Introduction 1
Turning On,
SINUMERIK 802D
SINUMERIK 802D base line
Programming and Operating
Turning
Reference−Point Approach
Setting Up 3
Manually Controlled Mode 4
Automatic Mode 5
Part Programming 6
System 7
Programming 8
2
Valid for
Control system Software version
SINUMERIK 802D 2
SINUMERIK 802D base line 1
Cycles 9
08/05 Edition
Safety information
This Manual contains information which you should carefully observe to ensure your own personal safety
and the prevention of material damage. The notices are highlighted by a warning triangle and, depending on
the degree of hazard, represented as shown below:
Danger
!
indicates that death or severe personal injury will result if proper precautions are not taken.
Warning
!
indicates that death or severe personal injury can result if proper precautions are not taken.
Caution
!
with a warning triangle indicates that minor personal injury can result if proper precautions are not taken.
Caution
without a warning triangle means that material damage can occur if the appropriate precautions are not
taken.
Attention
indicates that an undesired event or status can occur if the appropriate note is not observed.
If several hazards of different degrees occur, the hazard with the highest degree must always be given preference. If a warning note with a warning triangle warns of personal injury, the same warning note can also
contain a warning of material damage.
Qualified personnel
Start−up and operation of the device/equipment/system in question must only be performed using this documentation. The start−up and operation of a device/system must only be performed by qualified personnel.
Qualified personnel as referred to in the safety guidelines in this documentation are those who are authorized to start up, earth and label units, systems and circuits in accordance with the relevant safety standards.
Proper use
Please note the following:
Warning
!
The device may only be used for the applications described in the Catalog and only in combination with the
equipment, components and devices of other manufacturers as far as this is recommended or permitted by
Siemens. It is assumed that this product be transported, stored and installed as intended and maintained
and operated with care to ensure that the product functions correctly and properly.
Trademarks
All designations marked with the copyright notice ® are registered trademarks of Siemens AG. Other names
in this publication might be trademarks whose use by a third party for its own purposes may violate the rights
of the registered holder.
Disclaimer of liability
Although we have checked the contents of this publication for agreement with the hardware and software
described, since differences cannot be totally ruled out. Nonetheless, differences might exist and therefore
we cannot guarantee that they are completely identical. The information given in this publication is reviewed
at regular intervals and any corrections that might be necessary are made in the subsequent editions.
Siemens AG
Automation and Drives
Postfach 4848
90437 NÜRNBERG
GERMANY
Copyright (E) Siemens AG 2005.
6FC5698−2AA00−1BP4
Siemens AG 2005
Subject to change without prior notice.
Preface
SINUMERIK Documentation
The SINUMERIK Documentation is organized in 3 levels:
S General Documentation:
S User Documentation
S Manufacturer/Service Documentation:
For detailed information regarding further publications about SINUMERIK 802D, as well as
for publications that apply for all SINUMERIK control systems (e.g. Universal Interface, Measuring Cycles...), please contact your Siemens branch office.
A monthly overview of publications with specification of the available languages can be found
on the Internet at:
http://www.siemens.com/motioncontrol
Follow the menu items ”Support”/”Technical Documentation”/”Overview of Publications”.
The Internet edition of DOConCD − DOConWEB − can be found at:
http://www.automation.siemens.com/doconweb
Addressees of the documentation
Standard scope
Hotline
The present documentation is aimed at the machine tool manufacturer. This publication provides detailed information required for the machine tool manufacturer to start up the SINUMERIK 802D control system.
The present Instruction Manual describes the functionality of the standard scope. Any
amendments made by the machine manufacturer are documented by the machine manufacturer.
Other functions not described in this documentation can possibly also be performed on the
control system. However, the customer is not entitled to demand these functions when the
new equipment is supplied or servicing is carried out.
If you have any questions, do not hesitate to call our hotline:
A&D Technical Support
Tel.: +49 (0) 180 / 5050 − 222
Fax: +49 (0) 180 / 5050 − 223
Internet: http://www.siemens.de/automation/support−request
If you have any questions (suggestions, corrections) regarding the Documentation, please
send a fax to the following number or an e−mail to the following address:
Fax: +49 (0) 9131 / 98 − 63315
E−mail: motioncontrol.docu@siemens.com
Fax form: see return fax form at the end of this publication
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
iii
Preface
Internet address
http://www.siemens.com/motioncontrol
iv
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Contents
1 Introduction 1-11 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.1 Screen layout 1-11 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.2 Operating areas 1-14 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.3 Accessibility options 1-15 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.3.1 Calculator 1-15 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.3.2 Editing Chinese characters 1-20 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.3.3 Hotkeys 1-21 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.4 The help system 1-22 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.5 Coordinate systems 1-24 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2 Turning On and Reference Point Approach 2-27 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3 Setting Up 3-29 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3.1 Entering the tools and the tool offsets operating area”# 3-30 . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3.1.1 Use this softkey to create a new tool. 3-32 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3.1.2 Determining the tool offsets (manually) 3-33 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3.1.3 Determining tool compensations using a probe 3-36 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3.1.4 Determining the tool offsets using optical measuring instruments 3-37 . . . . . . . . . . . . . . . . . . . . .
3.1.5 Probe settings 3-38 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3.2 Tool monitoring 3-40 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3.3 Entering/modifying a work offset 3-42 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3.3.1 Determining the work offset 3-43 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3.4 Programming setting data - ”Parameter” operating area 3-44 . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3.5 R parameters − ”Offset/Parameter”operating area 3-47 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Contents
4 Manually Controlled Mode 4-49 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.1 Mode Jog - ”Position” operating area 4-50 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.1.1 Assigning handwheels 4-53 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.2 MDA mode (Manual input) - ”Machine” operating area 4-54 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.2.1 Face turning 4-57 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5 Automatic Mode 5-61 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5.1 Selecting / starting a part program - ”Machine” operating area 5-66 . . . . . . . . . . . . . . . . . . . . . . .
5.2 Block search - ”Machine” operating area 5-67 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5.3 Stopping / canceling a part program 5-68 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5.4 Reapproach after cancellation 5-69 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5.5 Repositioning after interruption 5-69 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5.6 Program execution from external source (RS232 interface) 5-70 . . . . . . . . . . . . . . . . . . . . . . . . . .
6 Part Programming 6-71 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
6.1 Entering a new program - ”Program” operating area 6-74 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
6.2 Editing part programs - ”Program” operating area 6-75 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
6.3 Blueprint programming 6-77 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
6.4 Simulation 6-95 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
6.5 Data transfer via the RS232 interface 6-96 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
v
Contents
7 System 7-99 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7.1 PLC diagnosis represented as a ladder diagram 7-120 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7.1.1 Screen layout 7-120 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7.1.2 Operating options 7-121 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8 Programming 8-131 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.1 Fundamentals of NC programming 8-131 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.1.1 Program names 8-131 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.1.2 Program structure 8-131 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.1.3 Word structure and address 8-132 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.1.4 Block structure 8-133 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.1.5 Character set 8-134 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.1.6 Overview of the instructions 8-136 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.2 Positional data 8-148 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.2.1 Absolute / incremental dimensioning: G90, G91, AC, IC 8-148 . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.2.2 Dimensions in metric units and inches: G71, G70, G710, G700 8-149 . . . . . . . . . . . . . . . . . . . . . .
8.2.3 Radius / diameter dimensional notation: DIAMOF, DIAMON 8-150 . . . . . . . . . . . . . . . . . . . . . . . . .
8.2.4 Programmable work offset: TRANS, ATRANS 8-151 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.2.5 Programmable scaling factor: SCALE, ASCALE 8-152 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.2.6 Workpiece clamping − settable work offset:
G54 to G59, G500, G53, G153 8-154 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.2.7 Programmable working area limitation:
G25, G26, WALIMON, WALIMOF 8-155 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3 Axis movements 8-157 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.1 Linear interpolation with rapid traverse: G0 8-157 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.2 Linear interpolation with feedrate: G1 8-158 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.3 Circular Interpolation: G2, G3 8-159 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.4 Circular interpolation via intermediate point: CIP 8-162 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.5 Circle with tangential transition: CT 8-162 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.6 Thread cutting with constant lead: G33 8-163 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.7 Thread cutting with variable lead: G34, G35 8-166 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.8 Thread Interpolation: G331, G332 8-167 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.9 Fixed point approach: G75 8-168 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.10 Reference point approach: G74 8-168 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.11 Measuring with touch−trigger probe: MEAS, MEAW 8-169 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.12 Feedrate F 8-170 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.13 Exact stop / continuous−path control mode: G9, G60, G64 8-171 . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.14 Acceleration pattern: BRISK, SOFT 8-173 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.15 Percentage acceleration override: ACC 8-174 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.16 Traversing with feedforward control: FFWON, FFWOF 8-175 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.17 3rd and 4th axes 8-176 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.18 Dwell Time: G4 8-176 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3.19 Travel to fixed stop 8-177 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.4 Spindle movements 8-181 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.4.1 Spindle speed S, directions of rotation 8-181 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.4.2 Spindle speed limitation: G25, G26 8-181 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.4.3 Spindle positioning: SPOS 8-182 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.4.4 Gear stages 8-183
8.4.5 2nd spindle 8-183 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.5 Special turning functions 8-185 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.5.1 Constant cutting rate: G96, G97 8-185 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.5.2 Rounding, chamfer 8-187 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.5.3 Blueprint programming 8-188 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.6 Tool and tool offset 8-191 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.6.1 General notes 8-191 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.6.2 Tool T 8-191 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.6.3 Tool offset number D 8-192 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
vi
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
8.6.4 Selecting the tool radius compensation: G41, G42 8-196 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.6.5 Corner behavior: G450, G451 8-197 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.6.6 Tool radius compensation OFF: G40 8-199 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.6.7 Special cases of the tool radius compensation 8-200 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.6.8 Example of tool radius compensation 8-201 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.6.9 Use of milling cutters 8-202 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.6.10 Special handling of tool compensation 8-204 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.7 Miscellaneous function (M) 8-205 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.8 H function 8-206 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.9 Arithmetic parameters R, LUD and PLC variables 8-207 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.9.1 Arithmetic parameters R 8-207 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.9.2 Local User Data (LUD) 8-208 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.9.3 Reading and writing PLC variables 8-210 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.10 Program jumps 8-211 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.10.1 Jump destination for program jumps 8-211 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.10.2 Unconditional program jumps 8-211 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.10.3 Conditional program jumps 8-212 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.10.4 Program example for jumps 8-214 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.11 Subroutine technique 8-215 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.11.1 General 8-215 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.11.2 Calling machining cycles 8-217 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.12 Timers and workpiece counters 8-218 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.12.1 Runtime timer 8-218 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.12.2 Workpiece counter 8-219 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.13 Language commands for tool monitoring 8-221 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.13.1 Tool monitoring overview 8-221 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.13.2 Tool life monitoring 8-222 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.13.3 Workpiece count monitoring 8-223 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.14 Milling on turning machines 8-226 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.14.1 Milling of the front face − TRANSMIT 8-226 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.14.2 Milling of the peripheral surface − TRACYL 8-228 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.15 G functions equivalent to the SINUMERIK 802S − Turning 8-233 . . . . . . . . . . . . . . . . . . . . . . . . . .
Contents
9 Cycles 9-235 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.1 Overview of cycles 9-235 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.2 Programming cycles 9-236 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.3 Graphical cycle support in the program editor 9-238 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.4 Drilling cycles 9-240 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.4.1 General 9-240 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.4.2 Prerequisites 9-241 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.4.3 Drilling, centering – CYCLE81 9-242 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.4.4 Drilling, counterboring – CYCLE82 9-245 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.4.5 Deep hole drilling – CYCLE83 9-247 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.4.6 Rigid tapping – CYCLE84 9-251 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.4.7 Tapping with compensating chuck – CYCLE840 9-254 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.4.8 Reaming1 (boring 1) – CYCLE85 9-258 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.4.9 Boring (boring 2) – CYCLE86 9-261 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.4.10 Boring with Stop 1 (boring 3) – CYCLE87 9-264 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.4.11 Drilling with stop 2 (boring 4) – CYCLE88 9-267 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.4.12 Reaming 2 (boring 5) – CYCLE89 9-269 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.4.13 Row of holes – HOLES1 9-271 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.4.14 Circle of holes – HOLES2 9-275 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.5 Turning cycles 9-278 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
vii
Contents
9.5.1 Prerequisites 9-278 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.5.2 Grooving – CYCLE93 9-280 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.5.3 Undercut (forms E and F to DIN) – CYCLE94 9-288 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.5.4 Machining with undercut – CYCLE95 9-292 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.5.5 Thread undercut – CYCLE96 9-305 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.5.6 Thread cutting – CYCLE97 9-309 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.5.7 Chaining of threads – CYCLE98 9-315 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.6 Error Messages and Error Handling 9-322 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.6.1 General notes 9-322 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.6.2 Error handling in the cycles 9-322 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.6.3 Overview of cycle alarms 9-322 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.6.4 Messages in the cycles 9-324 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
viii
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
SINUMERIK 802D Key Definition
SINUMERIK 802D Key Definition
Clear key
&
Insert key
Tabulator
ENTER / Input key
”Position” operating area key
”Program” operating area key
”Parameter” operating area
”Program Manager” operating area
”Alarm/System” operating area
not assigned
”Recall” key
ETC key
”Acknowledge alarm” key
without function
Info key
Shift key
Controlkey
Altkey
SPACE
Backspace
PageUp / PageDown keys
Cursor keys
Selection key / toggle key
Alphanumeric keys
Double assignment on the Shift level
Numeric keys
Double assignment on the Shift level
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
ix
External Machine Control Panel
External Machine Control Panel
%
Spindle override
User−defined key with LED
User−defined key without LED
INCREMENT
80
70
60
90
100
110
120
JOG
REFERENCE POINT
AUTOMATIC
60
70
40
20
10
6
2
0
80
90
100
110
120
SINGLE BLOCK
MANUAL DATA
SPINDLE START LEFT
SPINDLE STOP
RESET
NC STOP
NC START
EMERGENCY STOP
X axis
Z axis
%
SPINDLE START RIGHT
RAPID TRAVERSE OVERRIDE
Feedrate override
x
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Introduction
Note
The present Manual always uses ”802D bl” as an acronym for SINUMERIK 802D base line.
1.1 Screen layout
1
Status area
Applicationarea
Tip
and softkey area
Fig. 1-1 Screen layout
The screen is divided into the following main areas:
S Status area
S Applicationarea
S Tip and softkey area
G
function
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
1-11
Introduction
MDA
y
System
1. Alarm number with alarm text, or
1.1 Screen layout
Status area
Fig. 1-2 Status area
Table 1-1 Explanation of the display elements in the status area
Screen Con-
trol
1
2
3
4
Display Meaning
Active operating area, active mode
Position
JOG; 1 INC, 10 INC, 100 INC, 1000 INC, VAR INC (evaluation by increments in the
JOG mode)
MDA
AUTOMATIC
Offset
Program
Program Manager
S
stem
Alarm
Marked as an ”external language” using G291
Alarm and message line
In addition, the following is displayed:
1. Alarm number with alarm text, or
2. Message text
Program status
RESET Program canceled / default status
RUN Program running
STOP Program stopped
Program controls in the AUTOMATIC mode
1-12
5
6
7
Reserved
NC messages
Selected part program (main program)
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Tip and softkey area
Fig. 1-3 Tip and softkey area
Introduction
1.1 Screen layout
Table 1-2 Explanation of the screen elements in the tip and softkey area
Screen Con-
trol
1
2
3
4
Display Meaning
Recall symbol
Pressing the Recall key lets you return to the next higher menu level.
Tip line
Displays tips for the operator
MMCstatus information
ETC is possible (Pressing this key displays the horizontal softkey bar
providing further functions.)
Mixed notation active
Data transfer running
Connection to the PLC programming tool active
Softkey bar vertical and horizontal
Standard softkeys
Use this softkey to quit the screenform.
Use this softkey to cancel the input; the window is closed.
Selecting this softkey will complete your input and start the calculation.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
1-13
Introduction
1.2 Operating areas
Selecting this softkey will complete your input and accept the values you have entered.
This function is used to switch the screenform from diameter programming to radius programming.
1.2 Operating areas
The functions of the control system can be carried out in the following operating areas:
Position Machine operation
Offset/Parameters Input of offset values and setting data
Program Creation of part programs
Protection levels
Program Manager Part program directory
System Diagnosis, start−up
Alarm Alarm and message lists
To switch the operating area, use the relevant key (hard key).
The input and modification of vital data in the control system is protected by passwords.
In the menus listed below the input and modification of data depends on the protection level
set:
S Tool offsets
S Work offsets
S Setting data
S RS232 settings
S Program creation / program correction
1-14
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
1.3 Accessibility options
1.3.1 Calculator
The calculator function can be activated from any operating area using ”SHIFT” and ”=”.
To calculate terms, the four basic arithmetic operations can be used, as well as the functions
”sine”, ”cosine”, ”squaring” and ”square root”. A bracket function is provided to calculate
nested terms. The bracket depth is unlimited.
If the input field is already occupied by a value, the function will accept this value into the
input line of the calculator.
When you press the Input key, the result is calculated and displayed in the calculator.
Selecting the Accept softkey enters the result in the input field at the current cursor position
of the part program editor and closes the calculator automatically.
Introduction
1.3 Accessibility options
Note
If an input field is in the editing mode, it is possible to restore the original status using the
”Toggle” key.
Fig. 1-4 Calculator
Characters permitted for input
+, −, *, / Basic arithmetic operations
S Sine function
The X value (in degrees) in front of the input cursor is replaced by the sin(X) value.
O Cosine function
The X value (in degrees) in front of the input cursor is replaced by the cos(X) value.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
1-15
Introduction
1.3 Accessibility options
Q Square function
The X value in front of the input cursor is replaced by the X
R Square root function
The X value in front of the input cursor is replaced by the √⎮ value.
( ) Bracket function (X+Y)*Z
Calculation examples
100 + (67*3) 100+67*3 −> 301
sin(45_) 45 S −> 0.707107
cos(45_) 45 C −> 0.707107
2
4
√4 4 R −> 2
(34+3*2)*10 (34+3*2)*10 −> 400
To calculate auxiliary points on a contour, the calculator offers the following functions:
S Calculating the tangential transition between a circle sector and a straight line
S Moving a point in the plane
2
value.
Task Input −> Result
4 Q −> 16
Softkeys
S Converting polar coordinates to Cartesian coordinates
S Adding the second end point of a straight line/straight line contour section given from an
angular relation
This function is used to calculate a point on a circle. The point results from the angle of the
tangent created, as well as from the radius and the direction of rotation of the circle.
1-16
Fig. 1-5
Enter the circle center, the angle of the tangent and the circle radius.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Introduction
1.3 Accessibility options
G2/G3
Use the G2 / G3 softkey to define the direction of rotation of the circle.
Use this softkey to calculate the abscissa and ordinate values. The abscissa is the first axis,
and the ordinate is the second axis of the plane. The abscissa value is copied into the input
field from which the calculator function has been called, and the value of the ordinate is copied into the next following input field. If the function has been called from the part program
editor, the coordinates are saved with the axis names of the selected basic plane.
Example: Calculate the intersection point between the circle sector
and the straight line
in plane G18.
Given: Radius: 10
Circle center: Z 147 X 103
Connection angle of the straight line: −455
X
XZ
Z
Result: Z = 154.071
X = 110.071
This function calculates the Cartesian coordinates of a point in the plane, which is to be connected to a point in the plane (PP) on a straight line. For calculation, the distance between
the points and the slope angle (A2) of the new straight line to be created with reference to
the slope (A1) of the given straight line must be known.
Fig. 1-6
Enter the following coordinates or angles:
S the coordinates of the given point (PP)
S the slope angle of the straight line (A1)
S the distance of the new point with reference to PP
S the slope angle of the connecting straight line (A2) with reference to A1
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
1-17
Introduction
1.3 Accessibility options
Use this softkey to calculate the Cartesian coordinates which are subsequently copied into
two input fields following one after another. The abscissa value is copied into the input field
from which the calculator function has been called, and the value of the ordinate is copied
into the next following input field.
If the function has been called from the part program editor, the coordinates are saved with
the axis names of the selected basic plane.
This function converts the given polar coordinates into Cartesian coordinates.
Fig. 1-7
Enter the reference point, the vector length and the slope angle.
Use this softkey to calculate the Cartesian coordinates which are subsequently copied into
two input fields following one after another. The abscissa value is copied into the input field
from which the calculator function has been called, and the value of the ordinate is copied
into the next following input field.
If the function has been called from the part program editor, the coordinates are saved with
the axis names of the selected basic plane.
Use this function to calculate the missing end point of the straight line/straight line contour
section whereby the second straight line stands vertically on the first straight line.
The following values of the straight line are known:
Straight line 1:
Starting point and slope angle
Straight line 2:
Length and one end point in the Cartesian coordinate system
1-18
Fig. 1-8
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Introduction
1.3 Accessibility options
This function is used to select the given coordinate of the end point.
The ordinate value or the abscissa value is given.
The second straight line is rotated in the CW direction or in the CCW direction by 90 degrees
relative to the first straight line.
The missing end point is calculated. The abscissa value is copied into the input field from
which the calculator function has been called, and the value of the ordinate is copied into the
next following input field.
If the function has been called from the part program editor, the coordinates are saved with
the axis names of the selected basic plane.
Example
Fig. 1-9
Add the drawing above by the value of the center circle in order to be able to calculate the
intersection point between the circle sector of the straight line. The missing coordinate of the
center point is calculated using the calculator function
, since the radius in the tan-
gential transition stands vertically on the straight line.
Fig. 1-10
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
1-19
Introduction
1.3 Accessibility options
Calculating M1 in section 1:
The radius stands at an angle of 90° turned CW on the straight−line defined by the angle.
Use the softkey
to select the appropriate direction of rotation. Use the softkey
to define the given end point.
Enter the coordinates of the pole, the slope angle of the straight line, the ordinate angle
of the end point and the circle radius as the length.
Fig. 1-11
Result: X = 60
Z = −44.601
1.3.2 Editing Chinese characters
This function is only available in the Chinese language version.
The control system provides a function for editing Chinese characters in the program editor
and in the PLC alarm text editor. After activation, type the phonetic alphabet of the searched
character in the input field. The editor will then offer various characters for this sound, from
which you can choose the desired one by entering either of the digits 1 to 9.
Fig. 1-12 Chinese editor
Alt S Is used to turn on / turn off the editor
1-20
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
1.3.3 Hotkeys
This operator control can be used to select, copy, cut and delete texts using special key
commands. These functions are available both for the part program editor and for input
fields.
CTRL C Copy
CTRL B Select
CTRL X Cut
CTRL V Paste
Alt L Is used to switch to the mixed notation
Alt H Help system
or info key
Introduction
1.3 Accessibility options
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
1-21
Introduction
1.4 The help system
1.4 The help system
To activate the help system, use the Info key. It offers a brief description for all important operating functions.
In addition, the help offers the following topics:
S Overview of the NC commands with a brief description
S Cycle programming
S Explanation of the drive alarms
Show
Go to
topic
Fig. 1-13 Table of contents of the help system
This function opens the selected topic.
Fig. 1-14 Description for a help topic
Use this function to select cross references. A cross reference is marked by the characters
”>>....<<”. This softkey is only unhidden if a cross reference is displayed in the application
area.
1-22
Back to
topic
If you select a cross reference, in addition, the Back to topic softkey is displayed.
This function lets you return to the previous screenform.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Introduction
1.4 The help system
Find
Use this function to search for a term in the table of contents. Type the term you are looking
for and start the search process.
Help in the ”Program editor” area
The system offers an explanation for each NC instruction. To display the help text directly,
position the cursor after the appropriate instruction and press the Info key.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
1-23
Introduction
1.5 Coordinate systems
1.5 Coordinate systems
For machine tools, right−handed, right−angled coordinate systems are used. The movements on the machine are described as a relative movement between tool and workpiece.
+Z
Fig. 1-15 Determination of the axis directions another to one; coordinate system for programming
when turning
Machine coordinate system (MCS)
How the coordinate system is located with reference to the machine, depends on the machine type concerned. It can be rotated in different positions.
+X
+Y
+X
+Z
+Z
+X
Fig. 1-16 Machine coordinates/machine axes using the example of a turning machine
The origin of the coordinate system is the machine zero.
This point only represents a reference point defined by the machine manufacturer. It need
not be approachable.
The traversing range of the machine axes can by in the negative range.
1-24
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Workpiece coordinate system (WCS)
The coordinate system described above (see Fig. 1-15) is also used to describe the geometry of a workpiece in the workpiece program.
The workpiece zero can be freely selected by the programmer in the Z axis. In the X axis, it
lies in the turning center.
Introduction
1.5 Coordinate systems
Fig. 1-17 Workpiece coordinate system
Relative coordinate system
In addition to the machine and workpiece coordinate systems, the control system provides a
relative coordinate system. This coordinate system is used for setting freely selected reference points which have no influence on the active workpiece coordinate system. All axis
movements are displayed relative to these reference points.
Clamping the workpiece
For machining, the workpiece is clamped on the machine. The workpiece must be aligned
such that the axes of the workpiece coordinate system run in parallel with those of the machine. Any resulting offset of the machine zero with reference to the workpiece zero is determined along the Z axis and entered in a data area intended for the settable work offset. In
the NC program, this offset is activated, e.g. using a programmed G54 (see also Section
8.2.6).
Workpiece
W -workpiece zero
X
Workpiece
W
Z
Workpiece
X
Machine
M
Z
Machine
Fig. 1-18 Workpiece on the machine
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
e.g.
Workpiece
G54
X
Workpiece
W
Z
Workpiece
1-25
Introduction
1.5 Coordinate systems
Current workpiece coordinate system
The programmed work offset TRANS can be used to generate an offset with reference to
the workpiece coordinate system resulting in the current workpiece coordinate system (see
Section ”Programmable work offset: TRANS”).
1-26
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Turning On and Reference Point Approach
Note
When you turn on the SINUMERIK 802D and the machine, please also observe the Machine Documentation, since turning on and reference point approach are machine−dependent functions.
This documentation assumes an 802D standard machine control panel (MCP). Should you
use a different MCP, the operation may be other than described herein.
Operating sequence
First, turn on the power supply of CNC and machine. After the control system has booted,
you are in the ”Position” operating area, in the Jog mode.
The ”Reference point approach” window is active.
2
Fig. 2-1 The ”Jog−Ref” start screen
Use the Ref key on the machine control panel to activate ”reference point approach”.
The ”Reference point approach” window (Fig. 2-1) displays whether the axes are referenced
(approached to their reference points).
Axis must be referenced
Axis has reached its reference point
+X
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
...
-Z
Press a direction key.
2-27
Turning On and Reference Point Approach
If you select the wrong approach direction, no motion will be carried out.
Approach the reference points for each axis one after the other.
Quit the function by switching the mode (MDA, AUTOMATIC or Jog).
Note
”Reference point approach” is only possible in the Jog mode.
2-28
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Setting Up
Preliminary remarks
Before you can work with the CNC, set up the machine, the tools, etc. on the CNC as follows:
S Enter the tools and the tool offsets
S Enter/modify the work offset
S Enter the setting data
Menu tree
3
Tool
List
Tool
measure
Delete
tool
Extend
Edges
Find
New
tool
Tool
life
:
Work
offset
Measure
workpiece
R vari−
able
Find
Setting
data
Work area
limit.
Tim e
counter
Misc.
User
data
To o l
measure
Delete
tool
Extend
Edges
Find
New
tool
:
Fig. 3-1 Menu tree ”Parameters” operating area
Note
The softkeys marked in Fig. 3-1 with an asterisk (”:”) are missing in the 802D bl.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
3-29
Setting Up
3.1 Entering the tools and the tool offsets operating area”#
3.1 Entering the tools and the tool offsets operating area”#
Functionality
The tool offsets consist of several data describing the geometry, the wear and the tool type.
Depending on the tool type, each tool is assigned a defined number of parameters. Tools are
identified by a number (T number).
See also Section 8.6 ”Tool and tool compensation”
Operating sequences
Use this softkey to open the ”Tool offset data” window which contains a list of the tools
created. Use the cursor keys and the Page Up / Page Down keys to navigate in this list.
Tool
List
Softkeys
Tool
measure
Measure
manual
Fig. 3-2 Tool list
Enter the offsets by positioning the
S cursor bar on the input field to be changed,
S enter the value(s)
and either press Input or use a cursor key to confirm.
Extend
For special tools, the
softkey function is provided which offers a complete parameter
list which can be filled out.
Use this softkey to determine the tool compensation data.
Determining the tool offset data manually (see Section 3.1.2)
3-30
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Setting Up
3.1 Entering the tools and the tool offsets operating area”#
Delete
tool
Extend
Measure
auto
Calibrate
probe
Determining the tool offset data semi−automatically (see Section 3.1.3)
Use this softkey to calibrate the sensing probe.
Note
With the 802D bl, the Tool measur softkey opens the “Measure tool” window directly.
Use this softkey to delete the tool.
Use this function to display all parameters of a tool. For the meanings of the parameters,
please refer to the Section ”Programming”.
Activate
change
Edges
Find
D >>
<< D
New
tool edge
Reset
edge
Change
type
Fig. 3-3 Input screen for special tools
Selecting this softkey activates the compensation values of the cutting edge.
Opens a lower−level menu bar offering all functions required to create and display further
edges.
Use this softkey to select the next higher edge number.
Use this softkey to select the next lower edge number.
Use this softkey to create a new edge.
Use this softkey to reset all compensation values of the edge to zero.
This function is intended to change the tool type. select the tool type using the appropriate
softkey.
Use this function to search for a tool by its number.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
3-31
Setting Up
3.1 Entering the tools and the tool offsets operating area”#
New
tool
Use this softkey to create tool offset data for a new tool.
Max. 48 tools can be created with the 802D, and 18 tools with the 802D bl. For the 802D bl,
no milling tools are offered.
3.1.1 Use this softkey to create a new tool.
Operating sequence
New
tool
This function offers another two softkey functions to select the tool type. After selecting the
tool type, type the desired tool number (max. 3 digits) in the input field.
OK
Fig. 3-4 The ”New tool” window Input of the tool number
For milling and drilling tools, the machining directions must be selected.
Fig. 3-5 Selection of the machining direction for a milling tool
Select OK to confirm your input. A data record loaded with zero will be included in the tool
list.
3-32
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
3.1 Entering the tools and the tool offsets operating area”#
3.1.2 Determining the tool offsets (manually)
Functionality
This function can be used to determine the unknown geometry of a tool T.
Prerequisite
The relevant tool is loaded. In the JOG mode, you will approach the edge of the tool to a
machine point whose machine coordinate values are known. This can be a workpiece with
a known geometry.
Procedure
Enter the reference point in the appropriate field Ø or Z0.
Please observe: The assignment of length 1 or 2 to the axis depends on the tool type (turn-
ing tool, drill).
With a turning tool, the reference point for the X axis is a diameter dimension.
Setting Up
Using the actual position of the point F (machine coordinate) and the reference point, the
control system can calculate the offset value assigned to length 1 or length 2 for the axis.
Note: You can also use a zero already determined (e.g value of G54). In this case, use the
edge of the tool to approach the workpiece zero point. If the edge is positioned directly at
workpiece zero, the reference point is zero.
F − toolholder reference point
M − machine zero
W - workpiece zero
The offset value in the X axis is a diameter value.
X
Machine
M
Fig. 3-6 Determination of the length offsets using the example of a cutting tool
Xactual position
Workpiece
Length 1=?
W
Diameter
Length 2=?
e.g. G54
F
Zactual position
Z
Machine
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
3-33
Setting Up
3.1 Entering the tools and the tool offsets operating area”#
F − toolholder reference point
M − machine zero
W - workpiece zero
X
Machine
Workpiece
Zactual position
Fig. 3-7 Determination of the length offset using the example of a drill: Length 1 / Z axis
Note
The diagram 3-7 only applies if the variables are the machine data MD 42950
TOOL_LENGTH_TYPE and MD 42940 TOOL_LENGHT_CONST00; otherwise, length tool 2
will apply for the milling and drilling tools (see also Manufacturer Documentation ”SINUMERIK
802D Start−up”)
Operating sequence
Measure
tool
Use this softkey to open the list box for manual and semiautomatic measuring.
M
e.g. G55
W
Length 1=?
F
Z
Machine
.
3-34
Measure
manual
Fig. 3-8 Selecting manual or semiautomatic measuring
Use this softkey to open the Measure tool window.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Setting Up
3.1 Entering the tools and the tool offsets operating area”#
Fig. 3-9 The ”Measure tool” window
S Either type the workpiece diameter in the ”Ø” field or the workpiece length in the ”Z0”
field. The machine coordinates and the values from the work offsets will apply.
When using a spacer, it is also possible to enter the thickness of the spacer for taking
into account.
S After selecting the Set length 1 or Set length 2 softkey, the control system will deter-
mine the searched length 1 or length 2 of the preselected axis. The offset value determined will be stored.
Save
position
Selecting this softkey will save the X position. Thereafter, you can traverse in the X direction.
Thus, it is possible to determine, for example, the workpiece diameter. The stored value of
the axis position will then be used for calculating the length offset.
The activation of the softkey is dependent on the display machine data 373
MEAS_SAVE_POS_LENGTH2 (see also Manufacturer Documentation ”SINUMERIK 802D
Start−up”)
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
3-35
Setting Up
3.1 Entering the tools and the tool offsets operating area”#
3.1.3 Determining tool compensations using a probe
Note
This function is only offered by the 802D.
Operating sequence
Tool
Measur.
Measure
auto
Use this softkey to open the Measure tool window.
Fig. 3-10 The ”Measure tool” window
In this screenform, you can enter tool and cutting edge numbers. In addition, the tool tip
position is displayed after symbol.
After the screenform has been opened, the input fields are filled with the data of the tool currently working.
The tool can be either
S the currently active tool of the NC (loaded via a part program) or
S a tool loaded by the PLC.
If the tool was loaded by the PLC, the tool number in the input screenform can be different
than that in the T, F,S window.
If you change the tool number, no automatic tool change will be performed using this function. The entered tool, however, are assigned measurement results.
Measuring process
Approach the probe using either the traversing keys or the handwheel.
After the ”Probe triggered” has
measuring process is completed. During the automatic measurement, a dial appears
symbolizing the active measuring process.
3-36
appeared, release the traversing key and wait until the
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
3.1 Entering the tools and the tool offsets operating area”#
Note
To create the measuring program, the parameters ”Safety clearance” from the Settings screenform and the feedrate from the Probe data screenform are used (see Section 3.1.5).
If several axes are moved simultaneously, no offset data can be calculated.
3.1.4 Determining the tool offsets using optical measuring instruments
Note
This function is only offered by the 802D.
Setting Up
Fig. 3-11 Measuring using an optical measuring instrument (for the T and D input fields, please refer
Measuring process
For measuring, traverse the tool until its tip appears in the crosshair. With a milling tool, use
the highest point of the cutting edge to determine the tool length.
Subsequently, select the Set length softkeys to calculate the offset values.
to ”Measuring using a probe”)
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
3-37
Setting Up
3.1 Entering the tools and the tool offsets operating area”#
3.1.5 Probe settings
Note
This function is only offered by the 802D.
Settings
Data
probe
The screenform below is used to store the coordinates of the probe and to set the axis feedrate for the automatic measuring process.
All position values refer to the machine coordinate system.
Fig. 3-12 The ”Probe data” interactive screenform
Table 3-1
Absolute position P1 Absolute position of the probe in the Z− direction
Absolute position P2 Absolute position of the probe in the X+ direction
Absolute position P3 Absolute position of the probe in the Z+ direction
Absolute position P4 Absolute position of the probe in the X− direction
Feedrate Feedrate with which the tool approaches the probe
Calibrating the probe
Calibrate
probe
The calibration of the probe can be carried out either in the Settings menu or in the Mea-
sure tool menu.
Approach the four points of the probe.
For calibration, use a tool of the type 500 with tool tip position 3 or 4.
Parameters
Meaning
3-38
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Setting Up
3.1 Entering the tools and the tool offsets operating area”#
The offset parameters required to determine the four probe positions can be written to the
data records of two cutting edges.
Fig. 3-13 Calibrating the probe
After the screenform has appeared, an animation signaling the step to be executed is displayed next to the current positions of the probe. This point must be approached with the
appropriate axis.
After the ”Probe triggered” has
appeared, release the traversing key and wait until the
measuring process is completed. During the automatic measurement, a dial appears
symbolizing the active measuring process.
The positions delivered by the measuring program serve to calculate the real probe position.
The measuring function can be quit without approaching all positions. The points already
sensed are stored.
Note
To create the measuring program, the parameters ”Safety clearance” from the ”Settings”
screenform and feedrate from the ”Probe data” screenform are used.
If several axes are moved simultaneously, no offset data can be calculated.
Use the Next Step function to skip a point if this is not needed for measuring.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
3-39
Setting Up
3.2 Tool monitoring
3.2 Tool monitoring
Note
This function is only offered by the 802D.
Toollife
Each monitoring type is represented in 4 columns.
S Setpoint
S Prewarning limit
S Residual value
S active
Use the checkbox element of the 4th column to activate/deactivate the monitoring type.
life
Fig. 3-14 Tool monitoring
Reset
monitor
Symbols in the T column provide information on the tool status.
Prewarning limit reached
Tool disabled
Tool is monitored
Use this softkey to reset the monitoring values of the selected tool.
3-40
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Fig. 3-15
Setting Up
3.2 Tool monitoring
After
enable
Use this softkey to change the enable of the selected tool.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
3-41
Setting Up
3.3 Entering/modifying a work offset
3.3 Entering/modifying a work offset
Functionality
After the reference point approach, the actual−value memory and thus also the actual−value
display are referred to the machine zero. A machining program, however, is always referred
to the workpiece zero. This offset must be entered as the work offset.
Operating sequences
Use Offset Parameter and Work Offset to select the work offset.
An overview of all settable work offsets will appear on the screen. The screenform addition-
Work
offset
ally contains the values of the programmed work offset, of the active scaling factors, the status display and the total of all active work offsets.
Change
activated
Fig. 3-16 The ”Work offset” window
Position the cursor bar on the input field to be changed
and enter the value(s). Either move the cursor a press the Input key to accept the values
from the input fields into the work offsets.
The compensation values of the cutting edge come into effect immediately.
3-42
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
3.3.1 Determining the work offset
Prerequisite
You have select the window with the relevant work offset (e.g. G54) and the axis you want to
determine for the offset.
Setting Up
3.3 Entering/modifying a work offset
Procedure
Measure
workpiece
F − toolholder reference point
M − machine zero
W - workpiece zero
X
Machine
Workpiece
F
Zactual position
M
W
Length 2
Work offset Z=?
Z
Machine
Fig. 3-17 Determining the work offset for the Z axis
Select the ”Measure workpiece” softkey. The control system will switch to the ”Position” operating area and will open the dialog box for measuring the work offsets. The selected axis
will appear as a softkey with a black background.
Then scratch the workpiece with the tool tip. Enter the position for the workpiece in the workpiece coordinate system in the ”Set position to:” field.
Fig. 3-18 The Determine work offset in X” screenform The ”Determine work offset in Z” screenform
Set work
offset
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Selecting this softkey will calculate the offset and display the result in the ”Offset” field.
3-43
Setting Up
3.4 Programming setting data - ”Parameter” operating area
3.4 Programming setting data - ”Parameter” operating area
Functionality
The setting data are used to define the settings for the operating states. These can be
changed as necessary.
Operating sequences
Select Setting data using the Offset Parameter and Setting data keys.
Setting
data
The Setting data softkey branches to another menu level where various control options can
be set.
Fig. 3-19 The Setting datastart screen
JOG feedrate
Feedrate in the Jog mode
If the feedrate value is zero, the control system will use the value stored in the machine
data.
Spindle
Spindle speed
Minimum / maximum
A limitation of the spindle speed in the ”Max.” (G26) / ”Min.” (G25) fields can only be performed within the limit values defined in the machine data.
Programmed (limitation)
Programmable upper speed limitation (LIMS) at constant cutting rate (G96).
Dry run feed (DRY)
The feedrate which can be entered here will be used instead of the programmed feedrate
in the AUTOMATIC mode if the ”Dry run feed” function is selected.
3-44
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Softkeys
Setting Up
3.4 Programming setting data - ”Parameter” operating area
Start angle for thread cutting (SF)
For thread cutting, a start position for the spindle is displayed as the start angle. If the
thread cutting operation is repeated, a multiple thread can be cut by modifying the angle.
Position the cursor bar on the input field you want to change and enter the value(s).
Either press the Input key or move the cursor to confirm.
Work area
limit.
Time
counter
The working area limitation is active with geometry and additional axes. If you want to use a
working area limitation, its values can be entered in this dialog box. Selecting the Set Active
softkey will activate / deactivate the values for the axis highlighted by the cursor.
Fig. 3-20
Timers Counters
Fig. 3-21
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
3-45
Setting Up
3.4 Programming setting data - ”Parameter” operating area
Meaning:
S Parts total: Number of workpieces produced in total ( actual total )
S Parts required: Number of workpieces required ( require number of workpieces )
S Part count: This counter registers the number of all workpieces produced since the start-
ing time.
S Run time: Total runtime of NC programs in the AUTOMATIC mode
In the AUTOMATIC mode, the runtimes of all programs between NC START and end of
program / RESET are summed up. The timer is zeroed with each power−up of the control
system.
S Cycle time: Tool action time
The runtime between NC START and end of program / RESET is measured in the selected NC program. The timer is reset with starting a new NC program.
S Cutting time
The runtime of the path axes is measured in all NC programs between NC START and
end of program / RESET without rapid traverse active and with the tool active. The measurement is interrupted when a dwell time is active.
Misc
The timer is automatically reset to zero in the case of a ”Control power−up with default values”.
Use this function to display all setting data for the control system in the form of a list. The
data are divided into
S general
S axis−specific and
S channel setting data.
3-46
Fig. 3-22
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
3.5 R parameters − ”Offset/Parameter”operating area
3.5 R parameters − ”Offset/Parameter”operating area
Functionality
The R parameters start screen displays all R parameters existing in the control system in the form of a list (see also Section 8.9 ”R parameters”). These can be changed as necessary.
Setting Up
Fig. 3-23 The ”R parameters” window
Operating sequence
Use the Parameters and the R parameterssoftkeys
R vari−
able
Position the cursor bar on the input field to be changed
and enter the value(s).
Either press the Input key or move the cursor to confirm.
Find
Find R parameters
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
3-47
Setting Up
3.5 R parameters − ”Offset/Parameter”operating area
This sheet has been left empty for your notes
3-48
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Manually Controlled Mode
The manually controlled mode is possible in the Jog and MDA modes.
4
The softkeys marked with an asterisk (”
Set
base
x=0
z=0
Set rel
Delete
base W0
All
to zero
Back <<
Fig. 4-1 The ”Jog” menu tree
Measure
workpiece
Work
offset
X
Z
Set work
offset
Back <<
Tool
measure
Measure
manual
Measure
auto
Calibrate
probe
Back <<
:”) are not available with the 802D bl.
Settings
Data
:
probe
:
Switch
mm>inch.
:
:
Back <<
:
Set
basis
x=0
z=0
Set rel
Delete
base W0
All
to zero
Back <<
Fig. 4-2 The MDA menu tree
Face
Peripher.
surface
Abort
OK
Settings
Data
probe
Switch
mm>inch.
Back <<
:
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
4-49
Manually Controlled Mode
4.1 Mode Jog - ”Position” operating area
4.1 Mode Jog - ”Position” operating area
Operating sequences
Use the Jog key on the machine control panel to select the Jog mode.
+X
-Z
...
To traverse the axes, press the appropriate key of the X or Z axis.
The axes will traverse continuously at the velocity stored in the setting data until the key is
released. If the value of the setting data is zero, the value stored in the machine data is
used.
If necessary set the velocity using the override switch.
%
If you press additionally the Rapid traverse override key, the selected axis will be traversed
at rapid traverse speed until both keys are released.
In the Jog mode, you can traverse the axes by adjustable increments using the same operating sequence. The set number of increments is displayed in the Status area. To deselect
the Jog mode, press Jog once more.
The Jog start screen displays the position, feedrate and spindle values, as well as the current tool.
4-50
Fig. 4-3 The ”Jog” start screen
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Parameters
Manually Controlled Mode
4.1 Mode Jog - ”Position” operating area
Table 4-1 Description of the parameters in the JOG start screen
Parameter
MCS
X
Z
+X
-Z
Position
mm
REPOS offset If the axes are traversed in the ”Program interrupted” condition in the Jog mode, the distance tra-
G function Displays important G functions
Spindle S
r.p.m.
Feed F
mm/min
Tool Displays the currently active tool with the current edge number
Displays the axes existing in the machine coordinate system (MCS) or in the workpiece coordinate
system (WCS)
If you traverse an axis in the positive (+) or negative (-) direction, a plus or minus sign will appear in
the relevant field.
If the axis is already in the required position, no sign is displayed.
These fields display the current position of the axes in the MCS or WCS.
versed by each axis is displayed referred to the interruption point.
Displays the actual value and the setpoint of the spindle speed
Displays the path feedrate actual value and setpoint
Explanation
Note
If a second spindle is integrated into the system, the workspindle will be displayed using a smaller font.
The window will always display the data of only one spindle.
Softkeys
Set
base
The control system displays the spindle data according to the following aspects
:
The master spindle (large display) is displayed:
− in the idle condition;
− when starting the spindle;
− if both spindles are active.
The workspindle (small display) is displayed:
− when starting the workspindle.
The power bar applies to the spindle currently active.
This softkey is used to set the base work offset or a temporary reference point in the relative
coordinate system. After opening, this function can be used to set the base work offset.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
4-51
Manually Controlled Mode
4.1 Mode Jog - ”Position” operating area
The following subfunctions are provided:
S Direct input of the desired axis position
In the input window, position the input cursor on the desired axis; thereafter, enter the
new position. Then, press Input or move the cursor to confirm your input.
S Setting of all axes to zero
The softkey function All to zero overwrites the current position of the appropriate axis
with zero.
S Setting Setting of individual axes to zero
Use the X=0 or Z=0 softkey to overwrite the current position with zero.
Use the Set rel softkey to switch the display to the relative coordinate system. Any subsequent inputs will change the reference point in this coordinate system.
Note
A changed base work offset acts independently of any other work offsets.
Measure
workpiece
Tool
measure
Settings
Use this softkey to determine the work offset (cf. Chapter 3)
Use this softkey to measure the tool offsets (cf. Chapter 3)
The interactive screenform shown below is intended to set the retraction plane, the safety
clearance and the direction of rotation of the spindle for automatically generated part programs in the MDA mode. Furthermore, the values for the JOG feedrate and the variable size
of increments can be set.
4-52
Fig. 4-4
Retract plane: The Face function retracts the tool to the specified position (Z position) after
the function has been executed.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Manually Controlled Mode
4.1 Mode Jog - ”Position” operating area
Safety distance: Safety clearance to the workpiece surface
This value defines the minimum distance between the workpiece surface and the workpiece.
It is used by the functions ”Face” and ”Automatic tool gauging”.
JOG feedrate: Feedrate value in the JOG mode
Dir. of rot.: Direction of rotation of the spindle for automatically generated programs in the
JOG and MDA modes.
Data
probe
Switch to
mm > inch
The screenform below is used to store the coordinates of the probe and to set the axis feedrate for the automatic measuring process (see Section 3.1.5).This only applies to the 802D.
Use this softkey to switch between the metric and the inch system.
4.1.1 Assigning handwheels
Operating sequence
Hand
wheel
Use this softkey to display the handwheel window in the Jog mode.
After the window has been opened, all axis identifiers are displayed in the ”Axis” column,
which simultaneously appear in the softkey bar.
Select the desired handwheel using the cursor. Thereafter, select the relevant axis softkey
for the required axis for assignment or deselection.
The
symbol is display in the window.
Measure
Measure
workpiece
tool
Fig. 4-5 The Handwheel menu screen
MCS
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Use the MCS softkey to select the axes from the machine or workpiece coordinate system
for handwheel assignment. The current setting is displayed in the window.
4-53
Manually Controlled Mode
4.2 MDA mode (Manual input) - ”Machine” operating area
4.2 MDA mode (Manual input) - ”Machine” operating area
Functionality
In the MDA mode, you can create or execute a part program.
Caution
!
Operating sequences
The Manual mode is subject to the same safety interlocks as the fully automatic mode.
Furthermore, the same prerequisites are required as in the fully automatic mode.
Use the MDA key on the machine control panel to select the MDA mode.
Fig. 4-6 The ”MDA” start screen
Enter one or several blocks using the keyboard.
Press NC START to start machining. During machining, editing of the blocks is no longer
possible.
After machining, the contents is preserved so that the machining can be repeated by pressing NC START once more.
4-54
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Parameters
Manually Controlled Mode
4.2 MDA mode (Manual input) - ”Machine” operating area
Table 4-2 Description of the parameters in the MDAworking window
Parameter
MCS
X
Z
+X
−Z
Position
mm
Distance togoThis field displays the distance to go of the axes in the MCS or WCS.
G function Displays important G functions
Spindle S
r.p.m.
Feed F Displays the path feedrate actual value and setpoint in mm/min or mm/rev.
Tool Displays the currently active tool with the current edge number (T..., D...).
Editing win-
dow
Displays the existing axes in the MCS or WCS
If you traverse an axis in the positive (+) or negative (-) direction, a plus or minus sign will appear in
the relevant field.
If the axis is already in the required position, no sign is displayed.
These fields display the current position of the axes in the MCS or WCS.
Displays the actual value and the setpoint of the spindle speed
In the ”Stop” or ”Reset” program state, an editing window serves to input a part program block.
Explanation
Note
If a second spindle is integrated into the system, the workspindle will be displayed using a smaller font.
The window will always display the data of only one spindle.
The control system displays the spindle data according to the following aspects
The master spindle is displayed:
− in the idle condition;
− when starting the spindle;
− if both spindles are active.
The workspindle is displayed:
− when starting the workspindle.
The power bar applies to the spindle currently active.
:
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
4-55
Manually Controlled Mode
4.2 MDA mode (Manual input) - ”Machine” operating area
Softkeys
Set
base
Face
Settings
G
function
Auxiliary
function
Axis
feedrate
Delete
MDI prog.
Save
MDI prog.
Use this softkey to set the base work offset (see Section 4.1).
Face milling (see also Section 4.2.1)
see Section 4.1
The G function window displays G functions whereby each G function is assigned to a group
and has a fixed position in the window.
Use the PageDown and PageUp keys to display further G functions. Selecting the softkey
repeatedly will close the window.
This window displays the auxiliary and M functions currently active. Selecting the softkey
repeatedly will close the window.
Use this softkey to display the Axis feedrate window.
Selecting the softkey repeatedly will close the window.
Use this function to delete blocks from the program window.
Enter a name in the input field with which you wish the MDA program to be saved in the program directory. Alternatively, you can select an existing program from the list.
To switch between the input field and the program list, use the TAB key.
MCS/WCS
REL
4-56
Fig. 4-7
The actual values for the MDA mode are displayed depending on the selected coordinate
system. Use this softkey to switch between the two coordinate systems.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
4.2.1 Face turning
Functionality
Use this function to prepare a blank for the subsequent machining without creating a special
part program.
Operating sequence
Face
In the MDA mode, select the Face softkey to open the interactive screenform.
S Position the axes on the start point.
S Enter the values in the screenform.
After you have filled out the screenform completely, the function will create a part program
which can be started with NC START. The interactive screenform will be closed, and ”Ma-
chine” start screen will appear. Here you can observe the program progress.
Manually Controlled Mode
4.2 MDA mode (Manual input) - ”Machine” operating area
Important
The retraction plane and the safety clearance must be defined beforehand in the ”Settings”
menu.
Fig. 4-8 Accepting the current tool tip position
Table 4-3 Description of the parameters in the Face turning working window
Parameter
Tool Input of the tool to be used
The tool is loaded prior to machining. To this end, the function calls a working cycle performing
all steps required. This cycle is provided by the machine manufacturer.
Feed F Input of the path feedrate, in mm/min or mm/rev.
Explanation
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
4-57
Manually Controlled Mode
4.2 MDA mode (Manual input) - ”Machine” operating area
Table 4-3 Description of the parameters in the Face turning working window, cont’d
Parameter Explanation
Spindle S
r.p.m.
Machining Definition of the surface quality
Diameter Input of the blank diameter of the part
Z0
Blank dimension
Z1
Cutting dimension
DZ
Cutting dimension
UZ
Max. infeed
UX
Max. infeed
Input of the spindle speed
You can select between roughing and finishing.
Input of the Z position
Cutting dimension, incremental
Input of the cutting length in the Z direction
This dimensions is always specified in increments and is referred to the workpiece edge.
Stock allowance in the Z direction
Stock allowance in the X direction
Peripher.
surface
Longitudinal turning
Fig. 4-9 Longitudinal turning
Table 4-4 Description of the parameters in the Longitudinal turning working window
Parameter
Tool Input of the tool to be used
The tool is loaded prior to machining. To this end, the function calls a working cycle performing
all steps required. This cycle is provided by the machine manufacturer.
Feed F Input of the path feedrate, in mm/min or mm/rev.
Spindle S
r.p.m.
Mach. Definition of the surface quality
Input of the spindle speed
You can select between roughing and finishing.
Explanation
4-58
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Manually Controlled Mode
4.2 MDA mode (Manual input) - ”Machine” operating area
Table 4-4 Description of the parameters in the Longitudinal turning working window, cont’d
Parameter Explanation
X0
Blank diameter
X1
Cutting length
Z0
Position
Z1
Cutting length
DZ
Max. infeed
UZ Input field for the stock allowance when roughing
UX Stock allowance
Input of the blank diameter
Cutting length, incremental, in the X direction
Input of the position of the workpiece edge in the Z direction
Cutting length, incremental, in the Z direction
Input of the infeed dimension in the X direction
Get curr.
position
Use this softkey to accept the current tool tip position into the Z0 or X0 input field.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
4-59
Manually Controlled Mode
4.2 MDA mode (Manual input) - ”Machine” operating area
This sheet has been left empty for your notes
4-60
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Automatic Mode
Prerequisites
The machine is set up for the AUTOMATIC mode according to the specifications of the
machine manufacturer.
Operating sequence
Select the AUTOMATIC mode using the AUTOMATIC key on the machine control panel.
The AUTOMATIC start screen appears, displaying the position, feedrate, spindle, and tool
values, as well as the block currently active.
5
Fig. 5-1 The AUTOMATICstart screen
Note
The Real−time simulat. softkey is only offered by the 802D bl with color display option.
Spindle power and load displays are missing with the 802D bl.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
5-61
Automatic Mode
Parameters
Program
control
Program
test
Dry run
feedrate
Condit.
stop
Skip
SiBL fine
ROV active
Back <<
Fig. 5-2 Menu tree of the AUTOMATIC mode
Block
search
To
contour
To
endpoint
Without
calculate
Interr.
point
Find
Back <<
Real−time
simulat.
Zoom
Auto
To
origin
Display
All
Zoom +
Zoom −
Delete
window
Cursor
crs. / fine
Back <<
Correct
progr.
Back <<
Table 5-1 Description of the parameters in the working window
Parameter
MCS
X
Z
+ X
- Z
PositionmmThese fields display the current position of the axes in the MCS or WCS.
Distance togoThese fields display the current position of the axes in the MCS or WCS.
G function Displays important G functions
Spindle S
r.p.m.
Feed F
mm/min or
mm/rev.
Tool Displays the currently active tool with the current edge number (T..., D...).
Current block The block display displays seven subsequent blocks of the currently active part program. The dis-
Displays the existing axes in the MCS or WCS
If you traverse an axis in the positive (+) or negative (-) direction, a plus or minus sign will appear in
the relevant field.
If the axis is already in the required position, no sign is displayed.
Displays the actual value and the setpoint of the spindle speed
Displays the path feedrate actual value and setpoint
play of one block is limited to the width of the window. If several blocks are executed quickly one
after the other, it is recommended to switch to the ”Program progress” window. To switch back to the
seven−block display, use the ”Program sequence” softkey.
Explanation
5-62
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Automatic Mode
Note
If a second spindle is integrated into the system, the workspindle will be displayed using a smaller font.
The window will always display the data of only one spindle.
Softkeys
Progr.
control
Program
test
Dry run
feedrate
The control system displays the spindle data according to the following aspects
:
The master spindle is displayed:
− in the idle condition;
− when starting the spindle;
− if both spindles are active.
The workspindle is displayed:
− when starting the workspindle.
The power bar applies to the spindle currently active.
The program control softkeys are displayed (e.g. ”Skip block”, ”Program test”).
If ”Program test” is selected, the output of setpoints to axes and spindles is disabled. The
setpoint display will ”simulate” the traversing motion.
If you select this softkey, all traversing motions will be performed with the feedrate setpoint
specified via the ”Dry run feed” setting data. In other words: Instead of the programmed motion commands, the dry run feedrate will act.
Condit.
stop
Skip
SBL fine
ROV active
Back <<
Block
Search
To
contour
If this function is active, the program execution is stopped at the blocks in which the miscellaneous function M01 is programmed.
Program blocks marked with a slash in front of the block number are skipped during the program execution (e.g. ”/N100”).
If this function is enabled, the part program blocks are executed separately as follows: Each
block is decoded separately, and a stop is performed at each block; an exception are only
the thread blocks without dry run feedrate. In such blocks, a stop is only performed at the
end of the current thread block. ”Single Block fine” can only be selected in the RESET status.
The feedrate override switch will also act on the rapid traverse override.
Use this softkey to quit the screenform.
Use the block search function to go to the desired place in the program.
Forward block search with calculation
During the block search, the same calculations are carried out as during normal program
operation, but the axes do not move.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
5-63
Automatic Mode
To
end point
Without
calculate
Interr.
point
Find
Real−time
simulat.
Correct
progr.
G
funct
Forward block search with calculation to the block end point
During the block search, the same calculations are carried out as during normal program
operation, but the axes do not move.
Block search without calculation
During the block search, no calculation is carried out.
The cursor is positioned on the main program block of the interruption point. The search target is set in the subroutine levels automatically.
The ”Find” softkey provides the functions ”Find line”, ”Find text” etc.
Using broken−line graphics, the programmed tool path can be traced.
(see also Section 6.4)
Use this softkey to correct a fault program passage. Any changes will be stored immediately.
Opens the G functions window to display all G functions currently active.
The G functions window displays all G functions currently active whereby each G function is
assigned to a group and has a fixed position in the window.
Use the PageDown and PageUp keys to display further G functions.
Auxiliary
function
Axis
feedrate
Program
sequence
5-64
Fig. 5-3 The Active G functionswindow
This window displays the auxiliary and M functions currently active.
Selecting the softkey repeatedly will close the window.
Use this softkey to display the Axis feedrate window.
Selecting the softkey repeatedly will close the window.
Use this softkey to switch from the seven−block to the three−block display.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Automatic Mode
MCS/WCS
REL
External
programs
Switches the axis value display between the machine, workpiece and relative coordinate
systems.
Use this softkey to transmit an external program to the control system via the RS232 interface; to execute this program, press NC START.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
5-65
Automatic Mode
5.1 Selecting / starting a part program - ”Machine” operating area
5.1 Selecting / starting a part program - ”Machine” operating area
Functionality
Before starting the program, make sure that both the control system and the machine are
set up. Observe the relevant safety notes of the machine manufacturer.
Operating sequence
Select the AUTOMATIC mode using the AUTOMATIC key on the machine control panel.
An overview of all programs stored in the control system is displayed.
Position the cursor bar on the desired program.
Execute
Progr.
control
To select the program for execution, use the Execute softkey. The name of the selected program will appear in the ”Program name” screen line.
Use this softkey to specify settings for program execution (as necessary).
Fig. 5-4 Program control
Press NC START to start the part program execution.
5-66
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
5.2 Block search - ”Machine” operating area
5.2 Block search - ”Machine” operating area
Operating sequence
Prerequisite: The required program has already been selected (cf. Section 5.1) and the control system is in the RESET condition.
Automatic Mode
Block
Search
To
contour
To
end point
The block search function provides advance of the program to the required block in the part
program. The search target is set by positioning the cursor bar directly on the required block
in the part program.
Fig. 5-5 Block search
Block search to the block start
Block search to the end of the block
Without
calculate
Interr.
point
Find
Block search without calculation
The interruption point is loaded.
Use this softkey to perform the block search by entering a term you are looking for.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
5-67
Automatic Mode
5.3 Stopping / canceling a part program
Fig. 5-6 Entering the searched term
Search result
The required block is displayed in the Current blockwindow.
5.3 Stopping / canceling a part program
Operating sequence
Press NC STOP to cancel a part program.
Press NC START to continue the program execution.
Use RESET to interrupt the program currently running.
Pressing NC START again will restart the program you have interrupted and execute the
program from the beginning.
5-68
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
5.4 Reapproach after cancellation
After a program cancellation (NC STOP), you can retract the tool from the contour in the
Manual mode (Jog).
Operating sequence
Select the AUTOMATIC mode.
Automatic Mode
5.4 Reapproach after cancellation
BlockSearc
h
Interr.
Point
To
contour
Use this softkey to open the Block search window for loading the interruption point.
The interruption point is loaded.
Selecting this softkey will start the block search to the interruption point. An adjustment to
the start position of the interrupted block will be carried out.
Press NC START to continue the program execution.
5.5 Repositioning after interruption
After a program interruption (NC STOP), you can retract the tool from the contour in the
Manual mode (Jog); the coordinates of the interruption point are stored by the control system. The path differences traversed by the axes are displayed.
Operating sequence
Select the AUTOMATIC mode.
Press NC START to continue the program execution.
Caution
When reapproaching the interruption point, all axes will traverse at the same time. Make
sure that the traversing area is not obstructed.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
5-69
Automatic Mode
5.6 Program execution from external source (RS232 interface)
5.6 Program execution from external source (RS232 interface)
Functionality
Use this softkey to transmit an external program to the control system via the RS232 interface; to execute this program, press NC START. While the contents of the buffer memory
are being processed, the blocks are reloaded automatically.
For example, a PC with the PCIN tool installed for data transfer can be used as the external
device.
Important
Before connecting / removing the cable between the external device and the control system,
always first make sure that the device is disconnected from the mains.
Operating sequence
External
progr.
Prerequisite: The control system is in the RESET condition.
The RS232 interface is parameterized correctly (for the relevant text format, see also Chapter 7) and not occupied by any other application (DataIn, DataOut, STEP7).
Select the softkey.
On the external device (PC), activate the relevant program for data output via the PCIN tool.
The program is transmitted into the buffer memory and selected and displayed in the Program Selection automatically.
Before starting program execution by pressing NC START, first make sure that the buffer is
filled completely.
The program execution starts with NC-START ; subsequently, the program is reloaded successively.
At the end of the program or in case of RESET, the program is removed from the control
system automatically.
Note
Any transmission errors are displayed in the System / Data I/O area if you select the Error
log softkey.
Block search is not possible for programs read in from an external source.
5-70
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Part Programming
Operating sequence
Press the Program Manager key to open the program directory.
Fig. 6-1 The ”Program Manager” start screen
6
Use the cursor keys to navigate in the program directory. To find program names quickly,
simply type the initial letters of the program name. The control system will automatically
position the cursor on a program with matching characters.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
6-71
Part Programming
Softkeys
Programs
Execute
New
Copy
Open
Delete
Rename
Use this softkey to display all files contained in the part program directory.
Use this softkey to select the program on which the cursor is positioned for execution. The
control system will switch to the position display. With the next NC START, the program is
started.
Use the New softkey to create a new program.
Use the Copy softkey to copy the selected program into another program with a new name.
Use the ”Open” softkey to open the file highlighted by the cursor for processing.
Use this softkey to delete either only the program highlighted by the cursor or all part programs; first, however, a warning confirmation is displayed.
Use the OK softkey to execute the deletion order and Abort to discard.
Selecting the Rename softkey opens a window where you can rename the program you
have selected beforehand using the cursor.
Read out
Read in
Cycles
Delete
User
cycles
After you have entered the new name, either press OK to confirm or Abort to cancel.
Use this softkey to saved files via the RS232 interface.
Use this softkey to load part programs files via the RS232 interface.
For the settings of the interface, please refer to the System operating area (Chapter 7). The
part programs must be transmitted using the text format.
Use the User cycles softkey to display the ”Standard cycles” directory. This softkey will only
appear unhidden if you have the relevant access right.
Use this softkey to delete the cycle highlighted by the cursor; first, a confirmation warning
will appear.
Use the User cycles softkey to display the ”User cycles” directory.
With the appropriate access right, the softkeys New, Copy, Open, Delete, Rename, Read
out and Read in are displayed.
6-72
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Fig. 6-2
Part Programming
Save
data
Save data
This function is used to save the contents of the volatile memory into a non−volatile memory
area.
Prerequisite: There is no program currently executed.
Do not carry out any operator actions while the data backup is running!
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
6-73
Part Programming
6.1 Entering a new program - ”Program” operating area
6.1 Entering a new program - ”Program” operating area
Operating sequences
New
Programs
Select the Program operating area displaying an overview of the programs already created
in the NC.
Select the New softkey; a dialog box will appear where you can enter the name of the new
main program or subroutine. The extension for main programs ”.MPF” is entered automatically; the extension for subroutines ”.SPF” must be entered together with the program name.
The files in the ”User cycles” directory is also assigned the extension ”.SPF”.
Fig. 6-3 The New program interactive screenform
Enter the name for the new program.
Use the OK softkey to confirm your input. The new part program file will be created, and the
editor window is opened automatically.
Use Abort to cancel the creation of the program; the window will be closed.
6-74
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
6.2 Editing part programs - ”Program” operating area
6.2 Editing part programs - ”Program” operating area
Functionality
A part program can only be edited if it is currently not being executed.
Any modifications to the part program are stored immediately.
Find
Part Programming
Menu tree
Fig. 6-4 The ”Program editor” start screen
Edit Turning
Execute
Mark
block
Copy
block
Insert
block
Delete
block
Find
Renumber
Contour
Drilling
Milling
Simulation Recompile
Zoom
Auto
To
origin
Show
...
Zoom +
Zoom −
Delete
window
Cursor co
arse/fine
:
:
:
:
:
:
:
:
Fig. 6-5 The ”Program” menu tree (default assignment)
The softkeys marked with an asterisk (”:”) are only offered by the 802D bl with the color
display option.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
6-75
Part Programming
6.2 Editing part programs - ”Program” operating area
Operating sequence
Use the ”Program manager” to select the program you want to edit and select Open to open
the program.
Softkeys
Edit
Execute
Mark
block
Copy
block
Insert
block
Delete
block
Find
Use this softkey to edit a file.
Use this softkey to execute the selected file.
Use this softkey to select a text segment up to the current cursor position (alternatively:
<ctrl>B).
Use this softkey to copy a selected block to the clipboard (alternatively: <ctrl>C).
Use this softkey to paste a text from the clipboard at the current cursor position
(alternatively: <ctrl>V).
Use this softkey to delete a selected text (alternatively: <ctrl>X).
Use the Find and the Find Next softkeys to search for a string in the program file displayed.
Type the term you are looking for in the input line and use the OK softkey to start the
search.
If the string you are searching for is not found in the program file, an error message is issued.
Use Back to quit the dialog box without starting the search process.
Renumber
Contour
Drill
Milling
Turning
Recompile
Simulation
Use this softkey to replace the block numbers from the current cursor position up to the program end.
For programming the contour (”blueprint programming”), see Section 6.3
see Manual ”Cycles”
see Manual ”Cycles” (with the options ”Transmit” and ”Tracyl”)
see Manual ”Cycles”
For recompilation, position the cursor on the cycle calling line in the program. This function
decodes the cycle name and prepares the screenform with the relevant parameters. If there
are any parameters beyond the range of validity, the function will automatically use the default values. After closing the screenform, the original parameter block is replaced by the
corrected block.
Note: Only automatically generated blocks can be recompiled.
The simulation is described in Section 6.4.
6-76
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
6.3 Blueprint programming
Functionality
The control system offers various contour screenforms for the fast and reliable creation of
part programs. Use these screenforms to enter the required parameters.
The following contour elements or contour sections can be programmed using the contour
screenforms:
S Straight line section with specification of end point or angle
S Circle sector with specification of center point / end point / radius
S Contour section straight line − straight line with specification of angle and end point
S Contour section straight line − circle with tangential transition; calculated on the basis of
angle, radius and end point
S Contour section straight line − circle with any transition; calculated on the basis of angle,
center point and end point
S Contour section circle − straight line with tangential transition; calculated on the basis of
angle, radius and end point
Part Programming
6.3 Blueprint programming
S Contour section circle − straight line circle with any transition; calculated on the basis of
angle, center point and end point
S Contour section circle − circle with tangential transition; calculated on the basis of center
point, radius and end point
S Contour section circle − circle with any transition; calculated on the basis of center point
and end point
S Contour section circle − straight line − circle with tangential transitions
S Contour section circle − circle − circle with tangential transitions
S Contour section straight line − circle − straight line − circle with tangential transitions
Fig. 6-6 Softkey functions
The coordinates can be input either as an absolute, incremental or polar value. Input is
switched using the Toggle key.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
6-77
Part Programming
6.3 Blueprint programming
Softkeys
Use these softkey functions to branch into the individual contour elements.
If a contour screenform is opened for the first time, the starting point of the contour section
must be reported to the control system. All subsequent motions will refer to this point. If you
move the input bar with the cursor, all values must be reentered.
Fig. 6-7 Setting the starting point
Use this interactive screenform to define whether the following contour sections are to be
programmed using radius or diameter programming or whether the transformation axes are
to be used for TRANSMIT orTRACYL.
Note
The TRANSMIT and TRACYL softkeys are not offered by the 802D bl. The interactive
screenform should therefore only be used to define whether the following contour sections
are to be programmed using radius or diameter programming.
The Approach start point softkey function will generate an NC block approaching the entered coordinates.
6-78
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Part Programming
6.3 Blueprint programming
Programming aid for the programming of straight line sections
Fig. 6-8
Enter the end point of the straight line in absolute dimensions, in incremental dimensions
(with reference to the starting point) or in polar coordinates. The current settings are displayed in the interactive screenform.
Set
Pole
The end point can also be defined by a coordinate and the angle between an axis and the
straight line.
If the end point is determined via polar coordinates, you will need the length of the vector between the
pole and the end point, as well as the angle of the vector referred to the pole.
The prerequisite is that a pole was set beforehand. This pole will be applicable until a new pole is set.
A dialog box will appear where the coordinates of the pole point must be entered. The pole
point will refer to the selected plane.
Fig. 6-9
G0/G1
Addition.functions
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
If this function is selected, the selected block is traversed at rapid traverse or with the
programmed path feedrate.
If necessary you can enter additional functions in the fields. The commands can be separated from each other by spaces, commas or semicolons.
6-79
Part Programming
6.3 Blueprint programming
Fig. 6-10
This interactive screenform is provided for all contour elements.
OK
Pressing the OK softkey will accept all commands into the part program.
Select Abort to quit the interactive screenform without saving the values.
This function is intended to calculate the point of intersection between two straight lines.
Specify the coordinates of the end point of the second straight line and the angles of the
straight lines.
Fig. 6-11 Calculating the point of intersection between two straight lines
6-80
Table 6-1 Input in the interactive screenform
End point of straight
line 2
Angle of straight line 1 A1 The angle is specified in the counterclockwise direction from 0 to 360
Angle of straight line 2 A2 The angle is specified in the counterclockwise direction from 0 to 360
Feedrate F Feedrate
E Enter the end point of the straight line.
degrees.
degrees.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Part Programming
6.3 Blueprint programming
Use this interactive screenform to create a circular block using the coordinates end point and
center point.
Fig. 6-12
Enter the end point and center point coordinates in the input fields. Input fields no longer
needed are hidden.
G2/G3
OK
Use this softkey to switch the direction of rotation from G2 to G3. G3 will appear on the display.
Pressing this softkey again will switch back the display to G2.
Pressing the OK softkey will accept the block into the part program.
This function will calculate the tangential transition between a contour and a circle sector.
The straight line must be described by the starting point and the angle. The circle must be
described by the radius and the end point.
For calculating the points of intersection with any transition angles, the POI softkey function
will display the center point coordinates.
Fig. 6-13 Straight line − circle with tangential transition
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
6-81
Part Programming
6.3 Blueprint programming
Table 6-2 Input in the interactive screenform
G2/G3
POI
End point of the circle
Angle of straight line A The angle is specified in the counterclockwise direction from 0 to 360
Radius of the circle R Input field for the circle radius
Feedrate F Input field for the interpolation feedrate
Center point of the
circle
E Enter the end point of the circle.
degrees.
M If there is no tangential transition between the straight line and the
circle, the circle center point must be known. The specification is performed depending on the type of calculation (absolute, incremental or
polar coordinates) selected in the previous block.
Use this softkey to switch the direction of rotation from G2 to G3. G3 will appear on the display. Pressing this softkey again will switch back the display to G2. The display changes to
G2.
You can choose between tangential or any transition.
The screenform generates a straight line and a circle block from the data you have entered.
If several points of intersection exist, the desired point of intersection must be selected from
a dialog box.
If one coordinate was not entered, the program tries to calculate it from the existing specifi-
cations. If there are several possibilities, a dialog box is provided to choose from.
This function will calculate the tangential transition between a contour and a circle sector.
The circle sector must be described by the parameters starting point and radius, and the
straight line must be described by the parameters end point and angle.
Fig. 6-14 Tangential transition
6-82
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Table 6-3 Input in the interactive screenform
Part Programming
6.3 Blueprint programming
G2/G3
POI
End point of straight
line
Center point M Enter the center point of the circle in absolute, incremental or polar
Radius of the circle R Input field for the circle radius
Angle of straight line 1 A The angle is specified in the counterclockwise direction from 0 to 360
Feedrate F Input field for the interpolation feedrate
E Enter the end point of the straight line in absolute, incremental or po-
lar coordinates.
coordinates.
degrees and with reference to the point of intersection.
Use this softkey to switch the direction of rotation from G2 to G3. G3 will appear on the display. Pressing this softkey again will switch back the display to G2. The display changes to
G2.
You can choose between tangential or any transition.
The screenform generates a straight line and a circle block from the data you have entered.
If several points of intersection exist, the desired point of intersection must be selected from
a dialog box.
This function will insert a straight line tangentially between two circle sectors. The sectors
are determined by their center points and their radii. Depending on the direction of rotation
selected, different tangential points of intersection result.
Use the displayed screenform to enter the parameters center point and radius for the sector
1 and the parameters end point, center point and radius for the sector 2. Furthermore, the
direction of rotation of the circles must be selected. A help screen is provided to display the
current settings.
Pressing OK calculates three blocks from the entered values and inserts them into the part
program.
Fig. 6-15
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
6-83
Part Programming
6.3 Blueprint programming
Table 6-4 Input in the interactive screenform
G2/G3
End point
Center point of the circle 1 M1 1st and 2nd geometry axes of the plane(absolute coordi-
Radius of circle 1 R1 Input field for radius 1
Center point of circle 2 M2 1st and 2nd geometry axes of the plane(absolute coordi-
Radius of circle 1 R2 Input field for radius 2
Feedrate F Input field for the interpolation feedrate
E 1. and 2nd geometry axes of the plane
If no coordinates are entered, this function provides the
point of intersection between the circle sector you have
inserted and sector 2.
nates)
nates)
The screenform generates one straight line and two circle blocks from the data you have
entered.
Use this softkey to define the direction of rotation of the two circle sectors. You can choose
between
sector 1 sector 2
G2 G3,
G3 G2,
G2 G2
G3 G3
The end point and the center point coordinates can be entered either in absolute dimensions, incremental dimensions or polar coordinates. The current settings are displayed in the interactive screenform.
Example DIAMON
Fig. 6-16
6-84
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Part Programming
6.3 Blueprint programming
Given: R1 50 mm
R2 100 mm
R3 40mm
M1 Z −159 X 138
M2 Z −316 X84
M3 Z −413 X 292
Starting point: The point X = 138 and Z = −109 mm (−159 − R50) is supposed as the starting
point.
Fig. 6-17 Setting the starting point
After you have confirmed the starting point, use the screenform to calculate the con-
tour section − − .
Use the G2/G3 softkey to set the direction of rotation for the two circle sectors (G2|G3) and
to fill out the parameter list.
The center point coordinates must be entered as absolute coordinates, i.e. the X coordinate
with reference to zero.
The end point remains open.
Fig. 6-18
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
6-85
Part Programming
6.3 Blueprint programming
After you have filled out the interactive screenform, click on OK to quit the screenform. The
points of intersection are calculated and the two blocks are generated.
Fig. 6-19 Result of step 1
Since the end point has been left open, the point of intersection of the straight line
with the circle sector will be used as the starting point for the next contour definition.
Now, call the interactive screenform for calculating the contour section
end point of the contour section are the coordinates Z= −413.0 and X=212.
Fig. 6-20 Calling the screenform
− again. The
6-86
Fig. 6-21 Result of step 2
The function calculates the tangential transition between two circle sectors. Circle sector 1
must be described by the parameters starting point, center point and radius, and the circle
sector 2 be described by the parameters end point and radius.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Fig. 6-22 Tangential transition
Table 6-5 Input in the interactive screenform
Part Programming
6.3 Blueprint programming
G2/G3
POI
End point of circle 2
Center point of the
circle 1
Radius of circle 1 R1 Input field for the radius
Center point of circle 2 M2 1st and 2nd geometry axes of the plane
Radius of circle 1 R2 Input field for the radius
Feedrate F Input field for the interpolation feedrate
E 1st and 2nd geometry axes of the plane
M1 1st and 2nd geometry axes of the plane
The specification of the points is performed depending on the type of calculation (absolute,
incremental or polar coordinates) selected beforehand. Input fields no longer needed are
hidden. If only one center point coordinate is entered, the radius must be entered.
Use this softkey to switch the direction of rotation from G2 to G3. G3 will appear on the display. Pressing this softkey again will switch back the display to G2. The display changes to
G2.
You can choose between tangential or any transition.
The screenform generates two circle blocks from the data you have entered.
Selecting the point of intersection
If several points of intersection exist, the desired point of intersection must be selected from
a dialog box.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
6-87
Part Programming
6.3 Blueprint programming
Fig. 6-23 Selecting the point of intersection
POI 1
POI 2
The contour will be drawn using the point of intersection 1.
Fig. 6-24
The contour will be drawn using the point of intersection 2.
6-88
Fig. 6-25
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Part Programming
6.3 Blueprint programming
OK
Pressing OK accepts the point of intersection of the displayed contour into the part program.
This function will insert a circle sector between two adjacent circle sectors. The circle sectors are described by their center points and circle radii, and the inserted sector is described
only be its radius.
The operator is offered a screenform where he will enter the parameters center point, radius
for circle sector 1 and the parameters end point, center point and radius for the circle sector
2. Furthermore, the radius for the inserted circle sector 3 must be entered and the direction
of rotation be defined.
A help screen is provided to display the selected settings.
Pressing OK calculates three blocks from the entered values and inserts them into the part
program.
G2/G3
Fig. 6-26 Screenform for calculating the contour section circle−circle−circle
Table 6-6 Input in the interactive screenform
End point
Center point of the circle 1 M1 1st and 2nd geometry axes of the plane
Radius of circle 1 R1 Input field for radius 1
Center point of circle 2 M2 1st and 2nd geometry axes of the plane
Radius of circle 1 R2 Input field for radius 2
Radius of circle 3 R3 Input field for radius 3
Feedrate F Input field for the interpolation feedrate
E 1. and 2nd geometry axes of the plane
If no coordinates are entered, this function provides the
point of intersection between the circle sector you have
inserted and sector 2.
If it is not possible to determine the starting point from the previous blocks, use the ”Starting
point” screenform to enter the appropriate coordinates.
Use this softkey to define the direction of rotation of the two circles. You can choose between
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
6-89
Part Programming
6.3 Blueprint programming
sector 1 inserted sector sector 2
G2 G 3, G2,
G2 G2 G2,
G2 G2 G3,
G2 G3 G3,
G3 G2 G2,
G3 G3 G2,
G3 G2 G3,
G3 G3 G3
Center and end points can be acquired either in absolute dimensions, incremental dimensions or using
polar coordinates. The current settings are displayed in the interactive screenform.
Example DIAMON − G23
6-90
Fig. 6-27
Given: (C1) R1 39 mm
(C2) R2 69 mm
(C3) R3 39 mm
(C4) R4 49 mm
(C5) R5 39 mm
M1 Z −111 X 196
M2 Z −233 X 260
M3 Z −390 X 162
The coordinates Z −72, X 196 will be selected as the starting point.
After you have confirmed the starting point, use the screenform to calculate
tour section
− . The end point is left open, since the coordinates are not known.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
the con-
Part Programming
6.3 Blueprint programming
Use softkey 1 to set the direction of rotation of the two circles (G2 − G2 − G3) and to fill out
the parameter list.
Fig. 6-28 Setting the starting point
Fig. 6-29 Input of step 1
Fig. 6-30 Result of step 1
The function provides the point of intersection between circle sector 2 and circle sector 3 as
the end point.
In the second step, use the screenform to calculate the contour section
− . For calculation, select the direction of rotation G2 − G3 − G2. Starting point is the
end point of the first calculation.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
6-91
Part Programming
6.3 Blueprint programming
Fig. 6-31 Input of step 2
Fig. 6-32 Result of step 2
The function provides the point of intersection between circle sector 4 and circle sector 5 as
the end point.
To calculate the tangential transition between
and use the screenform ”Circle −
straight line”.
Fig. 6-33 Screenform ”Circle − straight line”
6-92
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Part Programming
6.3 Blueprint programming
Fig. 6-34 Result of step 3
The function inserts a circle sector (with tangential transitions) between two straight lines.
The circle sector is described by the center point and the radius. Specify the coordinates of
the end point of the second straight line and, optionally, the angle A2. The first straight line is
described by the starting point and the angle A1.
The screenform can be used if the following conditions are fulfilled:
Point Given coordinates
Starting point S Both coordinates in a Cartesian coordinate system
S Starting point as a polar coordinate
Circle sector S Both coordinates in the Cartesian coordinate system and the radius
S Center point as a polar coordinate
End point S Both coordinates in a Cartesian coordinate system
S End point as a polar coordinate
Point Given coordinates
Starting point S Both coordinates in a Cartesian coordinate system
S Starting point as a polar coordinate
Circle sector S One coordinate in the Cartesian coordinate system and the radius
S Angle A1 or A2
End point S Both coordinates in a Cartesian coordinate system
S End point as a polar coordinate
If it is not possible to determine the starting point from the previous blocks, the starting point
must be set by the operator.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
6-93
Part Programming
6.3 Blueprint programming
Fig. 6-35 Straight line − circle − straight line
Table 6-7 Input in the interactive screenform
G2/G3
End point of straight line 2
Center point of the circle M 1st and 2nd axes of the plane
Angle of straight line 1 A1 The angle is specified in the counterclockwise direction.
Angle of straight line 2 A2 The angle is specified in the counterclockwise direction.
Feedrate F Input field for the feedrate
E Enter the end point of the straight line.
End and center points can be specified either absolute, incremental or polar coordinates.
The screenform generates one circle and two straight line blocks from the data you have
entered.
Use this softkey to switch the direction of rotation from G2 to G3. G3 will appear on the display. Pressing this softkey again will switch back the display to G2. The display changes to
G2.
6-94
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
6.4 Simulation
Note
This function is only offered by the 802D bl with the color display option.
Functionality
By using broken−line graphics, the programmed tool path can be traced.
Operating sequence
You are in the AUTOMATIC mode and have selected a program for execution (cf. Section
5.1).
Part Programming
6.4 Simulation
Simulation
Softkeys
The start screen will appear.
Show
...
Cursor co
arse/fine
Fig. 6-36 The ”Simulation” start screen
Press NC START to start the simulation for the selected part program.
Zoom
Auto
To
origin
Show
...
Zoom +
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
If you select this softkey, the recorded tool path is scaled automatically.
If you select this softkey, the default setting is used for the scaling.
Select this softkey to display the whole workpiece.
Use this softkey to enlarge the displayed section.
6-95
Part Programming
6.5 Data transfer via the RS232 interface
Zoom −
Delete
window
Cursor co
arse/fine
Use this softkey to reduce the displayed section.
Use this softkey to delete the visible image.
Use this softkey to change the cursor increment.
6.5 Data transfer via the RS232 interface
Functionality
The RS232 interface of the control system can be used to output data (e.g. part programs)
to an external data backup device or to read in data from there. The RS232 interface and
your data backup device must be matched with each other. (see also Chapter 7)
File types
S Part programs
− Part programs
− Subroutines
S Cycles
Operating sequence
Programs
You have selected the Program Manager area. A list of all programs already created is displayed.
Read out
Use this softkey to saved files via the RS232 interface.
− Standard cycles
6-96
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
User
cycle
Fig. 6-37 Reading out a program
19200
None, 8, 1
RTS−CTS
TAPE
Part Programming
6.5 Data transfer via the RS232 interface
Start
<<
Back
All files
Start
Read in
Error
log
Use this softkey to select all files.
Selecting this softkey selects all files from the part program directory and starts the data
transfer.
Use this softkey to start the output.
Selecting this softkey starts the output of one or several files from the part program directory. To cancel the transfer, use the STOP key.
Use this softkey to load part programs files via the RS232 interface.
Transfer log
This log contains all transmitted files with a status information:
S For files to be output:
- the name of the file
- an error acknowledgment
S For files to be input:
- the name of the file and the path
- an error acknowledgment
Transmission messages:
OK Transmission completed successfully
ERR EOF End−of−text character received, but archive file incomplete
Time Out The time monitoring is reporting an interruption of the data transfer
User Abort Data transfer aborted by the Stop softkey
Error Com Error at the COM 1 port
NC / PLC Error Error message from the NC
Error Data Data error
1. Files read in with / without header
or
2. Files transmitted without file names in the punched−tape format
Error File Name The file name does not correspond to the name convention of the NC.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
6-97
Part Programming
6.5 Data transfer via the RS232 interface
This sheet has been left empty for your notes
6-98
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
System
Functionality
7
The ”System” operating area provides all functions required for parameterizing and analyzing the NCK and the PLC.
Fig. 7-1 The ”System” start screen
Depending on the functions selected, the horizontal and the vertical softkey bars change.
The menu tree shown below only shows the horizontal softkeys.
Start up
NC
PLC
Machine
data
General
MD
Axis
MD
Channel
MD
Drive
MD
Display
MD
Servo
trace
Fig. 7-2 The ”System” menu tree (only horizontal level)
Service
display
Service
Axes
Service
drives
Service
profibus
Servo
trace
Version
PLC
STEP 7
connect
PLC
status
Status
list
PLC
lprogram
Program
list
Edit PLC
alarm txt
:
:
Data I/O
Data
selection
RS232
settings
The softkeys marked with an asterisk (”:”) are not available with the 802D bl.
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
7-99
System
Softkey
Set
password
Setting the password
Three password levels are distinguished in the control system, which provide different access rights:
S System password
S Manufacturer password
S User password
Depending on the access levels (see also ”Technical Manual”), certain data can be changed.
If you do not know the password, access will be denied.
Expert
Change
password
Fig. 7-3 Entering the password
After you have selected the OK softkey, the password is set.
Use ABORT to return without any action to the System main screen.
Changing the password
Fig. 7-4 Changing the password
7-100
SINUMERIK 802D, 802D bl Operartion and Programming Turning (BP−D), 08/05 Edition
6FC5 698−2AA00−1BP4
Loading...