GSC GSB G code 0 0 G code system A 0 1 G code system B 1 0 G code system C
#7 #6 #5 #4 #3 #2 #1 #0
G23 CLR FPM G91 G01 3402
G23 CLR G91 G19 G18 G01
[Data type] Bit G01 Mode entered when the power is turned on or when the control is
cleared 0 : G00 mode (positioning) 1 : G01 mode (linear interpolation)
G18 and G19 Plane selected when power is turned on or when the control is cleared G19 G18 G17, G18 or G19 mode
0 0 G17 mode (plane XY) 0 1 G18 mode (plane ZX) 1 0 G19 mode (plane YZ)
G91 When the power is turned on or when the control is cleared
0 : G90 mode (absolute command) 1 : G91 mode (incremental command)
FPM When the power is turned on 0 : Feed per revolution on 1 : Feed per minute mode
CLR Reset button on the MDI panel, external reset signal, reset and rewind signal, and emergency stop signal 0 : Cause reset state. 1 : Cause clear state. For the reset and clear states, refer to Appendix in the Operator's Manual.
G23 When the power is turned on 0 : G22 mode (stored stroke check on) 1 : G23 mode (stored stroke check off)
#7 #6 #5 #4 #3 #2 #1 #0
3403 AD2 CIR
[Data type] Bit CIR When neither the distance (I, J, K) from a start point to the center nor
an arc radius (R) is specified in circular interpolation (G02, G03): 0 : The tool moves to an end point by linear interpolation. 1 : P/S alarm No.022 is issued.
AD2 Specification of the same address two or more times in a block is: 0 : Enabled (Next specification is enabled.) 1 : Disabled (P/S alarm No.5074)
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 171 -
NOTE 1 When 1 is set, specifying two or more G codes of
the same group in a block will also result in an alarm being issued.
2 Up to three M codes can be specified in a single block, when bit 7 (M3B) of parameter No.3404 is set to 1.
#7 #6 #5 #4 #3 #2 #1 #0
M3B EOR M02 M30 SBP POL 3404
M3B EOR M02 M30 SBP POL NOP
[Data type] Bit NOP When a program is executed, a block consisting of an O number, EOB,
or N number is: 0 : Not ignored, but regarded as being one block. 1 : Ignored.
POL For a command address allowing a decimal point, omission of the decimal point is: 0 : Enabled 1 : Disabled (P/S alarm No.5073)
SBP Address P of the block including M198 in the subprogram call function 0 : Indicating a file number 1 : Indicating a program number
M30 When M30 is specified in a memory operation: 0 : M30 is sent to the machine, and the head of the program is
automatically searched for. So, when the ready signal FIN is returned and a reset or reset and rewind operation is not performed, the program is executed, starting from the beginning.
1 : M30 is sent to the machine, but the head of the program is not searched for. (The head of the program is searched for by the reset and rewind signal.)
M02 When M02 is specified in memory operation 0 : M02 is sent to the machine, and the head of the program is
automatically searched for. So, when the end signal FIN is returned and a reset or reset and rewind operation is not performed, the program is executed, starting from the beginning.
1 : M02 is sent to the machine, but the head of the program is not searched for.
EOR When the end-of-record mark (%) is read during program execution: 0 : P/S alarm No.5010 occurs. (Automatic operation is stopped, and
the system enters the alarm state.) 1 : No alarm occurs. (Automatic operation is stopped, and the
system is reset.) M3B The number of M codes that can be specified in one block
0 : One 1 : Up to three
#7 #6 #5 #4 #3 #2 #1 #0
3405 QAB QLG DDP CCR G36 PPS DWL AUX
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 172 -
DWL AUX
[Data type] Bit AUX The least increment of the command of the second miscellaneous
function specified with a decimal point 0 : Assumed to be 0.001 1 : Depending on the input increment. (For input in mm, 0.001 is
assumed, or for input in inches, 0.0001 is assumed.) DWL The dwell time (G04) is:
0 : Always dwell per second. 1 : Dwell per second in the feed per minute mode, or dwell per
rotation in the feed per rotation mode. PPS The passing-point signal output function is:
0 : Not used 1 : Used
CCR Addresses used for chamfering and corner rounding 0 : Address used for chamfering and corner rounding is "I" or "K",
not "C". In direct drawing dimension programming, addresses ",C", ",R", and ",A" (with comma) are used in stead of "C", "R", and "A".
1 : Addresses used for chamfering, corner rounding, and direct drawing dimension programming are "C", "R", and "A" without comma. Thus, addresses A and C cannot be used as the names of axes.
DDP Angle commands by direct drawing dimension programming 0 : Normal specification 1 : A supplementary angle is given.
QLG When the passing-point signal output function is used, the remaining distance to be traveled specified in address ",Q" is: 0 : The combined distance of all axes 1 : The distance of the longest axis
NOTE This parameter is valid when bit 7 (QAB) of
parameter No.3405 = 0.
QAB When the passing-point signal output function is used, address ",Q" specifies: 0 : Remaining distance to be traveled 1 : Coordinate value of the longest axis
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 173 -
#7 #6 #5 #4 #3 #2 #1 #0
C07 C05 C04 C03 C02 C01 3406
C07 C05 C04 C03 C02 C01 #7 #6 #5 #4 #3 #2 #1 #0
C14 C11 C10 C08 3407
C15 C14 C13 C11 C10 C09 C08 #7 #6 #5 #4 #3 #2 #1 #0
C16 3408
C20 C19 C18 C17 C16 #7 #6 #5 #4 #3 #2 #1 #0
3409 CFH
[Data type] Bit Cxx (xx: 01 to 20) When bit 6 (CLR) of parameter No.3402 is 1, the reset button on the
MDI panel, the external reset signal, the reset and rewind signal, or emergency stop will, 0 : Clear the G code with group number xx. 1 : Not clear the G code with group number xx.
CFH When bit 6 (CLR) of parameter No.3402 is 1, the reset button on the MDI panel, the external reset signal, the reset and rewind signal, or emergency stop will, 0 : Clear F codes, H codes (for the M series), D codes (for the M
series), and T codes (for the T series). 1 : Not clear F codes, H codes (for the M series), D codes (for the M
series), and T codes (for the T series).
3410 Tolerance of arc radius
[Data type] 2-word [Unit of data]
Input increment IS-A IS-B IS-C Unit Millimeter input 0.01 0.001 0.0001 mm
Inch input 0.001 0.0001 0.00001 inch
[Valid data range] 1 to 99999999 When a circular interpolation command (G02, G03) is executed, the tolerance for the radius between the start point and the end point is set. If the difference of radii between the start point and the end point exceeds the tolerance set here, a P/S alarm No.20 is informed.
NOTE When the set value is 0, the difference of radii is
not checked.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 174 -
3411 M code preventing buffering 1 3412 M code preventing buffering 2 3413 M code preventing buffering 3
: : 3420 M code preventing buffering 10
[Data type] Byte [Valid data range] 0 to 255
Set M codes that prevent buffering the following blocks. If processing directed by an M code must be performed by the machine without buffering the following block, specify the M code. M00, M01, M02, and M30 always prevent buffering even when they are not specified in these parameters.
3421 Minimum value 1 of M code preventing buffering 3422 Maximum value 1 of M code preventing buffering 3423 Minimum value 2 of M code preventing buffering 3424 Maximum value 2 of M code preventing buffering 3425 Minimum value 3 of M code preventing buffering 3426 Maximum value 3 of M code preventing buffering 3427 Minimum value 4 of M code preventing buffering 3428 Maximum value 4 of M code preventing buffering 3429 Minimum value 5 of M code preventing buffering 3430 Maximum value 5 of M code preventing buffering 3431 Minimum value 6 of M code preventing buffering 3432 Maximum value 6 of M code preventing buffering
[Data type] Word [Valid data range] 0 to 65535
When a specified M code is within the range specified with parameter Nos. 3421 and 3422, 3423 and 3424, 3425 and 3426, 3427 and 3428, 3429 and 3430, or 3431 and 3432, buffering for the next block is not performed until the execution of the block is completed.
NOTE 1 The specification of a minimum value that exceeds
the specified maximum value is invalid. 2 When there is only one data item, set the following:
minimum value = maximum value.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 175 -
3435
Central angle limit of circular with R specification
[Data type] Byte [Unit of data] 1° [Valid data range] 0 to 180
Set a central angle limit that can be permitted in commands for circular interpolation with R specification (G02 and G03). If circular interpolation of which central angle exceeds the limit is specified, P/S alarm No.23 is issued. If this parameter is set to 0, the radius R specification alarm function is disabled.
#7 #6 #5 #4 #3 #2 #1 #0
NPS CQD 3450
BDX CQD AUP
[Data type] Bit AUP When a command for the second miscellaneous function contains a
decimal point or negative sign: 0 : The command is invalid. 1 : The command is valid.
NOTE For the T series, a decimal point and negative sign
are supported for commands for the second miscellaneous function, regardless of the setting made with this parameter.
CQD The method used for determining the amount of travel in circular
interpolation is: 0 : Series 16 type. 1 : Series 15 type.
NPS A block that contains M98 Pxxx or M99, and which contains no addresses other than O and N functions: 0 : As a one-block NC statement involving no movement. (A single-block stop is caused.) 1 : As a macro statement. (A single-block stop is not caused. Moreover, the block is not
regarded as a block involving no movement in tool-tip radius compensation mode.)
BDX A decimal point specified with address B is handled: 0 : In the conventional way. 1 : In the same way as in a system equipped with the second
auxiliary function. In a system without second auxiliary function, the decimal point specified with address B can be handled as in a system equipped with the second auxiliary function. The following parameters can be used: • Bit 0 (AUP) of parameter No. 3450 • Bit 0 (AUX) of parameter No. 3405
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 176 -
#7 #6 #5 #4 #3 #2 #1 #0
3451
NBN CCK SDP GQS
[Data type] Bit GQS When G33 is specified, the threading start angle shift function (Q) is:
0 : Disabled. 1 : Enabled.
SDP The function to specify an S command with decimal point is: 0 : Not used. 1 : Used. An S command with one decimal place can be specified. However, the S command value is rounded off to the nearest whole number. Example: Relationships between specified value and S code output/alarm S200.5 -> S code output value = 201 S200.2 -> S code output value = 200 S200.12 -> P/S007 alarm is raised.
CCK If chamfering or corner R is enabled and if the end point specified in an arc command is not complete, 0 : No alarm is raised. 1 : An alarm (P/S058 alarm) is raised. This parameter specifies whether an alarm is raised if chamfering or corner R is enabled, if the end point specified in an arc command is not complete, and if an address is omitted. If the end point is omitted in an arc command, chamfering or corner R may affect the omitted point, and the operation may not be performed as intended by the programmer. If this parameter is specified, an alarm can be raised for that type of program execution.
NBN If bit 0 (NOP) of parameter No. 3404 is set to 1, a block including just N (sequence number) is: 0 : Ignored. 1 : Not ignored but handled as a single block.
#7 #6 #5 #4 #3 #2 #1 #0
CRD 3453
[Data type] Bit CRD If the functions of chamfering or corner R and direct drawing
dimension programming are both enabled, 0 : Chamfering or corner R is enabled. 1 : Direct drawing dimension programming is enabled. If the functions of chamfering or corner R and direct drawing dimension programming are both specified, this parameter specifies which function is used. This parameter is displayed also on the setting screen. ("CHAMFERING/DIRECT DRAWING DIMENSION PROGRAMMING") The function to be enabled can be changed from the setting screen or parameter screen.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 177 -
#7 #6 #5 #4 #3 #2 #1 #0
3454 RF2
[Data type] Bit RF2 Reference position return commands G28.2 and G30.2, which
suppress in-position checks during reference position return, are: 0 : Invalid. 1 : Valid.
#7 #6 #5 #4 #3 #2 #1 #0
3455
AXDx
[Data type] Bit axis AXDx If a decimal point is omitted for an address with which a decimal point
can be used, the value is determined: 0 : In accordance with the least input increment. 1 : In millimeters, inches, or seconds. (calculator-type decimal point
input)
NOTE 1 This parameter is valid if bit 0 (DPI) of parameter
No. 3401 is set to 0. 2 Because some addresses (such as R and K) are
not related to an axis, setting this parameter for all axes is not equivalent to setting bit 0 (DPI) of parameter No. 3401 to 1.
3 This parameter cannot be used together with: - Macro executor - Basic operation package - Macro call argument
3460 Address for second miscellaneous function
[Data type] Byte
This parameter specifies the address used for the second miscellaneous function, as follows:
Address A B C U V W Set value 65 66 67 85 86 87
Address B is assumed when a value other than the above is set. Axes names cannot be used to specify the address.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 178 -
4.19 PARAMETERS OF PITCH ERROR COMPENSATION
#7 #6 #5 #4 #3 #2 #1 #0
3605 ROPx BDPx
NOTE When this parameter has been set, the power must
be turned off before operation is continued.
[Data type] Bit BDPx Both-direction pitch error compensation is:
0 : Not used. 1 : Used.
NOTE The function of both-direction pitch error
compensation is required.
ROPx The interval of pitch error compensation for a rotation axis (type A) is: 0 : Restricted by the following equation: Minimum value = maximum feedrate (rapid traverse rate)/7500. 1 : Not restricted by the following equation: Minimum value = maximum feedrate (rapid traverse rate)/7500.
3620 Number of the pitch error compensation position for the reference position
for each axis
NOTE When this parameter is set, the power must be
turned off before operation is continued.
[Data type] Word axis [Unit of data] Number [Valid data range] 0 to 1023
Set the number of the pitch error compensation position for the reference position for each axis.
3
2
1
-1
-2
Pitch error compensation value (absolute value)
Reference position Pitch error compensation position (number)
Compensation position number Set compensating value
31 32 33 34 35 36 37 -3 +1 +1 +1 +2 -1 -3
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 179 -
Fig.4.19 Pitch error compensation position number and value (example)
In the above example, set 33 as the number of the pitch error compensation position for the reference position.
3621 Number of the pitch error compensation position at extremely negative
position for each axis
NOTE When this parameter is set, the power must be
turned off before operation is continued.
[Data type] Word axis [Unit of data] Number [Valid data range] 0 to 1023
Set the number of the pitch error compensation position at the extremely negative position for each axis.
3622 Number of the pitch error compensation position at extremely positive
position for each axis
NOTE When this parameter is set, the power must be
turned off before operation is continued.
[Data type] Word axis [Unit of data] Number [Valid data range] 0 to 1023
Set the number of the pitch error compensation position at the extremely positive position for each axis. This value must be larger than set value of parameter (No.3620).
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 180 -
3623 Magnification for pitch error compensation for each axis
NOTE When this parameter is set, the power must be
turned off before operation is continued.
[Data type] Byte axis [Unit of data] 1 [Valid data range] 0 to 100
Set the magnification for pitch error compensation for each axis. If the magnification is set to 1, the same unit as the detection unit is used for the compensation data. If 0 is set, the same magnification selected by setting 1 is selected.
3624 Interval between pitch error compensation positions for each axis
NOTE When this parameter is set, the power must be
turned off before operation is continued.
[Data type] 2-word axis [Unit of data]
Input increment IS-A IS-B IS-C Unit Millimeter machine 0.01 0.001 0.0001 mm
Inch machine 0.001 0.0001 0.00001 inch Rotation axis 0.01 0.001 0.0001 deg
[Valid data range] 0 to 99999999
The pitch error compensation positions are arranged with equal spacing. The space between two adjacent positions is set for each axis. The minimum interval between pitch error compensation positions is limited and obtained from the following equation: Minimum interval between pitch error compensation positions = maximum feedrate (rapid traverse rate)/7500 Units: Minimum interval between pitch error compensation positions:
mm, inch, deg Maximum feedrate: mm/min, inch/min, deg/min Example: When the maximum feedrate is 15000 mm/min, the minimum
interval between pitch error compensation positions is 2 mm. If setting a magnification causes the absolute value of the compensation amount at a compensation position to exceed 100, enlarge the interval between the compensation positions by using a multiple calculated as follows: Multiple = maximum compensation amount (absolute value)/128 (Round the remainder up to the nearest integer.) Minimum interval between pitch error compensation positions = Value obtained from the above maximum feedrate × multiple
[Example 1] For linear axis • Machine stroke: -400 mm to + 800 mm
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 181 -
• Interval between the pitch error compensation positions: 50 mm • No. of the compensation position of the reference position: 40 If the above is specified, the No. of the farthest compensation point in the negative direction is as follows: No. of the compensation position of the reference position - (Machine stroke length in the negative direction/Interval between the compensation points) + 1 = 40 - 400/50 + 1 =33 No. of the farthest compensation position in the positive direction is as follows: No. of the compensation position of the reference position + (Machine stroke length in the positive direction/Interval between the compensation positions) = 40 + 800/50 = 56 The correspondence between the machine coordinate and the compensation position No. is as follows:
Machine coordinate (mm)
Compensation point No.
-400 -350 -100 -50 0 50 100 750 800
33 39 40 41 42 56
Compensation values are output at the positions indicated by f.
Therefore, set the parameters as follows:
Parameter Setting No. 3620: Compensation point number for reference position 40 No. 3621: Compensation point number for farthest point in the negative direction
33
No. 3622: Compensation point number for farthest point in the positive direction
56
No. 3623: Compensation magnification 1 No. 3624: Compensation point interval 50000
The compensation value is output at the compensation position No. corresponding to each section between the coordinates. The following is an example of the compensation values.
No. 33 34 35 36 37 38 39 40 41 42 43 44 45 46 47 48 49 Compensation values +2 +1 +1 -2 0 -1 0 -1 +2 +1 0 -1 -1 -2 0 +1 +2
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 182 -
Pitch error compensation amount (absolute value)
Reference position
-400 -300 -200 -100 0 100 200 300 400 (mm) -1
-2
-3
-4
+4
+3
+2
+1
[Example 2] For the rotation axis • Amount of movement per rotation: 360° • Interval between pitch error compensation position: 45° • No. of the compensation position of the reference position: 60 If the above is specified, the No. of the farthest compensation position in the negative direction for the rotation axis is always equal to the compensation position No. of the reference position. The No. of the farthest compensation position in the positive direction is as follows: No. of the compensation position of the reference position + (Move amount per rotation/Interval between the compensation position) = 60 + 360/45 = 68 The correspondence between the machine coordinate and the compensation position No. is as follows: The compensation value is output at the circled position. If the sum of the compensation value from 61 to 68 is not zero, the pitch error per rotation accumulates, resulting in a positional shift. For compensation position 60, set the same compensation value as for 68.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 183 -
Reference position 0.0
315.0
270.0
225.0
180.0
135.0
90.0
45.0 (68)
(60)
(67)
(66)
(65)(64)
(63)
(62)
(61)
(+)
Set the parameters as follows:
Parameter Setting No. 3620: Compensation point number for reference position 60 No. 3621: Compensation point number for farthest point in the negative direction
60
No. 3622: Compensation point number for farthest point in the positive direction
68
No. 3623: Compensation magnification 1 No. 3624: Compensation point interval 45000
The following is an example of compensation values.
No. of the compensation position 60 61 62 63 64 65 66 67 68
Compensation value +1 -2 +1 +3 -1 -1 -3 +2 +1
Pitch error compensation value (absolute value)
Reference position
0 90 (deg)
-1
-2
-3
-4
+4
+3
+2
+1
0 135 180 225 270 315 45 90 135 180 225 270 315 45
Machine coordinate
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 184 -
3625 Travel distance per revolution in pitch error compensation of rotation axis
type
NOTE When this parameter has been set, the power must
be turned off before operation is continued.
[Data type] 2-word axis [Valid data range] 0 to 99999999
If the pitch error compensation of rotation axis type is performed (bit 1 (ROSx) of parameter No. 1006 is set to 0 and bit 0 (ROTx) of parameter No. 1006 is set to 1), set the travel distance per revolution. The travel distance per revolution does not have to be 360 degrees, and a cycle of pitch error compensation of rotation axis type can be set. However, the travel distance per revolution, compensation interval, and number of compensation points must satisfy the following condition: (Travel distance per revolution) = (Compensation interval) × (Number of compensation points) The compensation at each compensation point must be set so that the total compensation per revolution equals 0.
NOTE 1 If 0 is set, the travel distance per revolution
becomes 360 degrees. 2 When setting a value other than 360 (and 0)
degrees, set the same value as the value set in parameter No. 1260.
3626 Number of pitch error compensation point at the farthest end in the negative
direction (for movement in the negative direction)
NOTE When this parameter has been set, the power must
be turned off before operation is continued.
[Data type] Word axis [Unit of data] Number [Valid data range] 0 to 1023, 3000 to 4023
When using both-direction pitch error compensation, set the number of pitch error compensation point at the farthest end in the negative direction for a movement in the negative direction.
NOTE 1 For a movement in the positive direction, set the
compensation point number at the farthest end in the negative direction in parameter No. 3621.
2 A set of compensation data items for a single axis should not be set to lie astride 1023 and 3000.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 185 -
3627 Pitch error compensation (absolute value) at reference position when a
movement to the reference position is made from the direction opposite to the direction of reference position return
NOTE When this parameter has been set, the power must
be turned off before operation is continued.
[Data type] Word axis [Unit of data] Detection unit [Valid data range] -32768 to 32767
Set the absolute value of pitch error compensation at reference position when a movement to the reference position is made from the negative direction if the direction of reference position return (bit 5 (ZMI) of parameter No. 1006) is positive or from the positive direction if the direction of reference position return is negative.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 186 -
4.20 PARAMETERS OF SPINDLE CONTROL
#7 #6 #5 #4 #3 #2 #1 #0
3700 ESP ESV MSE NRF
[Data type] Bit NRF The first move command (such as G00 and G01) after the serial
spindle is switched to Cs axis contouring control performs: 0 : Positioning after returning to the reference position. 1 : Normal positioning.
NOTE When using the Cs axis establishment function,
this parameter is recommended to be set to 1.
MSE Rigid tapping synchronization error data output when bit 5 (ESV) of parameter No. 3700 is set to 1 or when bit 7 (ESP) of parameter No. 3700 is set to 1 is: 0 : A synchronization error in the positional deviation. (equivalent
to DGN No. 456) 1 : A synchronization error in the machine position. (equivalent to
DGN No. 459) ESV When bit 7 (ESP) of parameter No. 3700 is set to 1, rigid tapping
synchronization error data is: 0 : Not output to the servo system. 1 : Output to the servo system.
NOTE Set this parameter as necessary when making
servo and spindle adjustments by using a servo guide and so forth. After completing adjustments, reset this parameter to 0.
ESP Rigid tapping synchronization error data is:
0 : Not output to the spindle. 1 : Output to the spindle.
NOTE Set this parameter as necessary when making
servo and spindle adjustments by using a servo guide and so forth. After completing adjustments, reset this parameter to 0.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 187 -
#7 #6 #5 #4 #3 #2 #1 #0
3701 SS2 ISI
NOTE When this parameter is set, the power must be
turned off before operation is continued.
[Data type] Bit ISI The serial interface for the first and second spindles are:
0 : Used. 1 : Not used.
NOTE 1 This parameter is valid when the spindle serial
output option is provided. 2 It is used when the CNC is started with serial
interface control for the first and second serial spindles disabled temporarily (for example, for CNC startup adjustment).
3 Usually, it should be set to 0. 4 If this parameter is set to 1 when using the serial
spindle and analog spindle at the same time, the analog spindle is set the first axis.
SS2 In serial spindle control, the second spindle is:
0 : Not used. 1 : Used.
NOTE 1 This parameter is valid, when the spindle serial
output option is provided and parameter ISI(bit 1 of parameter No.3701)is 0.
2 (a) Confirmation of connection of the second serial spindle amplifier, and communication with it
(b) Control of the second spindle during asynchronous control (SIND2)
When this parameter is set, it is also necessary to set the serial spindle parameter for the second spindle.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 188 -
#7 #6 #5 #4 #3 #2 #1 #0
3702 OR2 OR1
NOTE When this parameter is set, the power must be
turned off before operation is continued.
[Data type] Bit OR1 Whether the stop-position external-setting type orientation function is
used by the first spindle motor 0 : Not used 1 : Used
OR2 Whether the stop-position external-setting type orientation function is used by the second spindle motor 0 : Not used 1 : Used
#7 #6 #5 #4 #3 #2 #1 #0
MPP 3703
NOTE When this parameter is set, the power must be
turned off before operation is continued.
[Data type] Bit MPP Under multi-spindle control, the spindle is not selected by a spindle
signal (SWS1 to SWS3 <G027 bits 0 to 2>), and a programmed command (address P) is: 0 : Not used. 1 : Used.
NOTE If this parameter is set to 1, set parameters No.
3781 to No. 3783 as well.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 189 -
#7 #6 #5 #4 #3 #2 #1 #0
3704 CSS SSS
NOTE When this parameter has been set, the power must
be turned off before operation is continued.
[Data type] Bit
SSS Synchronous spindle control by each spindle is: 0 : Not performed. 1 : Performed. The master axis and slave axis of synchronous spindle control can be selected from the first to second spindles. The target spindle of synchronous spindle control is specified in parameters No. 4831 to 4832. In addition, the following signals affect the control. Synchronous spindle signal of each spindle SPSYC1 to SPSYC2 <G288 bits 0 to 1> Signal of synchronous control of the spindle phase for each spindle SPPHS1 to SPPHS2 <G289 bits 0 to 1>
CSS On the second spindle, Cs contour control is: 0 : Not performed. 1 : Performed. If Cs contour control is performed on each spindle as specified by this parameter, set parameter No. 1023 as indicated below. Setting -1 = Axis of Cs contour control by the first spindle -2 = Axis of Cs contour control by the second spindle
NOTE 1 A single spindle cannot be specified as multiple
axes of Cs contour control. 2 This parameter cannot be used with the spindle
positioning function. When using the spindle positioning function, set bit 7 (CSS) of parameter No. 3704 to 0.
#7 #6 #5 #4 #3 #2 #1 #0
EVS ESF 3705
SFA NSF SGT SGB GST ESF
[Data type] Bit ESF When the spindle control function (Spindle analog output or Spindle
serial output) is used, and the constant surface speed control function is used or bit 4 (GTT) of parameter No.3705 is set to 1: 0 : S codes and SF are output for all S commands. 1 : S codes and SF are not output for an S command in constant
surface speed control mode (G96 mode) or for an S command used to specify maximum spindle speed clamping (G50S---;)
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 190 -
NOTE For the T series, this parameter is enabled when bit
4 (EVS) of parameter No.3705 is set to 1. For the M series, SF is not output:
(1) For an S command used to specify maximum spindle speed clamping (G92S---;) in constant surface speed control mode
(2) When bit 5 (NSF) of parameter No.3705 is set to 1
GST The SOR signal is used for:
0 : Spindle orientation 1 : Gear shift
NOTE If the function of constant surface speed control or
bit 4 (GTT) of parameter No. 3706 is specified, this parameter is invalid.
SGB Gear switching method
0 : Method A (Parameters 3741 to 3743 for the maximum spindle speed at each gear are used for gear selection.)
1 : Method B (Parameters 3751 and 3752 for the spindle speed at the gear switching point are used for gear selection.)
SGT Gear switching method during tapping cycle (G84 and G74) 0 : Method A (Same as the normal gear switching method) 1 : Method B (Gears are switched during tapping cycle according to
the spindle speed set in parameters 3761 and 3762). EVS When the spindle control function (Spindle analog output or Spindle
serial output) is used, S codes and SF are: 0 : Not output for an S command. 1 : Output for an S command.
NOTE The output of S codes and SF for an S command in
constant surface speed control mode (G96), or for an S command used to specify maximum spindle speed clamping (G50S---;) depends on the setting of bit 0 (ESF) of parameter No.3705.
NSF If the function of constant surface speed control is specified or if bit 4
(GTT) of parameter No. 3706 is set to 1 and when an S code is specified, 0 : SF is output. 1 : SF is not output.
SFA The SF signal is output: 0 : When gears are switched. 1 : Irrespective of whether gears are switched.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 191 -
#7 #6 #5 #4 #3 #2 #1 #0
TCW CWM ORM PG2 PG1 3706
TCW CWM ORM GTT PG2 PG1
[Data type] Bit PG2 and PG1 Gear ratio of spindle to position coder
Magnification PG2 PG1 ×1 0 0 ×2 0 1
Number of spindle revolutions
×4 1 0 Magnification=
×8 1 1 Number of position coder revolutions
GTT Selection of a spindle gear selection method
0: Type M. 1 : Type T.
NOTE 1 The gear selection method differs as described
below. For details, refer to the description of spindle control in the connection manual (function part).
Type M: The CNC determines a proper gear from the
parameter setting and S command value, and requests the PMC to specify the gear and its switching.
In addition, spindle control is exercised according to a gear selected by the CNC.
Type T: The CNC exercises spindle control according to a
gear selected by the PMC. 2 When the constant surface speed control option is
selected, type T is selected, regardless of whether this parameter is specified.
3 When type T spindle gear switching is selected, the following parameters have no effect:
No.3705#2 SGB, No.3751, No.3752, No.3705#3 SGT,
No.3761, No.3762, No.3705#6 SFA, No.3735, No.3736
On the other hand, parameter No. 3744 becomes usable for ordinary spindle control.
ORM Voltage polarity during spindle orientation
0 : Positive 1 : Negative
TCW, CWM Voltage polarity when the spindle speed voltage is output TCW CWM Voltage polarity
0 0 Both M03 and M04 positive 0 1 Both M03 and M04 negative
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 192 -
1 0 M03 positive, M04 negative 1 1 M03 negative, M04 positive
#7 #6 #5 #4 #3 #2 #1 #0
3707 P22 P21
[Data type] Bit P22 and P21 Gear ratio of spindle to second position coder
Magnification P22 P21 ×1 0 0 ×2 0 1
Number of spindle revolutions
×4 1 0 Magnification=
×8 1 1 Number of position coder revolutions
NOTE This parameter is valid when the multi-spindle
control option is selected.
#7 #6 #5 #4 #3 #2 #1 #0
TSO SOC SVD SAT SAR 3708
TSO SOC SVD SAR
[Data type] Bit SAR The spindle speed arrival signal is:
0 : Not checked 1 : Checked
SAT Check of the spindle speed arrival signal at the start of executing the thread cutting block 0 : The signal is checked only when SAR, #0 of parameter 3708, is
set. 1 : The signal is always checked irrespective of whether SAR is set.
NOTE When thread cutting blocks are consecutive, the
spindle speed arrival signal is not checked for the second and subsequent thread cutting blocks.
SVD When the SIND signal is on, the detection of spindle speed fluctuation
is: 0 : Disabled 1 : Enabled
SOC During constant surface speed control (G96 mode), the speed clamp by the maximum spindle speed clamp command (M series: G92 S_; T series: G50 S_;) is carried out: 0 : Before spindle speed override. 1 : After spindle speed override. If this parameter is set to 0, the spindle speed may exceed the maximum spindle speed (numeric value following S in G92 S_; (M series) or G50 S_; (T series)). If this parameter is set to 1, the spindle speed is limited to the maximum spindle speed.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 193 -
The spindle speed is limited to the upper limit of spindle speed specified in parameter No. 3772, irrespective of the setting of this parameter.
TSO During a threading or tapping cycle, the spindle override is: 0 : Disabled (tied to 100%). 1 : Enabled.
NOTE During rigid tapping, the override is tied to 100%,
irrespective of the setting of this parameter.
#7 #6 #5 #4 #3 #2 #1 #0
THB MRS MSI RSC SAM 3709
SMC RSC
[Data type] Bit SAM The sampling frequency to obtain the average spindle speed
0 : 4 (Normally, set to 0.) 1 : 1
RSC In the constant surface speed control mode, the surface speed of a rapid traverse block is calculated: 0 : In accordance with the coordinates of the end point. 1 : In accordance with the current value, as in cutting feed.
MSI In multi-spindle control, the SIND signal is valid 0 : Only when the first spindle is valid (SIND signal for the 2nd, 3rd
spindle becomes ineffective) 1 : For each spindle irrespective of whether the spindle is selected
(Each spindle has its own SIND signal). MRS When the S 12-bit code signals and actual spindle speed signals are
output in multi-spindle control: 0: Signals common to the first through second spindles are used.
In this case, information about a spindle selected by the spindle selection signal (SWS1-SWS2<G027#0-#1>) is output.
1: Information about each of the first through third spindles is output on individual signals.
Signal When MRS is set to 0 When MRS is set to 1 S 12-bit code signals R01O-R12O<F036,F037> Actual spindle speed signals AR0-AR15<F040,F041>
First spindle (SWS1 = 1) Second spindle (SWS1 = 0, SWS2 = 1)
First spindle
S 12-bit code signals 2 R01O3-R12O2<F200,F201> Actual spindle speed signals 2 AR200-AR215<F202,F203>
- Second spindle
NOTE To use this parameter, the multi-spindle control
option and spindle serial output are required.
SMC The function to check a large S command is:
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 194 -
0 : Not used. 1 : Used. If a spindle gear of M type is selected, this function compares the specified S value and the settings of parameters No. 3741 to No. 3743 and raises an alarm if the S value is greater. If this function is used, specifying an S value larger than the settings of parameters No. 3741 to No. 3743 causes P/S alarm 5310 to be raised.
NOTE This function cannot be used together with any of
bit 4 (GTT) of parameter No. 3706, constant surface speed control, or multi-spindle control.
THB The threading start type is:
0 : Type A. 1 : Type B.
NOTE When using PMC axis control, set this parameter to
1.
#7 #6 #5 #4 #3 #2 #1 #0
CSL 3710
CSL SGR
[Data type] Bit SGR When method B is selected as the spindle gear switching method for a
tapping cycle (G84 or G74) (bit 3 (SGT) of parameter No. 3705 = 1), gear switching method B is used for: 0 : Both tapping and rigid tapping. 1 : Rigid tapping only.
CSL In Cs contour control mode, fine acceleration/deceleration is disabled for: 0 : An axis selected by the signal (CDFn <G0127>) issued from the
PMC. (n = 1 to 4) 1 : An axis for which interpolation is performed with the Cs contour
controlled axis (parameter No. 39n0). (n = 0 to 2)
#7 #6 #5 #4 #3 #2 #1 #0
3712 CSF
[Data type] Bit CSF The Cs axis coordinate setup function is:
0 : Disabled. 1 : Enabled.
NOTE When setting this parameter to 1, also set bit 5 of
parameter No. 4353 to 1.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 195 -
#7 #6 #5 #4 #3 #2 #1 #0
SIM 3713
NOTE When this parameter has been set, the power must
be turned off before operation is continued.
[Data type] Bit SIM In multi-spindle control, when address P is used for spindle selection
(bit 3 of parameter No. 3703 = 1), and an axis move command and S command are specified in the same block: 0 : The S command becomes valid after an axis movement is
completed. 1 : The S command becomes valid at the same time when an axis
movement is made.
#7 #6 #5 #4 #3 #2 #1 #0
3715 NSAx
[Data type] Bit axis NSAx This parameter specifies an axis for which confirmation of the spindle
speed reached signal (SAR) is unnecessary when a move command is executed for the axis. When a move command is issued only for an axis for which 1 is set in this parameter, the spindle speed reached signal (SAR) is not checked. 0 : Confirmation of SAR is necessary. 1 : Confirmation of SAR is unnecessary.
3730 Data used for adjusting the gain of the analog output of spindle speed
[Data type] Word [Unit of data] 0.1 % [Valid data range] 700 to 1250
Set data used for adjusting the gain of the analog output of spindle speed.
[Adjustment method] (1) Assign standard value 1000 to the parameter. (2) Specify the spindle speed so that the analog output of the spindle
speed is the maximum voltage (10 V). (3) Measure the output voltage. (4) Assign the value obtained by the following equation to parameter
No.3730. 10 (V)
Set value= Measured data (V)
×1000
(5) After setting the parameter, specify the spindle speed so that the analog output of the spindle speed is the maximum voltage. Confirm that the output voltage is 10V.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 196 -
NOTE This parameter needs not to be set for serial
spindles.
3731 Compensation value for the offset voltage of the analog output of the spindle
speed
[Data type] Word [Unit of data] Velo [Valid data range] -1024 to+1024
Set compensation value for the offset voltage of the analog output of the spindle speed.
-8191 × Offset voltage (V) Set value=
12.5 [Adjustment method]
(1) Assign standard value 0 to the parameter. (2) Specify the spindle speed so that the analog output of the spindle
speed is 0. (3) Measure the output voltage. (4) Assign the value obtained by the following equation to parameter
No.3731. -8191 × Offset voltage (V)
Set value= 12.5
(5) After setting the parameter, specify the spindle speed so that the analog output of the spindle speed is 0. Confirm that the output voltage is 0V.
NOTE This parameter usually need not to be set for serial
spindles (Set to 0).
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 197 -
3732 The spindle speed during spindle orientation or the spindle motor speed
during spindle gear shift
[Data type] Word [Valid data range] 0 to 20000
Set the spindle speed during spindle orientation or the spindle motor speed during gear shift. When GST, #1 of parameter 3705, is set to 0, set the spindle speed during spindle orientation in rpm. When GST, #1 of parameter 3705, is set to 1, set the spindle motor speed during spindle gear shift calculated from the following formula. For a serial spindle
Spindle motor speed during spindle gear shift Set value=
Maximum spindle motor speed ×16383
For an analog spindle
Spindle motor speed during spindle gear shift Set value=
Maximum spindle motor speed ×4095
3735 Minimum clamp speed of the spindle motor
[Data type] Word [Valid data range] 0 to 4095
Set the minimum clamp speed of the spindle motor. Minimum clamp speed of the spindle motor
Set value= Maximum spindle motor speed
×4095
NOTE If the function of constant surface speed control or
bit 4 (GTT) of parameter No. 3706 is specified, this parameter is invalid.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 198 -
3736
Maximum clamp speed of the spindle motor
[Data type] Word [Valid data range] 0 to 4095
Set the maximum clamp speed of the spindle motor. Maximum clamp speed of the spindle motor
Set value= Maximum spindle motor speed
×4095
NOTE If the function of constant surface speed control or
bit 4 (GTT) of parameter No. 3706 is specified, this parameter is invalid.
In this case, the maximum clamp speed of spindle motor cannot be specified. However, the maximum spindle speed can be specified by the following parameters.
Parameter No.3772 (for the first axis) Parameter No.3802 (for the second axis) Parameter No.3882 (for the third axis)
Spindle motor speed
Max. speed (4095, 10V)
Spindle motor max. clamp speed (Parameter No.3736)
Spindle motor minimum clamp speed (Parameter No.3735)
Spindle speed (S command)
Fig.4.20 (a) Maximum Clamp Speed of Spindle Motor
3740 Time elapsed prior to checking the spindle speed arrival signal
[Data type] Byte [Unit of data] msec [Valid data range] 0 to 225
Set the time elapsed from the execution of the S function up to the checking of the spindle speed arrival signal.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 199 -
3741 Maximum spindle speed for gear 1
3742 Maximum spindle speed for gear 2
3743 Maximum spindle speed for gear 3
Maximum spindle speed for gear 4 3744
(Note)
[Data type] Two-word [Unit of data] min-1 [Valid data range] 0 to 32767
Set the maximum spindle speed corresponding to each gear.
Spindle speed command (S command)
Spindle motor speed
Max. speed (4095, 10V)
Spindle motor max. clamp speed (Parameter No.3736)
Spindle motor minimum clamp speed (Parameter No.3735)
Gear 1 Max. speed (Parameter No.3741)
Gear 2 Max. speed (Parameter No.3742)
Gear 3 Max. speed (Parameter No.3743)
(Example for M series)
Fig.4.20 (b) Maximum Spindle Speed Corresponding to Gear 1/2/3
NOTE If a type-T gear shift scheme is selected for the M
series (with the constant surface speed control option installed or parameter GTT (bit 4 of parameter No. 3706) = 1), parameter No. 3744 is usable also in the M series.
Note, however, that, even in this case, only up to three main gear stages are usable for rigid tapping.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 200 -
3751
Spindle motor speed when switching from gear 1 to gear 2
3752
Spindle motor speed when switching from gear 2 to gear 3
[Data type] Word [Valid data range] 0 to 4095
For gear switching method B, set the spindle motor speed when the gears are switched.
Spindle motor speed when the gears are switched Set value=
Maximum spindle motor speed ×4095
Spindle motor max. clamp speed Parameter No.3736
Parameter No.3752
Spindle speed command (S command)
Max. speed (4095, 10V)
Speed at gear 1-2 change point Parameter No.3751
Spindle motor minimum clamp speed Parameter No.3735
Spindle motor speed
Gear 1 max. speed parameter No.3741
Gear 2 max. speed parameter No.3742
Gear 3 max speed parameter No.3743
Gear 1-2 change point
Gear 2-3 change point
Speed at gear 2-3 change point
Fig.4.20 (c) Spindle Motor Speed at Gear 1-2/2-3 Change Point
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 201 -
3761
Spindle speed when switching from gear 1 to gear 2 during tapping
3762
Spindle speed when switching from gear 2 to gear 3 during tapping
[Data type] 2-word [Unit of data] min-1 [Valid data range] 0 to 32767
When method B is selected (SGT,#3 of parameter 3705, is set to 1) for the tapping cycle gear switching method, set the spindle speed when the gears are switched.
Max. speed (4095, 10V)
Spindle motor max. clamp speed (Parameter No.3736)
Spindle motor minimum clamp speed (Parameter No.3735)
Spindle motor speed
Spindle speed command (S command)
Gear 1 Max. speed Parameter No.3741
Gear 2 Max. speed Parameter No.3742
Gear 3 Max. speed Parameter No.3743
Gear 1-2 change point parameter No.3761
Gear 2-3 change point parameter No.3762
Fig.4.20 (d) Spindle Motor Speed at Gear 1-2/2-3 Change Point during Tapping
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 202 -
3770 Axis as the calculation reference in constant surface speed control
[Data type] Byte [Valid data range] 0, 1, ..., number of control axes
Set the axis as the calculation reference in constant surface speed control.
NOTE When 0 is set, constant surface speed control is
always applied to the X-axis. In this case, specifying P in a G96 block has no effect on the constant surface speed control.
3771 Minimum spindle speed in constant surface speed control mode (G96)
[Data type] 2-word [Unit of data] min-1 [Valid data range] 0 to 32767
Set the minimum spindle speed in the constant surface speed control mode (G96). The spindle speed in constant surface speed control is clamped to the speed given by parameter 3771.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 203 -
3772 Maximum spindle speed
[Data type] 2-word [Unit of data] min-1 [Valid data range] 0 to 32767
This parameter sets the maximum spindle speed. When a command specifying a speed exceeding the maximum speed of the spindle is specified , or the speed of the spindle exceeds the maximum speed because of the spindle speed override function, the spindle speed is clamped at the maximum speed set in the parameter.
NOTE 1 For M series, this parameter is valid if the function
of constant surface speed control is provided or parameter GTT (bit 4 of No. 3706) is set to 1.
2 When the constant surface speed control is selected, the spindle speed is clamped at the maximum speed, regardless of whether the G96 mode or G97 mode is specified.
3 When 0 is set in this parameter, the speed of the spindle is not clamped.
4 When spindle speed command control is applied using the PMC, this parameter has no effect, and the spindle speed is not clamped.
5 When the multi-spindle control is selected (T series), set the maximum speed for each spindle in the following parameters: Parameter No.3772: Sets the maximum speed for the first spindle. Parameter No.3802: Sets the maximum speed for the second spindle. Parameter No.3822: Sets the maximum speed for the third spindle.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 204 -
P code for selecting the first spindle in multi-spindle control 3781
P code for selecting the second spindle in multi-spindle control 3782
P code for selecting the third spindle in multi-spindle control 3783
NOTE When this parameter has been set, the power must
be turned off before operation is continued.
[Data type] Word [Valid data range] 0, 1 to 32767
If bit 3 (MPP) of parameter No. 3703 is set to 1, set the P code to select each spindle under multi-spindle control. Specify the P code in a block containing the S command. Example) If the P code value for selecting the second spindle is set to 3, S1000 P3; causes the second spindle to rotate at S1000.
NOTE 1 This parameter is valid if bit 3 (MPP) of parameter
No. 3703 is set to 1. 2 If this parameter is set to 0, the corresponding
spindle cannot be selected by a P code. 3 Identical P code values cannot be used for different
spindles. 4 If this parameter is used (bit 3 (MPP) of parameter
No. 3703 is set to 1), signals SWS1 to SWS3 <G027 bits 0 to 2> become invalid.
5 To use this parameter, the multi-spindle control function is needed.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 205 -
3802 Maximum speed of the second spindle
[Data type] 2-word [Unit of data] min-1 [Valid data range] 0 to 32767
Parameter sets the maximum speed for the second spindle. When a command specifying a speed exceeding the maximum speed of the spindle is specified, or the speed of the spindle exceeds the maximum speed because of the spindle speed override function, the spindle speed is clamped at the maximum speed set in the parameter.
NOTE 1 This parameter is valid when the multi-spindle
control is selected. 2 When the constant surface speed control is
selected, the spindle speed is clamped to a maximum speed, regardless of whether the G96 mode or G87 mode is set.
3 When this parameter is set to 0, parameter No. 3772 (maximum speed of the first spindle) is valid. The spindle speed is not clamped when parameter No. 3772 is set to 0.
4 When spindle speed command control is applied using the PMC, this parameter has no effect, and the spindle speed is not clamped.
3811 Maximum spindle speed for gear 1 of the second spindle
3812 Maximum spindle speed for gear 2 of the second spindle
[Data type] 2-word [Unit of data] min-1 [Valid data range] 0 to 32767
Set the maximum spindle speed for each gear of the second spindle.
NOTE These parameters are used for the multi-spindle
control.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 206 -
3820 Data for adjusting the gain of the analog output of the third-spindle speed
[Data type] Word [Unit of data] 0.1% [Valid data range] 700 to 1250
Set the data used for adjusting the gain of the analog output of the third spindle speed.
NOTE This parameter is used for controlling the
multi-spindles.
3821 Offset-voltage compensation value of the analog output of the third-spindle
speed
[Data type] Word [Unit of data] Velo [Valid data range] -1024 to 1024
Set the offset-voltage compensation value of the analog output of the third-spindle speed. (See the description of parameter No. 3731.)
NOTE This parameter is used for controlling the
multi-spindles.
3822 Maximum speed of the third spindle
[Data type] Word [Unit of data] min-1 [Valid data range] 0 to 32767
This parameter sets the maximum speed for the third spindle. When a command specifying a speed exceeding the maximum spindle speed is specified, or the spindle speed exceeds the maximum speed because of the spindle speed override function, the spindle speed is clamped at the maximum speed set in the parameter.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 207 -
NOTE 1 This parameter is valid when the multi-spindle
control is selected. 2 When the constant surface speed control option is
selected, the spindle speed is clamped to a maximum speed, regardless of whether the G96 mode or G97 mode is set.
3 When this parameter is set to 0, parameter No. 3772 (maximum speed of the first spindle) is valid. The spindle speed is not clamped when parameter No. 3772 is set to 0.
4 When spindle speed command control is applied using the PMC, this parameter has no effect, and the speed of the spindle is not clamped.
3831 Maximum spindle speed for gear 1 of the third spindle
3832 Maximum spindle speed for gear 2 of the third spindle
[Data type] Word [Unit of data] min-1 [Valid data range] 0 to 32767
Set the maximum spindle speed for each gear of the third spindle.
NOTE These parameters are used for the multi-spindle
control.
List of parameters for control of serial interface spindle Cs contouring control axis No. Data
type Description
3900
3901
3902
3903
3904
Byte
Word
Word
Word
Word
First group
Number of the servo axis whose loop gain is to be changed according to the set values of parameters 3901 to 3904 when the Cs contouring axis is controlled (set values 0 to 8) Loop gain for the servo axis when the Cs contouring axis is controlled for spindle gear 1 selection Loop gain for the servo axis when the Cs contouring axis is controlled for spindle gear 2 selection Loop gain for the servo axis when the Cs contouring axis is controlled for spindle gear 3 selection Loop gain for the servo axis when the Cs contouring axis is controlled for spindle gear 4 selection
3910
3911
3912
3913
3914
Byte
Word
Word
Word
Word
Second group
Number of the servo axis whose loop gain is to be changed according to the set values of parameters 3911 to 3914 when the Cs contouring axis is controlled (set values 0 to 8) Loop gain for the servo axis when the Cs contouring axis is controlled for spindle gear 1 selection Loop gain for the servo axis when the Cs contouring axis is controlled for spindle gear 2 selection Loop gain for the servo axis when the Cs contouring axis is controlled for spindle gear 3 selection Loop gain for the servo axis when the Cs contouring axis is controlled for spindle gear 4 selection
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 208 -
List of parameters for control of serial interface spindle Cs contouring control axis No. Data
type Description
3920
3921
3922
3923
3924
Byte
Word
Word
Word
Word
Third group
Number of the servo axis whose loop gain is to be changed according to the set values of parameters 3921 to 3924 when the Cs contouring axis is controlled (set values 0 to 8) Loop gain for the servo axis when the Cs contouring axis is controlled for spindle gear 1 selection Loop gain for the servo axis when the Cs contouring axis is controlled for spindle gear 2 selection Loop gain for the servo axis when the Cs contouring axis is controlled for spindle gear 3 selection Loop gain for the servo axis when the Cs contouring axis is controlled for spindle gear 4 selection
<Setting method> First, select servo axes which perform interpolation with the Cs contouring axis. (Up to three axes can be selected.) When there is no servo axis for interpolation with the Cs contouring axis, set the parameters 3900, 3910, and 3920 to 0 to terminate parameter setting. When there are servo axes for interpolation with the Cs contouring axis, the parameters must be set according to the procedure below for each axis. (1) Set the number of a servo axis (1 to 4) for interpolation with the
Cs contouring axis in parameters 39n0 (n = 0, 1, and 2). (2) Set loop gain values of the servo axis specified in (1) above
which is used when the Cs contouring axis is controlled in parameters 39n1, 39n2, 39n3, and 39n4. (There are four stages for main gears used.)
(3) When the number of specified servo axes is less than 3, set the remaining parameters (39n0) to 0 to terminate parameter setting.
When the number of a Cs contouring axis is set to parameter 39n0, the parameter is assumed to be set to 0.
NOTE 1 In general, it is difficult to set a high loop gain for a spindle motor axis when
compared with a servo axis. These parameters are provided so that, by changing the loop gain of a servo axis that requires interpolation with the Cs contour axis, interpolation control can be exercised correctly between the Cs axis and servo axis while the spindle exercises Cs contour control.
2 The loop gain of the servo axis is changed using the parameter settings made for a spindle gear selected at the time of conversion from the spindle mode to the Cs contour control mode.
In normal use, it is unlikely that the gear of the spindle is switched during Cs contour control. However, note that if the gear of the spindle is changed during Cs contour control, the loop gain of the servo axis is not changed.
3 Even when multiple Cs axes are used (bit 7 (CSS) of parameter No. 3704 = 1), these parameters are shared.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 209 -
Parameters for Serial interface spindle or spindle Parameters Nos. 4000 to 4539 below are basically used with the serial spindle amplifier (SPM). For details of these parameters, refer to either of the following manuals and other related documents, depending on the spindle that is actually connected. • FANUC AC SPINDLE MOTOR αi series Parameter Manual
(B-65280EN) • FANUC AC SPINDLE MOTOR α series Parameter Manual
(B-65160E)
#7 #6 #5 #4 #3 #2 #1 #0
4000
: :
4015 (No user setting allowed = Note 1)
: :
#7 #6 #5 #4 #3 #2 #1 #0
4019 (Note 2)
[Data type] Bit axis (spindle)
4020
: :
4133
[Data type] Word axis (spindle)
4134
4135
[Data type] 2-word axis (spindle)
4136
: :
4175
[Data type] Word axis (spindle)
#7 #6 #5 #4 #3 #2 #1 #0
4176
: :
4191 (No user setting allowed = Note 1)
: :
#7 #6 #5 #4 #3 #2 #1 #0
4195 (Note 2)
[Data type] Bit axis (spindle)
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 210 -
4196
: :
4309
[Data type] Word axis (spindle)
4310
4311
[Data type] 2-word axis (spindle)
4312
: :
4351
[Data type] Word axis (spindle)
#7 #6 #5 #4 #3 #2 #1 #0
4352
#7 #6 #5 #4 #3 #2 #1 #0
4353
[Data type] Bit axis (spindle)
4354
: :
4372
[Data type] Word axis (spindle)
#7 #6 #5 #4 #3 #2 #1 #0
4373
#7 #6 #5 #4 #3 #2 #1 #0
4374
[Data type] Bit axis (spindle)
4375
: :
4393
[Data type] Word axis (spindle)
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 211 -
#7 #6 #5 #4 #3 #2 #1 #0
4394
#7 #6 #5 #4 #3 #2 #1 #0
4403
[Data type] Bit axis (spindle)
4404
: :
4466
[Data type] Word axis (spindle)
#7 #6 #5 #4 #3 #2 #1 #0
4467
#7 #6 #5 #4 #3 #2 #1 #0
4476
[Data type] Bit axis (spindle)
4477
: :
4539
[Data type] Word axis (spindle) Notes on parameters of the spindle amplifier with the serial interface
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 212 -
NOTE 1 Among the parameters of the spindle amplifier with the serial interface, parameters
Nos. 4015 and 4191 cannot be changed by the users. These parameters require to assign optional software to the CNC and are
automatically set depending on the type of the software. 2 To set the parameters of the spindle amplifier with the serial interface automatically,
set #7 of parameter No.4019 (if the sub spindle is set in the CNC with the spindle switching function, use parameter No.4195) to 1, assign the model code of the motor to be used to parameter No.4133 (if the sub spindle is set in the CNC with the spindle switching function, use parameter No.4309), turn off the power of the CNC and spindle amplifier, and restart the CNC and spindle amplifier.
3 Parameters No.4000 to No.4539 are used in the processing on the spindle amplifier. For details of these parameters, refer to either of the following manuals, depending on the serial spindle that is actually used. - FANUC AC SPINDLE MOTOR αi series Parameter Manual B-65280EN) - FANUC AC SPINDLE MOTOR α series Parameter Manual B-65160E)
4 The CNC can control up to two spindle amplifiers with the serial interface. When the spindle amplifier provides the spindle switching function, one spindle
amplifier can control two spindle motors using the switching function. The output switching function can be used in spindle motors to be connected. Up to four spindles, or eight types, can be used by switching the spindle motors.
(The number of spindles that can controlled simultaneously is the same as the number of spindle amplifiers, that is two spindles.) Parameters of the spindle amplifier with the serial interface correspond to the above functions as follows: (1) Parameter No.4000 to No.4539 "S1": First spindle amplifier Parameter No.4000 to No.4539 "S2": Second spindle amplifier (2) Parameter No.4000 to No.4175 "S1"/"S2": When the spindle switching function
is not provided, or for the main spindle in the spindle amplifier when the function is provided.
Parameter No.4176 to No.4351 "S1"/"S2": For the sub spindle in the spindle amplifier when the spindle switching function is provided.
(3) Parameters at low speed when the output switching function is provided. Parameters No.4136 to No.4175 "S1"/"S2": When the spindle switching
function is not provided, or for the main spindle when the function is provided. Parameters No.4284 to No.4351 "S1"/"S2": For the sub spindle when the
spindle switching function is provided.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 213 -
NOTE 5 The CNC stores the parameters of the spindle amplifier with the serial interface.
The CNC sends them to the spindle amplifier at the system power on and they are used in the unit.
These parameters are sent from the CNC to the spindle amplifier in a batch when: - The CNC is switched on. - The serial spindle is restarted by a reset that is carried out after spindle
communication alarm 749 occurs (because the spindle control unit is switched off or because of noise).
If these parameters are rewritten, they are sent from the CNC to the spindle amplifier sequentially when: - The parameters have been entered from the MDI. - The parameters have been entered as programmable (G10). - The parameters have been entered via the reader/punch interface.
If bit 4 (WSP) of parameter No. 8703 is set to 0, the CNC does not immediately perform data transfer to the spindle amplifier even when data has been written to a parameter by using the PMC window function. So, the new parameter value set by rewriting does not become valid automatically. To perform data transfer immediately, set bit 4 (WSP) of parameter No. 8703 to 1.
If you want to change such parameter settings during automatic operation, use programmable parameter input (G10).
To set parameters automatically, upload parameters corresponding to the motor model from the spindle amplifier to the CNC prior to the procedure specified above.
The parameters of the spindle amplifier with serial interface can be changed after the system starts. Changing the parameters (No.4000 to No.4539 "S1", "S2") in the CNC sends them to the spindle amplifier at an appropriate time and the parameters in the unit are updated. Be careful not to change parameters incorrectly.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 214 -
#7 #6 #5 #4 #3 #2 #1 #0
SYM ND2 ND1 4800
ND2 ND1
NOTE When this parameter is set, the power must be
turned off before operation is continued.
[Data type] Bit ND1 In controlling the spindle synchronization, the direction of the first
spindle motor rotation is: 0 : The direction indicated by the command sign 1 : The opposite direction to that indicated by the command sign
ND2 In controlling the spindle synchronization, the direction of the 2nd spindle motor rotation is: 0 : The direction indicated by the command sign 1 : The opposite direction to that indicated by the command sign
SYM As the maximum spindle speed in spindle synchronization control: 0 : The maximum spindle speed of the master spindle is used. 1 : The maximum spindle speed of the master spindle or slave
spindle, whichever lower, is used.
4810 Error pulse between two spindles when synchronizing phases in the serial
spindle synchronization control mode
[Data type] Byte [Unit of data] Pulse [Valid data range] 0 to 255
Set the difference in error pulses between two spindles when synchronizing phases in the serial spindle synchronization control mode. When the difference in error pulse between two spindles is within the value set in this parameter, the spindle phase synchronization completion signal FSPPH becomes "1". This parameter is used to check the difference in phase in synchronization control and to confirm the completion of synchronization in the serial spindle synchronization control mode. For spindle synchronization, serial spindle parameters such as parameter No. 4032 must be set.
4811 Allowable error count for the error pulses between two spindles in the serial spindle synchronization control mode or simple synchronous control mode
[Data type] Word [Unit of data] Pulse [Valid data range] 0 to 32767
Set the allowable error count for the error pulses between two spindles in the serial spindle synchronization control mode or simple synchronous control mode.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 215 -
NOTE This parameter is used to output the inter-spindle
phase error detection signal SYCAL in the serial spindle synchronization control mode. The SYCAL <F044#4> signal becomes "1" when a phase error exceeding the value set in this parameter is found.
Master spindle under synchronous spindle control
4812 Slave spindle under synchronous spindle control
4813
[Data type] Byte [Valid data range] 0, 1, 2
Set the master spindle and slave spindle in spindle synchronization control. Setting value : 1 to 2, First to second spindles
NOTE These parameters are valid only in spindle
synchronization control specified by programming. If 0 is set, turning on spindle synchronization control by programming (G51.8) results in an alarm.
4831 Master axis of first spindle under synchronous spindle control
4832 Master axis of second spindle under synchronous spindle control
NOTE When these parameters have been set, the power
must be turned off before operation is continued.
[Data type] Byte [Valid data range] 1 to Number of spindles
Set the slave axis and master axis of synchronous spindle control by spindles. Set the axis number of the master axis for the axis to be handled as the slave axis.
NOTE This parameter is valid if bit 4 (SSS) of parameter
No. 3704 is set to 1.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 216 -
#7 #6 #5 #4 #3 #2 #1 #0
FLR 4900
[Data type] Bit FLR When the spindle speed fluctuation detection function is used, the
rates of allowance (q) and fluctuation (r) those are set in parameter No.4911 and No.4912, respectively are set in steps of: 0 : 1% 1 : 0.1%
Rapid (q) of the fluctuation of spindle speed which is assumed to be the specified spindle speed 4911
[Data type] Word [Unit of data, valid data range]
Unit of data 1% 0. 1% (T series) Valid data range 1 to 100 1 to 1000
NOTE Unit of data depends on parameter No.4900#0 FLR
(T series only) Set the ratio (q) of the spindle speed which is assumed to be the specified spindle speed in the spindle speed fluctuation detection function. Let the commanded speed be Sc. When the actual spindle speed reaches between (Sc-Sq) and (Sc + Sq), it is assumed to be the commanded speed. The spindle speed fluctuation detection starts. where,
q Sq = Sc ×
100
Spindle speed fluctuation ratio (r) for which no alarm is activated in the spindle speed fluctuation detection function 4912
[Data type] Word [Unit of data, valid data range]
Unit of data 1% 0. 1% (T series) Valid data range 1 to 100 1 to 1000
NOTE Unit of data depends on parameter No.4900#0 FLR
(T series only). Set the spindle speed fluctuation ratio (r) for which no alarm is activated in the spindle speed fluctuation detection function (see Fig.4.20 (e)).
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 217 -
Spindle speed fluctuation value (d) for which no alarm is activated in the
spindle speed fluctuation detection function 4913
[Data type] Word [Unit of data] min-1 [Valid data range] 0 to 32767
Set the allowable fluctuation speed (Sd) for which no alarm is activated in the spindle speed fluctuation detection function. The function for detecting spindle speed fluctuation checks whether the actual speed varies for the specified speed or not. Sd or Sr, whichever is greater, is taken as the allowable fluctuation speed (Sm). An alarm is activated when the actual spindle speed varies for the commanded speed (Sc) under the condition that the variation width exceeds the allowable variation width (Sm). Sd: The allowable constant variation width which is independent of
the specified spindle speed (Sd is set with parameter 4913.) Sr: The allowable variation width which is obtained by multiplying
Sc (commanded spindle speed) by r (constant ratio). (r is set with parameter 4912.)
Sm: Sd or Sr, whichever is greater
No check
Spindle speed
Specified speed
Actual speed
Alarm Time
Check start
Command another speed
Check Check
Sm
Sm
Sd
Sd
Fig.4.20 (e) Sd and Sm
4914 Time (p) elapsed from when the commanded spindle speed is changed to the
start of spindle speed fluctuation detection
[Data type] 2-word [Unit of data] ms [Valid data range] 0 to 999999
Set the time elapsed from when the specified spindle speed is changed to the start of spindle speed fluctuation detection in the spindle speed fluctuation detection function. That is, the fluctuation in the spindle speed is not detected until the specified time elapses from when the specified spindle speed is changed.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 218 -
No check
Spindle speed
Specified speed
Check start
Command another speed
Sd
Sd
Actual speed
Alarm Time
Check
Sm
Sm
P
Fig.4.20 (f) Sd and Sm
#7 #6 #5 #4 #3 #2 #1 #0
IMB ESI TRV ISZ IDM IOR 4950
[Data type] Bit IOR Resetting the system in the spindle positioning mode
0 : Does not releases the mode. 1 : Releases the mode
IDM The positioning direction for the spindle using a M code is 0 : The positive direction 1 : The negative direction
ISZ When an M code for spindle orientation is specified in spindle positioning: 0 : The spindle rotation mode is cleared and the mode is switched to
the spindle positioning mode, and spindle orientation operation is performed.
1 : The spindle rotation mode is cleared and the mode is switched to the spindle positioning mode but spindle orientation operation is not performed.
TRV Rotation direction of spindle positioning is set to: 0 : The positive direction 1 : The reverse direction
ESI Selection of a spindle positioning specification 0 : The conventional specification is used. 1 : The extended specification is used.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 219 -
NOTE The extended specification includes the following
two extensions: (1) With the conventional specification, the number
of M codes for specifying a spindle positioning angle is always 6. With the extended specification, an arbitrary number of such M codes from 1 to 255 can be selected by parameter setting (See parameter No.4964.)
(2) The maximum feedrate for spindle positioning (setting of parameter No.1420) can be extended from 240000 to 269000 (in increments of 10 deg/min).
IMB When the spindle positioning function is used, half-fixed angle
positioning based on M codes uses: 0 : Specification A 1 : Specification B
NOTE In the case of half-fixed angle positioning based on
M codes, three types of spindle positioning operations can occur: (1) The spindle rotation mode is cleared, then the
mode is switched to the spindle positioning mode.
(2) Spindle positioning is performed in the spindle positioning mode.
(3) The spindle positioning mode is cleared, then the mode is switched to the spindle rotation mode.
In the case of specification A: Operations (1) to (3) are specified using separate
M codes. (1) Specified using M codes for performing spindle
orientation. (See parameter No.4960) (2) Specified using M codes for specifying a
spindle positioning angle. (See parameter No.4962)
(3) Specified using M codes for clearing spindle positioning operation. (See parameter No.4961.)
In the case of specification B: When M codes for specifying a spindle positioning
angle are specified, operations (1) to (3) are performed successively. (See
parameter No.4962.)
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 220 -
M code specifying the spindle orientation 4960
[Data type] Word [Unit of data] Integer [Valid data range] 6 to 97
Set an M code to change the spindle rotating mode to the spindle positioning mode. Setting the M code performs the spindle orientation. Spindle positioning can be specified from the next block.
M code releasing the spindle positioning mode 4961
[Data type] Word [Unit of data] Integer [Valid data range] 6 to 97
Set the M code to release the spindle positioning mode and to change the mode to the spindle rotating mode.
M code for specifying a spindle positioning angle 4962
[Data type] Word [Unit of data] Integer [Valid data range] 6 to 92
Two methods are available for specifying spindle positioning. One method uses address C for arbitrary-angle positioning. The other use an M code for half-fixed angle positioning. This parameter sets an M code for the latter method. • When bit 6 (ESI) of parameter No.4950=0 Six M code from M α to M(α+5) are used for half-fixed angle
positioning, when α is the value of this parameter. • When bit 6(ESI) of parameter No.4950=1 Set the start M code in this parameter, and set the number of M
codes in parameter No.4964. Suppose that the setting of parameter No. 4962 is α and the setting of parameter No. 4964 is β. Then β M codes from Mα to M (α+β-1) are used for half fixed angle positioning.
The table below indicates the relationship between the M codes and positioning angles.
M code Positioning angle Example: Positioning angle when θ = 30° Mα θ 30°
M (α+1) 2θ 60° M (α+2) 3θ 90° M (α+3) 4θ 120° M (α+4) 5θ 150° M (α+5) 6θ 180°
: : : M (α+n) (n+1) θ
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 221 -
NOTE θ represents the basic angular displacement set in
parameter No.4963.
Basic angular displacement used for spindle positioning using M code 4963
[Data type] Word [Unit of data] deg [Valid data range] 1 to 60
This parameter sets a basic angular displacement used for half-fixed angle positioning using M codes.
Number of M codes for specifying a spindle positioning angle 4964
[Data type] Byte [Unit of data] Integer [Valid data range] 0, 1 to 255
This parameter sets the number of M codes used for Half-fixed angle positioning using M codes. As many M codes as the number specified in this parameter, starting with the M code specified in parameter No.4962, are used to specify half-fixed angle positioning. Let α be the value of parameter No.4962, and let β be the value of parameter No.4964. That is, M codes from Mα to M (α+β-1) are used for half-fixed angle positioning.
NOTE 1 This parameter is valid when bit 6 (ESI) of
parameter No.4950=1. 2 Make sure that M codes from Mα to M (α+β-1) do
not duplicate other M codes. 3 Setting this parameter to 0 has the same effect as
setting 6. That is, M code from Mα to M (α+5) are used for half-fixed angle positioning.
Servo loop gain of the spindle
4970
[Data type] Word [Unit of data] 0.01 s-1 [Valid data range] 1 to 9999
Set the servo loop gain of the spindle in the spindle positioning mode.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 222 -
Servo loop gain multiplier of the spindle for gear 1 4971
Servo loop gain multiplier of the spindle for gear 2 4972
Servo loop gain multiplier of the spindle for gear 3 4973
Servo loop gain multiplier of the spindle for gear 4 4974
[Data type] Word Set the servo loop gain multipliers of the spindle for gears 1 to 4. The multipliers are used to convert the amount of the position deviation to the voltage used in the velocity command. Assign the data obtained from the following equation to the parameters. Loop gain multiplier = 2048000 × E × A/L
where; E : Voltage required to rotate the spindle motor at 1000 min-1 in the
velocity command L : Rotation angle of the spindle per one motor rotation (normally
360) A : Unit used for the detection (degree) [Example] Let E be 2.2 V, L be 360 degrees, and A be 0.088 degrees/pulse.
Loop gain multiplier = 2048000 × 2.2 × 0.088/360 = 1101 * When the voltage specified for the spindle motor is 10 V at
a spindle speed of 4500 min-1, E is regarded as 2.2 V.
NOTE The above parameters No.4971 to No.4974 are for
analog spindles.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 223 -
4.21 PARAMETERS OF TOOL COMPENSATION
#7 #6 #5 #4 #3 #2 #1 #0
EVO EVR TAL TLB TLC 5001
EVO TPH EVR TAL OFH TLB TLC
[Data type] Bit TLC Tool length compensation
0 : Tool length compensation A or B (Conforms to TLB in parameter No.5001)
1 : Tool length compensation C TLB Tool length compensation axis
0 : Always Z axis irrespective of plane specification (Tool length compensation A)
1 : Axis perpendicular to plane specification (G17, G18, and G19) (Tool length compensation B)
OFH Offset number of tool length compensation, cutter compensation and tool offset 0 : Specifies the tool length compensation using an H code, and
cutter compensation C using a D code Tool offset conforms to TPH in parameter No.5001#5. 1 : Specifies the tool length compensation, cutter compensation and
tool offset using H codes TAL Tool length compensation C
0 : Generates an alarm when two or more axes are offset 1 : Not generate an alarm even if two or more axes are offset
EVR When a tool compensation value is changed in cutter compensation C mode: 0 : Enables the change, starting from that block where the next D or
H code is specified. 1 : Enables the change, starting from that block where buffering is
next performed. TPH Specifies whether address D or H is used as the address of tool offset
number (G45 to G48). 0 : D code 1 : H code TPH is valid when OFH in parameter No.5001#2 is 0.
EVO When in tool length compensation A or tool length compensation B, the tool compensation amount is changed in offset mode (G43 or G44) (for the M series) or when in tool position compensation, the compensation amount is changed (for the T series): 0 : A block specifying the next G43, G44, or an H code and
subsequent blocks become valid. (M series) A block specifying the next T code and subsequent blocks
become valid. (T series) 1 : A block to be buffered next and subsequent blocks become valid.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 224 -
#7 #6 #5 #4 #3 #2 #1 #0
WNP LWM LGC LGT LWT LGN LD1 5002
[Data type] Bit LD1 Offset number of tool offset
0 : Specified using the lower two digits of a T code 1 : Specified using the lower one digit of a T code
LGN Geometry offset number of tool offset 0 : Is the same as wear offset number 1 : Specifies the geometry offset number by the tool selection
number LWT Tool wear compensation is performed by:
0 : Moving the tool. 1 : Shifting the coordinate system. (Only when the LGT parameter (bit 4 of No.5002) is set to 0)
LGT Tool geometry compensation 0 : Compensated by the shift of the coordinate system
(Compensation is made in the block of T code regardless of LWM at this time.)
1 : Compensated by the tool movement LGC Tool geometry compensation (It is effective when LGT = 0. When
LGT is 1, it is always canceled.) 0 : Not canceled by offset number 0 1 : Canceled by offset number 0
LWM Tool offset (Geometry and wear compensation when LGT = 1.) 0 : Is done in the T code block 1 : Is done together with the axis movement
NOTE When LGT = 0, the offset is done in a T code block
regardless of this parameter.
WNP Imaginary tool tip direction used for tool nose radius compensation, is the direction specified by: 0 : Geometry offset number 1 : Wear offset number
#7 #6 #5 #4 #3 #2 #1 #0
TGC LVC CCN 5003
LVK CCN SUV SUP
[Data type] Bit SUP Start up or cancel in cutter compensation C or cutter compensation for
5-axis machining 0 : Type A 1 : Type B
SUV Startup or cancellation of cutter compensation C is: 0 : Type A or type B. (The setting of bit 0 (SUP) of parameter No.
5003 is followed.) 1 : Perpendicular to the next movement.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 225 -
CCN When automatic reference position return (G28) is specified in the cutter compensation C mode (M series) or in tool nose radius compensation (T series): 0 : The cutter compensation or tool nose radius compensation vector
is cancelled in movement to an intermediate position. 1 : The cutter compensation or tool nose radius compensation vector
is not cancelled in movement to an intermediate position, but is cancelled in movement to the reference position.
LVC Offset value of tool offset 0 : Not cleared, but held by reset 1 : Cleared by reset
LVK Tool length offset value 0 : Cleared by reset 1 : Not cleared, but held by reset
TGC Tool geometry compensation value 0 : Not canceled by reset 1 : Canceled by reset (Valid when LVC, #6 of parameter No.5003, is "1")
#7 #6 #5 #4 #3 #2 #1 #0
Y03 TS1 ORC 5004
ODI
NOTE When this parameter is set, the power must be
turned off before operation is continued.
[Data type] Bit ORC Tool offset value
0 : Set by the diameter specification (Can be set in only the axis under diameter programming) 1 : Set by the radius specification
ODI A cutter compensation amount is set using: 0 : A radius. 1 : A diameter.
TS1 When the tool offset measurement value direct input B function is used, touch sensor contact detection is based on: 0 : Four-contact input. 1 : One-contact input.
Y03 Y axis offset is : 0 : Used for 4th axis. 1 : Used for 3rd axis.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 226 -
#7 #6 #5 #4 #3 #2 #1 #0
TLE QNI PRC CNI 5005
[Data type] Bit CNI On the offset screen, Y-axis offset screen, and macro screen, the
[INP.C] soft key is: 0: Used. 1: Not used. (The [INP.C] soft key is not displayed.)
PRC Direct input of tool offset value and workpiece coordinate-system shift value 0 : Not use a PRC signal 1 : Uses a PRC signal
QNI In the function of input of offset value measured B 0 : Not automatically select the tool offset number 1 : Automatically selects a tool offset number
TLE When the tool offset measurement value direct input B function is used, a tool offset value, set by the offset write signal, is: 0 : Always received in offset write mode. 1 : Received only in offset write mode and during movement along
an axis (where "during movement along an axis" means that the positional deviation value is other than 0).
#7 #6 #5 #4 #3 #2 #1 #0
TGC OIM 5006
TOS TCE OIM
[Data type] Bit OIM When the unit is switched between the inch and metric systems,
automatic tool offset value conversion is: 0 : Not performed 1 : Performed
NOTE If this parameter setting is changed, reset the tool
offset data.
TGC When a T code is specified in a block containing G50, G04, or G10: 0 : No alarm occurs. 1 : P/S alarm No.245 occurs.
TCE When a tool length offset is specified in a rigid tapping or drilling canned cycle, the axis to which the tool length offset applies is: 0 : Determined according to the specifications of tool length offset
C. 1 : The drilling axis.
NOTE This parameter is valid when tool length offset C is
selected (bit 0 (TLC) of parameter No. 5001 = 1).
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 227 -
TOS The operation of tool length compensation is set as follows: 0 : Tool length compensation is performed by axis movement. 1 : Tool length compensation is performed by shifting the coordinate
system.
#7 #6 #5 #4 #3 #2 #1 #0
QCR MCR CNV CNC CNI 5008
GCS QCR MCR CNV G39 CNC CNI
[Data type] Bit CNI Interference check for cutter compensation C (M series) or tool nose
radius compensation (T series) is: 0 : Performed 1 : Not performed
CNC During interference check for cutter compensation C (M series) or tool nose radius compensation (T series), when the direction of movement after application of the offset differs from the programmed direction by between 90° and 270°: 0 : An alarm is issued. 1 : No alarm is issued.
G39 The corner rounding function (G39) in cutter compensation C mode is: 0 : Disabled. 1 : Enabled.
CNV The interference check and vector erasure of cutter compensation C (M series) or tool nose radius compensation (T series) are: 0 : Performed. 1 : Not performed.
MCR If G41/G42 (cutter compensation C (M series) or tool nose radius compensation (T series)) is specified in the MDI mode, an alarm is: 0 : Not raised. 1 : Raised. (P/S5257)
NOTE In the MDI mode, cutter compensation C (M series)
or tool nose radius compensation (T series) is not performed, irrespective of the setting of this parameter.
QCR The travel distance of circular interpolation in cutter compensation C
(M series) or tool nose radius compensation (T series) is judged: 0 : In the FS0(FS16) format. 1 : In the FS15 format. FS0(FS16) and FS15 determine the travel distance in different ways if the radius of arc at the start point of circular interpolation is different from that at the end point (if the end point is not on the arc). By this parameter, the method of determining the travel distance of circular interpolation can be selected.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 228 -
[FS0(FS16) format]
If the end point viewed from the start point is in the A region, the movement is made along the shortcut. If the end point is in the B, C, or D region, almost a single turn is made.
C
D
Start point
End point
Center
A
[FS15 format]
Start point
End point
Center
If the end point is in the A region separated by the line L drawn between the start point and the center, the movement is made along the shortcut. If the end point is in the B region, almost a single turn is made.
A
NOTE The setting of this parameter determines the travel
distance determination method for circular interpolation not during cutter compensation C (M series) or tool nose radius compensation (T series) as well. Accordingly, if this parameter is set, the setting of bit 3 (CQD) of parameter No. 3450 is invalid.
GCS If G49 (G code for canceling tool length compensation) and G40 (G
code for canceling cutter compensation) are specified in a single block, the tool length compensation is cancelled: 0 : In the next block. 1 : In the specified block.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 229 -
#7 #6 #5 #4 #3 #2 #1 #0
NTT TSD QSA GSG 5009
NOTE When this parameter has been set, the power must
be turned off before operation is continued.
[Data type] Bit GSG In the mode of tool compensation direct input B, the offset write input
signal is input: 0 : From the machine side. <G004 bits 2 to 5> 1 : From the PMC side. <G132 bits 0 and 1, G134 bits 0 and 1>
QSA The angular axis control function is: 0 : Not supported by the tool compensation direct input B function. 1 : Supported by the tool compensation direct input B function.
TSD In the tool compensation direct input B function, the error prevention function is: 0 : Disabled. 1 : Enabled.
NTT When a shift type tool offset is applied during simplified synchronization control, and the master spindle and slave spindle are not related to the tool offset: 0 : An alarm is issued. (P/S alarm 214) 1 : No alarm is issued.
Limit value that ignores the vector when a tool moves on the outside of a
corner during tool nose radius compensation 5010
Limit value that ignores the vector when a tool moves on the outside of a
corner during cutter compensation C
[Data type] Word [Unit of data]
Input increment IS-A IS-B IS-C Unit Millimeter input 0.01 0.001 0.0001 mm
Inch input 0.001 0.0001 0.00001 inch
[Valid data range] 0 to 16383 This parameter sets the limit value that ignores a slight movement occurring when a tool moves on the outside of the corner during tool nose radius compensation (T series) or cutter compensation C (M series).
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 230 -
Very small amount of travel to be ignored
Programmed path
Actual tool path Very small amount of travel to be ignored
5013 Maximum value of tool wear compensation
[Data type] 2-word [Unit of data]
Input increment IS-A IS-B IS-C Unit Millimeter input 0.01 0.001 0.0001 mm
Inch input 0.001 0.0001 0.00001 inch
[Valid data range] Input increment IS-A IS-B IS-C Millimeter input 0 to 99999 0 to 999999 0 to 9999999
Inch input 0 to 99999 0 to 999999 0 to 9999999 This parameter sets the maximum allowable tool wear compensation value. If an attempt is made to set a tool wear compensation value, the absolute value of which exceeds the value set in this parameter, the following alarm or warning is output: Input from MDI Warning: Too many digits Input by G10 P/S alarm No.032: Offset value is out of range by G10.
5014 Maximum value of incremental input for tool wear compensation
[Data type] 2-word [Unit of data]
Input increment IS-A IS-B IS-C Unit Millimeter input 0.01 0.001 0.0001 mm
Inch input 0.001 0.0001 0.00001 inch
[Valid data range] Input increment IS-A IS-B IS-C Millimeter input 0 to 99999 0 to 999999 0 to 9999999
Inch input 0 to 99999 0 to 999999 0 to 9999999
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 231 -
Set the maximum allowable value for the tool wear compensation value, input as an incremental value. If the incremental input value (absolute value) exceeds the set value, the following alarm or warning message is output: Input from MDI Warning: Setting value out of range. Input using G10 P/S alarm No.032: Offset value is out of range by G10.
Distance (XP) between reference position and X axis + contact surface
Distance (X1P) between reference position and X axis + contact surface of touch sensor 1 5015
Distance (XM) between reference position and X axis - contact surface
Distance (X1M) between reference position and X axis - contact surface of touch sensor 1 5016
Distance (ZP) between reference position and Z axis + contact surface
Distance (Z1P) between reference position and Z axis + contact surface of touch sensor 1 5017
Distance (ZM) between reference position and Z axis - contact surface
Distance (Z1M) between reference position and Z axis - contact surface of touch sensor 1 5018
[Data type] 2-word [Unit of data]
Input increment IS-B IS-C Unit Millimeter input 0.001 0.0001 mm
Inch input 0.0001 0.00001 inch
[Valid data range] -99999999 to 99999999 These parameters are related to the function of input of tool offset value measured B. They set the distance (with sign) between the measurement reference position and sensor contact surface. For an axis under diameter programming, set it by a diameter value.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 232 -
Xm
Xp
Z-axis +contact face Z-axis -contact face
X-axis -contact face
X-axis +contact face
Zm
Zp
+Z
+X
measurement reference position
Fig.4.21 Distance along X and Z Axes from the Reference Position to +/- Contact Surfaces
Tool offset number used for the input of tool offset value measured B
5020
[Data type] Byte [Valid data range] 1 to the maximum number of tool compensation sets
Set a tool offset number to be used for setting the amount by which the workpiece coordinate system is shifted by the tool compensation direct input B function. This parameter is valid when the tool offset number is not selected automatically (QNI, #5 of parameter 5005, is zero).
Number of pulse interpolation cycles memorized prior to contacting the
touch sensor 5021
[Data type] Byte [Unit of data] Interpolation cycle [Valid data range] 0 to 8
When the error prevention function in the tool compensation direct input B function is used, or when a touch sensor with single-contact signal input is used, this parameter sets the number of interpolation cycles of pulses stored immediately before the tool is brought into contact with the touch sensor by manual operation. If 0 is set for this parameter, the specification of 8 (maximum allowable value) is assumed.
NOTE This parameter is enabled when the TS1
parameter (bit 3 of parameter No.5004) is set to 1.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 233 -
5030
Minimum grinding wheel diameter in minimum grinding wheel diameter
check
[Data type] 2-word [Unit of data]
Input increment IS-A IS-B IS-C Unit Millimeter input 0.01 0.001 0.0001 mm
Inch input 0.001 0.0001 0.00001 inch
[Valid data range] Input increment IS-A, IS-B IS-C Millimeter input -999999 to 999999 -9999999 to 9999999
Inch input -999999 to 999999 -9999999 to 9999999 If the compensation value corresponding to an offset number specified by an H code is smaller than the minimum grinding wheel diameter specified in this parameter during compensation with G43 or G44, the signal F0065#3 GWLF is output to the PMC.
NOTE This is a parameter for cylindrical grinding
machines.
#7 #6 #5 #4 #3 #2 #1 #0
OWD 5040
NOTE When this parameter has been set, the power must
be turned off before operation is continued.
[Data type] Bit OWD In radius programming (bit 1 (ORC) of parameter No. 5004 is set to
1), 0 : Tool offset values of both geometry compensation and wear
compensation are specified by radius. 1 : Tool offset value of geometry compensation is specified by
radius and tool offset value of wear compensation is specified by diameter, for an axis of diameter programming.
#7 #6 #5 #4 #3 #2 #1 #0
CRS 5041
NM2 UMD
[Data type] Bit UMD If a program contains no D command in cutter compensation C:
0 : Compensation data is not updated. 1 : If G41 or G42 command is present, the value of modal D is used
as a compensation number to update compensation data.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 234 -
CRS If a startup with a travel distance of 0 is performed after a reference position return operation when a T code specifying a virtual tool tip number other than 0 and 9 is specified, the startup block operation is as follows: 0 : The block does not make any movement. 1 : The block makes a movement so that the tool tip center is placed
at the current coordinates.
NOTE If the virtual tool tip number is 0 or 9, a movement
is made so that the tool tip center is placed at the current coordinates, regardless of the setting of this parameter.
NM2 When two or more blocks that specify no movement are specified
successively, or when an M code not buffered is specified in one block: 0 : No alarm is issued. 1 : An alarm is issued. (P/S 041 alarm)
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 235 -
4.22 PARAMETERS OF CANNED CYCLES
4.22.1 Parameter of canned Cycle for Drilling
#7 #6 #5 #4 #3 #2 #1 #0
M5T ILV RTR FXY 5101
M5B M5T RD2 RD1 EXC FXY
[Data type] Bit FXY The drilling axis in the drilling canned cycle is:
0 : Always the Z-axis 1 : The axis selected by the program
NOTE In the case of the T series, this parameter is valid
only for the drilling canned cycle in the FS10/11 format.
EXC G81
0 : Specifies a drilling canned cycle 1 : Specifies an external operation command
RTR G83 and G87 0 : Specify a high-speed peck drilling cycle 1 : Specify a peck drilling cycle
ILV Initial point position in drilling canned cycle 0 : Not updated by reset 1 : Updated by reset
RD2, RD1 Set the axis and direction in which the tool in drilling canned cycle G76 or G87 is got free. RD2 and RD1 are set as shown below by plane selection.
RD2 RD1 G17 G18 G19 0 0 +X +Z +Y 0 1 -X -Z -Y 1 0 +Y +X +Z 1 1 -Y -X -Z
M5T When a spindle rotates from the forward to the reverse direction and
vice versa in tapping cycles G84 and G74 for M series (G84 and G88 for T series), before M04 or M03 is output: For T series 0 : Not output M05 1 : Outputs M05 For M series 0 : Outputs M05 1 : Not output M05
M5B In drilling canned cycles G76 and G87: 0 : Outputs M05 before an oriented spindle stops 1 : Not output M05 before an oriented spindle stops
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 236 -
#7 #6 #5 #4 #3 #2 #1 #0
RDI RAB K0E RFC F16 QSR MRC 5102
[Data type] Bit MRC When a target figure other than a monotonically increasing or
monotonically decreasing figure is specified in a multiple repetitive turning canned cycle (G71, G72): 0 : No alarm occurs. 1 : P/S alarm No.064 is occurs.
NOTE This parameter is valid for multiple repetitive
turning canned cycle type I.
QSR Before a multiple repetitive canned cycle (G70 to G73) is started, a check to see if the program contains a block that has the sequence number specified in address Q is: 0 : Not made. 1 : Made. (If the sequence number specified in address Q cannot be
found, an alarm occurs and the canned cycle is not executed.) F16 When the FS10/11 format is used (with bit 1 (FCV) of parameter
No.0001 set to 1), a canned drilling cycle is specified using : 0 : FS10/11 format 1 : FS0 format. (However, the number of repetitions is specified
using address L.) RFC For the semifinish figure of G71 or G72 and for a cutting pattern of
G73, tool-nose radius compensation is: 0 : Not performed. 1 : Performed.
K0E When K0 is specified in a hole machining canned cycle (G80 to G89): 0 : Hole machining is performed once. 1 : Hole machining is not performed. Instead, the hole machining
data is merely memorized. RAB The R command for the drilling canned cycle in the Series 15 format
is: 0 : Regarded as an incremental command 1 : Regarded as: An absolute command in the case of G code system A An absolute command in the case of G code system B or C when
the G90 mode is specified. An incremental command in the case of G code system B or C
when the G91 mode is specified. RDI The R command for the drilling canned cycle in the FS10/11 format:
0 : Is regarded as the specification of a radius 1 : Follows the specification of a diameter/radius for the drilling axis
#7 #6 #5 #4 #3 #2 #1 #0
TCZ CID COD PNA P15 TFD 5103
TCZ DCP QZA SIJ
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 237 -
[Data type] Bit SIJ When the FS10/11 command format is used, a tool shift value for the
drilling canned cycle G76 or G87 is specified by: 0 : Address Q 1 : Address I, J, or K
TFD During a threading cycle, feed forward is: 0 : Enabled. 1 : Disabled.
QZA When the specification of the depth of cut (Q) for each time is omitted, or if Q0 is specified in a high-speed peck drilling canned cycle (G73) or peck drilling canned cycle (G83): 0 : No alarm is issued. 1 : An alarm (No.045) is issued.
P15 When the FS10/11 command format is used, the machining sequence for pocketing using multiple repetitive canned cycle G71 or G72 follows: 0 : FS0(FS16) specification 1 : FS10/11 specification
DCP When an axis perpendicular to or an axis parallel to a specified plane is specified in a canned cycle for drilling: 0 : The specified axis is regarded as the drilling axis. 1 : The specified axis is regarded as the positioning axis.
PNA If the FS10/11 tape format is used and if a plane without an axis is specified in the canned cycle mode of drilling, an alarm is: 0 : Raised. (P/S 028) 1 : Not raised.
COD In pocketing, the sequence of axis movements made to return the tool to the start point at the end of machining is as follows: 0 : X-axis to Z-axis 1 : Z-axis to X-axis
NOTE If this parameter is set to 1, specifying G71 causes
the tool to return to the start point in the sequence from Z-axis to X-axis. Therefore, when the tool returns to the start point after end facing, interference between the tool and workpiece surface can be prevented.
CID When the FS10/11 command format is used, application of the setting
of bit 7 (IPR) of parameter No. 1004 to the depth of cut in a multiple repetitive turning canned cycle is: 0 : Disabled. 1 : Enabled.
TCZ In a tapping cycle (excluding rigid tapping), an accumulated zero check in the tapping step (forward, backward) is: 0 : Not performed. 1 : Performed. Execute a tapping cycle (excluding rigid tapping) with the servo feed forward (bit 1 of parameter No. 2005). If an impact is detected, set this parameter to 1.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 238 -
#7 #6 #5 #4 #3 #2 #1 #0
PCT MCC SPE FCK BCR 5104
RDC
[Data type] Bit RDC A canned cycle for high-speed positioning and drilling is:
0 : Disabled. 1 : Enabled.
BCR In a boring cycle, retraction is made: 0 : At a cutting feedrate. 1 : At a rapid traverse rate.
FCK In a multiple repetitive canned cycle (G71/G72), the machining profile is: 0 : Not checked. 1 : Checked. If this parameter is specified, the machining profile specified in the multiple repetitive canned cycle for lathe (G71/G72) and the machining start point are checked. If the relationship is incorrect, the P/S 062 alarm is raised. An incorrect relationship between the machining profile and machining start point indicates either of the following cases. • Although the finishing allowance is specified with a positive sign,
the start point of the canned cycle is smaller than the maximum value of the machining profile.
• Although the finishing allowance is specified with a negative sign, the start point of the canned cycle is larger than the minimum value of the machining profile.
NOTE 1 The machining profile is checked before the
operation of the canned cycle (not during machining).
2 The machining profile to be checked is a programmed profile. The path of retraction or return is not checked.
3 This parameter is not valid for G71 or G72 of the canned cycle for grinder.
SPE In a multiple repetitive threading cycle in the FS10/11 tape format,
single-edge thread cutting and both-edge zigzag thread cutting with the depth of cut kept constant: 0 : Cannot be specified. 1 : Can be specified.
MCC In a multiple repetitive turning canned cycle (G71 or G72), whether an illegal arc is specified or not is: 0 : Not checked immediately before the start of a movement. 1 : Checked immediately before the start of a movement.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 239 -
NOTE 1 This parameter is valid when bit 1 (MRC) of
parameter No. 5102 is set to 1. 2 Regardless of the setting of this parameter, the
shape is checked during a movement made by an arc command.
PCT A Q command in a tapping cycle (G84 or G88) is:
0 : Invalid. 1 : Valid. (A peck tapping cycle is performed.) When this parameter is set, and the depth of cut for each time is specified with address Q in G84 or G88, a peck tapping cycle is performed. As a peck tapping cycle operation, high-speed peck tapping or peck tapping can be selected by bit 5 (PCP) of parameter No. 5200. This function can be used for both tapping and rigid tapping. Even when this parameter is set, ordinary tapping or rigid tapping is performed if Q is not specified or if Q0 is specified.
C-axis clamp M code in drilling canned cycle 5110
[Data type] 2-word [Valid data range] 0 to 99
This parameter sets the C-axis clamp M code in a drilling canned cycle.
Dwell time when C-axis unclamping is specified in drilling canned cycle 5111
[Data type] Word [Unit of data] ms [Valid data range] 0 to 32767
This parameter sets the dwell time when C-axis unclamping is specified in a drilling canned cycle.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 240 -
Spindle forward-rotation M code in drilling canned cycle 5112
[Data type] 2-word [Valid data range] 0 to 255
This parameter sets the spindle forward-rotation M code in a drilling canned cycle.
NOTE M03 is output when "0" is set.
Spindle reverse-rotation M code in drilling canned cycle
5113
[Data type] 2-word [Valid data range] 0 to 255
This parameter sets the spindle reverse-rotation M code in a drilling canned cycle.
NOTE M04 is output when "0" is set.
Return or clearance value of drilling canned cycle G83
5114 Return value of high-speed peck drilling cycle G73
[Data type] Word [Unit of data]
Input increment IS-A IS-B IS-C Unit Millimeter input 0.01 0.001 0.001 mm
Inch input 0.001 0.0001 0.0001 inch
[Valid data range] 0 to 32767 For M series this parameter sets the return value in high-speed peck drilling cycle G73 (G83 for T series).
q : Depth of cut d : Return value
R point
Z point
q
q
q
d
d
G73 for M series
Fig.4.22.1 (a) High-speed Peck Drilling Cycle G73
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 241 -
For T series this parameter sets the return or clearance value in drilling canned cycle G83.
Parameter No.5101 #2 RTR=0 (High speed peck drilling cycle)
Parameter No.5101 #2 RTR=1 (Peck drilling cycle)
q : Depth of cut d : Return value
R point
Z point
q
q
q
d
d
q : Depth of cut d : Clearance value
R point
Z point
q
q
q
d
d
G83 for T series
Fig.4.22.1 (b) Drilling Canned Cycle G83
5115 Clearance of canned cycle G83
[Data type] Word [Unit of data]
Input increment IS-A IS-B IS-C Unit Millimeter input 0.01 0.001 0.001 mm
Inch input 0.001 0.0001 0.0001 inch
[Valid data range] 0 to 32767 This parameter sets the clearance of peck drilling cycle G83.
G83 for 16-MC
q : Depth of cut d : Clearance value
R point
Z point
q
q
q
d
d
Fig.4.22.1 (c) Peck drilling cycle G83
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 242 -
Override value for retraction in boring cycle (G85, G89) 5121
[Data type] Byte [Unit of data] 100% [Valid data range] 0.1 to 20
Set the override value of retraction in a boring cycle. If 20 or a greater value is specified in this parameter, the override is set to 2000%. If 0 is specified, this parameter becomes invalid, and the retraction speed becomes two times the cutting speed.
4.22.2 Parameter of Thread Cutting Cycle
Chamfering distance in the thread cutting cycles G76 and G92 5130
[Data type] Byte [Unit of data] 0.1 pitch [Valid data range] 0 to 127
This parameter sets the chamfering in the thread cutting cycles G76 and G92.
Chamfering angle in threading cycle 5131
[Data type] Byte [Unit of data] 1 deg [Valid data range] 1 to 89
Set a chamfering angle in a threading cycle.
4.22.3 Parameter of Multiple Repetitive Canned Cycle
Depth of cut in multiple repetitive canned cycles G71 and G72 5132
[Data type] 2-word [Unit of data]
Input increment IS-B IS-C Unit Millimeter input 0.001 0.001 mm
Inch input 0.0001 0.0001 inch
[Valid data range] 0 to 99999999 This parameter sets the depth of cut in multiple repetitive canned cycles G71 and G72.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 243 -
Escape in multiple repetitive canned cycles G71 and G72. 5133
[Data type] 2-word [Unit of data]
Input increment IS-B IS-C Unit Millimeter input 0.001 0.001 mm
Inch input 0.0001 0.0001 inch
[Valid data range] 0 to 99999999 This parameter sets the escape in multiple repetitive canned cycle G71 and G72.
Escape in multiple repetitive canned cycle G73 in X-axis direction 5135
Escape in multiple repetitive canned cycle G73 in Z-axis direction 5136
[Data type] 2-word [Unit of data]
Input increment IS-B IS-C Unit Millimeter input 0.001 0.001 mm
Inch input 0.0001 0.0001 inch
[Valid data range] -99999999 to 99999999 This parameter sets the escape in multiple repetitive canned cycle G73 of an X, then Z axis.
Division count in multiple repetitive canned cycle G73 5137
[Data type] 2-word [Unit of data] Cycle [Valid data range] 1 to 99999999
This parameter sets the division count in multiple repetitive canned cycle G73.
Return in multiple canned cycles G74 and G75 5139
[Data type] 2-word [Unit of data]
Input increment IS-B IS-C Unit Millimeter input 0.001 0.001 mm
Inch input 0.0001 0.0001 inch
[Valid data range] 0 to 99999999 This parameter sets the return in multiple repetitive canned cycles G74 and G75.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 244 -
Minimum depth of cut in the multiple repetitive canned cycle G76 5140
[Data type] 2-word [Unit of data]
Input increment IS-B IS-C Unit Millimeter input 0.001 0.0001 mm
Inch input 0.0001 0.00001 inch
[Valid data range] 0 to 99999999 This parameter sets the minimum depth of cut in the multiple repetitive canned cycle G76.
Finishing allowance in the multiple repetitive canned cycle G76 5141
[Data type] 2-word [Unit of data]
Input increment IS-B IS-C Unit Millimeter input 0.001 0.0001 mm
Inch input 0.0001 0.00001 inch
[Valid data range] 1 to 99999999 This parameter sets the finishing allowance in multiple repetitive canned cycle G76.
Repetition count of final finishing in multiple repetitive canned cycle G76 5142
[Data type] 2-word [Unit of data] Cycle [Valid data range] 1 to 99999999
This parameter sets the repetition count in multiple repetitive canned cycle G76.
Tool nose angle in multiple repetitive canned cycle G76 5143
[Data type] 2-word [Unit of data] Degree [Valid data range] When FS10/11 format is used: 0 to 120
When FS10/11 format is not used: 0, 29, 30, 55, 60, 80 This parameter sets the tool nose angle in multiple repetitive canned cycle G76.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 245 -
The amount of retraction from the crest of a pocket of type II in roughing cycle (G71, G72) 5144
[Data type] 2-word [Unit of data]
Input increment IS-B IS-C Unit Linear axis (input in mm) 0.001 0.0001 mm
Linear axis (input in inches) 0.0001 0.00001 inch
[Valid data range] 0 to 99999999 This parameter sets the amount of retraction from a crest to be crossed to move to the next pocket to be roughed after roughing of a pocket of type II in roughing cycle (G71 or G72) ends. If this parameter is set to 0, 2000 (IS-B) or 20000 (IS-C) is assumed by default. When 0 is set for IS-B metric input, for example, the amount of retraction is assumed to be 1.0 mm if a radius is specified (bit 3 (DIA) of parameter No. 1006 = 0) or 2.0 mm if a diameter is specified (bit 3 (DIA) of parameter No. 1006 = 1).
5150 Inertial running distance in a canned cycle for high-speed positioning and
drilling
[Data type] 2-word [Unit of data]
Input increment IS-A IS-B IS-C Unit Millimeter input 0.01 0.001 0.0001 mm
Inch input 0.001 0.0001 0.00001 inch
[Valid data range] 0 to 99999999 This parameter sets the distance of inertial running in a canned cycle for high-speed positioning and drilling.
5151 Rapid traverse deceleration ratio for overlap between rapid traverse blocks
in a canned cycle for high-speed positioning and drilling
[Data type] Byte [Unit of data] % [Valid data range] 0 to 100
This parameter sets the rapid traverse deceleration ratio for an overlap between rapid traverse blocks in a canned cycle for high-speed positioning and drilling. In the cycle, the setting of this parameter is valid for all axes.
NOTE In a canned cycle for high-speed positioning and
drilling, a rapid traverse overlap is applied even when bit 4 (RTO) of parameter No. 1601 is set to 0. To disable the rapid traverse overlap, set this parameter to 0.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 246 -
4.22.4 Parameters of Peck Drilling Cycle of a Small Diameter
#7 #6 #5 #4 #3 #2 #1 #0
CYM 5160
CYM NOL OLS
[Data type] Bit OLS When an overload torque signal is received in a peck drilling cycle of
a small diameter, the feed and spindle speed are 0 : Not changed. 1 : Changed.
NOL When the depth of cut per action is satisfied although no overload torque signal is received in a peck drilling cycle of a small diameter, the feed and spindle speed are: 0 : Not changed. 1 : Changed.
CYM When a subprogram call (M98) and another NC command are specified in the same block in a canned cycle mode: 0 : No alarm is issued. 1 : AN alarm is issued. (P/S alarm 5329)
#7 #6 #5 #4 #3 #2 #1 #0
RLV PKG 5161
[Data type] Bit PKG Method for specifying a high-speed peck drilling cycle and a peck
drilling cycle 0 : G83 or G87 is used, and a high-speed peck drilling or peck
drilling cycle is selected by bit 2 (RTR) of parameter No. 5101. 1 : A specification is added to the G83 or G87 command so that a
high-speed peck drilling cycle can be specified using G83.5 or G87.5 and that a peck drilling cycle can be specified using G83.6 or G87.6.
NOTE When the FS10/11 format is used (when bit 1
(FCV) of parameter No. 0001 is set to 1), this parameter is invalid.
RLV For G code system A, the return operation in a drilling canned cycle
performs: 0 : A return to the initial level. 1 : A return to the level of the R point.
NOTE For G code systems B and C, a selection is made
using G codes. G98: Return to the initial level G99: Return to the level of the R point
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 247 -
5163 M code that specifies the peck drilling cycle mode of a small diameter
[Data type] 2-word [Valid data range] 1 to 99999999
This parameter sets an M code that specifies the peck drilling cycle mode of a small diameter.
5164
Percentage of the spindle speed to be changed when the tool is retracted
after an overload torque signal is received
[Data type] Byte [Unit of data] % [Valid data range] 1 to 255
This parameter sets the percentage of the spindle speed to be changed when the tool is retracted because the overload torque signal is received in a peck drilling cycle of a small diameter. S2 = S1 × d1 ÷ 100
S1: Spindle speed to be changed S2: Spindle speed changed d1 is set as a percentage.
5165
Percentage of the spindle speed to be changed when the tool is retracted
without an overload torque signal received
[Data type] Byte [Unit of data] % [Valid data range] 1 to 255
This parameter sets the percentage of the spindle speed to be changed when the tool is retracted without the overload torque signal received in a peck drilling cycle of a small diameter. S2 = S1 × d2 ÷ 100
S1: Spindle speed to be changed S2: Spindle speed changed d2 is set as a percentage.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 248 -
5166
Percentage of cutting feedrate to be changed when the tool is retracted after
an overload torque signal is received
[Data type] Byte [Unit of data] % [Valid data range] 1 to 255
This parameter sets the percentage of the cutting feedrate to be changed when the tool is retracted because the overload torque signal is received in a peck drilling cycle of a small diameter. F2 = F1 × b1 ÷ 100
F1: Cutting feedrate to be changed F2: Changed cutting feedrate b1 is set as a percentage.
5167
Percentage of the cutting feedrate to be changed when the tool is retracted
without an overload torque signal received
[Data type] Byte [Unit of data] % [Valid data range] 1 to 255
This parameter sets the percentage of the cutting feedrate to be changed when the tool is retracted without the overload torque signal received in a peck drilling cycle of a small diameter. F2 = F1 × b2 ÷ 100
F1: Cutting feedrate to be changed F2: Changed cutting feedrate b2 is set as a percentage.
5168
Lower limit of the percentage of the cutting feedrate in a peck drilling cycle
of a small diameter
[Data type] Byte [Unit of data] % [Valid data range] 0 to 255
This parameter sets the lower limit of the percentage of the cutting feedrate changed repeatedly in a peck drilling cycle of a small diameter to the specified cutting feedrate. FL = F × b3 ÷ 100
F: Specified cutting feedrate FL: Changed cutting feedrate Set b3 as a percentage.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 249 -
5170
Number of the macro variable to which the total number of retractions during
cutting is output
[Data type] Word [Valid data range] 100 to 149
This parameter sets the number of the macro variable to which the total number of times the tool is retracted during cutting in a peck drilling cycle mode of a small diameter is output.
NOTE The total number cannot be output to common
variables 500 to 531.
5171
Number of the macro variable to which the total umber of retractions
because of an overload signal is output
[Data type] Word [Valid data range] 100 to 149
This parameter sets the common variable number of the custom macro to which the number of times the tool is retracted after the overload signal is received during cutting in a peck drilling cycle mode of a small diameter is output.
NOTE The total number cannot be output to common
variables 500 to 531.
5172
Speed of retraction to point R when no address I is issued
[Data type] Word [Unit of data] mm/min [Valid data range] 0 to 400
This parameter sets the speed of retraction to point R when no address I is issued in a peck drilling cycle of a small diameter.
5173
Speed of advancing to the position just before the bottom of a hole when no
address I is issued
[Data type] Word [Unit of data] mm/min [Valid data range] 0 to 400
This parameter sets the speed of advancing to the position just before the bottom of a previously machined hole when no address I is issued in a peck drilling cycle of a small diameter.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 250 -
5174
Clearance in a peck drilling cycle of a small diameter
[Data type] Word [Unit of data]
Input increment IS-A IS-B IS-C Unit Linear axis (input in mm) 0.01 0.001 0.0001 mm
Linear axis (input in inches) 0.001 0.0001 0.00001 inch
[Valid data range] 0 to 32767 This parameter sets the clearance in a peck drilling cycle of a small diameter.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 251 -
4.23 PARAMETERS OF RIGID TAPPING
#7 #6 #5 #4 #3 #2 #1 #0
SRS FHD DOV SIG CRG VGR G84 5200
FHD PCP DOV SIG CRG VGR G84
[Data type] Bit G84 Method for specifying rigid tapping
0 : An M code specifying the rigid tapping mode is specified prior to the issue of the G84 (or G74) command. (See parameter No.5210).
1 : An M code specifying the rigid tapping mode is not used. (G84 cannot be used as a G code for the tapping cycle; G74 cannot be used for the reverse tapping cycle.)
VGR Any gear ratio between spindle and position coder in rigid tapping 0 : Not used (The gear ratio is set in parameter No.3706.) 1 : Used (The gear ratio is set by parameters Nos. 5221 through
5224 and 5231 through 5234.)
NOTE For serial spindles, set this parameter to 0 when
using the DMR function for position coder signals on the spindle side.
CRG Rigid mode when a rigid mode cancel command is specified (G80,
G01 group G code, reset, etc.) 0 : Canceled after rigid tapping signal RGTAP <G061#0> is set to
"0". 1 : Canceled before rigid tapping signal RGTAP <G061#0> is set to
"0". SIG When gears are changed for rigid tapping, the use of SIND <G032 and
G033> is 0 : Not permitted. 1 : Permitted.
DOV Override during extraction in rigid tapping 0 : Invalidated 1 : Validated (The override value is set in parameter No.5211 (M/T)
or No.5381(M).) PCP Tapping or rigid tapping
0 : Used as a high-speed peck tapping cycle 1 : Not used as a high-speed peck tapping cycle For the T series, this parameter is valid when bit 6 (PCT) of parameter No. 5104 is set to 1. According to the setting of this parameter, also set parameter No. 5213.
FHD Feed hold and single block in rigid tapping 0 : Invalidated 1 : Validated
SRS To select a spindle used for rigid tapping in multi-spindle control:
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 252 -
0 : The spindle selection signals SWS1 and SWS2 (bits 0 and 1 of G027) are used. (These signals are used also for multi-spindle control.)
1 : The rigid tapping spindle selection signals RGTSP1 and RGTSP2 (bits 4 and 5 of G061) are used. (These signals are provided expressly for rigid tapping.)
#7 #6 #5 #4 #3 #2 #1 #0
OV3 OVU TDR 5201
OV3 OVU TDR NIZ
[Data type] Bit NIZ Smoothing in rigid tapping is:
0 : Not performed. 1 : Performed.
TDR Cutting time constant in rigid tapping 0 : Uses a same parameter during cutting and extraction (Parameter
Nos. 5261 through 5264) 1 : Not use a same parameter during cutting and extraction Parameter Nos. 5261 to 5264: Time constant during cutting Parameter Nos. 5271 to 5274: Time constant during extraction
OVU The increment unit of the override parameter (No.5211 (M/T) or No.5381 (M)) for tool rigid tapping extraction is: 0 : 1% 1 : 10%
OV3 The spindle speed for tool extraction is specified by program. The tool extraction function based on this spindle speed is: 0 : Disabled. 1 : Enabled.
#7 #6 #5 #4 #3 #2 #1 #0
ORI 5202
RG3 ORI
NOTE When this parameter is set, the power must be
turned off before operation is continued.
[Data type] Bit ORI When rigid tapping is started:
0 : Spindle orientation is not performed. 1 : Spindle orientation is performed.
NOTE This parameter can be used only for a serial
spindle.
RG3 A rigid tapping return operation is specified: 0 : With input signal RTNT <G062#6>. 1 : With one-shot G code G30.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 253 -
#7 #6 #5 #4 #3 #2 #1 #0
OVS RGS 5203
RBL OVS RFF
[Data type] Bit REF Feed forward during movement from the initial point to point R in
rigid tapping is: 0 : Disabled. 1 : Enabled. When this parameter is set, the following function is also enabled: • When rigid tapping is specified in advanced preview control
mode, the system automatically exits from advanced preview control mode and executes rigid tapping. After termination of rigid tapping, the system automatically returns to look-ahead control mode.
RGS When bit 0 (MIF) of parameter No. 1403 is set to 1 and rigid tapping is specified in feed-per-minute mode, the spindle speed becomes: 0 : 1/1000 of the specified speed. 1 : 1/1 of the specified speed.
OVS In rigid tapping, override by the feedrate override signal and invalidation of override by the override cancel signal is: 0 : Disabled. 1 : Enabled. Setting this parameter enables override by the feedrate override signal <G012> to be applied for rigid tapping operation (cutting and extraction) in rigid tapping. The spindle speed override is fixed to 100%, but override is also applied to the spindle speed in synchronization with the feedrate along the tapping axis by feedrate override. The override cancel signal OVC <bit 4 of G006> also becomes available.
NOTE 1 When this parameter is set to override the feedrate,
override by parameters (see parameters Nos. 5211 (T/M) and 5381 (M)) is disabled.
2 Regardless of whether this parameter is set, when feedrate override is disabled by the override cancel signal OVC <bit 4 of G006>, override by parameters (see parameters Nos. 5211 (T/M) and 5381 (M)) is enabled.
RBL As acceleration/deceleration for rigid tapping cutting feed:
0 : Linear acceleration/deceleration is used. 1 : Bell-shaped acceleration/deceleration is used.
NOTE The bell-shaped acceleration/deceleration option
for rigid tapping is required.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 254 -
#7 #6 #5 #4 #3 #2 #1 #0
SPR DGN 5204
DGN
NOTE When this parameter is set, the power must be
turned off before operation is continued.
[Data type] Bit DGN On the diagnosis screen:
0 : A rigid tapping synchronization error is displayed. (Nos. 455 to 457)
1 : An error difference between the spindle and tapping axis is displayed. (Nos. 452 and 453)
SPR In rigid tapping, the parameters are: 0 : Not changed on a spindle-by-spindle basis. 1 : Changed on a spindle-by-spindle basis.
NOTE 1 When switching between the rigid tapping
parameters on a spindle-by-spindle basis in rigid tapping using the second serial spindle, set this parameter to 1. The following parameters are supported for each spindle:
First spindle Second spindle (2-stage gear) No.5214 No.5215 No.5221 to No.5224 No.5225, No.5226 No.5231 to No.5234 No.5235, No.5236 No.5241 to No.5244 No.5245, No.5246 No.5261 to No.5264 No.5265, No.5266 No.5271 to No.5274 No.5335, No.5336 No.5280 No.5341 No.5281 to No.5284 No.5342, No.5343 No.5300, No.5301 No.5302, No.5303 No.5310 to No.5314 No.5350 to No.5353
No.5321 to No.5324 No.5325, No.5326 2 For rigid tapping using the second serial spindle,
the multispindle control option is required.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 255 -
#7 #6 #5 #4 #3 #2 #1 #0
REF PKD RCK 5205
REF NRV RCK
[Data type] Bit RCK In rigid tapping, an excessive error during movement/at stop is:
0 : Checked regardless of whether mode is cutting (tapping) or rapid traverse.
1 : Checked only in cutting (tapping) mode. NRV For the rigid tapping function, the spindle returns back from the
bottom of a hole with: 0 : Rotating opposite to the drilling direction 1 : Rotating in the drilling direction (special purpose)
CAUTION This parameter is intended for special uses only.
When rigid tapping is performed, therefore, this parameter must not be set.
If rigid tapping is performed with this parameter set, a tapping tool, workpiece, or machine may be damaged.
PKD For rigid peck tapping, diagnostic number 457 (maximum rigid
tapping synchronization error) indicates: 0 : A value per tap operation. 1 : A total value until the hole bottom is reached.
REF Fine acceleration/deceleration during rigid tapping is: 0 : Disabled. 1 : Enabled. To use the spindle fine acceleration/deceleration (FAD) function, set 1.
NOTE When fine acceleration/deceleration is used, fine
acceleration/deceleration settings for the spindle and servo system must be made in addition to the setting of this parameter.
5210 Rigid tapping mode specification M code
[Data type] Byte [Valid data range] 0 to 255
This parameter sets an M code that specifies the rigid tapping mode.
NOTE 1 A setting value of 0 is assumed to be 29 (M29). 2 To use an M code whose number is greater than
256, Specify the code number with parameter No.5212.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 256 -
5211 Override value during rigid tapping extraction
[Data type] Byte [Unit of data] 1 % or 10 % [Valid data range] 0 to 200
The parameter sets the override value during rigid tapping extraction.
NOTE The override value is valid when DOV in parameter
No.5200 #4 is "1". When OVU (bit 3 of parameter No.5201) is 1, the
unit of set data is 10%. An override of up to 200% can be applied to extraction.
5212 M code that specifies a rigid tapping mode
[Data type] 2-word [Unit of data] Integer [Valid data range] 0 to 65535
This parameter sets the M code that specifies the rigid tapping mode. The M code that specifies the rigid tapping mode is usually set by parameter 5210. To use an M code whose number is greater than 256, specify the code number with parameter 5212.
NOTE If the setting of this parameter is 0, the M code
specifying the rigid tapping mode is determined by the setting of parameter 5210. Otherwise, it is determined by the setting of parameter 5212. The setting of parameter 5212 must always be within the above valid range.
5213 Return or clearance in peck tapping cycle
[Data type] Word [Unit of data]
Input increment IS-A IS-B IS-C Unit Millimeter input 0.01 0.001 0.001 mm
Inch input 0.001 0.0001 0.0001 inch
[Valid data range] 0 to 32767 This parameter sets the return or clearance in the peck tapping cycle.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 257 -
Parameter No.5200#5 PCP=1 (Clearance in peck tapping cycle)
Parameter No.5200#5 PCP=0 (Return in peck tapping cycle)
q : Depth of cut d : Return value
R point
Z point
q
q
q
d
d
q : Depth of cut d : Clearance value
R point
Z point
q
q
q
d
d
Fig.4.23 (a) High-speed Peck Drilling and Peck Drilling Cycles
5214 Setting of an allowable rigid tapping synchronization error range
Setting of an allowable rigid tapping synchronization error range for the
second spindle 5215
[Data type] Word [Unit of data] Detection unit (1/4096rev) [Valid data range] 0 to 32767
Each of these parameters is used to set an allowable synchronization error range between a spindle used for rigid tapping and the tapping axis. If the value set with each parameter is exceeded, rigid tapping alarm No.741 (excessive error during movement) is issued. When 0 is set, a synchronization error check is not made.
NOTE When rigid tapping is performed using the second
spindle • When the SPR parameter (bit 1 of parameter
No.5204) is set to 0, the setting of parameter No.5214 is applied to the second spindle, as well as to the first spindle.
• When the SPR parameter (bit 1 of parameter No.5204) is set to 1, the settings of parameter No.5215 is applied to the second spindle.
4.DESCRIPTION OF PARAMETERS B-64120EN/01
- 258 -
5221 Number of spindle gear teeth (first-stage gear) 5222 Number of spindle gear teeth (second-stage gear) 5223 Number of spindle gear teeth (third-stage gear)
Number of spindle gear teeth (fourth-stage gear) 5224
Number of second spindle gear teeth (first-stage gear)
5225 Number of second spindle gear teeth (second-stage gear)
5226
[Data type] Word [Valid data range] 1 to 32767
When an arbitrary gear ratio is used in rigid tapping, each of these parameters sets the number of teeth of each spindle gear.
NOTE 1 These parameters are enabled when the VGR
parameter (bit 1 of parameter No.5200) is set to 1. 2 When a position coder is attached to the spindle,
set the same value for all of parameters No.5221 through No.5224.
3 When the DMR function of the position coder signal is used with a serial spindle, set the VGR parameter (bit 1 of parameter No.5200) to 0, and set these parameters to 0.
4 When rigid tapping is performed using the second spindle • When the SPR parameter (bit 1 of parameter
No.5204) is set to 0, the settings of parameters No.5221 and No.5222 are applied to the second spindle, as well as to the first spindle.
• When the SPR parameter (bit 1 of parameter No.5204) is set to 1, the settings of parameters No.5225 and No.5226 are applied to the second spindle.
B-64120EN/01 4.DESCRIPTION OF PARAMETERS
- 259 -
5231 Number of position coder gear teeth (first-stage gear) 5232 Number of position coder gear teeth (second-stage gear) 5233 Number of position coder gear teeth (third-stage gear)
Number of position coder gear teeth (fourth-stage gear) 5234
Number of position coder gear teeth for the second spindle (first-stage gear)
5235 Number of position coder gear teeth for the second spindle (second-stage
gear) 5236
[Data type] Word [Valid data range] 1 to 32767
When an arbitrary gear ratio is used in rigid tapping, each of these parameters sets the number of teeth of each position coder gear.
NOTE 1 These parameters are enabled when the VGR
parameter (bit 1 of parameter No.5200) is set to 1. When a position coder is attached to the spindle,
set the same value for all of parameters No.5231 through No.5234.