Siemens SINUMERIK 828D Turning User manual

Manual
Mold making with 3-to 5-axis simultaneous milling
Milling with SINUMERIK
09/2018Edition
SINUMERIK
www.siemens.com/sinumerik

Milling with SINUMERIK
Mold-making with 3- to 5-axis simultaneous milling
Manual
Valid for:
Control
SINUMERIK 828D
SINUMERIK 840D sl
Edition 09.2018
Document Order No. 6FC5095-0AB10-0BP5
Basic information 1
General information on
workpiece production 2
Important functions for 3- to
5-axis machining 3
Aerospace, structural parts 4
Engine and turbine
components 5
Complex free-form surfaces 6
Difference between 3, 3+2
and 5 axes 7
Reference section 8

Introduction
Edition history, trademarks
0
© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
4
SINUMERIK® documentation
Edition history, trademarks
Brief details of this edition and previous editions are listed below.
The 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 number.
C.... Revised version with new edition status.
Trademarks
All product designations may be trademarks or product names of Siemens AG or supplier
companies whose use by third parties for their own purposes could violate the rights of the owners.
Edition Order no. Remark
09.2018 6FC5095-0AB10-0BP5 C
06.2016 6FC5095-0AB10-0BP4 C
09.2013 6FC5095-0AB10-0BP3 C
09.2011 6FC5095-0AB10-0BP2 C
05.2009 6FC5095-0AB10-0BP1 A
More information is available on the Internet at:
http://www.siemens.com/sinumerik
This document was created using a number of
layout and graphic tools.
The reproduction, transmission or use of this document or its
contents is not permitted without express written authority.
Offenders will be liable for damages. All rights, including rights
created by patent grant or registration of a utility model or
design, are reserved.
© Siemens AG 2009 - 2018. All rights reserved.
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. Nevertheless,
the information contained in this document is reviewed
regularly and any necessary changes will be included in
subsequent editions. Suggestions for improvement are
welcome.
Technical data subject to change.
Order no. 6FC5095-0AB10-0BP5 Siemens AG
0 Introduction

© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
Introduction
Content 0
5
Page
1 Basic information ................................................................................................................ 9
1.1 Introduction ................................................................................................................10
1.2 SINUMERIK MDynamics milling technology packages .............................................11
1.3 SINUMERIK Operate user interface ..........................................................................12
1.3.1 Operating and setup functions .......................................................................12
1.3.2 SINUMERIK Operate - Multitouch .................................................................13
1.4 Requirements for milling ............................................................................................16
1.5 Linear axes, rotary axes and kinematics ...................................................................17
1.5.1 Axes and programming ..................................................................................17
1.5.2 Kinematics of 5-axis machining centers .........................................................19
1.6 Surface quality, velocity, accuracy ...........................................................................20
1.7 Additional software ....................................................................................................22
1.7.1 SinuTrain ........................................................................................................22
1.7.2 VNC Viewer - remote control on an external PC ...........................................23
1.7.3 Analyze MyWorkpiece /Toolpath additional software ....................................24
2 General information on workpiece production................................................................ 25
2.1 Process chain for producing 3- to 5-axis workpieces ................................................26
2.2 CAM systems ............................................................................................................27
2.2.1 Tolerance and accuracy .................................................................................28
2.3 Program structure for milling .....................................................................................29
2.4 Programs, data transfer and editor ............................................................................33
2.4.1 Program manager ..........................................................................................33
2.4.2 External storage media - data transfer ...........................................................34
2.4.3 EES - Execution from External Storage (NC Extend) ....................................35
2.4.4 Graphic and file formats in the program manager .........................................36
2.4.5 Program editor - useful functions ...................................................................37
2.5 JOG mode, zeros, tools .............................................................................................38
2.5.1 Zero offsets ....................................................................................................38
2.5.2 Tool management ..........................................................................................39
2.5.3 Manual retraction - return ...............................................................................40
2.6 Fundamentals, measuring in JOG and AUTOMATIC ...............................................41
2.6.1 Measurement logs in JOG .............................................................................42
2.6.2 Measurement logs in AUTOMATIC ...............................................................44
2.7 Measuring workpiece/tool in JOG .............................................................................46
2.7.1 Workpiece measuring in JOG ........................................................................46
2.7.2 Workpiece measuring functions in JOG .........................................................46
2.7.3 Example for measuring a workpiece in JOG ..................................................47
2.7.4 Measure tool in JOG ......................................................................................48
0 Introduction Content

Introduction
Content
0
© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
6
Page
2.7.5 Tool reference point ....................................................................................... 48
2.7.6 Example: Measure tool in JOG ..................................................................... 50
2.8 Measure workpiece/tool in AUTOMATIC - process measuring ................................. 52
2.8.1 Measure workpiece in AUTOMATIC .............................................................. 52
2.8.2 Workpiece measuring cycles in AUTOMATIC ............................................... 52
2.8.3 Example for measuring a workpiece in AUTOMATIC .................................... 53
2.8.4 Tool measuring in AUTOMATIC - process measuring .................................. 54
2.8.5 Example for measuring tools in the AUTOMATIC mode ............................... 54
2.9 Checking and measuring machine/spindle ............................................................... 56
2.9.1 Spindle 3D angular deviation CYCLE995 ......................................................56
2.9.2 Checking/measuring the machine with the kinematics measuring
cycle CYCLE996 ........................................................................................... 57
2.9.3 CYCLE9960 measure kinematics completely ................................................ 59
2.10 Workpiece visualization ............................................................................................. 60
2.10.1 Simulation ...................................................................................................... 60
2.10.2 Quick viewer for mold-making ....................................................................... 61
2.10.3 Simultaneous recording ................................................................................. 63
2.11 Executing programs (AUTOMATIC) .......................................................................... 64
2.11.1 Display all relevant mold-making functions .................................................... 64
2.11.2 Program running time .................................................................................... 65
2.11.3 Handwheel override ....................................................................................... 66
2.11.4 Block search .................................................................................................. 67
2.12 Collision avoidance ................................................................................................... 68
3 Important functions for 3- to 5-axis machining ............................................................... 71
3.1 Introduction ...............................................................................................................72
3.2 Explanation of the terms: swivel, frames and TRAORI .............................................73
3.3 Transforming coordinate systems - Frames .............................................................. 74
3.4 Swivel - CYCLE800 .................................................................................................. 75
3.5 TRAORI 5-axis transformation .................................................................................. 81
3.5.1 Basics of simultaneous 5-axis machining ...................................................... 81
3.5.2 The TRAORI command ................................................................................. 85
3.5.3 Programming the tool orientation ...................................................................86
3.5.4 Orientation interpolation and orientation reference ........................................ 92
3.5.5 Example application involving TRAORI and frames .................................... 100
3.5.6 Useful NC commands for active TRAORI ....................................................101
3.6 High Speed Settings - CYCLE832 .......................................................................... 102
3.6.1 Parameters for CYCLE832 .......................................................................... 103
3.6.2 CYCLE832 and CUST_832 ......................................................................... 109

© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
Content
7
3.7 Advanced Surface and Top Surface .......................................................................110
3.7.1 Compressor (COMPCAD, COMPSURF) .....................................................112
3.7.2 Continuous-path mode, Look Ahead – G64, G645 ......................................113
3.7.3 Feedforward control and jerk limitation – FFWON, SOFT, ... ......................115
3.7.4 Smoothing tolerance CTOL, OTOL, ATOL ..................................................116
3.7.5 Path reference UPATH/SPATH ...................................................................116
3.7.6 Smoothing the orientation characteristic (ORISON, ORISOF) .....................117
3.7.7 Technology G groups ...................................................................................118
3.7.8 Pre-processing memory control FIFOCTRL ................................................119
3.8 Milling radius compensation 2D/3D-WRK ...............................................................120
3.8.1 3D-WRK cutter radius compensation for circumferential and face milling ........120
3.8.2 CUT3DC/CUT3DCD circumferential milling .................................................121
3.8.3 CUT3DF/CUT3DFD face milling ..................................................................122
3.8.4 Circumferential milling with limiting surfaces (CUT3DCC/CUT3DCCD) ......126
3.8.5 Overview of the tool types for the 3D compensations. .................................127
3.8.6 Explanation of the commands ......................................................................127
3.8.7 Programming example for circumferential milling ........................................129
3.9 Volumetric Compensation System (VCS) ...............................................................130
3.10 VNCK - virtual machine ...........................................................................................131
4 Aerospace, structural parts ............................................................................................ 133
4.1 Special functions for structural parts .......................................................................134
4.2 Programming example for the pocket on a structural part ......................................135
5 Engine and turbine components..................................................................................... 139
5.1 Special functions for engine and turbine components .............................................140
5.2 Example: Turbine blade ..........................................................................................141
6 Complex free-form surfaces............................................................................................ 145
6.1 Special functions for free-form surfaces ..................................................................146
6.2 Example: Milling a manta ray ..................................................................................147
7 Difference between 3, 3+2 and 5 axes ............................................................................ 151
7.1 5-axis simultaneous or 3+2-axes .............................................................................152
7.2 Example workpiece milled by 3 to 3+2 axes ...........................................................153
7.3 Example with 3 axes milled .....................................................................................155
7.4 Example with 3+1 axes milled .................................................................................156
7.5 Example with 3+2 axes milled .................................................................................157
7.6 Comparison of the three variants ............................................................................158

Content
© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
8
8 Reference section ........................................................................................................... 159
8.1 Overview of higher-order functions ......................................................................... 160
8.1.1 Motion commands ....................................................................................... 160
8.1.2 Dynamic response ....................................................................................... 162
8.1.3 5-axis functionality ....................................................................................... 164
8.2 Further information/documentation ......................................................................... 170
8.3 Index ....................................................................................................................... 172

Basic information
Content Page
1.1 Introduction 10
1.2 SINUMERIK MDynamics milling technology packages 11
1.3 SINUMERIK Operate user interface 12
1.4 Requirements for milling 16
1.5 Linear axes, rotary axes and kinematics 17
1.6 Surface quality, velocity, accuracy 20
1.7 Additional software 22

Basic information
1.1
© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
10
1.1 Introduction
With mold-making, the main objectives are to achieve perfect surface quality, precision, and
velocity without any need for remachining. Within this context, workflow is typically characterized
by the CAD-CAM-CNC process chain. From the CAD system right through to the control,
Siemens can offer an integrated solution for these requirements in the form of its SINUMERIK
products.
SINUMERIK controls have powerful, highly-developed functions which, if intelligently used,
significantly simplify the complete operation involving programming and milling, and at the same
time the production result is improved.
This manual is a compact resource aimed at experts working in machining environments who
need to get acquainted with the most important basic principles of milling. Based on this, it also
provides machine users with practical tips so that they can organize their work efficiently and
provides programmers with an insight into the functions of the control and the CAD/CAM system.
As regards the various application areas of machining, the dedicated functions that have been
specifically developed for each area are briefly introduced and considered in context.
Although, many aspects cannot be covered in depth by this manual, additional information can
be found in the appropriate SINUMERIK documentation and relevant literature, See "Further
information/documentation" on page 170.
Range of
milling
Blow mold for plastic bottles Turbine impeller

© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
Basic information 1.2
11
1.2 SINUMERIK MDynamics milling technology
packages
SINUMERIK MDynamics bundles SINUMERIK CNC hardware, intelligent CNC functions and our
unique CAD/CAM/CNC process chain in technology packages for 3-axis and 5-axis milling. The
SINUMERIK MDynamics 3/3+2 or 5-axis milling packages are available for the SINUMERIK
828D and SINUMERIK 840D sl CNC systems.
SINUMERIK 828D
SINUMERIK 840D sl
SINUMERIK 828D integrates the milling
package for 3 axes. The basic scope can be
expanded via optional functions (see also the
3-axis milling package for SINUMERIK 840D
sl)
Basic scope, 3/3+2 axes (excerpt):
Advanced Surface
User memory expansion on the user's CF
card
Additional options, 3/3+2 axes (excerpt):
Top Surface
DXF reader
EES
ShopMill machining step programming
3D simulation
For SINUMERIK 840D sl, you can choose
between two milling packages for 3-axis and
5-axis machining. The basic scope of the
packages includes all the functions needed for
the associated machining tasks and can be
expanded.
Basic scope, 3/3+2 axes (excerpt):
Advanced Surface
Spline interpolation
Transmit and peripheral surface
transformation
AUTOMATIC measuring cycles
3D simulation
Residual material identification
ShopMill machining step programming...
Additional options (excerpt):
Top Surface
DXF reader
EES
The 5-axis package additionally includes:
5-axis machining package TRAORI
3D tool radius compensation
Measure kinematics CYCLE996/9960

Basic information
1.3
© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
12
1.3 SINUMERIK Operate user interface
The new SINUMERIK Operate user interface is well laid out and easy to use. It combines the
known features of HMI Advanced, ShopMill and ShopTurn in a seamlessly integrated, innovative
user and programming interface. This allows machining step programming to be combined with
high-level language programming, resulting in rational and intuitive NC programming and
production planning.
1.3.1 Operating and setup functions
The machine setup display is clear and manageable thanks to graphical support. Complex
workpieces can be quickly and easily machined in one clamping operation. Various kinematics
can be easily set up thanks to the cycle support.
Animated elements clarify the parameters, for example during programming
Using animated elements, the SINUMERIK CNC achieves a unique level of user friendliness for
operating and programming - even for technological cycles.
Wide range of setup functions Support for many kinematics
Cycle multi-edge in the programGUIDE Animated elements - Moving image sequence

© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
Basic information 1.3
13
1.3.2 SINUMERIK Operate - Multitouch
SmartOperation permits an intelligent CNC operation in SINUMERIK Operate using current
technologies, such as multitouch and widescreen displays. The Display Manager permits you to
see a lot of information at a glance.
Multitouch operation
SINUMERIK Operate provides additional operator functions for multitouch panels.
Extended control elements via the function key block
Gesture operation (e.g. wiping, moving and zoom functions)
The selected functions can be activated directly via the function key block. These are, for
example, undo changes or restore and activate the virtual keyboard or of the calculator .
1
2
3




Basic information
1.3
© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
14
SINUMERIK Operate expansion using a sidescreen
Widescreen format panels offer the option of using the additional area for the faster display of
additional elements and operating. Using the navigation bar the so-called sidescreen is
shown and hidden .
You can display the following elements via the navigation bar:
Machine function direct selection e.g. machine, tool list, zero offsets or program.
Displaying (widgets)
Standard widgets are for example, zeros, alarms, tool service life and program run time.
Virtual keys (pages)
Activate the ABC keyboard or of the machine control panel
1
2
1
3
4
5







© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
Basic information 1.3
15
Display Manager (at least 22 inch Full HD SINUMERIK blackline plus panel)
With the Display Manager, the screen area is
divided into several display areas.
In addition to SINUMERIK Operate, widgets,
keyboards, a machine control panel and
various applications are provided in the
various areas.

Basic information
1.4
© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
16
1.4 Requirements for milling
Free-form surfaces
Mold-making
Engine and turbine
components
e.g. impellers
Structural parts
Aviation industry
Design standards in all application areas are
becoming increasingly demanding.
Expectations in terms of ergonomics, the air
drag coefficient (CW value) or simply aesthetic
appeal are creating a need for more complex
surface geometries to be achieved quicker
and with greatest precision. The design prima-
rily comes from CAD systems, the machining
programs from CAM systems.
With SINUMERIK, Siemens can provide CNC
systems that are perfectly suited to the
demands of 3- to 5-axis machining as well as
HSC (High Speed Cutting) and HPC (High
Performance Cutting) applications:
Simple to operate
User-friendly programming at the machine
Optimum performance throughout the
CAD-CAM-CNC process chain
Optimized 5-axis functions
Depending on the application, the
requirements imposed on the control will vary
and a whole range of different functions may
be demanded.
Within this context, milling can be broken
down into three broad areas:
Free-form surfaces (mold-making)
Turbine and engine components
(impellers, blisks)
Structural parts (aviation industry)
SINUMERIK can provide optimum support for
each of these areas.

© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
Basic information 1.5
17
1.5 Linear axes, rotary axes and kinematics
1.5.1 Axes and programming
Tool tip motion
Setting the tool at an
angle
Linear and rotary axes
3-axis area
The tool position is approached in space using
linear axes X, Y and Z. This enables the tool
center point to adopt any position.
With 3-axis machining, you program the three
linear axes to achieve the desired machining
operations. The contour is milled line-by-line
by moving the three linear axes.
If the tool also has to be set at an angle, you
will need rotary axes as well.
5(3+2)-axis area
The inclination of the tool (i.e. the tool
orientation) is changed using two axes of
rotation, e.g. B and C.
This is necessary, for example, if the tool
needs to be angled in relation to the
machining surface or if you want to mill a
pocket with inclined walls within the context of
circumferential milling.
Using three linear axes and two rotary axes,
theoretically any point in space can be
approached with any tool orientation. This is
the basis of 5-axis machining.
5-axis simultaneous
To accommodate machining scenarios
involving tools set at an angle or in order to
mill undercuts or geometries located
anywhere in space, the three linear axes X, Y
and Z are required along with two of the rotary
axes A, B or C. It must be possible to control
the axes simultaneously.

Basic information
1.5
© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
18
CNC programming options in the 5-axis area
Programming rotary
axes
Programming direction
vector
In addition to programming based on the direction vector and rotary axis positions, there are also
other forms of angle programming. These include, for example, Euler or RPY angles. Further
information regarding this topic can be found in Section "Programming the tool orientation" on
page 86.
For the purpose of 5-axis machining, the
orientation of the tool needs to be defined in
addition to the position setpoint of the
machining point. The position setpoint is
defined in the CNC program by means of the
coordinate axes X, Y, and Z.
The tool orientation can be specified on the
basis of the rotary axis positions. This enables
the position setpoint and tool orientation to be
defined in a unique manner.
The example below shows the tool tip in the
position (0,0,0), and the tool shank is the
diagonal of a cube (35.26° relative to the X-Y
plane).
N100 G1 X0 Y0 Z0 B=54.73561 C=45
When describing the tool orientation, it also
makes sense to specify the direction vectors
A3, B3, and C3 so that the orientation can be
programmed independently of the machine
kinematics.
The programming of the example above would
look like the following after specifying the
rotary axis positions:
N100 G1 X0 Y0 Z0 A3=1 B3=1 C3=1
C3
B3
A3

© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
Basic information 1.5
19
1.5.2 Kinematics of 5-axis machining centers
A 5-axis machine can control tool motion in five axes. These are the three linear axes (with which
you will already be familiar) and two additional rotary axes. There are different kinematic
solutions for the two rotary axes. We will present the most common of these schematically. With
SINUMERIK controls, even special kinematics can be controlled on the basis of the integrated,
kinematic transformation feature. Special cases such as hexapods, etc. will not be explored in
further detail here.
Two rotary axes in the head
Two rotary axes in the table
*: If the axis of rotation is not perpendicular to a linear axis, then this is known as a "nutated" axis.
Mixed kinematics
Fork head Head kinematics nutated *
Rotary/swiveling table Rotary/swiveling table nutated *

Basic information
1.6
© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
20
1.6 Surface quality, velocity, accuracy
Special attention must be paid to the CAD -> CAM -> (postprocessor) -> CNC process chain
when machining three-dimensional geometries, e.g. free-form surfaces. CAM systems generate
NC programs for free-form surface machining. The CAM system receives the workpiece
geometry from a CAD system. The CNC machine has to process the NC data generated and
convert it into axis movements.
In CAD systems, surfaces of higher orders
are constructed (free-form surfaces).
For example, in order to be able to mill an
entire surface - or for collision checking - the
CAM system generally converts the CAD free-
form surface into a polyhedron.
This means that the smooth design surface is
approximated by a number of individual
small planes.
This produces deviations from the original
free-form surface.
The CAM programmer overlays this
polyhedron with tool paths. From these, the
postprocessor generates NC blocks within the
specified error tolerances. These usually
comprise many short straight line elements,
G1 X Y Z.
Thus, the machining result is no longer a free-
form surface, but a polyhedron. The small
planes of the polyhedron can be visibly
mapped on the surface.
This can result in undesirable remachining.
1
1
2
2
3
1
G1
G1
G1
G1
3