siemens 802S Programming Manual

Download

Operating and Programming 01/2002 Edition

Milling

SINUMERIK 802S/802C

SINUMERIK 802S

Introduction 1

Power ON 2

SINUMERIK 802C

Operation and Programming Milling

Setup 3

Manually Controlled Operation

Automatic Mode 5

Part Programming 6

Valid for

Control System Software Version

SINUMERIK 802S 3 SINUMERIK 802C 3

01.2002 Edition

Services and Diagnosis 7

Programming 8

Cycles 9

3ls

SINUMERIKDocumentation

Printing history

Brief details of this edition and previous editions are listed below. IThe status of each edition is shown by the code in the ”Remarks” column.

Status code in the “Remarks” column:

A New documentation.. . . . .

B Unrevised reprint with new Order No.. . . . .

C Revised edition with new status. . . . . .

If actual changes have been made on the page since the last edition, this is indicated by a new edition coding in the header on the page.

Edition Order–No. Remark

02.99 6FC5598–2AA10–0BP1 A

04.00 6FC5598–3AA10–0BP1 C

01.02 6FC5598–3AA10–0BP2 C

This Manual is included on the documentation on CD–ROM (DOCONCD)

Edition Order–No. Remark

11.02 6FC5298–6CA00–0BG3 C

Trademarks

SIMATICr, SIMATIC HMIr, SIMATIC NETr, SIROTECr, SINUMERIKr and SIMODRIVEr are registered trademarks of Siemens. Third parties using for their own purposes any other names in this document which refer to trademarks might infringe upon the rights of trademark owners.

This publication was produced with Interleaf V 7 The reproduction, transmission or use of this document or its

contents is not permitted without express written authority. Offenders will be liable for demages. All rights, including rights created by patent grant or registration of utility model or design, are reserved.



Printed in the Federal Republic of Germany

Other functions not described in this documentation might be executable in the control. This does not, however, represent an obligation to supply such functions with a new control or when servicing.

We have checked that the contents of this document correspond to the hardware and software described. Nonetheless, differences might exist and therefore we cannot guarantee that they are completely identical. The information contained in this document is, however, reviewed regularly and any necessary changes will be included in the next edition. We welcome suggestions for improvement.

Subject to change without prior notice.

Siemens–AktiengesellschaftBestell–Nr. 6FC5598–3AA10–0BP2

Safety notices

This Manual contains notices intended to ensure your personal safety and to avoid material damage. The notices are highlighted by a warning triangle and, depending on the degree of hazard, represented as shown below:

Danger

indicates that loss of life, severe personal injury or substantial material damage will result if the appropriate pre- cautions are not taken.

Warning

indicates that loss of life, severe personal injury or substantial material damage may result if the appropriate pre- cautions are not taken.

Caution

indicates that minor personal injury or material damage may result if the appropriate precautions are not taken.

Caution

without a warning triangle means that a material damage can occur if the appropriate precau- tions are not taken.

Attention

means that an undesirede event or status can occur if the appropriate note is not observed.

Note

is used to draw your special attention to an important information on the product, the handling of the product or the corresponding part of the documentation.

Qualified personnel

Start–up and operation of a device may only be carried out by qualified personnel. Qualified personnel as referred to in the safety notices provided in this Manual are persons who are authorized to start up, ground and tag devices, systems and circuits according to the relevant safety standards.

Usage as per intended purpose

Please observe the following:

Warning

The device may only be used for the cases of application, as intended by the Catalog, and only in conjunction with third–party devices and components recommended or approved by Siemens.

The proper and safe operation of the product requires transport, storage and installation according to the relevant instructions and qualified operation and maintenance at the prescribed intervals.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

Table of Contents

1 Introduction 1-11. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.1 Screen Layout 1-11. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.2 Operating areas 1-14. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.3 Overview of the most important softkey functions 1-15. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4 Pocket calculator 1-16. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.5 Basic principles 1-22. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2 Turning On and Reference Point Approach 2-25. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3 Setup 3-27. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.1 Entering tools and tool offsets 3-27. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.2 Creating a new tool 3-28. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.3 Tool compensation data 3-29. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.4 Determining the tool offsets 3-30. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.5 Entering/modifying zero offsets 3-32. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.6 Determining the zero offset 3-34. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.7 Programming the setting data – “Parameters” operating area 3-36. . . . . . . . . . . . . . . . . . . . . . . .

3.8 R parameters - “Parameters” operating area 3-38. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4 Manually Operated Mode 4-39. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.1 Jog mode - ”Machine” operating area 4-39. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.1.1 Assigning handwheels 4-41. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.2 MDA Mode (Manual Data Input) - “Machine” operating area 4-43. . . . . . . . . . . . . . . . . . . . . . . . .

5 Automatic Mode 5-45. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.1 Selecting/starting a part program - “Machine” operating area 5-48. . . . . . . . . . . . . . . . . . . . . . . .

5.2 Block search - “Machine” operating area 5-49. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.3 Stopping/cancelling a part program - “Machine” operating area 5-49. . . . . . . . . . . . . . . . . . . . . .

5.4 Repositioning after interruption 5-50. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.5 Program execution from external (V.24 interface) 5-51. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.6 Teach In 5-52. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6 Part Programming 6-55. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.1 Entering a new program - “Program” operating area 6-57. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.2 Editing part programs - “Program” operating area 6-58. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.3 Programming support 6-61. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.3.1 Vertical menu 6-61. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.3.2 Cycles 6-62. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.3.3 Contour 6-63. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.3.4 Free softkey assignment 6-79. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7 Services and Diagnosis 7-81. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.1 Data transfer via the V24 Interface 7-81. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.1.1 Interface parameters 7-84. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.1.2 Special functions 7-85. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.1.3 Interface parameterization 7-85. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

7.2 Diagnosis and start–up - ”Diagnostics” operating area 7-87. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8 Programming 8-99. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.1 Fundamentals of NC programming 8-99. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.1.1 Program structure 8-99. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.1.2 Word structure and address 8-100. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.1.3 Block structure 8-100. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.1.4 Character set 8-102. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.1.5 Overview of instructions 8-104. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2 Position data 8-114. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2.1 Plane selection: G17 to G19 8-114. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2.2 Absolute/incremental dimensions: G90, G91 8-115. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2.3 Metric/inch dimensions: G71, G70 8-116. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2.4 Programmable zero offset and rotation: G158, G258, G259 8-117. . . . . . . . . . . . . . . . . . . . . . . . .

8.2.5 Workpiece clamping – settable zero offset:

G54 to G57, G500, G53 8-119. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3 Axis movements 8-121. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3.1 Linear interpolation at rapid traverse: G0 8-121. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3.2 Linear interpolation at feedrate: G1 8-122. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3.3 Circular interpolation: G2, G3 8-123. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3.4 Circular interpolation via intermediate point: G5 8-126. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3.5 Thread cutting with constant lead: G33 8-127. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3.6 Tapping with compensating chuck: G63 8-128. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3.7 Thread interpolation: G331, G332 8-129. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3.8 Fixed–point approach: G75 8-131. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3.9 Reference point approach: G74 8-131. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3.10 Feedrate F 8-131. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3.11 Feed overrride for circles: G900, G901 8-132. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3.12 Exact stop / continuous–path operation: G9, G60, G64 8-133. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3.13 Dwell time: G4 8-136. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4 Spindle movements 8-137. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4.1 Spindle speed S, directions of rotation 8-137. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4.2 Spindle speed limitation: G25, G26 8-137. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4.3 Spindle positioning: SPOS 8-138. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.5 Rounding, chamfer 8-139. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6 Tool and tool offset 8-141. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.1 General notes 8-141. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.2 Tool T 8-142. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.3 Tool offset number D 8-142. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.4 Selection of tool radius offset: G41, G42 8-146. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.5 Behavior at corners: G450, G451 8-148. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.6 Tool radius compensation OFF: G40 8-149. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.7 Special cases of tool radius compensation 8-151. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.8 Example of tool radius compensation 8-153. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.7 Miscellaneous function M 8-154. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8 Arithmetic parameters R 8-155. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.9 Program branches 8-157. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.9.1 Labels – destination for program branches 8-157. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.9.2 Unconditional program branches 8-157. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.9.3 Conditional branches 8-158. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.9.4 Example of program with branches 8-160. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.10 Subroutine technique 8-161. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9 Cycles 9-165. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1 General information about standard cycles 9-165. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.1 Overview of cycles 9-165. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

vii

9.1.2 Error messages and error handlingin cycles 9-166. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2 Drilling cycles 9-168. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2.1 Drilling, spot facing – LCYC82 9-168. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2.2 Deep hole drilling – LCYC83 9-170. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2.3 Tapping without compensating chuck – LCYC84 9-174. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2.4 Tapping with compensating chuck – LCYC840 9-176. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2.5 Boring – LCYC85 9-179. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.3 Drilling patterns 9-181. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.3.1 Drilling a row of holes – LCYC60 9-181. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.3.2 Hole circle – LCYC61 9-185. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.4 Milling cycles 9-187. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.4.1 Cutting square pockets, slots and circular pockets – LCYC75 9-187. . . . . . . . . . . . . . . . . . . . . . . .

viii

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

SINUMERIK 802S Slimline Operator Panel OP

Softkey

Machine area key

Recall key

ETC key

Area switchover key

Cursor UP

with shift: page up

Cursor LEFT

Delete key (backspace)

Numerical keys

shift for alternative assignment

Alphanumeric keys

Vertical menu

Acknowledge alarm

Selection key/toggle key

ENTER / input key

Shift key

Cursor DOWN

with shift: page down

Cursor RIGHT

SPACE (INSERT)

shift for alternative assignment

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

External Machine Control Panel

User–defined key with LED

User–defined key without LED

INCREMENT

JOG

REFERENCE POINT

AUTOMATIC

SINGLE BLOCK

MANUAL DATA

SPINDLE START LEFT Counterclockwise direction

SPINDLE START RIGHT Clockwise direction

SPINDLE STOP

RAPID TRAVERSE OVERLAY

RESET

NC STOP

X axis

NC START

Z axis

Spindle Speed Override

Feed Rate Override

(optional)

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Introduction

1.1 Screen Layout

1 2 3 4

Fig. 1-1 Screen layout

The abbreviations on the screen stand for the following:

Table 1-1 Explanation of display elements

Display Element

Active operating area

Program status

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

Abbreviation Meaning

MA Machine

PA Parameter

PR Programming

DI Services

DG Diagnosis

STOP Programm stopped

RUN Program running

RESET Program aborted

1-11

Introduction

1.1 Screen Layout

Table 1-1 Explanation of display elements

Display Element

Operating mode

Status display

MeaningAbbreviation

Jog Manual traverse

MDA Manual input with automatic function

Auto Automatic SKP Skip block

Program blocks marked by a slash in front of the block number are ignored during program execution.

DRY Dry run feed

Traversing movements are executed at the feed specified in the Dry Run Feed setting data.

ROV Rapid traverse override

The feed override also applies to rapid feed mode.

SBL Single block with stop after each block

When this function is active, the part program blocks are processed separately in the following manner:

Each block is decoded separately, the program is stopped at the end of each block. The only exception are thread blocks without dry run feed. In this case, the program is stopped only when the end of the current thread block is reached. SBL can only be selected in the RESET state.

M1 Programmed stop

When this function is active, the program is stopped at each block in which the miscellaneous function M01 is programmed.

In this case, the message “5 stop M00/M01 active“ appears on the screen.

PRT Program test

1...1000 INC Incremental mode If the control is in the Jog mode, incremental dimension is

displayed instead of the active program control function.

1-12

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Table 1-1 Explanation of display elements

Introduction

1.1 Screen Layout

Display Element

Operational messages

11 12 13 14 15 16 17 18 19 20 21 22 23

MeaningAbbreviation

1 2 3 4 5 6 7 8 9

Stop: No NC Ready Stop: EMERGENCY STOP active

Stop: Alarm active with stop Stop: M0/M01 sctive Stop: Block ended in SBL mode Stop: NC STOP active Wait: Read–in enable missing Wait: Feed enable missing Wait: Dwell time active Wait: Auxiliary function acknowl. missing Wait: Axis enable missing Wait: Exact stop not reached

Wait: For spindle Wait: Feed override to 0%

Stop: NC block incorrect

Wait: Block search active Wait: No spindle enable Wait: Axis feed value 0

Program name

Alarm line

Working window

Recall symbol

Menu extension

Softkey bar

Vertical menu

The alarm line is only displayed if an NC or PLC alarm is active. The alarm line contains the alarm number and reset criterion of the most recent alarm.

Working window and NC display

This symbol is displayed above the softkey bar when the operator is in a lower–level menu.

When the Recall key is pressed, you can return to the next– higher menu without saving data.

ETC is possible

If this symbol appears above the softkey bar, further menu functions are provided. These functions can be activated by the ETC key.

If this symbol is displayed above the softkey bar, further menu functions are provided. When the VM key is pressed, these functions appear on the screen and can be selected by Cursor UP and Cursor DOWN.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

1-13

Introduction

1.2 Operating areas

The basic functions are grouped in the CNC into the following operating areas:

Operating areas

Machine Parameter Program Services

Executing part programs Manual control

Fig. 1-2 SINUMERIK 802S operating areas

Editing program data

Switching between the operating areas

Press the “Machine area” key for direct access to the “Machine” operating area.

Use the area switching key to return from any operating area to the main menu.

Press the area switching key twice to return to the previous operating area. After turning on the control system, you will always find yourself in the

Machine operating area.

Creating part programs

Data import / export

Diagnosis

Alarm display Start–up

Protection levels

Sensible points of the control system are password–protected against entering and modifying data.

However, the operator can alter the classes of protection in the “Machine data display” menu in the “Diagnosis” operating area.

Default: protection level 3. In the following menus, entering and modifying data depends on the set protection class:

S tool offsets S zero offsets S setting data S V24 setting

1-14

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

1.3 Overview of the most important softkey functions

Introduction

Machine

Parameters Program

Alarms

Data Data in out

Progr.

Services

Service

display

Display Display bright. darker

RS232 setting

Execut f. ext.

Cycles

New Copy

Diagnosis

Start–up

Change lang.

Error log

Selection

Delete Rename

Machine data

Show

Open

Memory

info

R Tool Setting Zero parameters offset data

Program control WCS act.val.

Zoom block

Axis feed

Block search

Zoom block

Axis feed

Handwheel

Axis feed

Execut f. ext.

offset

Act.val. Zoom

Zoom G funct.

Act.val. WCS

Zoom act. val.

Zoom G funct.

Act.val. WCS/MCS

Zoom act.val.

Zoom M funct.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

1-15

Introduction

1.4 Pocket calculator

This function can be activated for all input fields intended for entry of numerical values by means of the “=” character. To calculate the required value, you can use the four basic arithmetic operations, and the functions sine, cosine, squaring, as well as the square root function.

If the input field is already loaded with a value, this function writes the value in the input line of the pocket calculator.

Fig. 1-3 Pocket calculator

Permissible character

The following characters are permitted for input:

+ Value X plus value Y – Value X minus value Y * Value X multiplied with value Y / Value X divided by value Y S Sine function

The value X in front of the input cursor is replaced by the value sin(X). C Cosine function

The value X in front of the input cursor is replaced by the value cos(X). Q Square function

The value X in front of the input cursor is replaced by the value X R Square root function

The value X in front of the input cursor is replaced by the value √X.

Calculation examples

100 + (67*3) 100+67*3 sin(45_) 45 S –> 0.707107 cos(45_) 45 C –> 0.707107

4 √4 4 R –> 2

The calculation is carried out when the Input key is pressed. The function writes the result to the input field and automatically closes the pocket calculator.

Task Input

4 Q –> 16

1-16

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Softkeys

Introduction

1.4 Pocket calculator

To calculate auxiliary points on a contour, the pocket calculator provides the following functions:

S calculating the tangential transition between a circle sector and a straight line S moving a point in a plane S converting polar coordinates into Cartesian coordinates S adding the second end point of a contour section ’straight line – straight line’ given via an-

gular interrelation.

These functions are directly linked with the input fields of the programming support. Any values in this input field are written by the pocket calculator into the input line, and the result is automatically copied into the input fields of the programming support.

This function is used to calculate a point on a circle. The point results from the angle of the created tangent and the direction of rotation of the circle.

Fig. 1-4 Calculation of a point on a circle

Enter the circle center, the angle of the tangent and the radius of the circle.

Use the softkeys G2 / G3 to define the direction of rotation of the circle.

The values of abscissa and ordinate are calculated. The abscissa is the first axis of the plane, and the ordinate the second axis of the plane.

Example

If plane G17 is active, the abscissa is the X axis, and the ordinate the Y axis.

The value of the abscissa is copied into that input field from which the pocket calculator function has been called, and the ordinate value into the next following input field.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

1-17

Introduction

1.4 Pocket calculator

Example

Calculating the intersection point between the circle sector and the straight line . Given: Radius: 10

Circle center point: X 20 Y20 Ongoing angle of the straight line: 45°

Result: X = 12.928

Y = 27.071

The function calculates the Cartesian coordinates from a straight line specified by length and rise angle.

Fig. 1-5 Conversion of the polar coordinates into Cartesian coordinates

Enter the pole point (PP) as both an abscissa and ordinate value, the length and the rise angle of the straight line.

1-18

The values of abscissa and ordinate are calculated.

The abscissa value is copied into the input field from which the pocket calculator function has been called, and the ordinate value into the next following input field.

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Example

Introduction

1.4 Pocket calculator

Calculating the end point of the straight line . The straight line is defined by the angle

° uand its length..

A=45

Result: X = 51.981

Y = 43.081

This function can be used to move a point in the plane. The point is on a straight line defined by its rise angle.

Fig. 1-6 Moving a point in the plane

Enter the rise angle of the straight line and the coordinates of the point. Enter line shift and rotation of the point with refer to the straight line in the fields “line shift” and

“rotation”.

The values of abscissa and ordinate are calculated.

The pocket calculator copies the abscissa value into the input field from which the pocket calculator function has been called, and the ordinate value into the next following input field.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

1-19

Introduction

1.4 Pocket calculator

Example

Calculating the end point of the straight line . The straight line stands vertical on the end point of the straight line (coordinates: X = 51.981, Y = 43.081). The length of the straight

line is also given.

Result: X = 68.668

Y = 26.393

This function calculates the missing end point of the contour section straight line – straight line, with the second straight line standing vertically on the first straight line.

The following values of the straight line are known: Straight line 1: Starting point and rise angle

Straight line 2: Length and one end point in the Cartesian coordinate system

Fig. 1-7

1-20

This function chooses the given coordinate of the end position. The value of ordinate and/or abscissa is given.

The second straight line is rotated in clockwise direction or, with refer to the first straight line, rotated by 90 degrees in counter–clockwise direction. The function chosses the appropriate setting.

The missing end position is calculated. The value of the abscissa is copied into that input field from which the pocket calculator function has been called, and the ordinate value into the next following input field.

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Example

Introduction

1.4 Pocket calculator

The drawing above must be added by the values of the of the circle center points to be able to calculate the intersection points between the contour sections. Calculating the missing coordi-

nates of the center points is carried out with the pocket calculator function , since the radius in the tangential transition stands vertical on the straight line.

Calculating M1 in section 1:

In this section, the radius stands on the straight line section in counter–clockwise direction. Use the softkeys and to select the given constellation.

Enter the coordinates, the pole point P1, the rise angle of the straight line, the given ordinate value and the circle radius as the length.

Result: X = –19.449

Y = 30

Calculating M2 in section 2:

In this section, the radius stands on the straight line section rotated in clockwise direction. Use the softkeys to select the given constellation.

Enter the parameters in the screen form.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

Result X = 21.399

Y = 30

1-21

Introduction

1.5 Basic principles

Coordinate sytems

Right–handed, rectangular coordinate systems are used for machine tools. Such systems describe the movements on the machine as a relative motion between tool and workpiece.

Fig. 1-8 Specification of mutual relationship between axis directions;

+ Z

90°

+ X

Machine coordinate system (MCS)

The orientation of the coordinate system on the machine tool depends on the particular machine type. It can be turned to various positions.

1-22

Fig. 1-9 Example of machine coordinates/axes

The origin of the coordinate system is the machine zero. All axes are in zero position at this point. This point is merely a reference point determined by the machine manufacturer. It need not to be approachable.

The traversing range of the machine axes can be negative.

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Workpiece coordinate system (WCS)

The workpiece coordinate system described above (see Fig. 1-8) is also used to describe the geometry of a workpiece in the workpiece program. The workpiece zero can be freely selected by the programmer. The programmer need not know the real movement conditions on the machine, i.e. whether the workpiece or the tool moves; this can be different in the individual axes. The definition of the directions is based on the assumption that the workpiece does not move and the tool moves.

Introduction

1.5 Basic principles

W=workpiece zero

Fig. 1-10 Workpiece coordinate system

Current workpiece coordinate system

If the programmer feels that it is better to continue his geometrical descriptions from another zero than the initially selected zero (workpiece zero), he can define a new zero using the programmable zero offset. Reference is always made to the original zero. The use of the programmable zero offset provides a completely new current workpiece coordinate system. The current workpiece coordinate system can also be turned to the original workpiece coordinate system (see Section “Programmable Zero Offset and Rotation”).

Programmable offset

G158

Z Current

W=workpiece zero

Fig. 1-11 Coordinates on the workpiece, current workpiece coordinate sy-

stem

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

1-23

Introduction

1.5 Basic principles

Workpiece clamping

To machine the workpiece, it is clamped on the machine. The workpiece must be aligned such that the axes of the workpiece coordinate system run in parallel with the machine axes. Any resultant offset of the machine zero is determined for each axis and entered into the intended data areas for the settable zero offset. This offset is activated during the NC program execution by means, for example, of a programmable G54 (see Section ”Workpiece Clamping – Settable Zero Offset ...”).

Machine

Workpiece

W=workpiece zero M=machine zero

z.B.

G54

Fig. 1-12 Workpiece on the machine

Machine

1-24

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Turning On and Reference Point Approach

Note

Before you switch on the SINUMERIK and the machines, you should also have read the machine documentation, since turning on and reference point approach are machine–dependent functions.

Operating sequence

First switch on the power supply of the CNC and of the machine. After the control system has booted, you are in the “Machine” operating area, in the Jog operating mode.

The Reference point approach window is active.

Fig. 2-1 Jog Ref basic screen

Reference–point approach can only be executed in the Jog mode.

Activate the “Approach reference point” function by selecting the Ref key on the machine control panel.

In the “Reference point approach” window (Fig. 2-1), it is displayed whether or not the axes have to be referenced.

Axis has to be referenced Axis has reached the reference point

...

Press the direction keys.

-Z

The axis does not move if you select the wrong direction. Approach the reference point in each axis successively.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

2-25

Turning On and Reference Point Approach

You can quit the function by selecting another operating mode (MDA, Automatic or Jog).

2-26

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Setup

Preliminary remarks

S Before you can use the CNC, set up the machine, tools, etc. on the CNC by: S entering the tools and tool offsets S entering/modifying the zero offset S entering the setting data

3.1 Entering tools and tool offsets

Functionality

The tool offsets consist of several data that describe the geometry, wear and tool type. Each tool has a defined number of parameters depending on the tool type. Each tool is identified by its own tool number (T number).

See also Section 8.6 “Tool and Tool Offset“.

Operating sequences

Parameter

Tool Corr.

This function opens the Tool Compensation Data window, which contains the offset values of the currently active tool. If you select another tool using the <<T or T>> softkeys, the setting remains when you quit the window.

Fig. 3-1 Tool list

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

3-27

Setup

3.2 Creating a new tool

Softkeys

<< D

D >>

<< T

T >>

Reset edge

New edge

Delete tool

New tool

Select next lower or next higher edge number.

Select next lower or next higher tool.

Pressing this softkey opens the dialog box and the overview of the tool numbers assigned. Enter the tool number you search for in the input window and start search with OK. If the searched tool exists, the search function opens the tool offset data box.

Press the ETC key to extend the softkey functions.

All edge compensation values are reset to zero.

Creates a new edge and loads it with the appropriate parameters.

The new edge is created for the currently displayed tool; it is automatically assigned the next higher edge number (D1 - D9).

Max. 30 edges (in total) can be stored in the memory.

Deletes the tool compensation data of all edges of the selected tool.

Creates new tool compensation data for a new tool. Note: Max. 20 tools can be created.

Get Comp.

Determines the length compensation values.

3.2 Creating a new tool

Operating sequence

Press this softkey to create a new tool.

New tool

Pressing this softkey opens the input window and an overview of the tool numbers assigned.

3-28

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Fig. 3-2 New Tool window

Setup

3.3 Tool compensation data

. . .

Enter the new T number (in the range from 1 to 32000) and specify the tool type.

Press OK to confirm your entry; the Tool Compensation Data window is opened.

3.3 Tool compensation data

The tool compensation data are divided into length and radius compensation data. The list is structured according to the tool type.

Fig. 3-3 Tool compensation data

Operating sequence

Enter the offsets by

positioning the cursor on the input field to be modified,

. . .

entering value(s)

and confirming your entry by pressing Input or a cursor selection.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

3-29

Setup

3.4 Determining the tool offsets

Functionality

This function can be used to determine the unknown geometry of a tool T.

Prerequisite

The appropriate tool has been changed. In JOG mode, approach a point on the machine, from which you knw the machine coordinates, with the edge of the tool. This can be a workpiece with a knwon position. The machine coordinate value can be split into two components: stored zero offset and offset.

Procedure

Enter the offset value in the intended Offset field. Then select the required zero offset (e.g. G54) or G500 if no zero offset is to be calculated. These entries must be made for each selected axis (see Fig. 3–5). Please note the following: For milling tools, length 1 and the radius must be determined, and for drilling tools only length 1.

Using the actual position of point F (machine coordinate), the offset entry and the selected zero offset Gxx (position of the edge), the control system can calculate the assigned compensation value of length 1 or the tool radius.

Note: You can also use a zero offset already determined (e.g. G54 value) as the known machine coordinate. In this case, approach the workpiece zero with the edge of the tool. If the edge stands directly at the workpiece zero, the offset value is zero.

F–tool carrier reference point M–machine zero

W–workpiece zero

Machine

Workpiece

Fig. 3-4 Determination of length compensation using the example of a drill: length 1/Z

axis

Interm. layer

Length 1=?

Actual position Z

Known machine coordinate value Z

Offset

Gxx, z.B. G54

Machine

3-30

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Operating sequence

Setup

3.4 Determining the tool offsets

Get Comp.

Select the softkey Get Comp. The window Compensation values opens.

Fig. 3-5 Window Compensation values

S Enter offset if the tool edge cannot approach the zero point Gxx. If you work withut zero

offset, select G500 and and enter offset.

S When the softkey Calculate is pressed, the control system determines the searched geo-

metry length 1 or the radius depending on the preselected axis. This geometry is calculated on the basis of the approached actual position, the selected Gxx function and the entered offset value. The determined compensation value is stored.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

3-31

Setup

3.5 Entering/modifying zero offsets

Functionality

The actual–value memory and thus also the actual–value display are referred to the machine zero after the reference–point approach. The workpiece machining program, however, refers to the workpiece zero. This offset must be entered as the zero offset.

Operating sequenc

Parameter

Zero offset

. . .

Use the Parameter and Zero Offset softkeys to select the zero offset.

An overview of settable zero offsets appears on the screen .

Fig. 3-6 Zero Offset window

Position the cursor bar on the input field to be altered,

enter value(s).

Softkeys

Deter– mine

3-32

The next zero offset overview is displayed by Page down. G56 and G57 are now displayed.

Return to next–higher menu level, without saving the zero offset values.

Use this function to determine the zero offset with refer to the coordinate origin of the machine coordinate system. When you have selected the tool, which you want to use for measuring, you can set the appropriate conditions in the Determine window.

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Setup

3.5 Entering/modifying zero offsets

Fig. 3-7 Zero offset measuring using the Determine function

The toggle fields can be used to calculate the tool compensation values. It is possible to specify an additional length in the Offset box, which must then be considered

in the calculation (for example, when using a spacer). The current axis position, the active compensation value and the tool compensation data are

displayed.

Next Uframe

Next Axis

Calcu– late

Programmed

Sum

Move the tool to the selected zero and set all compensation values for the selected axis. The Calculate softkey function will then caluclate the offset and enter the value in the respective field. This process must be repeated for all axes.

Selects the next settable zero offset.

Selects the next axis.

The compensation values are caluclated with the Offset field and the current axis position (MCS). The result will be assigned to the selected axis as an offset value.

Closes the window.

Opens a window with the programmed zero offset. The value shown in the window cannot be edited.

Displays the total of all active zero offsets. The values cannot be edited.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

3-33

Setup

3.6 Determining the zero offset

Prerequisite

You have selected the window with the corresponding zero offset (e.g. G54) and the axis for which you want to determine the offset.

Approach

Fig. 3-8 Determining the zero offset for the Z axis

S A zero offset can only be determined with a known (entered geometry) and active tool. En-

ter the active tool in the dialog box. Press OK to take over the tool; the Determine window is then opened.

S The selected axis appears in the Axis area.

The actual position of the tool support reference point (MCS) associated to the axis is displayed in the adjacent field.

S D number 1 is displayed for the tool edge.

If you have entered the valid offsets for the used tool under a D number other than D1, enter that D number here.

S The stored tool type is displayed automatically. S The effective length compensation value (geometry) is displayed. S Select the sign (–, +) for calculating the length offset, or select “without”

taking the length offset into account. A negative sign subtracts the length offset value from the actual position.

S If the tool can neither reach, nor “scrape” the desired position, an offset value can be ent-

ered in the Offset field.

3-34

S Approach the coordinates of the intended workpiece zero offset (if necessary with conside-

ration of the entered offset value) in JOG mode.

S The resulting zero offset is determined from the actual position and all active compensa-

tion values by means of the Calculate function.

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Fig. 3-9 Select Tool screen form

Setup

3.6 Determining the zero offset

Next UFrame

Calcu– late

Fig. 3-10 Determine Zero Offset form

Softkey can be used to select the zero offsets G54 to G57. The selected zero offset is displayed on the selected softkey.

Pressing the Calculate softkey calculates the zero offset.

Press the OK softkey to quit the window.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

3-35

Setup

3.7 Programming the setting data – “Parameters” operating area

Functionality

Use the setting data to define the settings for the operating states. These can also be modified if necessary.

Operating sequence

Parameter

Sett. data

. . .

Use the Parameter and Setting Data softkeys to select Setting Data.

The Setting Data softkey branches to another menu level in which various control options can be set.

Fig. 3-11 Setting Data basic screen

Use the paging keys to position the cursor on the desired line within the display areas.

Enter the new value in the input fields.

Softkeys

Jog data

3-36

Use Input or the cursor keys to confirm.

This function can be used to change the following settings:

Jog feed

Feed value in Jog mode If the feed value is zero, the control system uses the value stored in the machine data.

Spindle

Spindle speed Direction of rotation of the spindle

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Setup

3.7 Programming the setting data – “Parameters” operating area

Spindle data

Dry feed

Start angle

Minimum / Maximum

Limits for the spindle speed set in the Max. (G26)/Min. (G25) fields must be within the limit values specified in the machine data.

Programmed (LIMS)

Programmable upper speed limitation (LIMS) at constant cutting speed (G96).

Dry–run feedrate for dry–run operation (DRY)

The feedrate you enter here is used in the program execution instead of the programmed feed during the Automatic mode when the Dry–Run Feedrate is active (see Program Control, Fig. 5-3).

Start angle for thread cutting (SF)

A start angle representing the starting position for the spindle is displayed for thread cutting operations. It is possible to cut a multiple thread by altering the angle and repeating the thread cutting operation.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

3-37

Setup

3.7 Programming the setting data – “Parameters” operating area

3.8 R parameters - “Parameters” operating area

Functionality

All R parameters (arithmetic parameters) that exist in the control system are displayed on the R Parameters mainscreen as a list (see also Section 8.8 “Arithmetic Parameters /R Parameters/”). These can be modified if necessary.

Fig. 3-12 R Parameters window

Operating sequence

Parameters

R Para– meters

. . .

Use the Parameter and R Parameter softkeys

to position the cursor on the input field that you want to edit.

Enter value(s).

Press Input or use the cursor keys to confirm.

3-38

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Manually Operated Mode

Preliminary remarks

The manually operated mode is possible in the Jog and MDA mode. In the Jog mode, you can traverse the axes, and in the MDA mode, you can enter and ex-

ecute individual part program blocks.

4.1 Jog mode - ”Machine” operating area

Functionality

In the Jog mode, you can

S traverse the axes and S set the traversing speed by means of the override switch, etc.

Operating sequence

Use the Jog key on the machine control panel to select the Jog mode.

[ . ]

...

To traverse the axes, press the appropriate axis direction keys.

-Z

As long as the direction key is pressed and hold down, the axes traverse continuously at the speed stored in the setting data. If this setting is zero, the value stored in the machine data is used.

If necessary use the override switch to set the traversing speed.

If you press the Rapid Traverse Override key at the same time, the selected axis is traversed at rapid traverse speed for as long as both keys are pressed down.

In the Incremental Feed operating mode, you can use the same operating sequence to traverse the axis by settable increments. The set increment is displayed in the display area. Jog must be pressed again to cancel.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

4-39

Manually Operated Mode

4.1 Jog mode - ”Machine” operating area

The Jog basic screen displays position, feed and spindle values as well as the current tool.

Fig. 4-1 Jog basic screen

Parameters

Table 4-1 Description of parameters in the Jog basic screen

Softkeys

Parameter

MKS

Display of addresses of existing axes in machine coordinate system (MCS).

Explanation

X Y Z

- Z

If you traverse an axis in the positive (+) or negative (-) direction, a plus or minus sign appears in the respective field.

No axis is displayed, if the axis is in position.

Act.

The current position of the axes in the MCS or WCS is displayed in these fields.

Repos

offset

If the axes are traversed in the Jog mode in the Program Interrupted condition, the distance traversed by each axis in relation to the break point is displayed in this column.

Spindle S

Display of actual value and setpoint of spindle speed

rpm

Feed F mm/

Display of path feed actual value and setpoint

min

Tool Display of currently active tool with the current cutting edge number

Hand– wheel

Axis feed

Interp./ feed

4-40

Call the Handwheel window.

Call the Axis Feed or Interp. Feed window.

Use this softkey to change between the Axis Feed window and the Interp. Feed window. The softkey label changes to Interp. feed when the Axis/Feed window is opened.

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Manually Operated Mode

4.1 Jog mode - ”Machine” operating area

Act. val. WCS

Act.val. MCS

The actual values are displayed as a function of the selected coordinate system. There are two different coordinate systems, i.e. the machine coordinate system (MCS) and the workpiece coordinate system (WCS).

The softkey changes between MCS and WCS. When doing this, the softkey label changes as follows:

S The values of the machine coordinate system are selected, the softkey label changes to

Act. val. WCS.

S When the workpiece coordinate system is selected, the label changes to Act. val. MCS.

Zoom act.val.

Enlarged view of actual values

4.1.1 Assigning handwheels

An axis is assigned to the respective handwheel and becomes active as soon as you press

OK.

Operating sequence

In Jog mode, call the Handwheel window.

Handwheel

After the window has opened, all axis identifiers are displayed in the Axis column and also appear in the softkey bar. Depending on the number of connected handwheels, it is possible to change from handwheel 1 to handwheel 2 using the cursor.

Place the cursor on the line with the handwheel to which you wish to assign an axis. Then select the softkey that contains the name of the axis.

The symbol appears in the window.

Fig. 4-2 Handwheel window

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

4-41

Manually Operated Mode

4.1 Jog mode - ”Machine” operating area

WCS

MCS

De– select

The WCS/MCS softkey is used to select the axes from the machine or workpiece coordinate system for assignment to the handwheel. The current setting is displayed in the handwheel window.

Use the OK softkey to take over the selected setting; the window is then closed.

Menu extension

The assignment you have made is reset for the selected handwheel.

4-42

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Manually Operated Mode

4.2 MDA Mode (Manual Data Input) - “Machine” operating area

Functionality

You can create and execute a part program block in the MDA mode. Contours that require several blocks (e.g. roundings, chamfers) cannot be executed/program-

med.

Caution

Operating sequence

This mode is protected by the same safety interlocks as fully automatic mode. Furthermore, the MDA mode is subject to the same prerequisites as the fully automatic mode.

Use the MDA key on the machine control panel to select the MDA mode.

Fig. 4-3 MDA basic screen

. . .

Enter a block using the control keyboard.

The entered block is executed by pressing NC START. The block cannot be executed while machi- ning is taking place.

After processing, the contents of the input field remains stored so that the block can be traversed with new NC Start. The block is deleted by entering any new character.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

4-43

Manually Operated Mode

4.2 MDA Mode (Manual Data Input) - “Machine” operating area

Parameters

Table 4-2 Description of the parameters in the MDA working window.

Softkeys

Zoom block

Act.val. WCS

Act.val. MCS

Parameter

MCS

Display of existing axes in MCS or WCS

Explanation

X Y Z

If you traverse an axis in the positive (+) or negative (-) direction, a plus or minus

- Z

sign appears in the respective field. No sign is displayed if the axis is in position.

Act. value mmThe current position of the axes in the MCS or WCS is displayed in these fields.

Spindle S

Display of actual value and setpoint of spindle speed

rpm

Feed F Display of path feed actual value and setpoint in mm/min or mm/rev.

Tool Display of currently active tool with the current tool edge number (T..., D...).

Edit window In the Stop or Reset program state, an edit window is provided for input of the part

program block.

The window shows the currently edited block full length.

The actual values for the MDA mode are displayed as a function of the selected coordinate system. There are two different coordinate systems, i.e. the machine coordinate system (MCS) and the workpiece coordinate system (WCS).

Zoom act.val.

Axis feed

Interp. feed

Zoom G funct.

Zoom M funct.

Enlarged view of the actual values

Menu extension

Display of Axis Feed or Interp. Feed window This softkey can be used to change between the two windows. The softkey label changes to Interp. Feed when the Axis Feed window is opened.

The G Function window contains all active G functions. Each G function is assigned to a group and has a fixed position in the window. More G functions can be displayed by pressing the PAGE UP or PAGE DOWN keys. You can exit the window by pressing Recall.

Opens the M function window for displaying all active M functions of the block.

4-44

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Automatic Mode

Functionality

In the Automatic mode, part programs can be executed fully automatically, i.e. this is the operating mode for standard processing of part programs.

Preconditions

The preconditions for executing part programs are:

S Reference point approached. S You have already stored the required part program in the control system. S You have checked or entered the necessary offset values, e.g. zero offsets or tool offsets. S The required safety interlocks are activated.

Operating sequence

Use the Automatic key to select the Automatic mode.

The Automatic basic screen appears that displays the position, feed, spindle, and tool values, as well as the current block.

Execu t. f. ext.

Fig. 5-1 Automatic basic screen

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

5-45

Automatic Mode

Parameters

Table 5-1 Description of the parameters in the working window

Parameter

MCS

Display of existing axes in MCS or WCS.

Explanation

X Y Z

+ X

- Z

If you traverse an axis in the positive (+) or negative (-) direction, a plus or minus sign appears in the respective field.

No sign is displayed if the axis is in position.

Act. val.mmThe current position of the axes in the MCS or WCS is displayed in these fields.

Distance to go

Spindle S

The remaining distance to be traversed by these axes in the MCS or WCS is displayed in these fields.

Display of actual value and setpoint of spindle speed

rpm

Feed F

Display of path feed actual value and setpoint

mm/min or

mm/rev

Tool Display of currently active tool with the current cutting edge number (T..., D...).

Current

block

The block display contains the current block. The block is output in one line only and truncated if necessary.

Softkeys

Progr. control

Zoom block

Interr. point

Contin. search

Start B search

The window to select Program Control (e.g. skip block, program test) appears on the screen.

This window displays the previous, current and next block in full. In addition, the names of the current program or subroutine are displayed.

Use the Block Search function to jump to the desired point in the program.

The Search softkey provides the functions “Find line” and “Find text”.

The cursor is positioned to the main program block of the breakpoint (”interrupt point”). The search target is automatically set in the subroutine levels.

Continue search

The Start B Search softkey starts the search process in which the same calculations are carried out as in normal program mode, but without axis movements.

The block search can be canceled by NC Reset.

Act.val. WCS

Act.val. MCS

5-46

The values of the machine or workpiece coordinate system are selected. The softkey label changes to Act. val. WCS or Act. val. MCS.

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Automatic Mode

Zoom act.val.

Axis feed

Interp. feed

Execut f. ext.

Zoom G Funkt.

Enlarged view of actual values

Menu extension

When pressing these softkeys, the Axis Feed or Interp. Feed window appears.

This softkey can be used to change between the windows. The softkey label changes to In- terp. feed when the Axis Feed window is opened.

An external program is transferred to the control system via the V .24 interface and executed immediately by pressing NC Start.

Opens the G Function window to display all active G functions.

Zoom M funct.

Fig. 5-2 Active G Functions window

Opens the M Function window to display all active M functions.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

5-47

Automatic Mode

5.1 Selecting/starting a part program - “Machine” operating area

Functionality

The control system and the machine must be set up before the program is started. Please note the safety instructions provided by the machine manufacturer.

Operating sequence

Use the Automatic key to select the Automatic mode.

Program

Programs

Select

Progr. control

An overview of all programs stored in the control system is displayed.

Position the cursor bar on the desired program.

Use the Select softkey to select the desired program for processing.

If necessary now you can make settings for program control.

The following program control functions can be activated and deactivated:

5-48

Fig. 5-3 Program Control window

The part program is executed when NC START is pressed.

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

5.2 Block search - “Machine” operating area

Operating sequence

Precondition: The desired program has already been selected (cf. Section 5.1), and the control system is in the reset state.

Automatic Mode

Start B search

Search result

The block search function can be used to advance the program up to the desired point in the part program. The search target is set by positioning the cursor directly on the desired block in the part program.

DEMO.MPF

Fig. 5-4 Search window

The funktion starts program advance and closes the Search window.

The desired block is displayed in the Current Block window.

5.3 Stopping/cancelling a part program - “Machine” operating area

Functionality

Part programs can be stopped and aborted.

Operating sequence

The execution of a part program can be interrupted by selecting NC STOP. The interrupted program can be continued by NC START.

The current program can be aborted by pressing RESET. When you press NC START again, the aborted program is restarted and executed from the begin- ning.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

5-49

Automatic Mode

5.4 Repositioning after interruption

Functionality

After a program interruption (NC STOP), you can move the tool away from the contour in the manual mode (Jog). The control system stores the coordinates of the breakpoint (”interrupt point”). The path differences traversed by the axes are displayed.

Operating sequence

Select the Automatic mode.

Interr. point

Start B search

Open the Block Search window to load the breakpoint.

The breakpoint is loaded. The routine is adjusted to the start position of the interrupted block.

A block search to the breakpoint is started.

Continue execution of the program by NC START.

5-50

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Automatic Mode

5.5 Program execution from external (V.24 interface)

Functionality

An external program is transferred into the control system via the V.24 interface and executed immediatelyby pressing NC Start.

While processing the contents of the buffer memory, the program is automatically reloaded. For example, as an external device, a PC can be used, on which the PCIN tool for data transfer is installed.

Operating sequence

Prerequisite: The control system is reset. The V.24 interface is parameterized correctly (see Chapter 7) and not occupied by any other application (DataIn, DatatOut, STEP7).

Execute f. ext.

Press this softkey .

Use PCIN on the external device (PC) to set the program for data output active. The program is transferred to the buffer memory and automatically selected and displayed in

the program selection. For the program execution, it is advantageous to wait until the buffer memory is filled.

The program execution starts with NC START. The program is reloaded continuously.

Either at the end of the program or when pressing RESET, the program is automatically remo- ved from the control system.

Note

S As an alternative, External Program Execution can also be activated in the Services area. S Any transfer errors are displayed in the Services area when you press the Error log softkey.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

5-51

Automatic Mode

5.6 Teach In

Functionality

Use the submode Teach In to accept the axis position values directly into a parts program block to be generated or modified.

The axis positions are approached either in Automatic mode by traversing the JOG keys or by using the handwheel. However, first press the appropriate softkey (see below) in the Programming operating area to enable the submode Teach In.

Operating sequence

Prerequisite:

– Teach–in option is set; – The control system is either in the state Stop or Reset.

Programs

open

Edit

Teach In

A list of all programs existing in the control system is displayed.

Pressing Open calls the editor for the selected program and opens the editor window.

Menu extension

Select

Menu extension

Select

Softkeys

Technol. Data

5-52

Fig. 5-5 Teach In basic screen

Use this softkey to generate a block with technological data.

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Automatic Mode

5.6 Teach In

Use this screen form to enter

S feed value S spindle speed and direction of rotation (CW; CCW; stop) S tool and edge number S machining level S Feed mode (active; mm/min corresponds to G64; mm/rev. of spindle corresponds to G96) S Positioning behavior (active; exact stop G60; continuous–path control mode G64)

Teach In Records

Fig. 5-6 Input screen form for technological data

When you press OK, a block with the technological data entered is generated and inserted in front of the block to which the cursor is positioned. Pressing RECALL cancels your entry and lets you return to the Teach In basic screen.

Use this softkey to generate NC blocks using the traversing keys or the handwheel.

Simple NC blocks are generated by traversing with parallel axes using either the traversing keys of the axes or the handwheel. It is also possible to correct the values of an existing blocks.

Fig. 5-7 Teach In of NC blocks

Fast Trav.

Linear

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

Use this softkey to generate a rapid traverse block (G0).

Use this softkey to generate a linear feed block (G1).

5-53

Automatic Mode

5.6 Teach In

Circul.

Accept Insert

Accept Change

Finish Record

Progr. run

Teach In Off

Use this softkey to generate a circular block (G5 with intermediate point and end point).

Use this softkey to generate a block with the values taught. The new block is inserted in front of the block to which the cursor is positioned.

Values are corrected in the block (accepted from the screen form) to which the cursor is positioned.

Use RECALL to return to the Teach In basic screen. Any amendments you wish to make can be later inserted manually.

Use this softkey to generate an M2 block to be inserted after the current block (cursor position)

Use this softkey to traverse the programmed block.

The machine screen set in Automatic mode appears again. Use NC Start to continue the selected but interrupted program from the block selected last (if the control system has not been in Reset state). Teach In remains enabled. Block search with NCK is not possible.

Use this softkey to turn off the submode Teach In.

Note

After turning off Teach In, the interrupted program can no longer be edited.

Example

Teaching a G5 block

Fig. 5-8 Teach In of a circular block

S The program block with G5 is selected by the cursor . S Press the softkey Circul.

The circle start point is the end point of the previous block.

S Approach to the intermediate point of the contour and press Accept Change. S Approach to the end point of the contour and press Accept Change.

5-54

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Part Programming

Functionality

This Section describes how to create a new part program. The standard cycles can also be displayed provided you have the required access authoriza-

tion.

Operating sequence

You are in the main menu.

Programs

Softkeys

Cycles

The Programming main screen appears.

Fig. 6-1 Programming main screen

When the Program operating area is selected for the first time, the directory for part programs and subroutines is automatically selected (see above).

The Standard Cycles directory is displayed by pressing the Cycles softkey.

This softkey is only displayed if the operator has the appropriate access authorization.

Select

Open

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

This function selects the program highlighted by the cursor for execution. The program is started on next NC START.

Opens the files selected by the cursor for editing.

Menu extension

6-55

Part Programming

New

Copy

Delete

Rename

Memory Info

Use the New softkey to create a new program. A window appears in which you are prompted to enter program name and type.

After you have confirmed your inputs by OK, the program editor is called, and you can enter part program blocks. Select RECALL to cancel this function.

Use the Copy softkey to copy the selected program into another program.

The program highlighted by the cursor is deleted after the system has requested confirmation of the delete operation.

Press OK to confirm the Delete request and RECALL to cancel it.

When you select the Rename softkey, a window appears in which you can rename the program that you have already highlighted by the cursor.

After you have entered the new name, confirm your rename request by OK or cancel by RE- CALL.

The Programs softkey can be used to change to the program directory.

When you press this softkey, the totally available NC memory (in kbytes) is displayed.

6-56

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Part Programming

6.1 Entering a new program - “Program” operating area

Functionality

This Section describes how to create a new file for a part program. A window appears in which you are prompted to enter program name and type.

DEMO.MPF

Fig. 6-2 New Program input screenform

Operating sequence

Program

New

...

You have selected the Program operating area. The Program Overview window showing the programs already stored in the CNC is displayed on the screen.

Press the New softkey. A dialog window appears in which you enter the new main program or subroutine program name. The extension .MPF for main programs is automatically entered. The extension .SPF for subroutines must be entered with the program name.

Enter the new name.

Complete your input by selecting the OK softkey. The new part program file is generated and is now ready for editing.

The creation of the program can be interrupted by RECALL; the window is then closed.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

6-57

Part Programming

6.2 Editing part programs - “Program” operating area

Functionality

Part programs or sections of a part program can only be edited if not being executed. All modifications to the part program are stored immediately.

Fig. 6-3 Editor window

Operating sequence

Programs

Open

You are in the main menu and have selected the Program operating area. The program overview appears automatically.

Use the paging keys to select the program you wish to edit.

Pressing the Open softkey calls the editor for the selected program and pulss down the editor window.

The file can now be edited. All changes are stored immediately.

Select

Pressing the Select softkey selects the edited program for execution. This program is started with next NC–Start.

Softkeys

User–assignable softkeys

You can assign predefined functions to the softkeys 1 – 4 (see Section 6.3.4 “User–Assignable Softkeys”).

Contour

6-58

The softkeys are assigned process–specific functions by the control manufacturer.

The contour functions are described in Section 6.3 ”Programming Support”.

Menu extension

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Edit

Part Programming

6.2 Editing part programs - “Program” operating area

Mark

Delete

Copy

Past

Recomp. cycles

This function selects a section of text up to the current cursor position.

This function deletes the selected text.

This function copies the selected text to the clipboard.

This function inserts a text from the clipboard at the current cursor poisition.

For re–compilation, the cursor must stand on the cycle call line of the program. The required parameters must be arranged directly in front of the cycle call and may not be separated by instruction or comment lines. The function decodes the cycle name and prepares the screenform with the appropriate parameters. If there are any parameters outside the range of validity, the function automatically enters standard values. After the screenform has been quitted, the original parameter block is replaced by the corrected one.

Note Only automatically generated blocks can be recompiled.

Note

To carry out these functions outside the Edit menu, it is also possible to use the key combinations <SHIFT> and

softkey 1 Mark softkey 2 Delete block softkey 3 Copy block softkey 4 Insert block.

Assign SK

Text

Line no.

Contin. Search

Menu extension

This function can be used to change the assignment of the softkey functions 1 – 4. For more detail description refer to Section 6.3.4.

The softkeys Search and Contin. search can be used to search for a string chain in the program file displayed on the screen.

Type the text you wish to find in the input line and start the Search operation by selecting the OK softkey. If the character string you have specified cannot be found in the program file, an error message appears that must be acknowledged with OK. You can exit the dialog box without starting the search by selecting RECALL.

Type the line number in the input line.

The search is started by pressing OK. You can quit the dialog box without starting the search by selecting RECALL.

The functions searches through the file to find another character string that matches the target string.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

6-59

Part Programming

6.2 Editing part programs - “Program” operating area

This function stores the changes in the file system and automatically closes the file.

Editing cyrillic letters

This function is only avaiable if the Russiona language option is selected.

Procedure

The control system offers a window for cyrillic letters to choose from. This is enabled/disabled using the Toggle key.

Fig. 6-4

To select a character,

S use the letters X, Y or Z to choose the line S and then enter the digit or the letter assigned to the corresponding column.

When you enter the digit, the character will be copied into the edited file.

6-60

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

6.3 Programming support

Functionality

The programming support facility contains various help levels simplifying the programming of part programs without constraining your choice of inputs.

6.3.1 Vertical menu

Functionality

The vertical menu is displayed in the program editor . The vertical menu allows you to quickly insert certain NC instructions into the part program.

Operating sequence

Part Programming

6.3 Programming support

You are in the program editor.

Press the VM key and select the desired instruction from the list.

Fig. 6-5 Vertical menu

Lines that end in “...” contain a collection of NC instructions. You can list these instructions by pressing the Input key or entering the number of the line.

Fig. 6-6 Vertical menu

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

6-61

Part Programming

6.3 Programming support

Use the paging keys to browse through the list.

Confirm your entry by pressing Input.

Alternatively, the number of the lines from 1 to 7 can be entered to select instructions and take them over into the part program.

6.3.2 Cycles

Functionality

You can either specify your own machining cycles on assigning parameters or, alternatively, use input forms in which you set all the necessary R parameters.

Operating sequences

LCYC 60

LCYC 61

The screenforms are selected either with the available softkey functions or by means of the vertical menu.

Fig. 6-7

The cycle support provides a screenform in which you can fill in all the necessary R parameters. A graphic and a context–sensitive help will assist you to fill in the form.

Select the OK softkey to transfer the generated cycle call to the part program.

6-62

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

6.3.3 Contour

Functionality

To create part programs quickly and reliably, the control system offers various contour screenforms. To use them, enter the appropriate parameters in the interactive screenforms.

The following contour elements and contour sections can be programmed using the contour screenforms:

S Straight section with specification of end point or angle S Circle sector with specification of center point / end point / radius S Contour sector ’straight line – straight line’ with specification of angle and end point S Contour section ’straight line – circle’ with tangential transition; calculated from angle, ra-

dius and end point

S Contour section ’straight line – circle’ with any transition; calculated from angle, radius and

end point

Part Programming

6.3 Programming support

S Contour section ’circle – straight line’ with tangential transition; calculated from angle, ra-

dius and end point

S Contour section ’circle – straight line’ with any transition; calculated from angle, radius and

end point

S Contour section ’circle – circle’ with tangential transition; calculated from angle, radius and

end point

S Contour section ’circle – circle’ with any transition; calculated from center point, radius and

end point

S Contour section ’circle – circle’ with any transition; calculated from center points and end

point

S Contour section ’circle – straight line’ with tangential transitions S Contour section ’circle – circle – circle’ with tangential transitions S Contour section ’straight line – circle – straight line’ with tangential transitions

Fig. 6-8

Softkeys

The sofkey functions branch into the contour elements.

Programming aid for programming straight line sections.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

6-63

Part Programming

6.3 Programming support

Fig. 6-9

Enter the end point of the straight line.

G0/G1

G17/18/19

The block is traversed either at rapid traverse or with the programmed feedrate.

The end point can be entered either in the absolute dimension, as an incremental dimension (referred to the starting point) or in polar coordinates. The current setting is displayed in the interactive dialog screenform.

The end point can also be specified by a coordinate and the angle between the 1st axis and the straight line.

If the end point is determined using polar coordinates, the length of the vector between pole and end point is required, as well as the angle of the vector with reference to the pole. When using the possibility, first a pole must be set.

Pressing this softkey selects the plane G17 (X–Y), G18 (Z–X) or G19 (Y–Z)

6-64

Fig. 6-10 Type the values in the input fields and close the screenform with OK.

Pressing the OK softkey takes over the block into the part program and displays the Additional Functions form in which you can extend the block by adding more instructions.

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Additional functions

Fig. 6-11 Additional Functions screenform

Enter additional commands in the fields. The commands can be separated by means of blanks, commas or semi–colons.

This screenform is available for all contour elements.

Part Programming

6.3 Programming support

G2/G3

The OK softkey transfers the commands to the part program.

Select RECALL if you wish to exit the interactive form without saving the values.

The dialog screenform is used to create a circular block by means of the end and center point coordinates.

Fig. 6-12

This softkey changes the direction of rotation from G2 to G3. G3 appears on the display. When you press the softkey again, you will return to G2.

G17/18/19

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

Use this softkey to select the plane G17 (X–Y), G18 (Z–X) or G19 (Y–Z).

Pressing the OK softkey takes over the block into the part program and displays the Additional Functions form in which you can extend the block by adding more instructions.

6-65

Part Programming

6.3 Programming support

This function is intended to calculate the intersection point between two straight lines.

Specify the coordinates of the end point of the second straight line and the angles of the straight line. For the coordinate value, the toggle key can be used to choose between absolute, incremental or polar coorinates.

If the starting point cannot be selected based on the previous blocks, the operator must set the starting point.

Fig. 6-13 Calculating the intersection point between two straight lines

Table 6-1 Input in the interactive screenform

End point of straight line 2

Angle of straight line 1 A1 The angle must be specified in the CCW direction in the range

Angle of straight line 2 A2 The angle must be specified in the CCW direction in the range

Feedrate F Feedrate Plane X–Y, Z–X, Y–Z

This function is used to calculate the tangential transition between a straight line and a circle sector. The straight line must be described by starting point and anle. The circle must be described by the radius and by the end point.

E Specify the end point of the straight line depending on the selec-

ted plane (G17/18/19).

between 0 and 360 degrees.

6-66

Fig. 6-14 Straight line – circle with tangential transition

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Table 6-2 Input in the interactive screenform

Part Programming

6.3 Programming support

G2/G3

G17/18/19

POI

Circle end point

Straight line angle A The angle is specified in the CCW direction in the range between

Circle radius R Input field for the circle radius Feed F Input field for the interpolation feed. Circle center point M If there is no tangential transition between the straight line and the

This softkey is used to switch the direction of rotation from G2 to G3. G3 is displayed on the screen. Pressing this softkey once more will switch the display back to G2.

E The end point of the circle must be specified depending on the

selected plane.

0 and 360 degrees.

circle, the circle center must be known. The circle center point is specified depending on the calculation method (absolute or incremental dimension / polar coordinates) selected in the previous block.

Both the center and the end points can be acquired either in the absolute dimensions, in the incremental dimensions or as polar coordinates. The current setting is displayed in the interactive screenform.

Selection of the plane G17 (X–Y), G18 (Z–X) or G19 (Y–Z)

You can choose between tangential or any transition.

If the starting point cannot be determined from the previous blocks, the starting point must be set by the operator.

The screenform will generate a straight line and a circle block from the entered data. If there are several intersection points, the desired intersection point must be selected by the

operator in an interactive screenform.

This function is used to calculate the tangential transition between a circle sector and a straight line. 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. 6-15 Tangential transition

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

6-67

Part Programming

6.3 Programming support

Table 6-3 Input in the interactive screenform

G2/G3

G17/18/19

POI

Straight line end point

Center point M The center point of the circle must be entered either in absolute,

Circle radius R Input field for the circle radius Angle of straight line 1 A The angle is specified in the CCW direction in the range between

Feedrate F Input field for the interpolation feedrate

This softkey is used to switch the direction of rotation from G2 to G3. G3 is displayed on the screen. Pressing this softkey once more will switch back to G2; the display will change to G2.

The center point can be acquired either in absolute dimensions, incremental dimensions or polar coordinates. The current setting is displayed in the interactive screenform.

Selection of the plane G17 (X–Y), G18 (Z–X) or G19 (Y–Z)

Use this softkey to choose between tangential or any transition.

E Enter the end point of the straight line depending on the selected

plane (G17/18/19).

incremental or polar coordinates.

0 and 360 degrees.

If the starting point cannot be generated from the previous blocks, the starting point must be set by the operator.

The screenform will generate both a straight line and a circle block based on the entered data. If there are several intersection points, the desired intersection point must be selected by the

operator from a dialog box.

This function is used to caluclate the tangential transition between two circle sectors. Circle sector 1 must be described by the parameters starting point and center point, and circle sector 2 must be described by the parameters end point and radius.

To avoid an overdetermination, input fields not needed are hidden.

Fig. 6-16 Tangential transition

6-68

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Table 6-4 Input in the interactive screenform

Part Programming

6.3 Programming support

G2/G3

G17/18/19

POI

End point of circle 2

E 1st and 2nd geomtery axes of the plane Center point of circle 1 M1 1st and 2nd geometry axes of the plane Radius of circle 1 R1 Input field for the circle radius Center point of circle 2 M2 1st and 2nd geometry axes of the plane Radius of circle 2 R2 Input field for the circle radius Feedrate F Input field for the interpolation feedrate

This softkey is used to switch the direction of rotation from G2 to G3. G3 is displayed on the screen. Pressing this softkey once more will switch back to G2; the display will change to G2.

The center point can be acquired either in absolute dimensions, incremental dimensions or polar coordinates. The current setting is displayed in the interactive screenform.

Selection of the plane G17 (X–Y), G18 (Z–X) or G19 (Y–Z)

Use this softkey to choose between tangential or any transition.

If the starting point cannot be generated from the previous blocks, the starting point must be set by the operator.

The screenform will generate two circle blocks based on the entered data.

Selecting the intersection point

POI 1

POI 2

If there are several intersection points, the desired intersection point must be selected by the operator from a dialog box.

The contour is drawn using intersection point 1.

Fig. 6-17 selection of intersection point 1

The contour is drawn using intersection point 2.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

6-69

Part Programming

6.3 Programming support

Fig. 6-18 Selection of intersection point 2

Pressing this softkey will accept the intersection point of the displayed contour into the part program.

This function is used to insert a straight line tangentially between two circle sectors. The sectors are determined by their center points and their radii. Depending on the selected direction of rotation, different tangential intersection points result.

Use the screenform, which will appear, to enter the parameters center point and radius for sector 1, as well as the parameters end point, center point and radius for sector 2. in addition, the direction of rotation must be selected for the circles. The current setting is displayed in a help screen. The end and center points can be acquired either as absolute, incremental or polar coordinates.

The OK function will calculate three blocks from the given values and will insert them into the part program.

6-70

Fig. 6-19 Screenform for calculating the contour section ’circle – straight line – circle’

Table 6-5 Input in the interactive screenform

End point E 1st and 2nd geometry axes of the plane

If no coordinates are entered, the function will provide the inter-

section point between the inserted circle sector and sector 2.

Center point of circle 1 M1 1st and 2nd geometry axes Radius of circle 1 R1 Input field for radius 1 Center point of circle 2 M2 1st and 2nd geometry axes of the plane

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Part Programming

6.3 Programming support

Table 6-5 Input in the interactive screenform, Fortsetzung

Radius of circle 2 R2 Input field for radius 2 Feedrate F Input field for the interpolation feedrate

If the starting point cannot be determined based on the previous blocks, the appropriate coordinates must be entered in the “Starting point” screenform.

The screenform will generate both a straight line and two circle blocks based on the entered data.

G2/G3

G17/18/19

Example

Use this softkey to define the direction of rotation of the two circle sectors. You can choose between

Sector 1 G2 G3, G3 G2, G2 G2 and G3 G3

The end point and the center points can be acquired either in absolute, incremental or polar coordinates. The current setting is displayed in the intractive screenform.

Selection of the plane G17 (X–Y), G18 (Z–X) or G19 (Y–Z)

Sector 2

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

6-71

Part Programming

6.3 Programming support

Given: R1 18 mm

Starting point: The point X = 2 and Y = 30 mm is supposed as the starting point.

Fig. 6-20 Setting the starting point

After the starting point has been confirmed, the screenform can be used to calculate the

R2 15 mm R3 15 mm M1 X 20 Y 30 M2 X 50 Y 75 M3 X 75 Y 20

contour section – – . Use softkey 1 to set the direction of rotation of the two circle sectors and to fil out the parame-

ter list. The end point can be left open or the points X 50 Y 90 ( 75 + R 15) must be entered.

Fig. 6-21 Calling the screenform

6-72

Fig. 6-22 Result of step 1

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Part Programming

6.3 Programming support

After you have filled out the screenform, press OK to quit the screenform. The intersection points are caluclated and the two blocks are generated.

Since the end point has been left open, the intersection point between the straight line and the circle sector is also the starting point for the subsequent contour definition.

Now, call the screenform for calculating the contour section – again.

Fig. 6-23 Calling the screenform

Fig. 6-24 Result of step 2

The end point of step 2 is the intersection point of the straight line with the circle sector

. Then, calculate the contour section starting point 2 – circle sector .

Fig. 6-25 Calling the screenform

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

6-73

Part Programming

6.3 Programming support

Fig. 6-26 Result of step 3

Then, link the new end point with the starting point. To do so, use the function.

Fig. 6-27 Step 4

Fig. 6-28 Result of step 4

6-74

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Part Programming

6.3 Programming support

This function is used to insert a circle sector tangentially between two adjacent circle sectors. The circle sectors are described by their center points and their circle radii. The inserted sector is described by its radius.

Use the screenform to enter the parameters center point and radius for circle sector 1, and the parameters end point, center point and radius for circle sector 2. in addition, the radius for the inserted circle sector 3 must be entered and the direction of rotation be defined.

The end point and the center points can be acquired either as absolute, incremental or polar coordinates.

The selected setting is displayed in a help screen. The OK function will caluclate three blocks from the given values and will insert them into the

part program.

Fig. 6-29 Screenform for calculating the contour section ’circle – circle – circle

Table 6-6 Input in the dialog screenform

End point

Center point of 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 2 R2 Input field for radius 2 Radius of circle 3 R3 Input field for radius 3 Feed F Input field for the interpolation feed

E 1st and 2nd geometry axes of the plane

If no coordinates are entered, the function provides the intersection point between the inserted circle sector and sector 2.

If the starting point cannot be deteremined from the previous blocks, the respective coordinates must be entered in the “Starting point” screenform.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

6-75

Part Programming

6.3 Programming support

G2/G3

G17/18/19

Example

This softkey defines the direction of rotation of the three circles. It is possible to select between:

Sector 1 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

Selection of the plane G17 (X–Y), G18 (Z–X) or G19 (Y–Z)

Inserted Sector Sector 2

6-76

Fig. 6-30 Example

Given: R1 88 mm

R2 25 mm R3 14 mm M1 X 50 Y 0 M2 X 50 Y 50

The coordinates X 50, Y 75 (50 + R2) will be selected as the starting point.

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Part Programming

6.3 Programming support

After you have confirmed the starting point, use the screenform to calculate the contour section

(circle sector R2 – circle sector R1). The coordinates X50, Y 88 (R1) constitue the

end point for this contour section .

Fig. 6-31 Setting the starting point

Fig. 6-32 Calling the screenform ’circle – circle – circle’

Fig. 6-33 Result of step 1

In the second step, screenform is used to calculate the contour section (circle sector R1 – circle sector R2). For calculation, select direction of rotation G2 – G2 – G3. Since the end point of step 1 is at the same time the starting point for step 2, no new starting point needs to be set. For step 2, the coordinates X 50 Y 75 (50 + R2) constitute the end point. The contour is thus closed.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

6-77

Part Programming

6.3 Programming support

Fig. 6-34 Calling the screenform ’circle – circle – circle’

Fig. 6-35 Result of step 2

This function is used to insert a circle sector (with tangential transitions) between two straight lines. The circle sector is described by the center point and the radius. The coordinates of the end point of the second straight line and, optionally, angle A2. The first straight line is described by the starting point and the angle A1.

If the starting point cannot be determined from the previous blocks, the starting point must be set by the operator.

Fig. 6-36 Straight line – circle – ctraight line

6-78

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Table 6-7 Input in the interactive screenform

Part Programming

6.3 Programming support

End point of straight line 2

Circle center point M 1st and 2nd axes of the plane Angle of straight line 1 A1 The angle must be specified in the CCW direction. Angle of straight line 2 A2 The angle must be specified in the CCW 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 in absolute, incremental or polar coordinates. The screenform will generate a circle and two straight line blocks from the entered data.

G2/G3

G17/18/19

Use this softkey to switch the direction of rotation from G2 to G3. G3 is displayed on the screen. Pressing this softkey once more will switch back to G2; the display will change to G2.

Selection of the plane G17 (X–Y), G18 (Z–X) or G19 (Y–Z)

6.3.4 Free softkey assignment

Assign SK

You can assign the softkeys various cycles or contours. To this aim, the softkeys 1 to 4 in the softkey bar in the Program operating area are provided.

Once you have activated the Assign softkeys function, a list of all available cycles or contours appears on the screen.

Fig. 6-37

Position the cursor on the element you wish to assign.

Press the desired softkey from 1 to 4 to assign them the desired element. The assignment you have made appears in the softkey bar under the selection list.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

Confirm the assignment you have made by selecting the OK softkey.

6-79

Part Programming

6.3 Programming support

6-80

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Services and Diagnosis

7.1 Data transfer via the V24 Interface

Functionality

You can use the V.24 (RS 232) interface of the CNC to output data (e.g. part programs) to an external data storage medium or to read in them from there. The V.24 interface and the data storage device must be matched to one another. The control system provides an interactive screenform in which you can set the special data for your storage medium.

After you have selected the Services operating area, a list of all available part programs and subroutines appears on the screen.

Fig. 7-1 Services main screen

File types

Provided the access authorization is set, files can be read in or read out via the V24 interface. If the access authorization is set (cf. Technical Manual), the following data can be transmitted:

S Data

– Option data – Machine data – Setting data – Tool offsets – Zero offsets – R parameters

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

7-81

Services and Diagnosis

7.1 Data transfer via the V24 Interface

S Part programs

– Part programs – Subroutines

S Start–up data

– NCK data – PLC data – Alarm texts

S Compensation data

– Leadscrew pitch/encoder errors

S Cycles

– Standard cycles

Operating sequence

Use the Service softkey to select the Services operating area.

Service

Softkeys

Data In Start

DataOut Start

RS232 setting

This key starts reading in data.

This key starts reading out data to the PG/PC or another device.

With the access authorization set, this function can be used to modify the interface parameters and to save them.

Fig. 7-2 Interface settings

7-82

Position the cursor on the desired data. Use the selection key to modify the settings in the left column. The special functions can be

activated and deactivated by the Select key.

Activating the transmission log

These softkeys are intended to adapt the V.24 interface to the transmission log. 2 logs are set by default.

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Services and Diagnosis

7.1 Data transfer via the V24 Interface

RS232 text

RS232 binary

Error log

Use this softkey to produce a log for the transfer of data, part programs and cycles.

Use this softkey to produce a log for the transfer of start–up data. The baud rate can be adapted according to the receiver.

Press this softkey to save your settings.

Select RECALL to exit the window without saving your settings.

A log is output for the transferred data.

S For files to be output, it contains

- the file name and

- an error acknowledgement

S For imported files, it contains

- the file name and the path specification

- an error acknowledgement

Transmission messages:

OK Transmission completed successfully ERR EOF End–of–file character received, but the archive file is not com-

plete.

Time Out Timeout monitoring is signaling an interruption in the transmis-

sion. User Abort Transmission aborted by Stop softkey Error Com Error at COM 1 NC / PLC Error NC error message Error Data Data errors

1. Files read in with/without leader

2. Files transferred in tape format without file name Error File Name The file name does not comply with NC name conventions. no access right No access right for this function

Show

individual files.

Menu extension

Display of the data that are amongst the data types marked with “...”. Use this function to transfer

Execut f. ext.

An external program is transferred to the control system via the V.24 interface and executed immediately by pressing NC Start (see Section 5.5).

Note

As an alternative, program execution from external can also be activated in the Automatic area.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

7-83

Services and Diagnosis

7.1 Data transfer via the V24 Interface

7.1.1 Interface parameters

Table 7-1 Interface parameters

Parameter Device type S XON/XOFF

Description

One possible method of controlling the transmission operation is to use the XON (DC1, DEVICE CONTROL 1) and XOFF (DEVICE CONTROL 2) control characters. As soon as the buffer of the I/O device is full, it returns XOFF, and as soon as it can receive data again, it sends XON.

S RTS/CTS

The RTS signal ( Request to Send) controls the send operation of the data transmission device. Aktive signal: Send data Passive signal: Do not exit send mode until all transferred data have been sent.

The CTS signal is the acknowledgment signal for RTS and indicates that the data transmission device is ready to send.

XON This is the character that is used to start transmission. It is effective only for device

type XON/XOFF. XOFF This is the character with which data transmission is stopped. End of trans-

mission

Baud rate Interface speed settings

Data bits Number of data bits for asynchronous transmission.

Stop bits Number of stop bits for asynchronous transmission.

Parity Parity bits are used to detect errors. These are added to the coded character in

This is the character that signals end of transmission of a text file.

The special function “Stop with end of transmission” character may not be active if

binary data are to be transferred.

300 baud

600 baud

1200 baud

2400 baud

4800 baud

9600 baud

Input:

7 data bits

8 data bits (default)

Input:

1 stop bit (default)

2 stop bits

order to obtain either an even or odd number of positions set to “1” .

Input:

No parity (default)

Even parity

Odd parity

7-84

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

7.1.2 Special functions

Table 7-2 Special functions

Services and Diagnosis

7.1 Data transfer via the V24 Interface

Function

Start with XON Transmission starts if the transmitter

receives an XON character in the data flow.

Overwrite with confirmation

End of block with CR LF

Stop at end of transmission

Evaluate DSR signal

Leader and trailer

Tape format Import of part programs Import of archives in the

Timeout monitoring

When a file is imported, a check is made for an existing file of the same name in the NC.

CR characters (hexadecimal 0D) are inserted with tape format outputs.

The end–of–transmission character is active.

Transmission is interrupted if the DSR signal is missing.

Leader is skipped when data are received. A leader with 120 * 0 h is generated when data are output.

Transmission is interrupted after 5 seconds in case of transmission problems.

Active Inactive

Transmission starts independently of any XON character.

The files are overwritten without confirmation request.

No additional characters are inserted.

The character is not evaluated.

DSR signal has no effect.

Leader and trailer are read in with other data. No leader is generated when data are output.

SINUMERIK archive format No abortion of transmission

7.1.3 Interface parameterization

Please find examples for setting the V24 interface below.

Start–up data

Settings for trtansferring archives with the start–up data

Fig. 7-3

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

7-85

Services and Diagnosis

7.1 Data transfer via the V24 Interface

Punched–tape input / output

If a punched–tape reader/puncher is connected, check the “Leader/Trailer” box. If the punched–tape reader is controlled via CTS, then check the “Stop at end of transmission”

box. Device type: RTS/CTS XON: 0 XOFF: 0 End of transm.: 0 Baud rate: 9600 baud Data bits: 8 Stop bits: 2 Parity: No parity

Start with XON Overwrite with confirmation

X Ends of block with CR LF

Stop at transmission end

X Evaluate DSR signal

Leader and trailer X Tape format X Timeout monitoring

Parameters for a serial printer

A printer with a serial interface is connected via an appropriate cable (cable check at CTS). Device type: RTS/CTS XON: 11(H) XOFF: 13(H) End of transm.: 1A(H) Baud rate: 9600 baud Data bits: 8 Stop bits: 1 Parity: No parity

Start with XON

Overwrite with confirmation X End of block with CR LF

Stop at transmission end X Evaluate DSR signal X Leader and trailer X Tape format X Timeout monitoring

7-86

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Services and Diagnosis

7.2 Diagnosis and start–up - ”Diagnostics” operating area

Functionality

In the “Diagnostics” operating area, you can call service and diagnostic functions, set start–up switches, etc.

Operating sequence

Diagnostics

Selecting the Diagnostics softkey will open the Diagnostics main screen.

Fig. 7-4 Diagnostics main screen

Softkeys for diagnostic functions

Alarms

This window displays all pending alarms line by line, starting with the alarm with the highest priority.

Alarm number, cancel criterion and error text are displayed. The error text refers to the alarm number on which the cursor is positioned.

Explanations with regard to the screenform above:

S Number

The “Number” item displays the alarm number. The alarms are displayed in chronological sequence.

S Cancel criterion

The symbol of the key required to reset the alarm is displayed for every alarm.

– Switch the device off and on again.

– Press the RESET key.

– Press the “Acknowledge alarm“ key. – Alarm is reset by NC START.

S Text The alarm text is displayed.

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

7-87

Services and Diagnosis

7.2 Diagnosis and start–up - ”Diagnostics” operating area

Service display

Service axes

Servo trace

The Service Axes window appears on the screen.

The window displays information about the axis drive.

Fig. 7-5 The “Service Axes” window

In addition, the Axis+ and Axis- softkeys are displayed. They can be used to call the values for the next or previous axis.

To optimize the drives, an oscillograph function is provided for graphical representation of the velocity setpoint. The velocity setpoint corresponds to the +10V interface.

The start of recording can be linked with various criteria which permit recording in parallel to internal conditions of the control system. The setting needed for this option must be carried out in the “Select Signal” function.

The following functions can be used to analyze the result:

S Change scaling of abscissa and ordinate, S Measure value by means of a horizontal or vertical marker, S Measure the abscissa and ordinate values as a difference between two marker positions.

Fig. 7-6 The “Servo Trace” main screen

The heading of the diagram contains the current graduation of abscissa and ordinate, the current measured positions and the difference values of the markers.

The displayed diagram can be moved within the visible screen area by means of the cursor keys.

7-88

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Services and Diagnosis

7.2 Diagnosis and start–up - ”Diagnostics” operating area

Select signal

Graduation of abscissa

Initial values

Fig. 7-7 Meaning of the fields

Use this menu to select the axis to be measured, the measuring time, threshold value, pre–trigger/ post–trigger time and trigger conditions. The signal settings are fixed.

Current marker position

Graduation of ordinate

Difference display of Markers

Fig. 7-8 Signal selection

S Selecting the axis: The axis is selected in the Axis toggle field. S Signal type:

Velocity setpoint Actual position value of measuring system 1 Following error

S Determining the measuring time: The measuring time is entered in ms directly in the

“Measuring Time” input field.

S Determining trigger time to or after

With input values < 0, recording starts by the set time prior to the trigger event, and with values > 0 accordingly after the trigger event, whereby the following conditions must be observed:

Trigger time + measuring time ≥ 0.

S Selecting the trigger condition: Position the cursor on the Trigger Condition field and

select the condition using the toggle key.

– No trigger, i.e. the measuring starts immediately after pressing the Start softkey. – Negative edge – Exact stop fine reached – Exact stop coarse reached

SINUMERIK 802S/802C 6FC5 598–3AA10–0BP2 (01.02) (OP–M)

7-89

Services and Diagnosis

7.2 Diagnosis and start–up - ”Diagnostics” operating area

S Determining the trigger threshold: The threshold is entered directly in the Threshold

input field. It acts only for the trigger conditions “Positive edge“ and “Negative edge”.

Marker

Help

This function branches to another softkey level, in which the horizontal or vertical marker can be switched on or off. The markers are displayed in the status bar.

The markers are moved in steps of one increment by means of the cursor keys. Larger step widths can be set in the input fields. The value specifies the number of raster units per <SHIFT> + cursor movement by which the marker is to be moved.

If a marker reaches the margin of the diagram, the next raster in horizontal or vertical direction is automatically pulled down.

Fig. 7-9 Setting the markers

The markers can also be used to determine the differences in the horizontal or vertical direction. To this aim, position the marker on the start point and press either the Fix H – Mark. or the Fix T– Mark. softkey. The difference between the start point and the current marker position is now displayed in the status bar. The softkey labeling changes to “Free H – Mark.” or “Free T – Mark.”.

Pressing this functions calls explanations with regard to the displayed values on the screen.

Start

Stop

Zoom

Time + Zoom Time -

Zoom

V + Zoom V -

Auto. scaling

Version

Type

Pressing the Start softkey starts recording. The softkey labeling changes to Stop. The note “Recording active” is displayed.

When the measuring time is elapsed, the softkey labeling changes to Start.

Pressing the Stop softkey aborts the current measuring. The softkey labeling changes to Start.

The scaling changes in the following steps: 1, 2, 5, 10, 20, 50, 100, 200, 500, 1,000 ms/div.

The horizontal scaling changes in the following steps:

0.01, 0.05, 0.1, 0.5, 1, 5, 10, 50, 100, 500, 1,000, 5,000 unit/ div

This function calculates the vertical scaling from the peak values.

This window contains the version numbers and the creation date of the individual CNC components.

displays the control type

7-90

6FC5 598–3AA10–0BP2 (01.02) (OP–M)

SINUMERIK 802S/802C

Fig. 7-10 Control type

Softkeys for start–up functions

Note

siemens 802S Programming Manual

Specifications and Main Features

Frequently Asked Questions

User Manual