FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 137

3.MANUAL OPERATION

OPERATION

B-63944EN/03

- 1052 -

3.7

RIGID TAPPING BY MANUAL HANDLE

For execution of rigid tapping, set rigid mode, then switch to handle
mode and move the tapping axis with a manual handle. For rigid
tapping, refer to Section 4.4 in Part II of the User's Manual (T series)
or Section 5.2 in Part II of the User's Manual (M series) and the
relevant manual of the machine tool builder.

Rigid tapping by manual handle

Procedure

Stop the spindle and servo axes, then set MDI mode by pressing
the MDI switch among the mode selection switches.

Enter and execute the following program:
Example 1) M series / T series (G code systems B, C)

M29 S100 ;

G91 G84 Z0 F1000 ;

Example 2) T series (G code system A)

M29 S100 ;

G84 W0 F1000 ;

The program above is required to determine a screw lead and set
rigid tapping mode. In this program, a tapping axis must always
be specified. Specify a value that does not operate the tapping
axis. With the M series, specify G84 (G74). With the T series,
specify G84 (G88).

WARNING

In this MDI programming, never specify commands
to position the tool at a drilling position and at point
R. Otherwise, the tool moves along an axis.

When the entered program is executed, rigid tapping mode is set.

4 After rigid mode is set upon completion of MDI program

execution, switch to the handle mode by pressing the handle
switch among the mode selection switches.

CAUTION

At this time, never press the reset key. Otherwise,
rigid mode is canceled.

To perform rigid tapping, select a tapping axis with the handle
feed axis select switch, and move the tapping axis with the
manual handle.

B-63944EN/03

OPERATION

3.MANUAL OPERATION

- 1053 -

Explanation
- Manual rigid tapping

Manual rigid tapping is enabled by parameter HRG (No. 5203#0) to 1.

- Cancellation of rigid mode

To cancel rigid mode, specify G80 as same the normal rigid tapping.
When the reset key is pressed, rigid mode is canceled, but the canned
cycle is not canceled.
When the rigid mode switch is to be set to off for rigid mode
cancellation (when parameter CRG (No. 5200#2) is set to 0), the G80
command ends after the rigid mode switch is set to off.

- Spindle rotation direction

The rotation direction of the spindle is determined by a specified
tapping cycle G code and the setting of parameter HRM (No. 5203#1).
For example, when the HRM parameter is set to 0 in G84 mode, the
spindle makes forward rotations as the tapping axis moves in the
minus direction. (When the tapping axis moves in the plus direction,
the spindle makes reverse rotations.)

- Arbitrary tapping axis

With the M series, an arbitrary tapping axis can be selected by setting
bit 0 (FXY) of parameter No. 5101 to 1. With the T series, an
arbitrary tapping axis can be selected not by using bit 0 (FXY) of
parameter No. 5101 (but by using bit 0 (FXY) of parameter No. 5101
when the FS15 format is specified). In this case, specify a G code
for plane selection and the address of the tapping axis when setting the
rigid tapping mode in the MDI mode.

- G84 command/same block specifying both M29 and G84

As the MDI program command for setting the rigid mode, G84 can be
specified as a rigid tapping G code (by setting bit 0 (G84) of
parameter No. 5200 to 1), or M29 and G84 can be specified in the
same block.
Example 1: G91 G84 Z0 F1000 S100 ;
Example 2: G91 G84 Z0 F1000 M29 S100 ;

- Specification of manual handle feed faster than the rapid traverse rate

Set parameter (No.7117) to 0 so that when manual handle feed is
specified which is faster than the rapid traverse rate, the handle pulses
beyond the rapid traverse rate are ignored.

- Series 15 format command

By setting bit 1 (FCV) of parameter No. 0001 to 1, the Series15
format can be used for specification.
Example 1: G91 G84.2(G84.3) Z0 F1000 S100; (M series)
Example 2: G84.2 W0 F1000 S100; (T series : G code systems A)
Example 3: G91 G84.2 Z0 F1000 S100; (T series : G code system B,
C)

3.MANUAL OPERATION

OPERATION

B-63944EN/03

- 1054 -

- Acceleration/deceleration type

When manual rigid tapping is executed, the acceleration/deceleration
type and acceleration/deceleration time constant set in the rigid
tapping parameters are valid.
The same settings are valid also for extraction.

- In the case of multi-spindle operation

In the case of multi-spindle operation, a spindle can be selected by
specifying a P command as well as an S command.
Example : When the 2nd spindle is selected:
M29

S100

;

G91 G84 Z0 F1000 ;

Limitation
- Excessive error check

In manual rigid tapping, only an excessive error during movement is
checked.

- Tool axis direction handle feed

Tool axis direction handle feed is disabled.

- Extraction override

In manual rigid tapping, the extraction override function is disabled,
and the use of an acceleration/deceleration time constant for extraction
is disabled.

- Number of repeats

In MDI programming, never specify K0 and L0, which are used to
specify that the number of repeats is 0 and to disable the execution of
a G84 block. If K0 or L0 is specified, rigid mode cannot be set.

- Positioning of the tool to a drilling position

When positioning the tool to a drilling position, select the X-axis or
Y-axis with the axis select switch in handle mode. Never use the
method of positioning to a drilling position in MDI mode or MEM
mode. The method can operate the tapping axis.

- Three-dimensional rigid tapping

Three-dimensional rigid tapping cannot be used in rigid tapping using
the manual handle.

- Interpolation type rigid tapping

Interpolation type rigid tapping cannot be used in rigid tapping using
the manual handle. To perform rigid tapping using the manual
handle, select the conventional type of rigid tapping with bit 3 (CHR)
of parameter No. 5202.

B-63944EN/03

OPERATION

3.MANUAL OPERATION

- 1055 -

3.8

MANUAL NUMERICAL COMMAND

The manual numerical command function allows data programmed
through the MDI to be executed in jog mode. Whenever the system
is ready for jog feed, a manual numerical command can be executed.
The following eight functions are supported:
(1) Positioning

(G00)

(2)  Linear interpolation (G01)
(3)  Automatic reference position return (G28)
(4)  2nd/3rd/4th reference position return (G30)
(5)  M codes (miscellaneous functions)
(6)  S codes (spindle speed functions)
(7)  T codes (tool functions)
(8)  B codes (second auxiliary functions)
By setting the following parameters, the commands for axial motion
and the M, S, T, and B functions can be disabled:
(1)  Positioning (G00): .........................Parameter JAXx (No. 7010#0)
(2)  Linear interpolation (G01):............Parameter JAXx (No. 7010#0)
(3)  Automatic reference position return (G28):

.......................................Parameter JAXx (No. 7010#0)

(4) 2nd/3rd/4th reference position return (G30):

.......................................Parameter JAXx (No. 7010#0)

(5)  M codes (miscellaneous functions): Parameter JMF (No. 7002#0)
(6)  S codes (spindle speed functions):.... Parameter JSF (No. 7002#1)
(7)  T codes (tool functions):................... Parameter JSF (No. 7002#2)
(8)  B codes (second auxiliary functions):Parameter JBF (No. 7002#3)

Procedure Manual numerical command

Procedure

Press the jog switch (one of the mode selection switches).

Press function key

3 Press soft key [JOG] on the screen. The following manual

numerical command screen is displayed.

3.MANUAL OPERATION

OPERATION

B-63944EN/03

- 1056 -

Fig. 3.8 (a) Manual numerical command screen

The remaining portion of the axis information currently not
shown on the screen can be displayed by pressing the

key.

NOTE

1 The actual feedrate (F) and the actual spindle speed

(S) are displayed only for 9” window.

2 If two or more identical axis names exist for the

same path, they are not displayed.

B-63944EN/03

OPERATION

3.MANUAL OPERATION

- 1057 -

Enter the required commands by using address keys and numeric
keys on the MDI panel, then press soft key [INPUT] or the

key to set the entered data.

Fig. 3.8 (b) Example of inputting numerical value

The following data can be set:
1. G00: ................ Positioning
2. G01: ................ Linear

interpolation

3.  G28: ................ Automatic reference position return
4.  G30: ................ 2nd/3rd/4th reference position return
5.  M codes: ......... Miscellaneous functions
6.  S codes:........... Spindle speed functions
7.  T codes:........... Tool functions
8.  B codes: .......... Second auxiliary functions
The set data is maintained even when the screen or mode is changed.

NOTE

When an alarm state exists, data cannot be set.

Press the cycle start switch on the machine operator's panel to
start command execution. The status is indicated as "MSTR."
The automatic operation signal, STL, can be turned on by setting
bit 2 (JST) of parameter No.7001.

NOTE

If the cycle start switch is pressed while an alarm
state exists, a "START REJECTED (ALARM
EXISTED)" warning is generated, and the entered
data cannot be executed.

3.MANUAL OPERATION

OPERATION

B-63944EN/03

- 1058 -

Upon the completion of execution, the "MSTR" status indication
is cleared from the screen, and automatic operation signal STL is
turned off. The set data is cleared entirely. G codes are set to G00
or G01 according to the setting of parameter G01 (No.3402#0).

Explanation
- Positioning

An amount of travel is given as a numeric value, preceded by an
address such as X, Y, or Z. This is always regarded as being an
incremental command, regardless of whether G90 or G91 is specified.

Manual rapid traverse selection switch

Off On

Feedrate

(parameter)

Jog feedrate for each axis

(No.1423)

Rapid traverse rate for each axis

(No.1420)

Automatic

acceleration/

deceleration

(parameter)

Exponential acceleration/

deceleration in jog feed for each axis

(No.1624)

Linear acceleration/deceleration

in rapid traverse for each axis

(No.1620)

Override

Manual feed override

Rapid traverse override

NOTE

1 When the manual rapid traverse switch is off, the

feedrate is clamped so that the axis-by-axis manual
rapid traverse rate (parameter No. 1424) is not
exceeded.

2 The tool cannot move if linear interpolation type

positioning (where the tool path is linear) has been
performed by setting bit 1 (LRP) of parameter No.
1401.

- Linear interpolation (G01)

An amount of travel is given as a numeric value, preceded by an
address such as X, Y, or Z. This is always regarded as being an
incremental command, regardless of whether G90 or G91 is specified.
Axial movements are always performed in incremental mode even
during scaling or polar coordinate interpolation. In addition,
movement is always performed in feed per minute mode regardless of
the specification of G94 or G95.

Feedrate

(parameter)

Dry run feedrate

(No. 1410)

Automatic acceleration/deceleration

(parameter)

Exponential acceleration/deceleration

in cutting feed for each axis

(No.1622)

Override

Manual feed override

B-63944EN/03

OPERATION

3.MANUAL OPERATION

- 1059 -

NOTE

Since the feedrate is always set to the dry run
feedrate, regardless of the setting of the dry run
switch, the feedrate cannot be specified using F.
The feedrate is clamped such that the maximum
cutting feedrate, set in parameter No. 1430, is not
exceeded.

- Automatic reference position return (G28)

The tool returns directly to the reference position without passing
through any intermediate points, regardless of the specified amount of
travel. For axes for which no move command is specified, however, a
return operation is not performed.

Feedrate

(parameter)

Rapid traverse rate

(No. 1420)

Automatic acceleration/deceleration

(parameter)

Linear acceleration/deceleration in

rapid traverse for each axis

(No. 1620)

Override

Rapid traverse override

- 2nd, 3rd, or 4th reference position return (G30)

The tool returns directly to the 2nd, 3rd, or 4th reference position
without passing through any intermediate points, regardless of the
specified amount of travel. To select a reference position, specify 2, 3,
or 4 in address P. If address P is omitted, a return to the second
reference position is performed.

Feedrate

(parameter)

Rapid traverse rate

(No. 1420)

Automatic acceleration/deceleration

(parameter)

Linear acceleration/deceleration in

rapid traverse for each axis

(No. 1620)

Override

Rapid traverse override

NOTE

The function for 3rd/4th reference position return is
optional.

1 When the option is not selected
If "P2" is not specified in address P, the alarm

PS0046 is generated and the function cannot be
executed.

2 When the option is selected
If "P2," "P3," or "P4" is not specified in address P,

the alarm PS0046 is generated and the function
cannot be executed.

Content .. 135 136 137 138 ..