0% found this document useful (0 votes)

670 views75 pages

FANUC 16i/18i High-Precision Lathe Guide

This document provides specifications for a high-precision contour control function for complex lathes. The function allows for milling machining with compound lathes at high accuracy. It includes features like multiple-block look-ahead acceleration/deceleration for smoothing, automatic feedrate control considering figure changes and speeds, coordinate conversion functions, and interpolation for smooth curves. The high-precision contour control mode is turned on with G05 P10000 and off with G05 P0. It has requirements like specific G codes being set and is temporarily canceled by positioning, auxiliary functions, or spindle functions.

Uploaded by

mike

We take content rights seriously. If you suspect this is your content, claim it here.

Available Formats

Download as PDF, TXT or read online on Scribd

0% found this document useful (0 votes)

670 views75 pages

FANUC 16i/18i High-Precision Lathe Guide

Uploaded by

mike

We take content rights seriously. If you suspect this is your content, claim it here.

Available Formats

Download as PDF, TXT or read online on Scribd

You are on page 1/ 75

FANUC Series 16i /18i –TA/TB

Specifications of

High–precision Contour Control function

for Complex Lathe

FANUC Series 16i /18i -TA/TB

1 Outline................................................................................................................................ 3
2 Operation ........................................................................................................................... 4
3 Parameter ........................................................................................................................ 54
4 Signal ............................................................................................................................... 68
5 Alarm and message......................................................................................................... 69
6 Notes................................................................................................................................ 70
7 The function table which can be used by a high-precision contour control .................... 73

FANUC Series 16i /18i -TA/TB

1.1 Outline
The milling machining can be done with the compound lathe in high accuracy by using this
function. The following functions can be used in the high-precision contour control mode.

(1) Function for multiple–block look–ahead acceleration/deceleration before interpolation.

This function eliminates machining errors due to acceleration/deceleration.
(2) Automatic feedrate control function which enables smooth acceleration/ deceleration by
considering changes in the figure and speed and allowable acceleration for the machine.
This is performed by reading multiple blocks in advance.
(3) Coordinate conversion functions to make programming simple.(Scaling*, Coordinate
system rotation*,Programmable mirror image*)
(4) Interpolation functions to process smooth curve.(Smooth interpolation*, NURBS
interpolation*)
(5) Programming by G code system of M series.
(6) Radius programming.

Furthermore, smoother acceleration/deceleration is achieved, enabling the feed–forward

coefficient to be increased. This feature also reduces follow–up error in the servo system.

Note) * marked are optional function.

FANUC Series 16i /18i -TA/TB

2.1 Format
The high-precision contour control mode can be turned on or off by following instructions. The
character of "HPCC" is blinking displayed under the right of the screen in the high-precision
contour control mode.

G05 P10000 : Start high-precision contour control mode

G05 P0 : End high-precision contour control mode
Please command G05 alone.

The mode used to perform high–precision contour control is called HPCC mode.

2.2 Condition that HPCC is permitted

Before G05P10000 can be specified, the following modal values must be set. If they are not set,
the P/S alarm No.5012 is issued.

G code Meaning
G13.1 Cancels polar coordinate interpolation.
G40 Cancels tool nose radius compensation.
G50 Cancels scaling.
G50.1 Cancels the programmable mirror image function.
G50.2 Cancels Polygonal turning
G64 Cutting mode
G69.1 Cancels coordinate conversion.
G80 Cancels canned cycles.
G98[G94] Feed per minute
G97 Cancels constant surface speed control.

2.3 Commands that HPCC is cancelled temporarily

The HPCC mode is automatically canceled once when the undermentioned instruction is done
in the HPCC mode, and buffering is stopped. Moreover, the HPCC operating signal EXHPCC
becomes "0".

• Positioning (G00) of TYPE-A(*1)

• Auxiliary function (M command)
• The second auxiliary function
• Multiple M commands in a same block
• Spindle function (S command)

(*1) Please refer to section 2.7.

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 4/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
2.4 G code system
G code system in the HPCC mode becomes G code system of the machining centre system.
To distinguish from other G codes, the G code of the group which cannot instruct excluding the
HPCC mode is displayed in reverse video as shown in the figure below.

Reverse display

2.5 Absolute and incremental command

Absolute or incremental of the instruction value follows G90/G91 displayed in reverse video
for G code system A. Even if the HPCC mode is turns off and on, this modal data is held.

Example)
N1 G00 X100. Z100. ; Absolute
N2 G98 non-HPCC
N3 G05 P10000 ;
N4 G91 G01 X50. Z50. F1000 ; Incremental HPCC
N5 G05 P0
N6 G00 X10. Z10. ; Absolute
; non-HPCC
N7 G05 P10000 ;
N8 G01 X50. Z50. F1000 ; This block becomes incremental motion,
N9 G05 P0 ; HPCC
because of G91 which is commanded in
last HPCC mode (N4) is held. G90 in N6
has no influence.

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 5/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
When the G code system is B or C, absolute or incremental of the instruction value follows
G90/G91 which is commanded most later, regardless of off and on of HPCC mode.

Example)
N1 G00 G90 X100. Z100. ; Absolute
N2 G94 non-HPCC
N3 G05 P10000 ;
N4 G91 G01 X50. Z50. F1000 ; Incremental HPCC
N5 G05 P0
N6 G00 G90 X10. Z10. ; Absolute
; non-HPCC
N7 G05 P10000 ;
N8 G01 X50. Z50. F1000 ; This block becomes absolute motion,
N9 G05 P0 ; HPCC
because of it follows last G90/G91
command (in N6). G91 which is
commanded in last HPCC mode (N4)
has no influence this block.

Moreover, an incremental instruction which uses address U, V, W, and H in the HPCC mode
cannot be commanded for G code system A. (The alarm of P/S009 is generated.)

2.6 Diameter programming and radius programming

Even if the machine specification is diameter programming, the instruction in the HPCC mode
can be assumed to be radius programming by setting of parameter No.8414#0(RRD).

• Manual operation Manual operation in the HPCC mode applies to parameter No.1006#3(DIA) regardless of
setting parameter No.8414#0(RRD).

• Alarm If the instruction that the HPCC mode is temporarily canceled(*1) is commanded to the axis
assumed to be radius sprogramming in the HPCC mode, the P/S5000 alarm is generated.

Example) When X is diameter programming axis and parameter No.8414#0(RRD) of X is “1”,

Z is radius programming axis.

(1) When positioning of Type-A (*2) is commanded.

:
G05 P10000 ;
G00 Z100. ; Z is exected.
G00 X100. ; X brings alarm of P/S5000.
:

(2) Movement instruction with auxiliary function

:
G05 P10000 ;
G01 Z100. F1000 M00 ; Z is exected
X100. M00 ; X brings alarm of P/S5000.
:
(*1) Please refer to section 2.3 and section 4.
(*2) Please refer to section 2.7.

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 6/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
2.7 Positioning and auxiliary functions
• Type of positioning
The type of positioning instruction (G00) in the HPCC mode is selected according to the
undermentioned parameter.
No.8403 #1(MSU),#7(SG0)
No.8404 #0(STG)

Parameter setting
8403#1 8403#7 8404#0 Explanatiom
(MSU) (SG0) (STG)
- 0 0 0 Alarm is generated.

Positioning type
Type-A 1 0 0 Executed with HPCC cancel.

Type-B - 1 1 Executed whthout HPCC cancel.

Note)
Even if Type-B has been selected, the block in which the auxiliary
function was instructed automatically becomes Type-A.

• Specifications
The specification of the positioning operation by each type is as follows.

Type-A Type-B
Applied feedrate Parameter No.1420 Parameter No.1420
Tool path Follows to parameter Follows to parameter
No.1401#1(LRP) No.1401#1(LRP)
In-position check Available Available
Applied override signal Rapid traverse override Rapid traverse override
Acc/deceleration before Not effective Not effective
interpolation
Acc/deceleration after Effective (Rapid) Effective (Rapid)
interpolation
Feed-forword control Follows to parameter Always effective
No.1800#3(FFR)
Block overlap in Rapid Not available Not available
traverse
External deceleration Available Not available
G00 command in each mode Not available Available
of scaling or coordinate
rotation or programmable
mirror image
Output of RPD signal Output Output
(F0002#1)
Backlash compensation for Available Available
each rapid traverse and
cutting feed

• Auxiliary function
Auxiliary function can be commanded in the HPCC mode by setting “1” in parameter MSU.
(No.8403#1). The P/S5000 alarm is generated if the auxiliary function is instructed when this
parameter is “0”.
The HPCC mode is temporarily canceled when instructing in the auxiliary function.(Please
refer to section 2.3)

FANUC Series 16i /18i -TA/TB

2.9 Tool position offset

Tool position offset (T code) con not be commaned in HPCC mode. The P/S5000 alarm is
generated when commanded.
The tool position offset should be made effective before the HPCC mode is turned on.

2.10 Cutter compensation C

Cutter compensation C can be used in HPCC mode. The specifications of cutter compensation
C is similar to that of FANUC Series 15-MB. Plese refer to “FANUC Series 15-MODEL B For
Machining Center OPERATORS MANUAL (Programming) B-62564E” for detail.
To use this function, option of tool nose radius compensation is necessary.

• Offset Number Please instruct in the offset number by D code.

• Offset amount In cutter compensation C, the value set in tool nose radius amount amount is used as an offset
amount.

• Tool geometry and wear offset

When the option of tool geometry and wear offset is effective, an actual amount of the cutter
compensation C becomes the value by which the geometry offset amount and the wear offset
amount of commanded D code are added. A wear offset number different from the geometry
offset number cannot be specified.

• D code Even if the HPCC mode is turned off, D code is held. The held D code is used as a cutter
compensation number if not instructing in D code when a HPCC is turned on again.

• Corner offset circular interpolation(G39)

Specify the corner offset circular interpolarion (G39) for the outside of a curve. If this command
is specified for the inside of a curve, an excessive cut can occur.

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 8/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
• Instruction form When G05 P10000 and G05 P0, and G41/G42 and G40 are to be specified together, G41/G42
to G40 must be nested between G05 P10000 and G05 P0. This means that HPCC mode cannot
be started or canceled in cutter compensation (G41/G42) mode. If such a specification is made,
the P/S alarm No.0178 or P/S alarm No.5013 P/S alarm is issued.

(Example of a correct program)

·
·
G05 P10000 ;
·
G41 X___ Y___ D01 ;
·
· Cutter compensation
· (G41) mode
G40 X___ Y___ ;
·
· HPCC mode
G42 X___ Y___ D01 ;
·
· Cutter compensation
· (G42) mode
G40 X___ Y___ ;
·
G05 P0 ;
·

(Example of an incorrect program (1))

·
·
G41 X___ Y___ D01 ;
·
·
G05 P10000 ; When the start of HPCC mode is specified in tool nose
radius compensation mode, the P/S alarm No.0178 is
issued.

(Example of an incorrect program (2))

·
·
G05 P10000 ;
·
G41 X___ Y___ D01 ;
·
·
· When cancellation of HPCC mode is specified in cutter
G05 P0 ; compensation mode, the P/S alarm No.5013 alarm is
issued.

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 9/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
• Cancel When a block containing no movement operation is specified together with the cutter
compensation cancel code (G40), a vector with a length equal to the offset value is created in a
direction perpendicular to the movement direction of the previous block. Cutter compensation
mode is canceled while this vector still remains. This vector is canceled when the next move
command is executed.

N7 N8
·
·
N6
N6 G91 X100. Z100. ;
N7 G40
N8 X100. ;
·
·

If cutter compensation mode is canceled while a vector still remains and HPCC mode is
canceled before a move command is specified, the P/S alarm No.5013 is issued.

·
·
N6 G91 X100. Z100. ;
N7 G40
N8 G05 P0 ; The P/S alarm No. 5013 is issued.
·
·

2.11 Cs contour control

Cs axis can be instructed in the HPCC mode.

• Paremeter setting Please set a parameter No.1602#5(G8S) to 1 in case of using Cs contour control in HPCC 02
mode. 02

• Instruction form The Reference point return of Cs axis can not be specified in HPCC mode. Please enter the
HPCC mode according to the following procedures when you use Cs axis in the HPCC mode.

(1) Turning on the Cs contour control mode.

(2) Reference point retiurn of Cs axis.
(3) Turning on the HPCC mode.

FANUC Series 16i /18i -TA/TB

2.12.1 Outline
Either of two types of machining can be selected, depending on the program command.

(1) For those portions where the accuracy of the figure is critical, such as at corners,
machining is performed exactly as specified by the program command.
(2) For those portions having a large radius of curvature where a smooth figure must be
created, points along the machining path are interpolated with a smooth curve, calculated
from the polygonal lines specified with the program command (smooth interpolation).

This function can use only in the HPCC mode.

This function is an option.

2.12.2 Format
G05 P10000 ; : Starting of HPCC mode
G05.1 Q2 X0 Y0 Z0 ; : Starting of smooth interpolation mode
…
G05.1 Q0 ; : Ending of smooth interpolation mode
G05 P0 ; : Ending of HPCC mode

2.12.3 Explanations
To machine a part having sculptured surfaces a part program usually approximates the
sculptured surfaces with minute line segments. As shown in the following figure, a sculptured
curve is normally approximated using line segments with a tolerance of about 10 µm.

Enlarged
:Specified point
10µm

Fig. 2.12.3(a) Approximation with Line Segments

When a program approximates a sculptured curve with line segments, the length of each
segment differs between those portions that have mainly a small radius of curvature and those
that have mainly a large radius of curvature. The length of the line segments is short in those
portions having a small radius of curvature, while it is long in those portions having a large
radius of curvature. The high–precision contour control moves the tool along a programmed
path thus enabling highly precise machining. This means that the tool movement precisely
follows the line segments used to approximate a sculptured curve. This may result in a non–
smooth machined curve if control is applied to machining a curve where the radius of curvature
is large and changes only gradually. Although this effect is caused by high–precision machining,
which precisely follows a pre–programmed path, the uneven corners that result will be judged
unsatisfactory when smooth surfaces are required.

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 11/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
Table 2.12.3 (a)
Profile Portions having mainly Portions having mainly
a small radius of a large radius of
curvature curvature
Example of machined Automobile parts Decorative parts, such as
parts body side moldings
Length of line segment Short Long
Resulting surfaces Smooth surface even Uneven surfaces may
produced using high– when machining is result when machining is
precision contour control performed exactly as performed exactly as
specified by a program specified by a program

Fig. 2.12.3(b) Example of uneven surfaces (polygon) resulting

from machining that precisely follows the line
segments.

In smooth interpolation mode, the CNC automatically determines, according to the program
command, whether an accurate figure is required, such as at corners, or a smooth figure is
required where the radius of curvature is large. If a block specifies a travel distance or direction
which differs greatly from that in the preceding block, smooth interpolation is not performed for
that block. Linear interpolation is performed exactly as specified by the program command.
Programming is thus very simple.

Note )
When the result of the automatic judgment of CNC is different
from the movement which the programmer intended, cancel a
smooth interpolation temporarily or change the instruction point
or the correspondence of the adjustment of the parameter etc. is
needed.

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 12/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
Smooth interpolation
Interpolated by smooth curve
N17
N16 N13 N12
N15 N14 N11
N10
N1
N2 N5 N6
N3 N4 N7
N8
N9
Interpolated by smooth curve
Linear interpolation
Linear interpolation

N17
N16 N13 N12
N15 N14 N11

N1 N10
N2 N5 N6
N3 N4 N7
N8 N9

Fig. 1.3.3 (c) Smooth Interpolation and Linear Interpolation

• Conditions for performing smooth interpolation

Smooth interpolation is performed when all the following conditions are satisfied. If any of the
following conditions is not satisfied for a block, that block is executed without smooth
interpolation then the conditions are checked for the next block.

(1) The length of the block is shorter than that of the parameter No.8486, and it is longer than
the parameter No.8490.
(2) The difference between the angles specified in blocks is smaller than the value specified
with parameter No.8487.
(3) The tolerance specified in the block is smaller than the value specified with parameter No.
7676 and larger than that specified with parameter No.8492.
(4) The modes are:
G01 : Linear interpolation
G05 P10000 : HPCC mode
G40 : Cutter compensation cancel
G94 : Feed per minute
(5) Machining is specified only along the axes specified with G05.1Q2.
(6) The internal algorithm of the CNC judges the block to be suitable for smooth interpolation.

• Commands which cancel smooth interpolation

When one of the following commands is specified, smooth interpolation is canceled:

(1) Auxiliary and second auxiliary functions

(2) M98,M99 : Subprogram call
M198 : Calling a subprogram in external memory

FANUC Series 16i /18i -TA/TB

• Controlled axes
Smooth interpolation can be specified only for the X–, Y–, and Z–axes and any axes parallel to
these axes (up to three axes at one time).

• Back-and-forth path machining

When back-and-forth path machining is performed for a path that includes inflection points, the
back and forth level difference may increase. In particular, if the positions of specified points
differ greatly between the back and forth paths, a large back and forth level difference is
produced.

Fig. 2.12.4 (a) Example When a Large Back and Forth Level
Difference is Produced

In such a case, modify the program as follows:

(1) Perform machining with a unidirectional path.
(2) In portions near inflection points, specify closely spaced points.

• Modal
G code of group 01 when instructing in G05.1 Q2 should be G01.
When G code is not G01, the alarm of P/S010 is generated.

FANUC Series 16i /18i -TA/TB

G05 P10000
G05. 1 Q2 X0 Y0 Z0
N01 G91 G01 X1000 Z-300 F500
N02 X1000 Z-200
N03 X1000 Z-50
N04 X1000 Z50
N05 X1000 Z50
N06 X1000 Z-25
N07 X1000 Z-175
N08 X1000 Z-350
N09 Y1000
N10 X-1000 Z350
N11 X-1000 Z175
N12 X-1000 Z25
N13 X-1000 Z-50
N14 X-1000 Z-50
N15 X-1000 Z50
N16 X-1000 Z200
N17 X-1000 Z300
G05.1 Q0
G05 P0

Interpolated by smooth curve

N17
N16 N13 N12
N15 N14 N11
N1 N10

N2 N5 N6
N3 N4 N7
N8 N9
Interpolated by smooth curve
Linear interpolation

Fig. 2.12.5 (a) Sample program of smooth interpolation

FANUC Series 16i /18i -TA/TB

2.13.1 Outline
This function enables NURBS(non–uniform rational B–spline) curve expression to be directly
specified to the CNC. This eliminates the need for approximating the NURBS curve with
minute line segments. This offers the following advantages:

1. No error due to approximation of a NURBS curve by small line segments

2. Short part program
3. No break between blocks when small blocks are executed at high speed
4. No need for high–speed transfer from the host computer to the CNC

When this function is used, a computer–aided machining (CAM) system creates a NURBS
curve according to the NURBS expression output from the CAD system, after compensating for
the length of the tool holder, tool diameter, and other tool elements. The NURBS curve is
programmed in the NC format by using these three defining parameters: control point, weight,
and knot.

This function can use only in the HPCC mode.

This function is an option.

CAD (Designing a metal die)

Generating a metal die surface

(NURBS surface or curve)

CAM (Creating an NC part program)

Studying the machining method and others

Tool compensation file

NC part program after tool compensation

(NURBS curve)

NURBS curve (control point, weight, knot)

CNC equipment Machine tool

Fig. 2.13.1 (a) NC part program for machining a metal die

according to a NURBS curve

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 16/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
2.13.2 Format
G05 P10000 ; : Starting of HPCC mode
G06.2 [P_] K_ X_ Y_ Z_ [R_] [F_] ; : Starting of NURBS interpolation mode
K_ X_ Y_ Z_ [R_] ;
K_ X_ Y_ Z_ [R_] ;
K_ X_ Y_ Z_ [R_] ;
...
K_ X_ Y_ Z_ [R_] ;
K_ ;
...
K_ ;
G01 ... ; : Ending of NURBS interpolation mode
G05 P0 ; : Ending of HPCC mode

Each code has the following meaning.

G06.2 : Start NURBS interpolation mode

P_ : Rank of NURBS curve
X_ Y_ Z_ : Control point
R_ : Weight
K_ : Knot
F_ : Feedrate
2.13.3 Explanations

• G code
NURBS interpolation mode is selected when G06.2 is programmed in high–precision contour
control mode. G06.2 is a modal G code of group 01. NURBS interpolation mode ends when a G
code of group 01 other than G06.2 (G00, G01, G02, G03, etc.) is specified. NURBS
interpolation mode must end before the command for ending high–precision contour control
mode is programmed.
In NURBS interpolation mode, any command other than the NURBS interpolation command
(miscellaneous function and others) cannot be specified.

• Controlled axes
NURBS interpolation can be performed on up to three axes. The axes of NURBS interpolation
must be specified in the first block. A new axis cannot be specified before the beginning of the
next NURBS curve or before NURBS interpolation mode ends.

• Rank of NURBS
A rank of NURBS can be specified with address P. The rank setting, if any, must be specified in
the first block. If the rank setting is omitted, a rank of four (degree of three) is assumed for
NURBS. The valid data range for P is 2 to 4. The P values have the following meanings:

P2: NURBS having a rank of two (degree of one)

P3: NURBS having a rank of three (degree of two)
P4: NURBS having a rank of four (degree of three) (default)

This rank is represented by k in the defining expression indicated in the description of NURBS
curve below. For example, a NURBS curve having a rank of four has a degree of three. The
NURBS curve can be expressed by the constants t3, t2, and t1.

• Weight
The weight of a control point programmed in a single block can be defined. When the weight
setting is omitted, a weight of 1.0 is assumed.

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 17/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
• Knot
The number of specified knots must equal the number of control points plus the rank value. In
the blocks specifying the first to last control points, each control point and a knot are specified
in an identical block. After these blocks, as many blocks (including only a knot) as the rank
value are specified. The NURBS curve programmed for NURBS interpolation must start from
the first control point and end at the last control point. The first k knots (where k is the rank)
must have the same values as the last k knots (multiple knots). If the absolute coordinates of the
start point of NURBS interpolation do not match the position of the first control point, P/S
alarm No. 5117 is issued. (To specify incremental values, G06.2 X0 Y0 Z0 K_ must be
programmed.)

2.13.4 Example
G05 P10000;
G90;
...
G06.2 K0. X0. Z0.;
K0. X300. Z100.;
K0. X700. Z100.;
K0. X1300. Z-100.;
K0.5 X1700. Z-100.;
K0.5 X2000. Z0.;
K1.0;
K1.0;
K1.0;
K1.0;
G01 Y0.5;
G06.2 K0. X2000. Z0.;
K0. X1700. Z-100.;
K0. X1300. Z-100.;
K0. X700. Z100.;
K0.5 X300. Z100.;
K0.5 X0. Z0.;
K1.0;
K1.0;
K1.0;
K1.0;
G01 Y0.5;
G06.2 ...
...
G01 ...
G05P0;
Z
Y

1000.

X
2000.
Fig. 2.13.3 (a) Example of NURBS interpolation

FANUC Series 16i /18i -TA/TB

k : Rank
Pi : Control point

wi : Weight

x i
: Knot ( x i ≤ x i +1
)
Knot vect or [ x 0 , x 1
,..., x m
] (m = n + k )
t : Spline parameter,

The spline basis function N can be expressed with the de Boor–Cox recursive formula, as
indicated below:

ìï 1 (x i
≤ t ≤ x i+1 )
(t) = í
N i ,1
ïî 0 (t < x i
, x i+1
< t )
(t − x i) N i,k − 1 (t ) (x i+ k − t ) N i + 1,k −1 (t)
N i,k (t ) = +
x i+ k −1 − x i xi+ k − xi+1

The NURBS curve P(t) of interpolation can be expressed as follows:

n
å N i,k (t ) w i P i
P (t ) = i= 0
n
å N i,k (t ) w i
i= 0
( x 0
≤ t ≤ x m
)

2.13.6 Limitations

• Manual intervention
If manual intervention is attempted while manual absolute mode is set, P/S alarm No. 5118 is
issued.

• Cutter compensation
Cutter compensation cannot be simultaneously executed. NURBS interpolation can only be
specified after cutter compensation has been canceled.
• Reset
A reset during NURBS interpolation results in the clear state. The modal code of group 1 enters
the state specified in the G01 bit (bit 0 of parameter 3402).

FANUC Series 16i /18i -TA/TB

2.14.1 Scaling
(1) All axis scaling
• Outline
A programmed figure can be magnified or reduced (scaling).
Please set “1” in parameter No.8485#0(G51) and No.5401#0(SCLx) to make this function
effective.
This function can use only in the HPCC mode.
This function is an option.

• Format

G05 P10000 ; : Starting of HPCC mode

G51.X_ Y_ Z_ P_ ; : Starting of scaling mode
...
G50 ... ; : Ending of scaling mode
G05 P0 ; : Ending of HPCC mode

Each code has the following meaning.

G51 : Scaling start

X_ Y_ Z_ : Absolute command for center coordinate value of scaling
P_ : Scaling magnification
G50 : Scaling cancel

• Scaling center
The point instructed by X, Y, and Z of the same to G51 block becomes the center of scaling.
When X, Y, and Z are omitted, the position of the instruction in G51 becomes the center of
scaling.

• Scaling magnification
Movement amount is scaled by the magnification instructed by P of the block of G51.
If P is not instructed, the magnification set by parameter No.5411 is used.
The magnification which can be instructed is as follows :
0.00001 -- 9.99999 or 0.001 -- 999.999

P4 P3

P4’ P3’ P1--P4 : Programmed figure

Po P1’--P4’ : Scaled figure
Po : Scaling center
P1’ P2’

P1 P2

FANUC Series 16i /18i -TA/TB

• Outline
Each axis can be scaled by different magnifications.
Please set “1” in parameter No.8485#0(G51) , No.5401#0(SCLx), and No.5400#6(XSC) to
make this function effective.
This function can use only in the HPCC mode.
This function is an option.(Included in option of scaling)

• Format

G05 P10000 ; : Starting of HPCC mode

G51.X_ Y_ Z_ I_ J_ K_ ; : Starting of scaling mode
...
G50 ... ; : Ending of scaling mode
G05 P0 ; : Ending of HPCC mode

Each code has the following meaning.

G51 : Scaling start

X_ Y_ Z_ : Absolute command for center coordinate value of scaling
I_ J_ K_ : Scaling magnification for X, Y and Z axis respectively
G50 : Scaling cancel

• Magnification
If scaling magnification rates I, J, and K are not specified, the magnification set in parameter
No.5421 is used. Moreover, the value set by the parameter No.5421 is used as a magnification
in the axis from which I, J, and K are not instructed and axes other than three basic axes. In this
case, scaling is not performed to the axis that 0 is set in this parameter.
The magnification which can be instructed is as follows :
0.00001 -- 9.99999 or 0.001 -- 999.999
Y

Programmed figure

Scaled figure
c

o a
b

X
b/a : Scaling magnification of X axis
d/c : Scaling magnification of Y axis
o : Scaling center

FANUC Series 16i /18i -TA/TB

• Instruction form
Specify G51 in a separate block. Please cancel with G50 when scaling becomes unnecessary.

• Position display
The position display represents the coordinate value after scaling.

• Magnification
(1) If a parameter setting value is employed as a scaling magnification without specifying P, the
setting value at G51 command time is employed as the scaling magnification, and change of
this value, if any, is not effective.
(2) The decimal point cannot be input to magnification I, J, and K.

• Manual operation
Scaling is effective only to the automatic operation. It is not effective in the manual operation.

• Move amount
If scaling results are rounded by counting fractions of 5 and over as a unit and disregarding the
rest, the move amount may become zero. In this case, the block is regarded as a no movement
block, and therefore, it may affect the tool movement by cutter compensation C.

• Circular interpolation
Even if different magnifications are applied to each axis in circular interpolation, the tool will
not trace an ellipse.

Example ) G90 G00 X0.0 Y100.0 Z0.0 ;

G51 X0.0 Y0.0 Z0.0 I2000 J1000;
G02 X100.0 Y0.0 I0 J-100.0 F500 ;
Above commands are equivalent to the following command:
G90 G00 X0.0 Y100.0 Z0.0 ;
G02 X200.0 Y0.0 I0 J-100.0 F500 ;
Because the end point is not corresponding to the radius, the circular interpolation at this time
becomes a spiral interpolation.

Y
Figure without scaling

Figure after scaling

X
O

Scaling center

• Absolute and incremental

It is assumed that the scaling center is not instructed for an incremental instruction until the
absolute position instruction appears after the G51 mode turns on.. (That is, the position of the
instruction in G51 becomes a scaling center)

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 22/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
• Invalid scaling
This scaling is not applicable to cutter compensation values, tool length offset values, and tool
offset values.

1/2 scaling

• Coordinate system rotation

When both scaling and coordinate system rotation are specified, the coordinate system is
rotated after scaling is applied. In this case, scaling is effective for the center of rotation.

Example) O0001 ;
G90 G00 X20. Y10. ;
G05 P10000 ;
G01 X50. F500 ;
Y30. ; (a)
X20. ;
Y10. ;
G51 X20. Y10. I3000 J2000;
G01 X50. F500 ;
Y30. ;
X20. ; (b)
Y10. ;
G17 G68 X35. Y20. R3000 ;
G01 X50. F500 ;
Y30. ;
X20. ; (c)
Y10. ;
G69 ;
G50 ;
G05 P0 ;
M30 ;
Y
Center of rotation after scaling

Center of rotation before scaling

(b)

(a)

O X
Original figure specified
in the program Scaled figure
Figure after the coordinate
Center of scaling system is rotated

FANUC Series 16i /18i -TA/TB

• Outline
It is possible to instruct in the coordinate system rotation in the HPCC mode. Only the
coordinate system rotation in the HPCC mode is explained in the following descriptions.
Please set “1” in parameter No.8485#0(G51) to make this function effective.
This function is an option.

• Format

G05 P10000 ; : Starting of HPCC mode

G17
G18 G68 α_ β_ R_ ; : Starting of coordinate system rotation mode
G19
...
G69 ... ; : Ending of coordinate system rotation mode
G05 P0 ; : Ending of HPCC mode

Each code has the following meaning.

G68 : Coordinate system rotation start

α_ β_ : Absolute command for two of the X_, Y_, and Z_ axes that correspond
to the current plane selected by a command (G17, G18, or G19). The
command specifies the coordinates of the center of rotation for the
values specified subsequent to G68.
R_ : Angular displacement with a positive value indicates counter
clockwise rotation. Bit 0 of parameter 5400 selects whether the
specified angular displacement is always considered an absolute
value or is considered an absolute or incremental value depending on
the specified G code (G90 or G91).
G69 : Coordinate system rotation cancel

(α, β)

• Rotation angle
Please instruct in the rotating angle degree by the unit of 0.001deg within the range of
-360000 to 360000.
When R_ is not specified, the value specified in parameter No.5410 is assumed as the angular
displacement.

• Rotation center
When (α, β) is omitted in the block of G68, the position of the instruction in G68 becomes a
center of rotation.
The center of rotation for an incremental command programmed after G68 but before an
absolute command is the tool position when G68 was programmed.

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 25/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
• Plane
The coordinate system rotation is executed on selected plane (G17,G18,G19) when G68 is
instructed.
The G code for selecting a plane (G17,G18,or G19) can be specified before the block
containing the G code for coordinate system rotation (G68).

• Cutter compensation C
Cutter compensation operations are executed after the coordinate system is rotated.

• Notes concerning coordinate system rotation

• Instruction form
(1) When a decimal fraction is used to specify angular displacement (R_), the 1’s digit
corresponds to degree units.
(2) Please do not instruct in the block of G68 other than a plane selection, the rotation center
coordinates, and the rotating angle.
(3) Specify G69 in a separate block.
(4) Please instruct in the plane selection command(G17,G18,G19) in the G69 mode.

• Other notes
Please refer to notes in clause 2.14.4.

• Example
N01 G50 X-5000. Y-5000. G69.1 G17 ;
N02 G05 P10000 ;
N03 G68 X7000. Y3000. R60. ;
N04 G90 G01 X0 Y0 F2000 ;
( G91 X5000. Y5000. ; )
N05 G91 X10000. ;
N06 G02 Y10000. R10000.;
N07 G03 X-10000. I-5000. J-5000. ;
N08 G01 Y-10000. ;
N09 G69 ;
N10 G90 X-5000. Y-5000. ;
N11 G05 P0 ;
N12 M02 ;
Tool path when the incremental command is
designated in the N4 block (in parenthesis)
Originally programmed
tool path

60°

Rotation center
(-5000,-5000)

Tool path after rotation

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 26/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
• Relationship with other functions
Cutter compensation C
It is possible to specify G68 and G69 in cutter compensation mode. The rotation plane must
coincide with the plane of cutter compensation.

Example) N01 G01 G90 X0 Y0 ;

N02 G42 X1000 Y1000 F1000 D01 ;
N03 G68 R-30000 ;
N04 G91 X2000 ;
N05 G03 Y1000 I-1000 J500 ;
N06 G01 X-2000 ;
N07 Y-1000 ;
N08 G69 ;
N09 G40 G90 X0 Y0 ;

Programmed shape before coordinate

system rotation

Programmed shape after

coordinate system rotation

30°

Tool path
(0,0)

Scaling
If a coordinate system rotation command is executed in the scaling mode (G51 mode), the
coordinate value (α, β) of the rotation center will also be scaled, but not the rotation angle (R).
When a move command is issued, the scaling is applied first and then the coordinates are
rotated and instruct in the programming according to the following procedures.

(Exapmle 1) G51 …… ; (Scaling start)

G68 …… ; (Coordinate system rotation start)
:
:
G69 ; (Coordinate system rotation end)
G50 ; (Scaling end)

A coordinate system rotation command (G68) should not be issued in cutter compensation
mode (G41, G42) on scaling mode (G51). The coordinate system rotation command should
always be specified prior to setting the cutter compensation mode.

(Exapmle 1) G51 …… ; (Scaling start)

G68 …… ; (Coordinate system rotation start)
:
:
G41 ; (Cutter compensation)
:

FANUC Series 16i /18i -TA/TB

When scaling and coordinate

system rotation are applied

When only scaling is

applied

Cutting program

O X

FANUC Series 16i /18i -TA/TB

• Outline
By a programmed command, the mirror image function can be used for each axis.
If the programmable mirror image function is specified when the command for producing a
mirror image is also selected by a CNC external switch or CNC setting, the programmable
mirror image function is executed first.
This function can use only in the HPCC mode.
This function is an option.

• Format

G05 P10000 ; : Starting of HPCC mode

G51.1 X_ Y_ Z_ ; : Starting of programmable mirror image mode
:
:
G50.1 X_ Y_ Z_ ; : Ending of programmable mirror image mode
G05 P0 ; : Starting of HPCC mode

The mirror image is effective as the mirror was put on the position of the instructed each axis by
X, Y, and Z instructed with G51.1.
The mirror image of the instructed each axis is canceled by X, Y, and Z instructed with G50.1.
In this case, the instruction value does not care about any value.

• Notes concerning programmable mirror image

Operation of program
When a mirror image is produced on the other side of one axis on a specified plane, other
commands are processed as follows:
(1) Circular command: The direction of rotation is reversed.
(2) Cutter compensation: The direction of offset is reversed.
(3) Coordinate system rotation: The direction of rotation is reversed.
Movig direction
Relation between move command and machine travel/coordinate value is as follows in the
programmable mirror image.

Move command Machine travel Machine Relative Absolute

coordinate coordinate coordinate
+ - - - -
- + + + +

Instruction form
The first move command coming after G50.1 or G51.1 must be specified with absolute values.

Coordinate system rotation and scaling

G50.1 and G51.1 must be specified in the G68 or G51 mode.

(Example of an incorrect program (1))

G68 … ;
G51.1…;
……
G50.1 …;
G69 ;

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 29/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
(Example of an incorrect program (2))
G51.1…;
G68…;
……
G50.1…;
G69 ;
(Example of a correct program)

G51.1…;
G68…;
……
G69 ;
G50.1…;

Other notes
Please refer to notes in clause 2.14.4.

• Example
If the contour of workpiece to be machined is symmetrical about an axis, use the programmable
mirror image function and subprograms. The entire contour can be produced by programming a
part of it.

100
N50 N30

60
50

N70 N90

O X
50 60 100

Subprogram Main program

O9000 ; N10 G05 P10000 ;
G00 G90 X60. Y60. ; N20 G00 G90 ;
G01 X100. Y60. F100 ; N30 M98 P9000 ;
G01 X100. Y100. ; N40 G51.1 X50. ;
G01 X60. Y60. ; N50 M98 P9000 ;
M99 ; N60 G51.1 Y50. ;
N70 M98 P9000 ;
N80 G50.1 X0 ;
N90 M98 P9000 ;
N100 G50.1 Y0 ;
N110 G05 P0 ;

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 30/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
2.14.4 Notes concerning scaling, coordinate system rotation and programmable mirror
image

• Modal
(1) Please instruct in starting of HPCC (G05 P10000) in the state of G50(scaling cancel),
G69.1(coordinate system rotation .cancel), and G50.1(programmabel mirror image cancel).
When the HPCC is started in either of G51, G68.1 or G51.1 mode, an alarm of P/S5012 is
generated.
(2) Please instruct in G51, G68, and G51.1 in the G01 mode. The P/S010 alarm is generated
when instructing in the G00 mode.
However, it is possible to instruct in the G00 mode when “1” is set in parameter
No.8403#7(SG0).

• Instruction form
Please turn on and off scaling, the coordinate rotation, and the programmable mirror image in
the HPCC mode.

Example) G05 P10000 ;

:
G51 …… ;
:
: Scaling mode HPCC mode
G50 ;
:
G05 P0 ;

When the HPCC mode is turned off in G51, G68, and the G51.1 mode, the alarm of P/S5313 or
P/S5013 is generated.

• G code which can be specified

G code which can be instructed in G51, G68, and the G51.1 mode is limited at the following.

G01/G02/G03
G17/G18/G19 (It is not possible to instruct in the G68 mode.)
G40/G41/G42/G39
G50/G51
G50.1/G51.1
G68/G69
G90/G91
G00

• Positioning
Please set “1” in parameter No.8403#7(SG0) to instruct in G00 in G51, G68, and the G51.1
mode.

• Auxiliary function
Please set “1” in parameter No.8403#1(MSU) to use the auxiliary function(M,S,B command) in
G51, G68, and the G51.1 mode.
Please instruct in the auxiliary function in the G51, G68, and G51.1 mode in an identical block.
When it is not an identical block, the alarm of P/S5000 is generated.

FANUC Series 16i /18i -TA/TB

• Function which cannot be used with HPCC

The following funtions can not be used in HPCC mode.

• Sequence Number Comparison and Stop

It is not possible to stop by the sequence number in the HPCC mode.
• Manual handle retrace
• Tool life management
Please do not instruct related to the tool life management.
• Macro executor (execution macro)

The following function is used and busy cannot use a HPCC. Moreover, these function cannot
be used in the HPCC mode.

• Simple synchronous control

• B-axis control
• Synchronous control and composite control (Two-path control)
However, only Cs axis is possible the composite control.
• Superimposed Control

• Function which cannot be instructed in HPCC mode

The following funtions can not be commanded in HPCC mode. Moreover, do not instruct in a
HPCC in the mode of the function of * mark.
(In the [ ] means G code system B or C)

Please refer to "7. The function table which can be used by a high-precision contour control"
for the function which can be used. Functions other than being described there cannot be used.

• Custom macro B
• Interruption type custom macro
• Dwell -G04
• High speed cutting* -G05(Except G05P0)
• Hypothetical axis interpolation* -G07
• Cylindrical interpolation* -G07.1
• Look-ahead control -G08
• Tool retract & recover -G10.6
• Polar coordinate interpolation* -G12.1,G13.1
• Stored stroke check 2 on/off -G22,G23
• Spindle speed fluctuation detection on/off -G25,G26
• Reference position return check -G27
• Return to reference position -G28
• 2nd, 3rd and 4th reference position return -G30
• Floating reference point return -G30.1
• Skip function -G31
• Thread cutting* -G32[G33]
• Variable–lead thread cutting* -G34
• Circular threading * -G35,G36
• Automatic tool compensation -G36,G37(G37.1,G37.2)
• Coordinate system setting or
Max. spindle speed setting -G50[G92]
• Polygonal turning * -G50.2,G51.2
• Workpiece coordinate system preset -G50.3[G92.1]
• Local coordinate system setting -G52
• Machine coordinate system setting -G53
• Workpiece coordinate system selection -G54∼G59,G54.1 P__
• Single direction positioning -G60
• Automatic corner override -G62

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 32/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
• Cutting mode -G64
• Macro call -G65,G66,G67,G66.1
(The subprogram call is possible.)
• Three dimensional coordinate conversion -G68.1/G69.1
• Multiple repetitive cycle* -G70∼G76[G72∼G78]
• Canned grinding cycle* -G71∼G74[G72∼G78]
• Canned cycle for drilling* -G80∼G89
• Hobbing machine function* -G80.4∼G84.4
• Canned cycle* -G90[G77,G20],G92[G78,G21],
………………………………………… G94[G79,G24]
• Constant surface speed control -G96,G97
• Per revolution feed * -G99[G95]
• Tool offset -T code

FANUC Series 16i /18i -TA/TB

2.16.1 Acceleration/deceleration type

There are three types of acc/decelerations as follows. The bell type is smoother than linear type.
(1) Linear acc/deceleration before interpolation
(2) Bell-shaped acc/deceleration before interpolation (acceleration variable ratio constant
type)
(3) Bell-shaped acc/deceleration before interpolation (acceleration variable time constant
type)

2.16.2 Linear acc/deceleration before interpolation

To make this function enabel, please set an acceleration by the parameter No.8400 and
No.8401.

(1) Example of deceleration

To ensure that the feedrate specified for a block is reached when the block is executed,
deceleration is started in the previous block.
Feedrate

Specified feedrate
F3
P1 Feedrate after acceleration/
deceleration before
interpolation is applied

F2
P2

F1 Time
N1 N2
To reduce feedrate F3 to feedrate F2, deceleration must be started at P1.
To reduce feedrate F2 to feedrate F1, deceleration must be started at P2.
The tool can be decelerated over several blocks, because several tens of blocks are read in
advance.

(2) Example of acceleration

Acceleration is started to reach the specified feedrate for a block when the block is executed.
Feedrate
Specified feedrate
F3 Feedrate after acceleration/
deceleration before
interpolation is applied

F1 Time
N1 N2

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 34/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
2.16.3 Look–ahead bell–shaped acc/deceleration before interpolation
(acceleration variable ratio constant type)

To use this function, set bit 7 (BDO) and bit 1 (NBL) of parameter No. 8402 to 1, and also set
the following parameters:

Parameter No. 8400: Parameter 1 for setting the acceleration used for acceleration/
deceleration before interpolation
Parameter No. 8401: Parameter 2 for setting the acceleration used for acceleration/ deceleration
before interpolation
Parameter No. 8402, bit 5 (DST) = 1, bit 4 (BLK) = 0
Parameter No. 8416: Time needed to reach maximum acceleration

For details, see the description of the parameters.

Look–ahead bell–shaped acceleration/deceleration before interpolation controls acceleration as

described below.

Setting of parameter No. 8400 [mm/min, inch/min]

Maximum acceleration ACC_MAX =
Setting of parameter No. 8401 [ms]

Time needed to reach maximum acceleration: ACC_TIME = Setting in parameter No. 8416 [ms]

(1) When maximum acceleration is reached

A c c e le r a tio n
ACC_M AX
+

T im e

A C C _ T IM E A C C _ T IM E

− −A C C _M A X

F e e d ra te A C C _ T IM E A C C _ T IM E

T im e

FANUC Series 16i /18i -TA/TB

A c c e le r a tio n
+

T im e

F e e d ra te

T im e

(1) Acceleration
The tool is accelerated to a specified feedrate, starting at the beginning of a block.
The tool can be accelerated over multiple blocks.

Feedrate Feedrate control by look–ahead

bell–shaped acceleration/ dec-
eleration before interpolation
Specified feedrate

Time
N1 N2 N3 N4 N5

FANUC Series 16i /18i -TA/TB

When the distance required to decelerate the tool from a specified feedrate is less than the total
travel of the tool in the blocks read in advance, the feedrate is automatically clamped to a
feedrate from which the tool can be decelerated to a feedrate of zero.

Feedrate Feedrate control by look–ahead

bell–shaped acceleration/ dec-
eleration before interpolation
Specified feedrate

Clamp
Feedrate

Total travel of the

tool in the blocks
read in advance

Time

When several blocks, each specifying a short travel, are specified in succession, the following
situation can occur:
The total travel of the tool in the blocks read in advance at the start of acceleration is less than
the distance required to decelerate the tool from a specified feedrate, but the total travel of the
tool in the blocks read in advance at the end of acceleration is greater than the distance required
to decelerate the tool from a specified feedrate.
In such a case, the tool is accelerated once and clamped to the feedrate obtained based on the
total travel of the tool in the blocks read in advance.
Then, the tool is accelerated to a specified target feedrate.

(1) At the start of acceleration

Feedrate Feedrate control by look–ahead

bell–shaped acceleration/ dec-
eleration before interpolation
Specified feedrate

Clamp
feedrate

Total travel of the

tool in the blocks
read in advance

Time

FANUC Series 16i /18i -TA/TB

Feedrate Feedrate control by look–ahead

bell–shaped acceleration/ dec-
eleration before interpolation
Specified feedrate

Clamp
feedrate

Total travel of the

tool in the blocks
read in advance at
the end of acceleration
Time

• Feedrate command and feedrate

If an F command is changed by, for example, another F command, the corner deceleration
function, or the automatic feedrate determination function, look–ahead bell–shaped
acceleration/deceleration before interpolation treats the changed feedrate as a new target
feedrate, and restarts acceleration/deceleration.
Whenever an F command is changed, bell–shaped acceleration/decelera-tion is performed.
Bell–shaped acceleration/deceleration is performed each time a different feedrate command is
specified, for example, in a program containing
successive blocks, each specifying a short travel.

Feedrate
Feedrate control by look–ahead
bell–shaped acceleration/ dec-
eleration before interpolation
Specified feedrate

Time

FANUC Series 16i /18i -TA/TB

(1) While applying constant or increasing acceleration

Starting at the point where the feed hold function is specified, the acceleration is gradually
reduced to 0. Then, the feedrate for the tool is gradually reduced to 0. Thus, the feed hold
function does not always immediately reduce the feedrate of the tool; it instead may
sometimes increase the feedrate for a brief instant before reducing the feedrate.

(2) While applying decreasing acceleration

First, the acceleration is gradually reduced to 0. Then, the feedrate is gradually reduced to 0.

(2) Deceleration
The tool is decelerated to the feedrate specified for a block, starting at the previous block.
The tool can be decelerated over multiple blocks.
Feedrate control by look–ahead
Feedrate bell–shaped acceleration/ dec-
Deceleration start point eleration before interpolation
Specified feedrate

Deceleration start point

Time

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 39/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
• Feedrate command and deceleration
If an F command is changed by, for example, another F command, the corner deceleration
function, or the automatic feedrate determination function, look–ahead bell–shaped
acceleration/deceleration before interpolation treats the changed feedrate as a new target
feedrate, and restarts acceleration/deceleration.
Whenever an F command is changed, bell–shaped acceleration/deceleration is performed.
When the distance required to decelerate the tool from a specified feedrate is longer than the
total travel of the tool in the blocks read in advance, the feedrate is automatically clamped, as in
the case of acceleration.
Feedrate control by look–ahead
Feedrate bell–shaped acceleration/ dec-
eleration before interpolation
Specified feedrate

Clamp feedrate

Time

• Deceleration based on tool travel

The deceleration of the tool is started when the total travel of the tool in the blocks read in
advance is less than the distance required to decelerate the tool from the current feedrate.
When the total travel of the tool in the blocks read in advance increases at the end of
deceleration, the tool is accelerated.
When blocks specifying a short travel are specified in succession, the tool may be decelerated,
then accelerated, then decelerated, and so on, resulting in an unstable feedrate. In such a
situation, specify a smaller feedrate.

• Feed hold during deceleration

When the feed hold function is used during deceleration, control is performed as described
below.
(1) While applying constant or increasing deceleration
The point where the deceleration starts being reduced to 0 is shifted from the usually used
point (i.e., that used when feed hold is not applied) to ensure that the feedrate for the tool is
gradually reduced to 0.
(2) While applying decreasing deceleration
The deceleration is gradually reduced to 0, after which the feedrate is reduced to 0.

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 40/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
(3) Single block
When the single block function is specified while look–ahead bell–shaped
acceleration/deceleration before interpolation is used, control is performed as described below.

• While the tool is being accelerated or decelerated when the single block function is specified
(a) A + B ≤ Remaining travel for the tool in the block being executed when the single block
function is specified
The tool is gradually decelerated so that the feedrate is 0 upon completion of the execution
of the block that was being executed when the single block function was specified.

Feedrate

Single block function specified

A B

Time

A: Distance traveled before the tool reaches the specified feedrate from the current
acceleration/deceleration
B: Distance traveled before the feedrate falls to 0 from a feedrate to which no
acceleration/deceleration is applied

(b) A + B > Remaining travel for the tool in the block being executed when the single
block function is specified
The tool may be decelerated over multiple blocks until it stops.
How the tool is stopped is described later.

Feedrate

Single block function specified

A B

Time

A: Distance traveled before the tool reaches the specified feedrate with the current
acceleration/deceleration
B: Distance traveled until the feedrate falls to 0 from a feedrate to which no
acceleration/deceleration is applied

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 41/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
• While the tool is not being accelerated or decelerated when the single block function is
specified
(a) A + B ≤ Remaining travel for the tool in the block being executed when the single block
function is specified
The tool is gradually decelerated so that the feedrate is 0 upon completion of the execution
of the block that was being executed when the single block function was specified.
Feedrate

Single block function specified

Time

A: Distance traveled until the feedrate falls from the current feedrate value to 0

(b) A > Remaining travel of the tool in the block being executed when the single block
function is specified
The tool may be decelerated over multiple blocks until it stops.
How the tool is stopped is described later.
Feedrate

Single block function specified

Time

A: Distance traveled until the feedrate falls from the current feedrate value to 0

FANUC Series 16i /18i -TA/TB

The tool is decelerated (or accelerated) over multiple blocks until the feedrate becomes 0.

Feedrate

Single block function specified

Time

CAUTION
1 Depending on the stop point and remaining blocks, two or more
acceleration/deceleration operations may be performed.
2 When the single block function is specified, an acceleration /
deceleration curve recalculation is required while the tool is moving
along an axis. So, the tool is not always decelerated over the minimum
number of blocks before stopping.

(4) Dry run/feedrate override

When a change in the specification of the dry run function or feedrate override function results
in a change in the specified feedrate (feedrate change due to an external cause) while look–
ahead bell–shaped acceleration/ deceleration before interpolation is being used, control is
performed as described below.

• While the tool is being accelerated or decelerated when the specification of the dry run function
or feedrate override function is changed
After the current acceleration/deceleration operation brings the tool to a specified feedrate and
is terminated, the tool is accelerated or decelerated to the new target feedrate.

• While the tool is not being accelerated or decelerated when the specification of the dry run
function or feedrate override function is changed
The tool is accelerated or decelerated from the current feedrate to the specified feedrate.

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 43/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
(5) Caution
CAUTION
1 When the specification of the dry run function or feedrate override
function is changed, the acceleration/deceleration curve must be
recalculated while the tool is actually moving along an axis. For this
reason, there will be a slight delay before a feedrate change is actually
started after the specification of the dry run function or feedrate
override function is changed.
2 When the specification of the dry run function or feedrate override
function is changed, the tool may be decelerated to below a specified
feedrate and then accelerated, depending on the remaining amount of
travel, current feedrate, and target feedrate.

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 44/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
2.16.4 Look–ahead bell–shaped acc/deceleration before interpolation
(acceleration variable time constant type)
To use this function, please set “1” in parameter No.1603#3(SBL) in addition to setting the
bell-shaped acc/deceleration of acceleration valiable ratio constant type.

• Difference with acceleration variable ratio constant type

Control method of acceleration

In an acceleration variable ratio constant type, the variable ratio of the acceleration is fixed. On
the other hand, the change time of the acceleration is fixed in this bell-shaped acc/deceleration.
The acceleration will change for a fixed time of setting in the parameter No.8416 when the
deceleration occurs while accelerating. Therefore, the variable ratio of change of the
acceleration becomes not constant.

Bell-shaped acc/decceleration
of this method
Feedrate t Bell-shaped acc/decceleration
of acceleration variable ratio
2t constant type
t Time constant of bell-shaped
acc/deceleration

Time

When the feedrate is changed

In an acceleration variable ratio constant type, the bell-shaped acc/deceleration is done every
time the feedrate is changed by the F command and the corner deceleration function and the
automatic feedrate control function..
On the other hand, the bell-shaped acc/deceleration is not done in the block without a distance
enough to reach the changed feedrate in this bell-shaped acc/deceleration.

Bell-shaped acc/decceleration
Feedrate of this method
Bell-shaped acc/decceleration
of acceleration variable ratio
constant type

Time

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 45/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
When the pre-reading block becomes insufficient
In an acceleration variable ratio constant type, the deceleration is done until the speed becomes
0 once when the pre-reading block becomes insufficient.
On the other hand, when the pre-reading block becomes insufficient, the deceleration is done,
however, acceleration is done at once in this bell-shaped acc/deceleration when the pre-reading
block increases while decelerating.

Bell-shaped acc/decceleration
of this method
Bell-shaped acc/decceleration
of acceleration variable ratio
constant type

Feedrate

Time

FANUC Series 16i /18i -TA/TB

2.17.1 Outline
This function reads several tens of blocks ahead to exercise automatic feedrate control in HPCC
mode.

A feedrate is determined on the basis of the conditions listed below. If a specified feedrate
exceeds a calculated feedrate, acceleration/deceleration before interpolation is used so that the
calculated feedrate can be established.
(1) Feedrate change and specified allowable feedrate difference along each axis at a corner
(2) Anticipated acceleration and specified allowable acceleration along each axis
(3) Cutting load change anticipated from the direction of motion along the Z–axis

Specified tool path

Machining error reduced
due to deceleration
based on an allowable Tool path when fee-drate
feedrate difference control is not used
Tool path when fee-drate
control is used

Machining error reduced due to

deceleration based on an allowable
acceleration

Fig. 2.17.1 (a)

To use this function, set bit 0 (USE) of parameter No. 8451 to 1, and set the following
parameters:

Parameter No. 8410: Allowable feedrate difference used for feedrate determination, based
on a corner feedrate difference
Parameter No. 8475, bit 2 (BIP) = 1: Enables deceleration at a corner.
Parameter No. 8470: Parameter specifying an allowable acceleration for feedrate
determination, based on acceleration
Parameter No. 8459, bit 1 (CTY) = 1, bit 0 (CDC) = 0
Parameter No. 8464: Initial feedrate for automatic feedrate control
Parameter No. 8465: Maximum allowable feedrate for automatic fee-drate control

For details, see the description of each parameter.

FANUC Series 16i /18i -TA/TB

(a) The feedrate required at a corner is calculated from the specified feedrate difference at the
corner along each axis, the tool being decelerated to the calculated feedrate at the corner.

Example
N1 Specified
Y feedrate

N2
X
N1 N2 N3 t
N3

(b) The feedrate required in a block is calculated from the specified acceleration along each
axis at the start point and end point of the corner, the tool being decelerated so that the
feedrate in the block does not exceed the calculated feedrate.

Example N2 N3
N1 N4
Specified
Y feedrate
N5
X N8 N6
N7 N1 N2 N3 N6 N7 N8 t

(c) The feedrate required in a block is calculated from the angle of downward movement along
the Z–axis, the tool being decelerated so that the feedrate in the block does not exceed the
calculated feedrate.

Example
Specified
Z N1 N2 feedrate

X
N3 N1 N2 N3 t

FANUC Series 16i /18i -TA/TB

• Example
Suppose that the specified feedrate for the tool is 1,000 mm/min, and that the direction of tool
movement changes by 90 degrees (from along the X–axis to along the Y–axis). Suppose also
that an allowable feedrate difference of 500 mm/min is set. Then, the tool will decelerate as
shown below.

N1 G01 G91 X100. F1000 ;

N2 N2 Y100. ;

N1
Tool path when the tool
does not decelerate at
the corner

←Tool path when the tool decelerates at the

corner

Feedrate
F1000
When the tool does not
decelerate at the corner
Feedrate along the
X–axis When the tool decelerates at
F500 the corner

Feedrate Time

F1000

Feedrate along the

Y–axis

F500

Feedrate N2 Time

F1000

Feedrate along
the tangent to the
path
F500

N1 N2 Time

Fig. 2.17.1(a) Example of deceleration by deference of each axis feedrate

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 49/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
2.17.3 Feedrate determination based on acceleration along each axis
As shown below, when a curve is formed by very short successive line segments, there is no
significant feedrate difference along each axis at each corner. Consequently, the tool need not
be decelerated to compensate for feedrate differences. When taken as a whole, however,
successive feedrate differences generate a large acceleration along each axis.
In this case, the tool must be decelerated to minimize the stress and strain imposed on the
machine, as well as the machining error that may result from such excessive acceleration.
The decelerating speed is a feedrate by which the acceleration of each axis of all axes becomes
below a permissible acceleration which is set by parameter No.8470..
The deceleration speed is determined at each corner. The deceleration speed is calculated
respectively of the starting point and the end point of the block, and the speed in the small
becomes an actual feedrate.

• Example
In the example shown below, the tool is accelerated too quickly from N2 to N4 and from N6 to
N8 (as indicated by the dashed–line inclinations in the feedrate graphs) when automatic
feedrate control is not used. So, the tool is decelerated.

N8
N7 N9
N6

N5
Y
N1
X N4
N3
N2

Feedrate along
the X–axis

Feedrate along
the Y–axis

Feedrate along
the tangent to
the path
N1 N5 N9 N1 N5 N9

Fig. 2.17.3 (a) Example of feedrate determination based on acceleration

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 50/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
2.17.4 Feedrate determination based on an allowable acceleration during circular
interpolation
When a block specifies circular feed per minute and bit 3 (CIR) of parameter No. 8475 is set to
1, the feedrate of the tool is automatically determined so that the acceleration along each axis
does not exceed an allowable acceleration.
The allowable acceleration is determined from the maximum cutting feedrate (set in parameter
No. 1432, No. 1430, or No. 1422) and the time needed to reach the maximum cutting feedrate
(set in parameter No. 8470).
During circular interpolation, the tool is controlled so that it always moves along the path at the
specified feedrate. At this time, the feedrate is clamped so that a synthetic acceleration of two
axes of circular interpolation should not exceed the small of permissible accelerations of each
axis.

2.17.5 Feedrate determination based on cutting load

This function can be used when bit 4 (ZAG) of parameter No. 8451 is set to 1.

Fig. 2.17.5 (a) When the tool is moving up along the Z–axis

Fig. 2.17.5 (b) When the tool is moving down along the Z–axis

Cutting the workpiece with the end of the cutter (Fig. 2.17.5 (b)) incurs a greater resistance than
when cutting the workpiece with the side of the cutter (Fig. 2.17.5 (a)). Therefore, for (Fig.
2.17.5 (b)), the tool must be decelerated. To calculate the required degree of feedrate
deceleration, the automatic feedrate control function uses the angle of downward movement of
the tool along the Z–axis.
When the tool is moving down along the Z–axis, the angle (θ) of downward movement formed
by the XY plane and cutter path is as shown in the Fig. 2.17.5 (b). The angle of downward
movement is divided into four areas, with an override value for each area specified in a
parameter, as follows:
Area 2: Parameter No. 8456
Area 3: Parameter No. 8457
Area 4: Parameter No. 8458

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 51/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
No override parameter is provided for area 1; the override value for area 1 is always 100%. A
feedrate determined with a separate feedrate control function is multiplied by the override value
specified for the area to which the angle θ of downward movement belongs.
Area 1: 0˚ ≤ θ < 30˚
Area 2: 30˚ ≤ θ < 45˚
Area 3: 45˚ ≤ θ < 60˚
Area 4: 60˚ ≤ θ ≤ 90˚

XY plane

30° Area 1
90°
60°
Area 4 45°
Area 3 Area 2

CAUTION
1. Mounting direction of the tool should be parallel to Z axis to use this
function. Therefore, this function might not be able to be applied
according to the structure of the machine.
2. The feedrate determination function that is based on cutting load
uses an NC command to determine the direction of movement along
the Z–axis. This means that the direction of movement along the Z–
axis cannot be found if the movement along the Z–axis is subject to
manual intervention with manual absolute on/off function set to on,
or if the mirror image function is used with the Z–axis. So, never use
these functions when using feedrate determination based on
cutting load.

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 52/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
2.17.6 Ignoring F code commands
In a block for which the automatic feedrate control function is enabled, the ignoring of all feed
commands (F commands) can be specified by setting bit 7 (NOF) of parameter No. 8451. The
feed commands are:
(1) Modal F command specified before a block for which the automatic feedrate control
function is enabled
(2) Modal F command and F command specified in a block for which the automatic feedrate
control function is enabled
Note, however, that specified F commands and modal F commands are stored in the CNC.
This means that in a block for which the automatic feedrate control function is disabled, a
modal F command of (1) or (2) is used instead of a modal F command calculated by the
automatic feedrate control function.

2.17.7 Override to determined feedrate

The spesifications of oveeride to the feedrate which determined besed on a feedrate difference
along each axis or acceleration along each axis, etc. is as follows.
· When a parameter OVR of No.8459#3 is set “0”.
Override is invalid to the deceleration function of the deceleration according to the speed
difference and the acceleration etc.
· When a parameter OVR of No.8459#3 is set “1”.
Override is effective to the deceleration function of the deceleration according to the speed
difference and the acceleration etc.
When a parameter OVR of No.8459#3 is set “1”, override becomes effective for the following
feedrate.
· Feedrate which determined based on a feedrate difference along each axis.
· Feedrate which determined based on acceleration along each axis.
· Feedrate which determined based on an allowable acceleration during circular interpolation.
· Maximum feedrate of automatic feedrate control function.

Maximum cutting feedrate (parameter No.1422 or No.1430 or No.1432) is never exceeded

even when override is effective.

2.17.8 Other conditions of feedrate determination

If a calculated feedrate exceeds the maximum allowable feedrate for automatic feedrate control,
specified in parameter No. 8465 or with an F command, the feedrate is clamped to the
maximum allowable feedrate or F command, whichever is smaller.

FANUC Series 16i /18i -TA/TB

3.1 Parameters of look–ahead acceleration and deceleration before interpolation

#7 #6 #5 #4 #3 #2 #1 #0
8402 BDO DST BLK NBL

[Data type] Bit

BDO,NBL Set the type of acceleration/deceleration before interpolation.

BDO NBL Meaning

0 0 Acceleration/deceleration prior to interpolation is of linear
type
1 1 Acceleration/deceleration prior to interpolation is of bell-
shape type

BLK Be sure to set to 0.

DST Be sure to set to 1.

3.1.1 Linear acceleration and deceleration before interpolation

8400 Parameter 1 for determining a linear acc/deceleration before interpolation

[Data type] Two-word

[Unit of data, Valid data range]
Valid data range
Increment system Unit of data
IS-B IS-C
Millimeter machine 1 mm/min 10—60000 1--6000
Inch machine 0.1 inch/min 10—60000 1--6000
Rotation axis 1 deg/min 10—60000 1--6000

This parameter determines a linear acceleration and deceleration before interpolation. Usually, set the
maximum cutting speed (parameter No.1422).

8401 Parameter 2 for determining a linear acc/deceleration before interpolation

[Data type] Word

[Unit of data] 1ms
[Valid data range] 0 to 4000

This parameter specifies the time required until the speed specified in parameter 1 is achieved.
Speed
Acceleration
Parameter 1

Time
Parameter 2

NOTE
The function for linear acceleration/deceleration before interpolation is
canceled when either parameter no. 8400 or 8401 is set to 0.

FANUC Series 16i /18i -TA/TB

8400 Parameter 1 for determining a linear acc/deceleration before interpolation

[Data type] Two-word

This parameter determines a linear acceleration and deceleration before interpolation. Usually, set the
maximum cutting speed (parameter No.1422).

8401 Parameter 2 for determining a linear acc/deceleration before interpolation

[Data type] Word

[Unit of data] 1ms
[Valid data range] 0 to 4000

The data set by parameter 1 and parameter 2 becomes a maximum acceleration of bell-shaped
acc/deceleration.
Speed
Acceleration
Parameter 1

Time
Parameter 2

#7 #6 #5 #4 #3 #2 #1 #0
1603 SBL

[Data type] Bit

SBL The type of bell-shaped acc/deceleration before interpolation is

0: acceleration variable ratio constant type.
1: acceleration variable time constant type.

When an acceleration variable time constant type is selected, data range which can be set in
parameter No.8416 becomes 400ms or less.

FANUC Series 16i /18i -TA/TB

[Data type] Two-word

[Unit of data] 1ms
[Valid data range] 0 to 99999999 (When a parameter No.1603#3(SBL) is set to “0”) or
0 to 400 (When a parameter No.1603#3(SBL) is set to “1”)

● When an acceleration variable ratio constant type is selected. (parameter No.1603#3=0)

Acceleration

+ Max. Acceleration

Time

- Max. Acceleration

Set the same time

Speed

V t1: Time constant assumed in linear acc/deceleration

(ParameterNo.8401)

t2: Time for corner rounding (parameter No. 8416)

V: Speed to set acceleration time t1 (Parameter No. 8400)

Usually set the max. cutting speed.

Total time =T
Time of linear part = T – 2 * t2
Time Time of curved part = t2
t1
When target speed is different, total time also changes
t2 t2 (constant acceleration).

FANUC Series 16i /18i -TA/TB

The “tb” of the figure below is set in this parameter. It becomes a linear acc/deceleration before interpolation
when “0” is set.

Speed Linear acc/deceleration

Bell-shaped acc/deceleration

ta Depends on a acceleration of
linear acc/deceleration.
tb Time constant of bell-shaped
acc/deceleration
tc Acc/decelerating time of bell-
shaped acc/deceleration.

tc = ta + tb

“ta” depends at not constancy but the

instruction speed.

tb tb tb Time
tb Specified feedrate
ta =
Accelerati on of linear acc/decele ration
ta ta

tc tc
tb is constant.

Acceleration
tb tb

Time

tb tb
ta ta

tc tc

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 57/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
3.2 Automatic feedrate control function
8410 Allowable velocity difference in velocity determination considering the
velocity difference at corners

[Data type] Word axis

If zero is specified for all axes, the machine does not decelerate at corners.
When the function for determining the velocity considering the velocity difference at corners is used, the
system calculates the feedrate whereby a change in the velocity element of each axis does not exceed this
parameter value at the interface between blocks. Then the machine decelerates using acceleration/
deceleration before interpolation.

#7 #6 #5 #4 #3 #2 #1 #0
8451 NOF ZAG USE

[Data type] Bit

USE Automatic velocity control is:

0 : Not applied.
1 : Applied.

ZAG The velocity is:

0: Not determined according to the angle at which the machine descends along the
Z–axis.
1: Determined according to the angle at which the machine descends along the
Z–axis.

NOF In a block where automatic velocity control is validated, the F command is:
0 : Validated.
1 : Ignored.
(Maximum speed of automatic feedrate control set by parameter No. 8465 is used for command
speed in spite of F command)

8452 Range of velocity fluctuation to be ignored

[Data type] Byte

[Unit of data] %
[Valid data range] 0 to 100 (Standard setting: 10)

FANUC Series 16i /18i -TA/TB

[Data type] Word

[Unit of data] %
[Valid data range] 0 to 100 (Standard setting: 80)

This parameter specifies an override in area 2 of velocity calculation considering the cutting
load.

8457 Area–3 override

[Data type] Word

[Unit of data] %
[Valid data range] 0 to 100 (Standard setting: 70)

This parameter specifies an override in area 3 of velocity calculation considering the cutting
load.

8457 Area–4 override

[Data type] Word

[Unit of data] %
[Valid data range] 0 to 100 (Standard setting: 60)

This parameter specifies an override in area 4 of velocity calculation considering the cutting
load.

#7 #6 #5 #4 #3 #2 #1 #0
8459 OVR CTY CDC

[Data type] Bit

CDC Be sure to set this value to 0.

CTY Be sure to set this value to 1.

OVR In the HPCC mode, override to determined feedrate by automatic feedrate control is
0: Not effective
1: Effective

When this parameter is set “1”, override becomes effective for the following feedrate.
· Feedrate which determined based on a feedrate difference along each axis.
· Feedrate which determined based on acceleration along each axis.
· Feedrate which determined based on an allowable acceleration during circular interpolation.
· Maximum feedrate of automatic feedrate control function.
Maximum cutting feedrate (parameter No.1422 or No.1430 or No.1432) is never exceeded
even when override is effective.

FANUC Series 16i /18i -TA/TB

[Data type] Two-word

[Unit of data, Valid data range]
Valid data range
Increment system Unit of data
IS-B IS-C
Millimeter machine 1 mm/min 10—240000 1—100000
Inch machine 0.1 inch/min 10—96000 1—48000
Rotation axis 1 deg/min 10—240000 1—100000

This parameter sets the initial feedrate for automatic feedrate control.
In automatic feedrate control, the initial feedrate set with this parameter is used at the beginning
if no F command is specified in the program.
Usually, set the maximum cutting feedrate (specified in parameter No. 1422).

8465 Maximum allowable feedrate for automatic feedrate control

[Data type] Two-word

This parameter sets the maximum allowable feedrate for automatic feedrate control. Usually, set
the maximum allowable cutting feedrate (set in parameter No. 1422).

8470
Parameter for determining allowable acceleration in feedrate
calculation considering acceleration

[Data type] Word axis

[Unit of data] msec
[Valid data range] 0 to 32767

When the function for calculating the feedrate considering the acceleration is used under
automatic feedrate control, this parameter is used to determine the allowable acceleration. The
time required until the maximum cutting feedrate is reached must be specified here.
Allowable acceleration is determined from the maximum cutting feedrate and the value set in
this parameter. Where, the maximum cutting feedrate is any of value set in parameter No. 1432,
1430 or 1422. Which parameter No. is used depends on the following conditions:
· When a value other than 0 is set to No. 1432, the value set to No. 1432 is used.
· When 0 is set to No. 1432 and a value other than 0 is set to No. 1430, the value set to No. 1430
is used.
· When 0 is set to No. 1432 and 1430, the value set to No. 1422 is used.
The shock of the machine and the processing error becomes small by setting this parameter
greatly.

FANUC Series 16i /18i -TA/TB

Max. cutting feedrate Allowable acceleration

(parameter No.1432, 1430,
or 1422)

Time
Parameter No.8470

#7 #6 #5 #4 #3 #2 #1 #0
8475 CIR BIP

[Data type] Bit

CIR The function of automatic feedrate control considering acceleration and deceleration during
circular interpolation is:
0: Not used.
1: Used.
When 1 is set, parameter No.8470 for determining the allowable acceleration must be specified.

BIP The function of deceleration at corners is:

0: Not used.
1: Used. (Always set 1.)

3.3 Axis control

7510 Maximum number of axes in High Precision Contour Control

[Data type] Byte

[Valid data range] 1, 2, 3, … to the maximum number of control axes

This parameter specifies the maximum number of axes to controlled by High Precision Contour
Control.
Example) Axis configuration is X, Z, C, Y, and A from the 1st axis in this order and to make
HPCC valid to the 4th axis (Y), set this parameter to 4. In this case, HPCC is also
effective for the X, Z, C axes.
X, Z, C, Y axes Axes on which HPCC is valid
A axis on which HPCC is not valid.

#7 #6 #5 #4 #3 #2 #1 #0
8480 RI2 RI1 RI0

[Data type] Bit

Set the interpolation frequency during the high precision contour control mode (HPCC mode).
Be sure to set the following values:
RI2 RI1 RI0 Interpolation
frequency
0 0 1 2ms

FANUC Series 16i /18i -TA/TB

[Data type] Bit

LS2 Acceleration/deceleration after interpolation for cutting feed in the high precision contour
control mode (HPCC mode) is:
0: Not used. (Exponential acceleration/deceleration)
1: Used. (The function for linear acceleration/deceleration after interpolation for cutting feed
is required.)

1768 Time constant for linear acceleration/deceleration during cutting feed in

HPCC mode

[Data type] Word

[Unit of data] msec
[Valid data range]
RI2 RI1 RI0 Data range
0 0 1 2 to 128

The range of data is different according to the command of (RI0,RI1,RI2) of parameter

No.8480.

3.5 Cutter compemsation C

#7 #6 #5 #4 #3 #2 #1 #0
5000 SBK

[Data type] Bit

SBK An internally created block for cutter compensation C:

0: Does not cause a single block stop.
1: Cause a single block stop.

#7 #6 #5 #4 #3 #2 #1 #0
5003 BCK ICK

[Data type] Bit

ICK In HPCC mode, when cutter compensation C interference check is:

0: Done
1: Not done

BCK In HPCC mode, when cutter compensation C interference check determines that the
programmed move direction differs from the offset move direction by between 90 and 270
degrees:
0: An alarm is issued.
1: No alarm is issued.

FANUC Series 16i /18i -TA/TB

[Data type] Bit

ICK In HPCC mode, smooth interpolation is:

0: Disabled
1: Enabled

8486 Maximum travel distance of a block where smooth interpolation is applied

[Data type] Two-word

[Unit of data]
Increment system IS-B IS-C Unit of
data
mm input 0.001 0.0001 mm
inch input 0.0001 0.00001 inch
[Valid data range] 0 to 99999999

This parameter specifies a block length used as a reference to decide whether to apply smooth
interpolation. If the line specified in a block is longer than the value set in the parameter,
smooth interpolation will not be applied to that block. This parameter can be used, for example,
to specify the maximum line length of a folded line to which a metal die workpiece is
approximated with some tolerance.

8487 Angle by which smooth interpolation is turned off

[Data type] Word

[Unit of data] 0.1°
[Valid data range] 0 to 32767
This parameter specifies an angle to judge whether to smooth interpolation shoud be executed.
When the block with larger angle difference than this value appears, a smooth interpolation is
turned off once.
When 0 is set, it is considered 10 degrees.

8490 Minimum travel distance of a block where smooth interpolation is applied

[Data type] Two-word

[Unit of data]
Increment system IS-B IS-C Unit of
data
mm input 0.001 0.0001 mm
inch input 0.0001 0.00001 inch
[Valid data range] 0 to 99999999

This parameter specifies a block length used as a reference to decide whether to apply smooth
interpolation. If the line specified in a block is shorter than the value set in the parameter,
smooth interpolation will not be applied to that block.

FANUC Series 16i /18i -TA/TB

[Data type] Word

[Unit of data]
Increment system IS-B IS-C Unit of
data
mm input 0.001 0.0001 mm
inch input 0.0001 0.00001 inch
[Valid data range] 0 to 32767

This parameter specifies a tolerance used as a reference to decide whether to apply smooth
interpolation. If the tolerance specified in a block is larger than the value set in the parameter,
smooth interpolation will not be applied to that block.

The tolerance is a distance of straight line L and curve C which instruction

points are smoothly connected.

Curve C

instruction points
Line L

tolerance

8492 Minimum tolerance of a block where smooth interpolation is applied

[Data type] Word

[Unit of data]
Increment system IS-B IS-C Unit of
data
mm input 0.001 0.0001 mm
inch input 0.0001 0.00001 inch
[Valid data range] 0 to 32767

This parameter specifies a tolerance used as a reference to decide whether to apply smooth
interpolation. If the tolerance specified in a block is smaller than the value set in the parameter,
smooth interpolation will not be applied to that block.
Please set the value of about 1/10 of the maximum tolerance (parameter No.8491) usually.
When 0 is set, 1/10 of the maximum tolerance (parameter No.8491) is assumed to be minimum
tolerance. When a negative value is set, the minimum tolerance is assumed to be 0.

FANUC Series 16i /18i -TA/TB

[Data type] Bit

G51 In high–precision contour control (HPCC) mode, scaling/coordinate system rotation is:
0: Disabled.
1: Enabled.

#7 #6 #5 #4 #3 #2 #1 #0
5400 SCR XSC RIN

[Data type] Bit

RIN Coordinate rotation angle command (R)

0: Specified by an absolute method
1: Specified by G90 or G91

XSC Axis scaling and programmable mirror image

0: Invalidated (The scaling magnification is specified by P.)
1: Validated

SCR Scaling magnification unit

0: 0.00001 times (1/100,000)
1: 0.001 times

#7 #6 #5 #4 #3 #2 #1 #0
5401 SCLx

[Data type] Bit

SCLx Scaling for every axis

0: Invalidated
1: Validated

5410 Angular displacement used when no angular displacement is specified for

coordinate system rotation

[Data type] Two-word

[Unit of data] 0.001°
[Valid data range] -360000 to 360000

This parameter sets the angular displacement for coordinate system rotation. When the angular
displacement for coordinate system rotation is not specified with address R in the block where
G68 is specified, the setting of this parameter is used as the angular displacement for coordinate
system rotation.

FANUC Series 16i /18i -TA/TB

[Data type] Two-word

[Unit of data] 0.001 or 0.00001 times (Selected using SCR, #7 of parameter No.5400)
[Valid data range] 1 to 999999

This parameter sets the scaling magnification. This setting value is used when a scaling
magnification (P) is not specified in the program.

NOTE) Parameter No.5421 becomes valid when scaling for every axis is valid. (XSC,
#6 of parameter No.5400 is “1”.)

5421 Scaling magnification for each axis

[Data type] Two-word axis

[Unit of data] 0.001 or 0.00001 times (Selected using SCR, #7 of parameter No.5400)
[Valid data range] 1 to 999999

This parameter sets the scaling magnification for each axis.

3.8 The other parameter

#7 #6 #5 #4 #3 #2 #1 #0
8403 SG0 MSU

[Data type] Bit

MSU When G00, or an M, S, or B code is specified in HPCC mode:

0: An alarm is issued.
1: The CNC executes the command.

SG0 When G00 is specified in HPCC mode:

0: The setting of bit 1 (MSU) of parameter No. 8403 is followed.
1: Executed in HPCC mode.

NOTE) Please set (STG) of parameter No.8404#0 in “1” when you set “1” in this
parameter.

#7 #6 #5 #4 #3 #2 #1 #0
8404 EIL STG

[Data type] Bit

STG Please set the same value as parameter 8403#7(SG0).

EIL In HPCC mode, each axis inter-lock is:

0: Not effective.
1: Effective.

FANUC Series 16i /18i -TA/TB

[Data type] Bit

G02 In HPCC mode, helical interpolation is:

0: Disabled.
1: Enabled.

#7 #6 #5 #4 #3 #2 #1 #0
8414 RRD

[Data type] Bit

RRD In the axis of the diameter programming, the program instruction in the HPCC mode is:
0: Radius programming
1: Diameter programming

When “1” is set in this parameter, the movement amount in the HPCC mode becomes twice of
usually operation.

#7 #6 #5 #4 #3 #2 #1 #0
8411 RDM RDR RDA

[Data type] Bit

RDM When a parameter No.8414#0(RRD) is “1”, the display of the machine coordinate system of the
actual position display is:
0: displayed by the diameter value.
1: displayed by the radius value.

RDR When a parameter No.8414#0(RRD) is “1”, the display of the relative coordinate system of the
actual position display is:
0: displayed by the diameter value.
1: displayed by the radius value.

RDA When a parameter No.8414#0(RRD) is “1”, the display of the absolute coordinate system and
distance to go of the actual position display are:
0: displayed by the diameter value.
1: displayed by the radius value.

FANUC Series 16i /18i -TA/TB

HPCC mode signal

MHPCC (F066#6)
[Classification] Output signal
[Function] Indicates that the system is set to high–precision contour control mode (HPCC mode).
[Output condition] The signal is set to 1 if G05 P10000 (HPCC mode ON) is specified in a program. The signal is
set to 0 if G05 P0 is specified in a program or if HPCC mode is canceled by a reset.

HPCC operation signal

EXHPCC (F066#7)
[Classification] Output signal
[Function] Indicates that the system is operating in high–precision contour control mode (HPCC operation
is in progress).
[Output condition] The signal is set to 1 if G05 P10000 (HPCC mode ON) is specified in a program and if
specifiable data of except G00 of Type-A(*1) and auxiliary function is executed.
The signal is set to 0 when:
(1) Automatic operation is halted.
(2) Automatic operation is stopped.
(3) HPCC mode is canceled.
(4) While executing the G00 instruction of type-A.
(5) While executing the block with auxiliary function (M code, S code, or second auxiliary
function).
(6) While executing the block with subprogram call.
(7) When either address U, V, W, or H is specified in G code system B or C.
(8) When the axis which HPCC is not effective(*2) is instructed.

When this signal is "0", the blinking display of "HPCC" under the right of the screen is not
done.

(*1) Please refer to section 2.7.

(*2) Please refer to description of parameter No.7510 (section 3.3).

Siganl addresses

#7 #6 #5 #4 #3 #2 #1 #0
F066 EXHPCC MHPCC

FANUC Series 16i /18i -TA/TB

Number Message Description

10 IMPROPER G–CODE · There is no option of the corresponding function.
· An unusable G code G is specified.
· The following instructions are commanded in G00
mode.
G50 / G51 (Scaling)
G68 / G69 (Coordinate system rotation)
G50.1 / G51.1 (Programmable mirror image)
G05.1 Q2 (Smooth interpolation)
G06.2 (NURBS interpolation)
· G05 P10000 was commanded in in the MDI mode.
5000 ILLEGAL COMMAND · The instruction (G code and T code, etc.) which was
CODE (HPCC) not able to be used in HPCC mode was commanded.
· The instruction for an axis with parameter No.1006#3
(DIA) and No.8414#0 (RRD) is set “1” is commanded.
· The interrupt type custom macro was started in HPCC
mode.
· The instruction that the EXHPCC signal becomes 0 in
either of scaling, the coordinate rotation or the
programmable mirror image mode was commanded.
5003 ILLEGAL PARAMETER The parameter setting is incorrect.
(HPCC)
5004 HPCC NOT READY High–precision contour control is not ready.

5006 TOO MANY WORD IN The number of words specified in a block exceeded 26
ONE BLOCK in the HPCC
5012 G05 P10000 ILLEGAL G05 P10000 has been specified in a mode from which
START UP HPCC mode cannot be entered.
5013 HPCC:CRC OFS REMAIN · G05 P0 was commanded with in the G41/G42 mode or
AT CANCEL the amount of the offset remained.
· G05 P0 was instructed in in G51.1 (programmable
mirror image) mode.
5115 SPL:ERROR In the NURBS interpolation,
· There is an error in the specification of the rank.
· No knot is specified.
· The knot specification has an error.
· The number of axes exceeds the limits.
· Other program errors
5116 SPL:ERROR In the NURBS interpolation,
· There is a program error in a block under look–ahead
control.
· Monotone increasing of knots is not observed.
· A mode that cannot be used together is specified.
5117 SPL:ERROR The first control point of NURBS is incorrect.
5118 SPL:ERROR After manual intervention with manual absolute mode
set to on, NURBS interpolation was restarted.
5196 ILLEGAL OPERATION The control axis detaching was done in HPCC mode.
(HPCC) After the block being executed now ends, this alarm is
generated if the control axis detaching is done in HPCC
mode.
5313 G05 P0 COMMANDED IN G05 P0 was commanded in the coordinate system
G68.1/G51 rotation or in the scaling mode.
5314 SMOOTH IPL ERROR 1 The mistake is found in the format of smooth
interpolation block.

FANUC Series 16i /18i -TA/TB

6.1 Notes on operation

Interlock
(1) The interlock signal for each axis and direction is not effective in HPCC operation.
(2) Please set “1” in parameter No.8404#7(EIL) to make each axis interlock signal effective in
HPCC operation.

Each axis machine lock and mirror image

Neither the mirror image by the signal, the mirror image by the setting nor the each axis
machine lock immediately become effective even if they changes in HPCC operation. Please
switch them before HPCC is turned on.

Pocket calculator type decimal point input

Pocket calculator type decimal point input (parameter No.3401#0(DPI)) is not effective in
HPCC operation.

Single block
The block of G05 P10000 does not stop in a single block.

External deceleration and automatic corner override

An external deceleration and automatic corner override are invalid in HPCC operation.

MDI operation
It is not possible to operate by switching to the MDI mode in HPCC mode. The edit of the MDI
operation is prohibited in HPCC mode. Moreover, the alarm of P/S010 is generated if cycle-
start is applied without inputting the program.
Moreover, it is not possible to instruct in a HPCC in the MDI mode.(An alarm of P/S010 is
generated.)

Program restart function

The program which includes G05 P10000 cannot be used program restart function.

6.2 Notes on programming

Cooredinate systen rotation, scaling, programmable mirror image, NURBS interpolation and
smooth intrpolation
When Cooredinate systen rotation (G68/G69), scaling(G50/ G51), programmable mirror image
(/G50.1/G51.1), NURBS interpolation(G06.2) and smooth intrpolation(G05.1Q2) are used in
the HPCC mode, a modal G code of group 01 when these instructions are executed should be
G01,G02 or G03. (The P/S010 alarm is generated) Moreover, please command these functions
to become a nest between G05 P10000-G05 P0.

Cutter compensation C
It is not possible to command reference point return (G28) in HPCC mode. Therefore, the
instruction by which the offset is temporarily canceled cannot be commanded.

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 70/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
Positioning or auxiliary function and cutter compensation C
When the G00 of Type-A or the auxiliary function is executed in the cutter compensation mode,
the offset vector made in the block before of that is held.

Exapmle 1 ) When the undermentioned program is executed, the starting point of N6 is decided
by the vector made with N3 and N4.
N5
N1 N2 N3 N4 N6

This vector is used as the

vector between N4 and N6.
N8

Programmed path O0001 ;

G50 X-10. Y-20. ;
Tool path G05 P10000 ;
N1 G01 G42 X0 D1 F1000 ;
An incorrect offset N2 X20. ;
value is used in this N3 X40. Y0 ;
range. N4 X60. Y20. ;
N5 M01 ;
N6 X80. ;
N7 X90. Y-20. ;
N8 G40 Y-50. ;
G05 P0 ;

Example 2 ) When the undermentioned program is executed, the starting point of N5 is decided
by the vector made with N3 and N4.
If (SG0) of parameter No.8403#7 is set in one, the intersection vector of N4 and
N5 is correctly obtained.

N1 N2 N3 N4 N5

This vector is used as the vector

between N4 and N5, and N5 and N6.
N7

Programmed path O0001 ;

G50 X-10. Y-20. ;
Tool path G05 P10000 ;
N1 G01 G42 X0 D1 F1000 ;
N2 X20. ;
An incorrect offset
N3 X40. Y0 ;
value is used in this N4 X60. Y20. ;
range. N5 G00 X80. ;
N6 X90. Y-20. ;
N7 G40 Y-50. ;
G05 P0 ;

FANUC Series 16i /18i -TA/TB

6.4 Automatic feedrate control

Maximum feedrate
If the upper limit for automatic feedrate control is set to 0 in parameter No. 8465, no feedrate
exceeding 0 is permitted, such that the issue of an F command causes an alarm of P/S011. To
prevent this, specify a value other than zero in the parameter.

Override
If the override is changed while the automatic feedrate control function is enabled, the
calculated clamp feedrate is overridden.

6.5 Multi path

It is possible to command a HPCC only in the 1st path. The alarm of P/S010 is generated when
it was commanded in other path.

6.6 Angular axis control

Rapid feedrate
In Type-B of rapid traverse, the feedrate of the straight axis occasionally exceeds the value of
parameter No.1420 if the movement instruction of the straight axis and slope axis are
commanded in the same block. The maximum value can be calculated by the following
expressions.

Actual feedrate of straigth axis (max. value) = Fx + Fy * tanθ

Fx : Parameter No.1420 of straight axis.

Fy : Parameter No.1420 of slope axis.
θ : Parameter No.8210.

Automatic feedrate control

In the velocity control of HPCC, the speed clamping etc. are done based on the speed difference
and the acceleration in program coordinate system. Therefore, please set the value by which the
value in mechanical system is converted into the value in program coordinate system when you
set the parameter concerning the acceleration and the speed.

6.7 Manual handle interruption

Parameter setting
Please set “1” in parameter No.7100#2(IHD) when you use the manual handle interruption for
the axis of the angular axis control in the HPCC mode.

6.8 Rotary axis 02

The Rotary Axis Control Function 02

The optional Rotary Axis Control Function is not available in HPCC mode. 02

FANUC Series 16i /18i -TA/TB

Title Specifications of High-Precision Contour
Control forComplex Lathe
Draw
No.
A-78395E
02 2001.10.04 Description of Cs axis and rotary axis are added.
Edit Date Design Description Sheet 72/75
Date 2001.02.14 Desig. A.Fukumoto Apprv.
7 The function table which can be used by a high-precision contour control
The function excluding this cannot be used.
Item Specifications Remarks

Controlled axis
Controlled axis 2 axes
Controlled path 1 path
Simultaneously controlled axes 2 axes
Controlled axis expansion(total) Max. 8 axes
Simultaneously controlled axes Max. 6 axes
expansion(total)
Axis control by PMC The axis of HPCC cannot command by PMC in HPCC mode
Angular axis control, Arbitrary angular The feedrate control is done in the program coordinate system.
axis control
Cs contouring control In the instruction in Cs axis in the HPCC mode, the advanced
feedforward control is canceled once.
Simple spindle synchronous control Only for 1 path system
Axis recomposition Only for 2 path system
Synchronous control can not be used. Only Cs axis is possible
the composite control.
Axis name In case of G code system A,
basic 2 axes are X and Z, additional
axes are optional from Y,A,B and
C.
In case of G code system A,
basic 2 axes are X and Z, additional
axes are optional from
Y,U,V,W,A,B and C.

Least input increment 0.001mm,0.001deg,0.0001inch

increment system 1/10 0.0001mm,0.0001deg,0.00001inch
Inch/metric conversion The inch/metric mode cannot be switched in the HPCC mode.
Interlock All axes, each axis
Machine lock All axes, each axis The each axis machine lock signal cannot be changed in the
HPCC mode.
Emergency stop
Stored stroke check 1
Stored stroke check 2 G22/G23 can not be commanded in the HPCC mode. (Become
P/S5000 alarm) Please instruct them before the HPCC is turned
on.
Mirror image The state cannot be changed in the HPCC mode.
Backlash compensation for each
rapid traverse and cutting feed
Manual handle interruption Please set parameter 7100#2(IHD) to “1” when the angular axis
control or arbitrary angular axis control is used..

Operation
Automatic operation
Cycle start / feed hold
Program stop / Program end
Reset
Dry run
Single block

FANUC Series 16i /18i -TA/TB

Interpolation function
Positioning G00
Linear interpolation G01
Circular interpolation G02,G03
Helical interpolation Circular interpolation plus max. 2 The option of helical interpolation is necessary.
axes linear interpolation
Smooth interpolation G05.1 Q2 Only in the HPCC mode.
NURNS interpolation G06.2 Only in the HPCC mode.

Feed function
Feed per minute G94(G98)
Cutting feedrate clamp
Linear acceleration/deceleration after This is an optional function.
cutting feed interpolation
Bell-shaped acceleration/deceleration This is an optional function.
after cutting feed interpolation
Feedrate override 0～254% 1% Step
2nd Feedrate override 0～254% 1% Step This is an optional function.
Linear acceleration/deceleration
before look ahead interpolation
Bell-shaped acceleration/deceleration
before look ahead interpolation

Program input
Tape code EIA/ISO automatic recognition
Program format Word and address format
Control in/out
Optional block skip
Absolute/incremental programming G90/G91
Input unit 10 time multiply
Plane selection G17,G18,G19
Rotary axis roll-over
Manual absolute on and off FS15 specification
Programmable data input G10 The HPCC mode is automatically canceled once, and buffering is
stopped.
External sub program call M198 The HPCC mode is automatically canceled once, and buffering is
stopped.
Sub program call M98 The HPCC mode is automatically canceled once, and buffering is
stopped.
Circular interpolation by R
programming
Scaling G50,G51 Alarm (P/S5012) is generated if turned on or off of HPCC is
commanded in scaling mode(G51).
The scaling mirror image by a negative magnification instruction
cannot be done.
Coordinate system rotation G68,G69 Alarm (P/S5012) is generated if turned on or off of HPCC is
commanded in coordinate system rotation mode(G68).
Programmable mirror image G50.1,G51.1 Alarm (P/S5012) is generated if turned on or off of HPCC is
commanded in programmable mirror image mode(G51.1).

FANUC Series 16i /18i -TA/TB

Auxiliary/Spindle speed function

Auxiliary function It is necessary to set “1” in parameter No.8403#1 (MSU). The
HPCC mode is automatically canceled once when instructing in
the auxiliary function, and buffering is stopped.
2nd auxiliary function It is necessary to set “1” in parameter No.8403#1 (MSU). The
HPCC mode is automatically canceled once when instructing in
the 2nd auxiliary function, and buffering is stopped.
Multiple command of auxiliary Max.3 It is necessary to set “1” in parameter No.8403#1 (MSU). The
function HPCC mode is automatically canceled once when instructing in
the auxiliary function, and buffering is stopped.
Spindle speed function It is necessary to set “1” in parameter No.8403#1 (MSU). The
HPCC mode is automatically canceled once when instructing in
the spindle speed function, and buffering is stopped.

Tool function/Tool compensation

Cutter compensation C G39,G40,G41,G42 If the instruction that the HPCC mode is automatically canceled
once (auxiliary function etc.) is commanded, the vector is held
because Buffering is stopped

FANUC Series 16i /18i -TA/TB

MML Reference Pro3 Eng
No ratings yet
MML Reference Pro3 Eng
153 pages
FANUC 16i-18i-21i-MODEL B
No ratings yet
FANUC 16i-18i-21i-MODEL B
13 pages
FANUC Series 0 / 00: Remote Buffer
No ratings yet
FANUC Series 0 / 00: Remote Buffer
79 pages
Fourth-Axis Beta-I Drive Kit User Manual B-165A
No ratings yet
Fourth-Axis Beta-I Drive Kit User Manual B-165A
20 pages
Procedura Settaggio Ethernet Per 30i
No ratings yet
Procedura Settaggio Ethernet Per 30i
30 pages
Fanuc Oi-MF Datasheet
No ratings yet
Fanuc Oi-MF Datasheet
2 pages
01022E B61863E-13-5 SA1 SB7 Programming Manual
100% (2)
01022E B61863E-13-5 SA1 SB7 Programming Manual
145 pages
FD Tial: Servicetechnical Report
100% (1)
FD Tial: Servicetechnical Report
11 pages
Qx522 Mitsubishi Manual
100% (1)
Qx522 Mitsubishi Manual
81 pages
How To Use Memory Card As Program Memory: FANUC Series 30 /31 /32 - Model B FANUC Series 0 FANUC Series 0
No ratings yet
How To Use Memory Card As Program Memory: FANUC Series 30 /31 /32 - Model B FANUC Series 0 FANUC Series 0
21 pages
Fanuc 31i-BM Standard Features and Options
No ratings yet
Fanuc 31i-BM Standard Features and Options
11 pages
Fanuc PM
No ratings yet
Fanuc PM
26 pages
Fanuc 0i - 0imate Model B - Alarm List
100% (1)
Fanuc 0i - 0imate Model B - Alarm List
77 pages
Ib1500034e PDF
No ratings yet
Ib1500034e PDF
293 pages
M520A RS-232 Procedure
100% (1)
M520A RS-232 Procedure
12 pages
M70-700 4th or 5th Axis Install Procedure
No ratings yet
M70-700 4th or 5th Axis Install Procedure
5 pages
Gv-500&780 Operation Manual 04 Ver
No ratings yet
Gv-500&780 Operation Manual 04 Ver
395 pages
ES400 F 21iMB Mag Zero Set 033007
No ratings yet
ES400 F 21iMB Mag Zero Set 033007
3 pages
FANUC 5-Axis Tool Control Guide
No ratings yet
FANUC 5-Axis Tool Control Guide
47 pages
62543en1 PDF
100% (1)
62543en1 PDF
519 pages
Mitsubishi Manuals 924 PDF
0% (1)
Mitsubishi Manuals 924 PDF
46 pages
Fanuc 31i-BM Standard Features and Options PDF
No ratings yet
Fanuc 31i-BM Standard Features and Options PDF
10 pages
CNC M500 RS-232 Backup Procedure
No ratings yet
CNC M500 RS-232 Backup Procedure
10 pages
PLC Ladder Diagram Guide
No ratings yet
PLC Ladder Diagram Guide
672 pages
Basic CNCPMC Interfacing Manual
No ratings yet
Basic CNCPMC Interfacing Manual
137 pages
910-911-914-915 Fanuc Ram Parity Alarm
100% (1)
910-911-914-915 Fanuc Ram Parity Alarm
2 pages
Gts-200 Operation Manual 11 Ver
No ratings yet
Gts-200 Operation Manual 11 Ver
398 pages
21 Series Mill Controller Operation Manual: Date: 2013/11/08
100% (1)
21 Series Mill Controller Operation Manual: Date: 2013/11/08
138 pages
Saving and Restoring The PLC: Digital Manuf@cturing Solutions
No ratings yet
Saving and Restoring The PLC: Digital Manuf@cturing Solutions
55 pages
04018E - A-77223E@02 Bis IO Link Description
No ratings yet
04018E - A-77223E@02 Bis IO Link Description
80 pages
FANUC Series 16i 18i 21i-TATB Outputting Signal Near End Point
100% (1)
FANUC Series 16i 18i 21i-TATB Outputting Signal Near End Point
3 pages
B-64305en@04-4 - Fanuc Series 0i0i Mate-Model D The Addition of Maintenance Manual
100% (1)
B-64305en@04-4 - Fanuc Series 0i0i Mate-Model D The Addition of Maintenance Manual
42 pages
B Series / SVSP-B Series Servo Amplifier Fan Speed Information of Servo Amplifier
No ratings yet
B Series / SVSP-B Series Servo Amplifier Fan Speed Information of Servo Amplifier
11 pages
FANUC Fuses
No ratings yet
FANUC Fuses
1 page
B 64303en1
No ratings yet
B 64303en1
1,042 pages
Restore Operation ROBODRILL DiA Series
No ratings yet
Restore Operation ROBODRILL DiA Series
15 pages
Fanuc Ot Turning Offline Pogr
No ratings yet
Fanuc Ot Turning Offline Pogr
138 pages
Fanuc Pmc-Model Nb6 Supplemental Programming Manual (LADDER Language)
100% (1)
Fanuc Pmc-Model Nb6 Supplemental Programming Manual (LADDER Language)
19 pages
Add Info B-64305EN 03
No ratings yet
Add Info B-64305EN 03
4 pages
1.5 SRAM Clear
100% (1)
1.5 SRAM Clear
1 page
63005en PDF
0% (1)
63005en PDF
848 pages
CNC Boot System Guide
No ratings yet
CNC Boot System Guide
8 pages
Serial No. 211716
100% (2)
Serial No. 211716
339 pages
Fanuc Pmc-Model Nb6 Supplemental Programming Manual (LADDER Language)
No ratings yet
Fanuc Pmc-Model Nb6 Supplemental Programming Manual (LADDER Language)
56 pages
M720BM Class Power Point
No ratings yet
M720BM Class Power Point
20 pages
Fanuc 6m
No ratings yet
Fanuc 6m
3 pages
MFG-0129 A FX Machine Data Server Installation Procedure
No ratings yet
MFG-0129 A FX Machine Data Server Installation Procedure
27 pages
Gtz-2000 Operation Manual 02 Vers
No ratings yet
Gtz-2000 Operation Manual 02 Vers
424 pages
H6C M e 1
No ratings yet
H6C M e 1
242 pages
H6D T Manual E
No ratings yet
H6D T Manual E
352 pages
H8C M e
No ratings yet
H8C M e
262 pages
HUST H8M CNC Controller Manual
No ratings yet
HUST H8M CNC Controller Manual
262 pages
H6CT Manual 29263
No ratings yet
H6CT Manual 29263
152 pages
Experiment Ii Introduction To Computer Numerical Control Ii
No ratings yet
Experiment Ii Introduction To Computer Numerical Control Ii
5 pages
Emco Winnc Ge Series Fanuc 0-TC
No ratings yet
Emco Winnc Ge Series Fanuc 0-TC
84 pages
Concerning The Addition of Coordinate System Rotation: 1. Type of Applied Technical Documents
No ratings yet
Concerning The Addition of Coordinate System Rotation: 1. Type of Applied Technical Documents
6 pages
FME CNC Unit 5
No ratings yet
FME CNC Unit 5
78 pages
(SN) G-C Codes PDF
No ratings yet
(SN) G-C Codes PDF
24 pages
G & M Codes (All CNC)
100% (4)
G & M Codes (All CNC)
24 pages
Option Addendum
No ratings yet
Option Addendum
11 pages
Fanuc Pmc-Model Sa1/Sb7 Supplemental Programming Manual (LADDER Language)
No ratings yet
Fanuc Pmc-Model Sa1/Sb7 Supplemental Programming Manual (LADDER Language)
23 pages
Fanuc Pmc-Model Sb7 Supplemental Programming Manual (LADDER Language)
No ratings yet
Fanuc Pmc-Model Sb7 Supplemental Programming Manual (LADDER Language)
5 pages
Fanuc Pmc-Model Sa1/Sb7 Supplemental Programming Manual (LADDER Language)
No ratings yet
Fanuc Pmc-Model Sa1/Sb7 Supplemental Programming Manual (LADDER Language)
12 pages
CNC Lathe Tool Offset Guide
No ratings yet
CNC Lathe Tool Offset Guide
13 pages
FANUC Machining Condition Guide
No ratings yet
FANUC Machining Condition Guide
31 pages
CNC Tilted Plane Commands Guide
100% (2)
CNC Tilted Plane Commands Guide
54 pages
5-Axis Tool Radius Compensation Guide
No ratings yet
5-Axis Tool Radius Compensation Guide
61 pages
5-Axis Machining Manual Guide
100% (1)
5-Axis Machining Manual Guide
32 pages
FANUC Series 16 Trouble Diagnosis Specifications: i/18i/21i-MB/TB
No ratings yet
FANUC Series 16 Trouble Diagnosis Specifications: i/18i/21i-MB/TB
17 pages
Die Casting Technology Guide
100% (2)
Die Casting Technology Guide
23 pages
Countermeasure For DC Defective Products: DC School Text Book
100% (2)
Countermeasure For DC Defective Products: DC School Text Book
13 pages
PLC Installation & Cooling Guide
No ratings yet
PLC Installation & Cooling Guide
18 pages
Toshiba Machine Co., Ltd. Die Cast Machine Engineering Div
No ratings yet
Toshiba Machine Co., Ltd. Die Cast Machine Engineering Div
27 pages
PQ TOS555 How To Check PQ Amplifier (During Pump Run)
100% (1)
PQ TOS555 How To Check PQ Amplifier (During Pump Run)
3 pages
PLC Device Settings: CPU Type - If Available, Choose The CPU Type To Match The Selected PLC's CPU
No ratings yet
PLC Device Settings: CPU Type - If Available, Choose The CPU Type To Match The Selected PLC's CPU
5 pages
Troubleshooting, Inspections, and Maintenance
No ratings yet
Troubleshooting, Inspections, and Maintenance
16 pages
TOS555 How To Adjust PQ Amplifier
No ratings yet
TOS555 How To Adjust PQ Amplifier
4 pages
Toshiba Machine Co., Ltd. Die Cast Machine Engineering Div
No ratings yet
Toshiba Machine Co., Ltd. Die Cast Machine Engineering Div
23 pages
DC School Text Book: Setting Method of Toscast
No ratings yet
DC School Text Book: Setting Method of Toscast
43 pages
DC School Text Book: Intermediate DC Hydraulic Circuit
No ratings yet
DC School Text Book: Intermediate DC Hydraulic Circuit
53 pages
DC School Text Book: Interpretation of Injection Wave
100% (2)
DC School Text Book: Interpretation of Injection Wave
32 pages
Toshiba Machine Co., Ltd. Die Cast Machine Engineering Div
No ratings yet
Toshiba Machine Co., Ltd. Die Cast Machine Engineering Div
25 pages
DC School Text Book: Electricity
No ratings yet
DC School Text Book: Electricity
88 pages
Toshiba Machine Co., Ltd. Die Cast Machine Engineering Div
No ratings yet
Toshiba Machine Co., Ltd. Die Cast Machine Engineering Div
46 pages
CC Module 5
No ratings yet
CC Module 5
26 pages
AI For Marketing
No ratings yet
AI For Marketing
198 pages
Gear Pump Performance Analysis
No ratings yet
Gear Pump Performance Analysis
9 pages
Visual Media Portfolio
No ratings yet
Visual Media Portfolio
21 pages
3 Main Lessons From Steve Jobs's Speech
No ratings yet
3 Main Lessons From Steve Jobs's Speech
3 pages
Finacle Core Banking System Overview
No ratings yet
Finacle Core Banking System Overview
2 pages
MambaVision: NVIDIA's Hybrid Vision Transformer For AI
No ratings yet
MambaVision: NVIDIA's Hybrid Vision Transformer For AI
8 pages
Bharatiya Antariksh Hackathon 2025 Idea Submission
No ratings yet
Bharatiya Antariksh Hackathon 2025 Idea Submission
17 pages
Thesis Guidelines Lsu
100% (1)
Thesis Guidelines Lsu
7 pages
The GET Method Is Not Supported For Route Add-Proposal-Action.
No ratings yet
The GET Method Is Not Supported For Route Add-Proposal-Action.
1 page
Chapter3 - Circuit Analysis Methods
100% (2)
Chapter3 - Circuit Analysis Methods
189 pages
Have A Question?: Customers Who Viewed This Item Also Viewed
No ratings yet
Have A Question?: Customers Who Viewed This Item Also Viewed
1 page
Medium Error During Reconstruction
No ratings yet
Medium Error During Reconstruction
3 pages
No.260 HO2019260F Aircloud Gateway IOM ENTCN - 202004 - 2021100613043524
No ratings yet
No.260 HO2019260F Aircloud Gateway IOM ENTCN - 202004 - 2021100613043524
64 pages
CSC 208 Web and Application Development Group Assessment 234
No ratings yet
CSC 208 Web and Application Development Group Assessment 234
9 pages
Chennai Water Resource Management Using GIS
No ratings yet
Chennai Water Resource Management Using GIS
7 pages
小六閱讀理解 - PDF
No ratings yet
小六閱讀理解 - PDF
8 pages
All My Work Backup 2023
100% (2)
All My Work Backup 2023
3 pages
Vpls Configuration Ios XR With BGP and LDP Autodiscovery
No ratings yet
Vpls Configuration Ios XR With BGP and LDP Autodiscovery
104 pages
Top 40 PLC Interview Questions and Answers - 2025
No ratings yet
Top 40 PLC Interview Questions and Answers - 2025
14 pages
Home Connect App ConditionsOfUse
No ratings yet
Home Connect App ConditionsOfUse
17 pages
Re Fix Match
No ratings yet
Re Fix Match
11 pages
Angkasa Cerah PL 28-11-2024
No ratings yet
Angkasa Cerah PL 28-11-2024
4 pages
SC200 Controller Datasheet
No ratings yet
SC200 Controller Datasheet
4 pages
GAC041 - SIG - Aula01 - Conceitos - A
No ratings yet
GAC041 - SIG - Aula01 - Conceitos - A
30 pages
First Hello World Program in JavaScript
No ratings yet
First Hello World Program in JavaScript
2 pages
Sap Law 20221208
No ratings yet
Sap Law 20221208
7 pages
Krishneeyam of Sree Krishna Achaarya: PDF-KOSKA-9-2 - 42 Pages - Size 2,769 KB - 5 Jan, 2015
No ratings yet
Krishneeyam of Sree Krishna Achaarya: PDF-KOSKA-9-2 - 42 Pages - Size 2,769 KB - 5 Jan, 2015
2 pages
YASKAWA AC Drive A1000: Technical Manual
No ratings yet
YASKAWA AC Drive A1000: Technical Manual
590 pages
Bsc-Ty 2019-20
No ratings yet
Bsc-Ty 2019-20
15 pages