osai 10 CNC Reference Manual
10 Series CNC
High Speed Machining
Reference Manual
Code: 45006842M
Rev. 02
PUBLICATION ISSUED BY:
OSAI S.p.A.
Via Torino, 14 - 10010 Barone Canavese (TO) – Italy
e-mail: sales@osai.it
Web: www.osai.it
Copyright 2001-2002 by OSAI
All rights reserved
Edition: July 2001
IMPORTANT USER INFORMATION
This document has been prepared in order to be used by OSAI. It describes the latest release of the
product.
OSAI reserves the right to modify and improve the product described by this document at any time
and without prior notice.
Actual application of this product is up to the user. In no event will OSAI be responsible or liable for
indirect or consequential damages that may result from installation or use of the equipment described
in this text.
abc
10 Series CNC High Speed Machining
UPDATES IN THIS ISSUE
PAGE TYPE OF UPDATE
INDEX updated
CHAPTER 4 new chapter containing additional programming modes
CHAPTER 5
page 2 added: the parameter “Format” to the triletteral PNT for specifying the input
type for the profile programming
UPDATE
page 12 added: the parameter “Diam” to the triletteral AXI and the value TAO in the
parameter “Type”
page 16 inserted: an extension of the machine kinematics for positioning 2 rotation
axes to the linear axes. Extension of the triletteral MAC with new values.
page 25 inserted: a paragraph dealing with the Smoothing tolerances and
parameters
CHAPTER 6 Inserted: a new chapter concerning the Path Optimizer
10 Series CNC High Speed Machining (02)
abc
Preface
10 Series CNC High Speed Machining
PREFACE
Mechanical technology has evolved to such a degree that what were once considered insuperable
limits as regards machining speeds and accelerations have now become the norm in the world of
machine tools. It is now common to hear of machines capable of transverse speeds of the order of 80
- 100 m/minute and accelerations in the order of one or more g, traverse. The field of application
typical of these machines is the high-speed milling of surfaces.
The solution normally adopted with numeric controls, that is, the machining of profiles as a sequence
of linear micro steps is no longer applicable, because the mechanics follow the continual changes in
direction, with undesirable effects on the surface finish. The programmed points are taken as
obligatory points, through which machining must pass. In addition, “G01” programming is understood
strictly as a linear interpolation between points. This means that, to obtain a sufficiently accurate
curve, the points must be programmed so close to one another that the programmed broken line is
indistinguishable from the desired curve. This type of approach is still normally used with machine
tools having a high level of inertia which has the effect mechanically smoothing the broken line.
With the introduction of particularly rigid machines together with motor drives of an acceptable size
capable of providing high torque levels (brushless motors), this solution was no longer applicable, as
all the sudden changes in direction could be recognized by the machine tool resulting, at best, in a
poor quality surface finish.
At this point, there were two possible ways of solving the problem, by modifying the motion dynamics
and the geometry of the paths. In fact, the execution of the commands has to be filtered, in order to
obtain a “smooth” output to the servo motors, and the path program design has to be modified through
the interpretation of the programmed values as a set of points to be approximated in the best possible
way.
The solution chosen by Osai led to the implementation of the new Polynomial Interpolation
Algorithms.
This manual provides all the information necessary for the use of the new feature known as High
Speed Machining. In particular, this manual refers to the HIGH SPEED INTERPOLATION option,
specific for applications in which machining involves more than 3 axes.
The HSM feature for machining processes that involve 3 axes or less, is
IMPORTANT
10 Series CNC High Speed Machining (00) 1
included as standard in the E69 System Software for all models of 10 Series
numeric controls.
To extend this feature to more than three axes (max.6), the E96 option (High
Speed Interpolation) has to be installed.
Preface
CAUTION
10 Series CNC High Speed Machining
WARNINGS
To ensure that the system is used correctly, the indications given in the manual should be followed,
paying particular attention to the paragraphs preceded by the signs: WARNING, CAUTION or
IMPORTANT.
WARNING
IMPORTANT
Indicates situations that may cause damage to the system, the equipment or
the operator.
Precedes information to be borne in mind to avoid damage to the equipment in
general.
Precedes operations that must be performed with care to ensure the complete
success of the application.
2 10 Series CNC High Speed Machining (00)
END OF PREFACE
Chapter 1
Title of Chapter
CNC Serie 10 Titolo Manuale (00) 3
INDEX
HIGH SPEED MACHINING
Indice
10 Series CNC High Speed Machining
GENERAL CONSIDERATIONS..................................................................................1-1
PROGRAMMING POINTS AND CHARACTERISTICS OF THE PROFILE......................1-3
Considerations on the use of the G62,G63,G66 and G67 functions
(transition codes).............................................................................................1-6
GENERAL HIGH SPEED MACHINING PROGRAMMING STRUCTURE .........................1-7
Interaction with Machine Logic ..........................................................................1-7
POINT DEFINING CONVENTIONS
POINTS AND MACHINING COORDINATES ...............................................................2-1
Tool Direction ..................................................................................................2-2
Normal to the Surface Direction ........................................................................2-2
Tool Radius Application Direction ......................................................................2-3
Tangential Axis ...............................................................................................2-3
FEATURES PROVIDED BY HIGH SPEED MACHINING
MACHINES WITH 5 AXES ........................................................................................3-1
Tool Radius and Length Compensation ..............................................................3-2
Tool Length Compensation...............................................................................3-2
No Tool Compensation .....................................................................................3-3
Tangential Axis Management ............................................................................3-3
MACHINES WITH 3 AXES ........................................................................................3-4
Tool Radius and Length Compensation ..............................................................3-4
Tool Length Compensation...............................................................................3-5
No Tool Compensation .....................................................................................3-5
Tangential Axis Management ............................................................................3-6
ADDITIONAL PROGRAMMING MODES
POLYNOMIAL PROGRAMMING ...............................................................................4-1
POLYNOMIAL PROGRAMMING TYPES AND LIMITS................................................4-3
10 Series CNC High Speed Machining (02) i
Contents
10 Series CNC High Speed Machining
Polynomial for the Cutter Contact......................................................................4-3
Polynomials for the Cutter Location ...................................................................4-4
Polynomials for the Axis Location.....................................................................4-5
B-SPLINES PROGRAMMING....................................................................................4-6
B-SPLINE PROGRAMMING TYPES AND LIMITS.......................................................4-7
B-Splines for Cutter Contact.............................................................................4-7
B-Splines for Cutter Location............................................................................4-7
B-Splines for Axis Location ..............................................................................4-7
SETUP
TYPE OF POINTS DESCRIBED IN THE PART PROGRAM ..........................................5-2
VERSOR MANAGEMENT METHODS .........................................................................5-3
LOOK AHEAD MANAGEMENT ..................................................................................5-4
THRESHOLDS .........................................................................................................5-6
TOOL DEFINITION ...................................................................................................5-7
TOOL DIRECTION (3D).............................................................................................5-8
CHANGE IN CURVATURE MANAGEMENT.................................................................5-9
EDGE MANAGEMENT ..............................................................................................5-10
AXIS DEFINITION....................................................................................................5-11
AXIS PARAMETERS ................................................................................................5-13
AXIS DYNAMICS .....................................................................................................5-14
MACHINE KINEMATICS ...........................................................................................5-15
Definition of the Kinematic Chain.......................................................................5-15
Description of the Kinematic Chain....................................................................5-20
SMOOTHING TOLERANCES AND PARAMETERS .....................................................5-25
SPECIAL SMOOTHING PARAMETERS.....................................................................5-27
PATH OPTIMIZER
GENERAL................................................................................................................6-1
PROGRAM INSTALLATION ON A PC .......................................................................6-2
EXECUTION MODES................................................................................................6-3
USAGE MODES .......................................................................................................6-4
Tolerances: Toll, TollX and TollV........................................................................6-4
Buffer management: Pnt ...................................................................................6-4
Edge management: Racc, C0, RaccX, C0X, RaccV, C0V....................................6-5
POINT TYPES ..........................................................................................................6-6
ISO Part program for a 3-axes machine.............................................................6-6
ISO Part program for a 5-axes machine.............................................................6-6
END OF INDEX
ii 10 Series CNC High Speed Machining (02
Chapter
1
HIGH SPEED MACHINING
GENERAL CONSIDERATIONS
The High Speed Machining feature is used for machining surfaces (profiles) defined by points, created
by CAD/CAM systems, on machine tools having 3 to 5 axes (3 linear + 2 rotary).
The High Speed Machining feature must be enabled in the AMP environment, by selecting the
appropriate field in the PROCESS CONFIG section (PROC CHAR softkey).
WARNING
To program this feature, proceed as follows:
1. Create a setup file (part program) that contains all the parameters for handling the profile: tools,
axes and kinematics of the machine.
The setup file (whose structure is described in chapter 5) will be recalled in the main program by
means of a three-letter command with the following format:
(HSM, setup file name)
2. Create the profile by inserting it directly in the main program:
Example:
; HSM PROGRAMMING EXAMPLE
G1 X..Y..Z.. A.. B.. F…
------
(HSM, CONFIG1)
G61
G1 X..Y..Z..A..B..
-----G60
; END OF PROGRAM
This feature may only be enabled for the first 4 processes.
10 Series CNC High Speed Machining (00) 1-1
Chapter 1
High Speed Machining
The profile may also be inserted in a specific file which will be recalled as a subprogram by the
CLS instruction.
Example 2:
; HSM PROGRAMMING EXAMPLE
G0 X..Y..Z.. A.. B.. F…
------
(HSM, CONFIG1)
------
(CLS,PROFILO1--------------------------------------------------à G61
------ G1 X…Y..Z..A..B..
------ ------------------------------
; END OF PROGRAM ------------------------------
------ G60
1-2 10 Series CNC High Speed Machining (00)
Chapter 1
High Speed Machining
PROGRAMMING POINTS AND CHARACTERISTICS OF THE PROFILE
A profile is a set of points that make up the ISO part-program of the surface to be machined, created
by the CAD/CAM system in which the characteristics described in this chapter are to be respected.
On the basis of the programmed points a polynomial curve will be constructed, defining the path to be
followed. This path will pass through the programmed points with a configurable tolerance. The
methods by which the points are to be linked will be defined by the G01 and G00 codes that may be
programmed together with the points.
IMPORTANT
The sections executed in G00 will be considered as individual positioning operations; each point will
be linked to the next by means of a “linear” movement to be performed with the dynamic traverse
positioning (each section in G00 will start at zero speed and end at zero speed). For this reason, G00
mode will not calculate the polynomial curve. At the end of a section in G00 there will be no pause
(end of movement synchronism, entry into tolerance status, etc..) and the next movement will be
carried out immediately. This behaviour is similar to the programming of G01 and G09 codes in the
same block.
To ensure that the polynomial curves are calculated correctly, we recommend
the points be programmed with at least 5 figures after the decimal point (e.g.
10.37854); programming with fewer figures may cause irregularities on the
profile.
p3
p1
p2
p4
p0
With G01, each point will be linked geometrically to the following ones by means of a polynomial
curve, so the generated path may be considered “continuous”. This link will be interrupted by the
programming of a G00 or the programming of special G codes described below. The dynamics of the
sections in G01 are the same as the “cutting” movements (such as normal G01 movements in ISO
programming).
p3
p1
p2
p4
p0
10 Series CNC High Speed Machining (00) 1-3
Chapter 1
G62
High Speed Machining
In addition to the G01 and G00 functions, the following G functions, specific for the HSM feature, may
be programmed in the profile.
G61
Determines the start of the profile and must be programmed in a block on its own. When the G61
function is activated, there must be no form of virtualization active (UPR,UVP,UVC,TCP).
Before activating the G61 function, the setup file must be defined by means of the instruction:
(HSM, setup file name)
The G61 command may ONLY be executed within a part program in AUTO or BLK BY BLK status.
G60
Determines the end of the profile and must be programmed in a block on its own.
If the machine is in single STEP execution, the profile between G61 and G60 is considered as a
single instruction. To stop its execution, it is necessary to switch to HOLD status.
G62
Splits a profile in two parts and determines the point where one profile ends and another begins,
maintaining continuity between the two curves.
The points preceding the G62 function will be used to generate a first curve, while the subsequent
points will be used to generate another one. These curves will be linked and will therefore be
continuous; the initial inclination of the second curve will correspond to the final inclination of the
previous curve.
G62
p1
p2
p3
p4
p0
As regards dynamics, with G62 no deceleration and acceleration ramp will be generated to link the
two curves. This G function must be programmed in a part program block on its own.
1-4 10 Series CNC High Speed Machining (00)
Chapter 1
t
High Speed Machining
G63
Splits a profile into two parts and determines the point where one profile ends and the other one
begins, maintaining continuity between the two curves. The points preceding the G63 function will
be used to generate a first curve, while the subsequent points will be used to generate another one.
While with G62, the initial inclination of the second curve depends strictly on the final inclination of
the first, with G63, the initial inclination of the second curve IS NOT influenced by that of the first. To
maintain continuity, a “radius” that depends on the chordal error with which the splines are to be
calculated is inserted.
With G63 a reduction in speed may occur at the point where the two curves are linked. This G
function must be programmed in a part program block on its own.
G66
Splits a profile into two parts and determines the point where one profile ends and the other one
begins, creating a discontinuity between the two curves, that is, the point preceding the G66
represents an edge. At this point, two curves are generated, the first using the points preceding the
G66 function and the second using the subsequent points. These curves will NOT be linked, and so
there will be a discontinuity.
G66
p3
p1
p4
p2
p0
This discontinuity will be reached at zero speed; the first curve will therefore end with a deceleration
ramp to 0 (zero) speed after which the second curve will be tackled with an acceleration ramp to
reach the required machining speed. This G function must be programmed in a part program block on
its own.
v
G66
10 Series CNC High Speed Machining (00) 1-5
Chapter 1
High Speed Machining
G67
With G67, a “discontinuity” may be defined on the profile defined with G66. What changes is the
dynamic approach to the edge, that is, the end of the curve is not reached at zero speed but at a
speed value (vs) that enables the axes to reach the edge without any dynamic problems. This speed
value is calculated on the basis of the acceleration that may be withstood by each axis. This G
function must be programmed in a part program block on its own.
v
G67
vs
Considerations on the use of the G62,G63,G66 and G67 functions (transition
codes)
The transition G codes are particularly useful when “similar”, repetitive curves are to be defined
(providing the programmed points are also similar and repetitive).
Supposing we have a profile defined by 100 points of which the first 50 represent the first machining
pass (from p1 to p50) and the other 50 (from p50 to p99) the same profile shifted slightly (second
pass).
p1
p50
As the points between p1 and p50 are “similar” to the points between p50 and p99, the conditions for
calculating the two polynomial curves will also be similar. Two “parallel”, almost identical curves will
therefore be generated.
If the G62 function has not been programmed on point p50 the NC may generate curves that are not
perfectly parallel. This normally undesired effect is due to the fact that the calculation of the
polynomial takes into account the “history” along the calculated paths.
The “history” of point p1 is clearly different from that of point p50. In fact, point p1 has no history while
in point p50, the NC has followed a path determined by the first 49 points.
p99
When the G62 function is inserted, it cancels the “history” and produces a geometrical pattern almost
identical to the one calculated starting from point p1.
In machining processes that entail several passes, failure to program G62 would have the undesirable
effect of producing different levels of machining between one pass and another.
1-6 10 Series CNC High Speed Machining (00)
Chapter 1
High Speed Machining
GENERAL HIGH SPEED MACHINING PROGRAMMING STRUCTURE
Between the G61 and G60 blocks it will only be possible to program the points that make up the
profile to be machined or the G codes for defining their management method: no other type of
programming will be allowed.
Points may be programmed using, absolute programming may be used by means of (G90) or
incremental programming by means of (G91). All numerical parameters required may be defined
directly or by means of E or L variables: programming with expressions is not valid so XE(E2) or
X(E1+E2) type programming is not allowed, while XE1 is allowed.
The syntax of the allowed program lines will be:
N… [G00 | G01] [G90 | G91] [points] F….
N… [G62 | G63 | G66 |G67 ]
Activation of the HSM (High Speed Machining) feature G61 forces of G01 and G90, modes while at
the exit (G60) the G functions active when G61 was programmed will be restored.
The first point programmed MUST be expressed in absolute positions (G90) and must contain the
programming of all axes associated with the HSM programming (axes configured in the HSM setup
file).
Interaction with Machine Logic
The G61/G60 program section will be considered, from the system point of view, as a single program
block. As regards interfacing with the machine logic, a request for consent for movement will be made
when the G61 function is reached, and an end of movement request will be made when the G60
function is reached (in the same way as for the G27 and G28 continuous movements).
A regards consent for movement, the XW03 variable, which contains the type of movement, will be
set as shown below:
10 Series CNC High Speed Machining (00) 1-7
Chapter 1
High Speed Machining
END OF CHAPTER
1-8 10 Series CNC High Speed Machining (00)
Chapter
2
Axis location points
POINT DEFINING CONVENTIONS
POINTS AND MACHINING COORDINATES
Before defining how the points are handled, it is necessary to specify what they represent as
programming may be executed in relation to three types of coordinates, that is:
• Cutter Contact Points, which refer to the actual cutting point
• Cutter Location Points, which refer to the point normally indicated as the centre of the tool
• Axis Location Points, which refer to an arbitrary point fixed to the machining axes
The cutter contact points are linked to the cutter location points through the geometry and orientation
of the tool. The axis location points are linked to the cutter location points through the geometry of
the machine tool. In machining processes with three axes, the coordinates will simply be translated
while, in those with five coordinated axes, rototranslation matrices that take into account the
geometrical transformations due to the movement of the rotary axes will be applied. The figure below
shows what is meant by cutter contact points, cutter location points and axis location points.
Tool direction
Cutter contact points
Points are defined by means of normal axis coordinates in the format [Axis name][Position];
example: X100 Y200 Z40.
Normal
to surface
Tool
length
Radius
Edge
radius
Cutter location points
10 Series CNC High Speed Machining (00) 2-1
Chapter 2
Point Defining Conventions
Tool Direction
The tool direction represents the orientation of the tool (from the tip to the attachment) within the part
reference system.
WARNING
Two methods may be used to define the tool direction. The first is by directly programming the versor
that identifies the tool direction. This versor is expressed using the ijk coordinates in the format:
[i] [X-coordinate component] [j][Y-coordinate component] [k][Z-coordinate component]
The system will automatically normalize the length of the versor to the unitary length (1.0).
The second way of defining the tool direction is by programming the rotary axes. The system will
automatically determine the three components of the ijk versor depending on the kinematics of the
machine.
In the following sections reference to versor means versor of unitary lenght.
Normal to the Surface Direction
The normal to the surface direction represents the direction of the “line” perpendicular to the surface
to be machined (starting from the surface) within the part reference system.
There are two ways of defining the direction normal to the part. The first is by directly programming
the versor that identifies the normal direction. This versor (of a unitary length) is expressed using the
mno coordinates in the format:
[m] [X-coordinate component] [n][Y-coordinate component] [o][ Z-coordinate component]
The system will automatically normalize the length of the versor to the unitary length (1.0).
The second way is to have this direction calculated automatically by the system. The direction is
calculated on the basis of the tangent to the profile (direction of the movement), on the basis of the
tool direction (ijk versor) and an angle of contact between the part and the tool. This calculation
makes sure that the mno versor is normal to the tangent to the profile and that it defines an angle αα
(angle of contact) with the tool versor ijk.
ijk
mno
α
This type of approach is only significant when the contour is to be machined. When a surface is to be
machined, this approach could fail as there is no information about the “surface” to be machined, only
information about the “direction” of displacement.
α
tg profile
2-2 10 Series CNC High Speed Machining (00)
Chapter 2
ijk
x
Point Defining Conventions
Tool Radius Application Direction
The direction of application of the tool radius represents the direction in which radius compensation is
to be applied (starting from the centre of the tool) within the part reference system.
There are two ways of defining the tool radius application direction. The first is by directly
programming the versor that identifies the direction. This versor (of a unitary length) is expressed
using the pqd coordinates in the format
[p] [X-coordinate component] [q][Y-coordinate component] [d][Z-coordinate component]
The system will automatically normalize the length of the versor to the unitary length (1.0).
The second way is to have this direction calculated automatically by the system. The direction is
calculated automatically on the basis of the tool direction (ijk versor) and the normal to the part (mno
versor). This calculation ensures that the pqd versor is normal to the tool direction and is on the plane
formed by the ijk and mno versors.
ijk
pqd
pqd
mno
mno
Programming of the versor pqd is only significant when specific cutting strategies are applied.
Tangential Axis
The tangential axis is an axis whose position is calculated so as to remain tangential to the profile
described. It is calculated on the basis of the tangent to the polynomial curve on the work plane.
y
Tangential axis
An initial value of the tangential axis (first programmed point) may be defined and the subsequent
positions may be calculated on the basis of this value.
10 Series CNC High Speed Machining (00) 2-3
Chapter 2
Point Defining Conventions
END OF CHAPTER
2-4 10 Series CNC High Speed Machining (00)
Chapter
3
FEATURES PROVIDED BY HIGH SPEED MACHINING
Depending on the type of machine tool used, the points programmed and a series of additional
parameters, the features may be obtained using “High Speed Machining”.
MACHINES WITH 5 AXES
Machines with 5 axes are characterised by the fact that they have two rotary axes that are used to
orient the tool during the machining phase. The direction of the tool and the position of the rotary axes
are two closely related parameters.
One feature of High Speed Machining is that it “automatically” calculates the position of the rotary
axes on the basis of the tool direction (ijk vector). In this way, the same part program may be used on
machines having different kinematics providing both machines can reach the same positions.
10 Series CNC High Speed Machining (00) 3-1
Loading...