 G79 Z-5
G1 Z……
G1 X….. Y……
(CLS ,CLRVAR)
G0
T.x M 6
E4 = 10
(CLS, CALIB)
G0
M0 (programmed cycle stop)
(GTO,N1) (macro repeat)

B.14 Tool length adjustment

The MEASURE macro is used to measure the effective length of a cutting tool (E6=0).
The tool length measuring cycle is suitable for "on-centre" adjustment of tools such as drills and
mills with rounded ends and for "off-centre" adjustment of tools such as face mills and cylindrical
end mills.
The length is measured during tool rotation.
The following figure illustrates two types of cycle.

Length adjustment without input E5 Length adjustment with input E5

Length setting
with no ES
Input

Length setting
with ES input

21

E5

BIESSE S.p.A. ©
(a732h0001.fm-181103)

B - 23

Appendix B.
Renishaw NC1 tool adjustment system

For shaped tools the variable E5 may be considered as shown in the following figure, where, for
machining requirements, the length does not necessarily need to be the base of the tool; In fact,
there are no cutting edges on the base. In this case the variable E4 is not considered.

Acquisition point
Tool length
Moving from the centre of ES

ES

Tool cutting edges

The effective tool length is written in the tool correction register. If the controller has separate wear
and geometry registers, the wear register is reset and the length value is written in the geometry
register.

Format

T. 1M 6
(CLS, CLRVAR)
[E6 = 0]
[E5 = 5.]
(CLS, MEASURE)
where [ ] indicates the optional inputs

Macro inputs

The following inputs are used with the MEASURE macro:

E6=0; Adjust the tool length.

The default input is 0.
With the MAIN program, E6 is automatically defined.

E5; Radial step-over for length adjustment. Default Value: on centre.

E15; Overlimit distance. For further information consult the paragraph “Macro variables for

adjustment data” on page B - 5.

Default Value: 5.0 mm (0.197 in).

E55; Spindle speed at which diameter measurement occurs. For further information consult the
paragraph “Macro variables for adjustment data” on page B - 5. Default Value: 3000 rpm

Output

After execution of the cycle, the output "Active tool length register" is set or updated.

B - 24

BIESSE S.p.A. ©

(a732h0001.fm-181103)

Appendix B.

Renishaw NC1 tool adjustment system

Alarms

After execution of the cycle, the following alarms may be activated:

BEAM LOCKED
PROBE PARAMETERS NOT SPECIFIED
CHECK VIA PROBE NOT EXECUTED

For further clarification on the meaning of the alarms, consult the paragraph B.17 “Error

messages and alarms” on page B - 31.

Examples:

 Tool length adjustment - tool "on-centre":

N1
G0 G79 Z-5
G1 Z……

G1 X….. Y.......

(CLS, CLRVAR)
G0
T. 1M 6
(CLS, MEASURE)
G0
M0
(GTO,N) (programmed cycle stop)

(macro repeat)

 Tool length adjustment - tool "off-centre":

N1
G0 G79 Z-5
G1 Z……
G1 X….. Y…….
(CLS, CLRVAR)
G0
T. 1M 6
(CLS, CLRVAR)
E5 = 38

Adjust the tool (1) correction to a radial step-over of 38 mm (1.496 in)

(CLS,
MEASURE)
G0
M0

(programmed cycle stop)
(macro repeat)

(GTO,N1)

BIESSE S.p.A. ©
(a732h0001.fm-181103)

B - 25

Appendix B.
Renishaw NC1 tool adjustment system

B.15 Tool diameter and length adjustment

The MEASURE macro is used to measure the effective length and diameter of a tool (E6=2). The
tool length and diameter measuring cycle is suitable for the boring tools and for the following mills:
front, two-fluted, end, disk, dovetail.

The figure below illustrates the movements of the combined cycle. Radial measurements (3) can
be made on one or both sides of the beam (see E2, paragraph “Macro variables for adjustment

data” on Page B - 5).

21

3

E5

E5

E15

E4

The single cycle combines the tool length measuring cycle (consult the paragraph B.14 “Tool

length adjustment” on Page B - 23).

The length and diameter values are written in the tool correction register. If the controller has
separate wear and geometry registers, the wear registers are reset and the values are written in
the geometry registers.

Format

T.1 M 6
(CLS, CLRVAR)
E6 = 2.
[E4 = 8.]
[E5 = 5.]
[E55 = 1000.]
(CLS, MEASURE)
where [ ] indicates the optional inputs

Macro inputs

The following inputs are used with the MEASURE macro:

E6=2; measure the tool length and diameter.

B - 26

BIESSE S.p.A. ©

(a732h0001.fm-181103)