Fanuc cnc automatic programming

Fanuc manual is for conversational automatic programming function.
The conversational automatic programming function II is software in which
functions of an epoch-making automatic programming system "Symbolic FAPT" are
assembled, and this "Symbolic FAPT" allows even inexperienced NC programmers
to produce NC data for machining at once simply by depressing buttons
according to the instructions on the graphic display CRT. The CNC can execute
machining according to a program soon after programming it at a site, or it
can execute another programming during machining.
The Symbolic FAPT produces NC data and loads them into built-in memory
(machining memory). Machining is made according to the NC data in memory
(also called NC program).
During machining, another program can also be produced by using Symbolic
FAPT function. When the machining memory has been unloaded after machining,
another program being prepared at the automatic programming section is
registered to the machining memory.
Since NC data loaded in machining memory are prepared in standard NC
language, an operator who knows the standard NC language can directly check or
modify NC data of standard NC language in machining memory by using the CRT.
(Since NC data can be registered again to machining memory after
modifying NC data at the automatic programming section without any need of
modifying machining memory data, it is not necessary to modify machining
memory data usually.)

2. CONVERSATIONAL AUTOMATIC PROGRAMMING FUNCTION

The NC data thus produced automatically by Symbolic FAPT are not directly
used for machining, but they are once loaded to the machining memory.
The automatic programming unit is not capable of storing various
information of machine tools and machine control unit.
Note that control information of machine tools can be processed only in
machine control unit.
(3) The machining information can be input to CNC by the following two
methods.

Method of loading automatic programming results into the machining
memory after automatic programming has been made by using the
Symbolic FAPT. This is a standard method, which can be used without
any knowledge on NC tape format.
Method of inputting the machining information into the machining
memory of the machine control unit by MDI operation.
Since this operation is the same as in NC unit for ordinary MDI
input, you are requested to be familiar with NC tape format, etc.

This manual does not cover the functions on the NC side.
The function of an NC machine tool system does not depend only on the NC,
but on the combination of the machine tool, its magnetic cabinet, servo
system, the NC, operator's panels, etc. It is too difficult to describe
the function, programming, and operation in various combinations of them.
This manual generally describes them from the standpoint of the NC. So,
for a particular NC machine tool, refer to the manual issued by the
machine tool builder, which should take precedence over this manual.
Notes refer to detailed and specific items. So, when a note will be
encountered, terms used in it sometimes will not have been explained it.
In such a case, first skip the note, then return to it after having read
the manual in outline for details.
For 16-T CAP II and 16-TT CAP II, the manual covers only the 5710 system
and the 5800 system series and later. The earlier series may not support
some functions described in the manual. See Appendix 2 for the unsupported functions.

The mode in which the CRT/MDI unit is used for the creation of CNC data
with the Symbolic FAPT is called FAPT mode. The mode in which the CRT/MDI is
used for operations related to the CNC functions, such as editing of created
data, setting and check of various parameters for CNC machining and tool
offset amounts, and check of travel during CNC machining, is called CNC mode.
To change the mode of the CRT/MDI unit between FAPT and CNC/PMC, press
the mode selector keys with lamps as shown below.

KEYS EFFECTIVE IN FAPT MODE
The diagram at under shows only the keys used in the symbolic FAPT. The
symbols omitted are not used in FAPT mode.

SOFT KEY
The 12 keys under the CRT are called soft keys. The function of the keys change according to the screen displayed. The function for each screen are framed at the bottom of the screen.

SYMBOLIC FAPT
The Symbolic FAPT is an epoch-making NC automatic programming system
which enables even inexperienced NC operators to prepare NC tape
immediately according to the instructions on the graphic display CRT.
Each process from design drawings to NC tape preparation is entirely
advanced by the conversational operation with the graphic display CRT.
For (1) selection of coordinate system by drawing methods (2)
selection of figures of blank and input of dimensions (3) input of parts
figures and dimensions, and (4) selection of machining process and decision
or cutting conditions etc., the operator has only to answer questions from
the CRT.
The parts figure can be input simply by depressing corresponding
symbol keys on the operator's panel according to the profiles of a
workpiece described on design drawings.
When dimensions and various data are input, various pieces of
reference information are illustrated on the CRT from time to time, and
questions are given to the operator using daily language.
When data are input, the figure of blank and parts profile are drawn
immediately, and automatic calculations of NC command data are started.
The tool path is concurrently displayed as figures.
Unless otherwise specified, this manual uses the screens of the 15-TFB
or 16-T CAP II to describe functions.

Changing the color of a part figure or blank figure when it is modified
When a part figure or blank figure is modified (or created), the
elements before and after the element on which the cursor is placed are
displayed in different colors. As a result, the operator can easily
tell which element is currently being modified on the drawing.
System parameter 552 specifies the color of elements already determined
and system parameter 586 specifies the color of elements to be
determined.

Select the software key "CORRECTION" or "LIST MODE" and "NEW" to prepare
the blank figure referring to the machined figure and to prepare it newly,
respectively.
Similar to input of parts figure data, use a symbolic key for entry of
blank figure. In this case, however, "G", "T" and "N" keys cannot be used for
parts figure definition.
Input a blank figure according to any one of the following three formats.

The element figure created so far is redrawn and the following message is
displayed: "Select software key"
Press the "NEXT PAGE" if there are no areas modified and when proceeding
to the next process.

Part figure input (Directory input system)
The parts figure input system includes the system of entering the
definition data with displaying a defined figure, and the method of entering
the definition data while displaying in the table format. The former is
called "Graphic input system" (refer to para. 3.2.2 and 3.2.3 II) and the
latter is called "Directory input system". The "Directory input system" will
be described here.

In this screen, select the element to be modified, using ELEMENT FORWARD
and ELEMENT BACK soft keys. (when the element is inserted, it is
inserted before the element is selected:)
Next,

press "INPUT" when changing the figure data.
When it is desired to insert the element, key in the element symbol and
press "INPUT". When only checking the data without modifying it, check
the objective element data, using ELEMENT FORWARD and ELEMENT BACK soft
keys.
When the element is changed or inserted, the figure data input screen is
selected. The inquiry is displayed under the figure data list display.

In this screen, all data on the figure data are inquired. Adjust the
cursor to the data to be entered and input the data. Upon completion of
keying-in operation, press "NEXT PAGE" soft key.

Chamfering
Normally, it is customary practice to chamfer a corner unless otherwise
specified for the machined parts in the drawing. Unlike the specified
chamfer, this chamfering is not described in the drawing, the chamfering
amount is constant and many in most cases.
Consequently, when the machined figure is prepared, it may be troublesome
to enter many chamfering elements. This function inputs a given amount
of chamfer exclusively to all corners to which no chamfer (element symbol
C) is input yet after all machined figures are completely entered.

After the machined figure for turning is entered, the following screen is
displayed.

Corner R
The batch input function for corner R is similar to the batch
function for chamfering. The function specifies identical corner
for corners whose chamfering data is left unspecified after the
machining profile is specified.
The batch input function for corner R cannot be used for 5700
16-T CAP II.
After entering the turning figure, press the rightmost soft key
Then, press the CORNER R key.
The yellow cursor lights at the corner whose chamfering data
yet been specified.

After entering the required data, press the EXEC soft key. The
corner R data is specified for the lighted corner. Then, the original
screen is displayed again.

As a standard for a corner to be chamfered, set the maximum
angle to system parameter No. 756. (Setting range 0° < Angle ≤ 180°) For example, if the angle is set to 100, the cursor
lights up as a chamfering corner with 100° or less angle. No
cursor lights up for the portion more than 100° angle.
Example) when setting system parameter No. 756 as 100:

The initial value of Corner R amount can be set to system
parameter No. 755. For example, if 0.2 is set to system
parameter No. 755, when the control asks the chamfering amount,
the numeral 0.2 is entered as the initial value.
The inquiry for "SURFACE ROUGHNESS" can be omitted. (System
parameter No. 0010) When omitted, "Standard Surface Roughness"
is adopted for surface roughness.

"Pattern Figure" refers to a given shape or specified shape. This is a
convenient input method: a figure consisting of several elements can be
defined promptly by just answering the minimum question required for its
figure.

FIGURE": the screen display changes to the soft key layout showing the
pattern figure input.

Input of equal pitch/continuous groove
This input function is used for defining a figure in which a plurality of
grooves are arranged at an equal pitch. Press "REPEAT GROOVE": the
display as shown below will appear.

Input the end point of a straight line subsequent to a continuous groove.
When defining the groove arranged in parallel to the Z-axis, it is not
necessary to input the end point value of X.
In contrast to the above, when defining a groove arranged in parallel to the
X-axis, it is not necessary to input the Z end point value.

Input the number of V marks indicating the surface roughness. This surface
roughness is applied to all elements forming this figure. Further, it is
also possible to skip this question by system parameter No. 0010 bit 2
(surface roughness to G). When skipped, "Standard Surface Roughness" is
adopted for the surface roughness.

System parameters 125 and 174 specify the constants to be used when
the elements of threading are manually defined.
If the automatically specified value is not suitable, change it
manually.
To define a trapezoid thread, manually enter the data.
After the value of D1 is entered, the system automatically specifies
the values of WIDTH (WT), DEPTH (DT), and CORNER R (R). The values are
calculated as shown below:

The threading depth (D1) can be automatically determined by
pressing the OUTER THREAD, INNER THREAD, or SQUARE THREAD soft key
only when the values of LD (LEAD) and NT (MULTIPLE) are specified.
Note 2) If the value of LD (LEAD) or NT (MULTIPLE) is changed, the D1
(threading depth) and DT (depth) must be calculated again. Press
the OUTER THREAD, INNER THREAD, or SQUARE THREAD soft key to have
the system automatically specify suitable values.

Figure element copy function
Having specified the start and end points of the figure to be copied, once
the number of copies has been keyed in, it is possible to define the same
figure repeatedly. This is useful when repeatedly inputting special
groove figures and complicated circular figures.

In the case illustrated above, when the soft key "PATTERN INPUT" is pressed
followed by "FIGURE COPY", the following copy area specification screen
appears. Note however that when the "PATTERN INPUT" key is pressed, the cursor
must be next to the very last element, as illustrated above. When the cursor
has been moved by corrections to element data etc., press the "FIGURE COPY"
only after having made sure to move the cursor next to the very last element.
If the "FIGURE COPY" key is pressed when the cursor is at an element other
than the final one, an error message will be displayed saying "CAN NOT USE
THIS FUNCTION" and the copy area specification screen will not appear.

The following explanation is based on an example where the above mentioned
data has been defined and one copy is required from No. 3 element to No. 8
element.
By pressing the soft key "ELEMENT COPY", the copy area specification screen
will be displayed, set the repeat number to 1 and specify the No. 3 element at
copy start point and No. 8 element at the copy end point.

Machine Zero Point and Turret Position
When the figure has been defined, the screen asks about the "Home position" 

HOME POSITION
DXH =
ZH =
Input the coordinate value of home position of NC lathe.
If data has already been properly input, press the "Cursor" key. Do not
input data and leave it undefined when not starting from the home position.

INDEX POSITION
DXI =
ZI =
Input the coordinate value of turret revolution center position.
If data has already been input properly, press the "NEXT PAGE" soft key.
In the case of 15-TTFB, 16-TT CAP II, the question for home position and
index position at No.2 also appears.
Note: Input the distance from the programmed coordinate axis for both home
position and index position. Let the sign of Z be positive whichever
direction the Z axis of coordinate axis programmed faces. The home
position is used to indicate the relationship between the program
coordinate system and machine coordinate system.
When the home position and index position are determined and it is
troublesome to input these data every time, it is possible to set initial
values to the system parameters 206 - 213. Also, it is possible to skip
questions. For details, see Chapter 8-1. This screen does not appear
when skipping the questions of home position and index position.

When the machining definition soft key (No. 4) is pressed on the initial
screen, the following screen appears. On this screen, the manual machining
definition item and the automatic process determination function can be
selected.

When a tool identification number is entered, the registered tool figure
data and tool setting data are displayed.
To use a tool whose tool data is not registered, do not define the tool
identification number.
If the entered tool identification number is not registered, the NOT FOUND
TOOL ID. NO. message is displayed.
If the tool type corresponding to the selected tool identification number
is not suitable for the current process, the TOOL TYPE DON'T FIT THIS
PROCESS message is displayed.

A value is assigned to Z in accordance with the system of coordinates
on this screen. Where the Z axis is plotted as shown in the figure
on the right, the value of Z will always be negative.
Whatever the drawing format, the right-hand end of the Z axis is
always positive on the "Machining definition" screen of menu No.4.
Specifications of the machining start points and intermediate points
are all made in accordance with this system of coordinates. The
cutting points are also therefore specified in accordance with the
same coordinate system.

The operator is not prompted to enter the data of pecking if finishing
of a groove or necking is selected.
In roughing and finishing, the first cut is made from the virtual tool tip
side of the tool.
The position of the virtual tool tip is determined by AC and AN of the
tool data.
If AC is set to 90 and AN is set to -90 for a tool for outer surface
machining, the virtual tool tip is on the left side of the tool. Therefore,
the first cut is made from the left side.

When the tool DATA soft key is pressed on the machining process list
screen, the tool list screen shows the data of turning tools. To set
the data of a milling machining tool, press the MILLING TOOL soft key.
When the TOOL DATA soft key is pressed on the tool data setting screen
of a process, the data of tools of the current process is displayed.
If the current process is turning, the list of turning tools is
displayed. If the current process is C-axis machining or Y-axis
machining, the list of milling machining tools is displayed.

Precautions to be taken with background animated simulation:
1. Background animated simulation is possible only in the 15-TFB, 16-T CAP II, not in the 15-TTFB, 16-TT CAP II.
2. Background animation drawing is valid only when the animated simulation function (option) is provided.
3. Chucks and tailstocks are not displayed.
4. Only linear interpolation, arc interpolation, and threading are simulated.
5. Background animated simulation is not performed with the vertical lathe.
6. Background animated simulation is not performed when single process output is selected.
7. Blanks are not cut in the bar feed process, threading process, and C-axis/Y-axis machining process.
8. Tool pictures do not appear in the bar feed process.
9. In the sub-cycle process, blank cuttings, tool pictures, and tool paths
are not drawn on the screen.

Thus, cutting operations for each turret are displayed. For the section
on spindle speed, "N" means spindle speed, "V" means cutting speed. For
simultaneous operation; No. 2 and 3, "ROUGHING OF OUTER FIGURE" and "ROUGHING
OF INNER FIGURE", operation No. 8 and 9, "THREADING" and "DOWN" (or set the
cursor to No. 3 and depress "HEAD 2 UP"), and then set the cursor to No. 8 and
depress the soft key, "HEAD 1 DOWN" (or set the cursor to No. 9 and depress
"HEAD 2 UP") continuously. For changing the cutting speed of operation No. 6,
"GROOVING", 125 m/min for instance, set the cursor to No. 6 and input 125
through keys for the question, V(N) =. When performing such operations, the
operation procedure is displayed as follows.

Notes:
- To enable execution of the complex threading cycle (G76), the complex
turning cycle function of the NC must be supported.
- Face threading cannot be executed with the complex threading cycle
(G76). For face threading, G32 is output as before, even if the
complex threading cycle is selected.
- To use the complex threading cycle with the FANUC Series 15-TFB,
create the corresponding NC statements after setting identical values
for the final depth of cut for threading in system parameter No. 119
of FAPT and the finishing allowance in parameter No. 6219 of the NC.
- If the FANUC Series 16-T is being used, restrictions are imposed on
the tool angle that can be specified. (If an angle other than 0, 29,
30, 55, 60, or 80 degrees is specified, P/s alarm 62 is output.) If
the FANUC Series 15-TFB is being used, the tool angle can be specified
within a range of 0 to 120 degrees, in 1-degree increments.
- The thread radius, thread height, depth of first cut, and finishing
allowance (in the format for the FANUC Series 16) are referenced with
MTF1021 (X-axis least input increment) and MTF1031 (number of decimal
places of the X-axis least input increment).
The thread height and depth of first cut cannot be output with decimal places.

Checking NC Data (Animated Simulation Function)
The function which allows a practical cutting simulation to take place by
displaying the blank, chuck, tailstock and tool configuration is called an
Animated Simulation Function.
The manner in which a blank is being cut can be monitored by
selecting the screen on which animated simulation is done and
executing cycle operation under the machine lock condition. Each
time a T code is specified, the

**4.6 Cautions**

(1) Insert movement statements
This function involves the creation of a macro call message. It is a precondition, therefore, that the macro body has previously been created on the NC side.
If the sub cycle process is to be corrected in the definition of machining, a sub cycle file which is completely identical to that during new creation must be existing in the main memory.

(2) The family program does not include the sub cycle file which has been set. To correct the sub cycle process by inputting a family program including the sub cycle into the process, therefore, a sub cycle file which is completely identical to that during new creation must also be input.

(3) The tool locus is not drawn during the NC data preparation.

(4) M01 is not output when the sub cycle ends even if "1" is set to MTF N0. 1136 (to output M01 when the process ends).

(5) The sub cycle does not stop in the single step of the process.

(6) It is impossible to create NC data for the 4-axis lathe or NC data in the main and sub format if the process includes a sub cycle.

**BALANCE CUT FAPT FUNCTION (15-TTFB, 16-TT CAP 11 only)**

Machining conducted in one process by the tools of both head 1 and head 2 is called balance cut. The balance cut FAPT function automatically generates NC statements for balance cut. There are the following two types of balance-cut machining:

Type A: This type aims at machining thin and long works with a high precision. The two tools move in perfect synchronization with each other.

Type B: This type aims at machining works more efficiently. After the tool on head 1 cuts the work, the tool on head 2 cuts it deeper, following the movement of the tool on head 1.

**5.1 Balance Cutting Process**

Balance cut can be used in the following processes.
Type A: 
- Roughing of outer diameter (not edges)
- Semi-finishing of outer diameter (not edges)
- Finishing of outer diameter (not edges)

Type B:
- Roughing of outer diameter

Type A and type B are distinguished by the value that is set for "DELAY AMOUNT" on the data screen. The delay amount determines how much the head 2 tool lags behind the head 1 tool during machining. Type A is selected by setting DELAY AMOUNT to 0 (no delay), and type B by setting it to a positive value.