SITRAIN Training for Tool Offset and Measuring

SITRAIN Training for
Automation and Industrial Solutions Page 1
NC-84D-HP
Tool Offset and Measuring
SITRAIN
NC-84D-HP /Tool Offset and Measuring Page 1
Automation and Drives
1/2008
© Siemens AG 2008 - All rights reserved
Tooloffset and Measuring
0 ca.X100 X200
Content Page
Tool data .......................................................................................................................................... 3
Tool Offset Variables ........................................................................................................................ 4
Read/Change Tool Offsets in the NC Program ................................................................................. 5
Comparing the Different Tool Data Management Types .................................................................... 6
Fine Offsets Relative to Location ...................................................................................................... 7
Mirroring the Tool Geometry ............................................................................................................ 8
Program Commands for Tool Management ...................................................................................... 9
Program Runtime (from Software V.6) .............................................................................................. 10
Workpiece Counter (From Software V.6) .......................................................................................... 11
Measurement, MEAS, MEAW .......................................................................................................... 12
Exercise - Measuring ....................................................................................................................... 13
Axial Measurement Functions MEASA, MEAWA .............................................................................. 14
Continuous measurement MEAC in the FIFO ................................................................................... 15

NC-84D-HP

NC-84D-HP
Structure of the offset memory
Every data set can be invoked with a T and D number; in addition to the
geometrical data for the tool, it contains other information such as the tool type.
Altogether max. 600 data sets per NCU. (From software V.5 max.1500)
depending on setting in $MN_MM_NUM_CUTTING_EDGES_IN_TOA and max.
9 data sets per tool. (From software V.5 max.12) depending on setting in MD
18106
Several entries exist for the geometric variables (e.g., length 1 or radius). These
are added together to produce a value (e.g. total length 1, total radius) which is
then used for the calculations.
Exception: In $MC_TOOL_PARAMETER_DEF_MASK geometry value (from
software V.5.3) and wear value of the facing axis can be switched to diameter
for turning operations.
The "reserved" parameters are only taken into account for 3D tool compensation
(CUT3DC, CUT3DF) and grinding tools.
SITRAIN
1/2008
Tool data

NC-84D-HP
Data set structure
Reserved25
For turningclearance angle24
Applicant (z in G17)Length 112
Ordinate (y in G17)Length 213
Abscissa (x in G17)Length 314
Technology
For drills not neededRadius15
End radius for CUT3DReserved16
Reserved17
Reserved18
Reserved19
cone angle for CUT3DReserved20
Base/ Holder
cone angle for CUT3DReserved11
Reserved10
Reserved9
Wear
Reserved8
End radius for CUT3DReserved7
For drills not neededRadius6
Geometry: length & radius corrections
For turningCutting edge position2
Tool type1
NotesMeaningTool
parameter
Tool parameter are store in system variables
of form $TC_DPn[i,j]
$TC_DP1[2,3]
T2
D3

NC-84D-HP
The modified values only take effect the next time T or D is programmed -
even when changed by the operator!
From Software V.5 Any changes the operator makes to the tool offset and zero offset in NC STOP
are effective and implemented immediately after a new NC START if MD9440=1
Delete Contours: $TC_DP1 [1, 6] =0 Deletes T1 D6
$TC_DP1 [3, 0] =0 Deletes T3 completely
$TC_DP1 [0, 0] =0 Deletes complete tool memory
The current (selected) offset values can also be read in the system variables:
Caution When these system variables are accessed there is no implicit preprocessing
stop.
With time-critical program sections you therefore need to program STOPRE
first.
"Flat" Tool Offsets(from software V. 4)
In contrast with the standard setting described until now
($MN_MM_TYPE_OF_CUTTING_EDGE=0) it is also possible to assign D
numbers that are not connected to the T numbers, e.g. when the tool
management is conducted externally.
D1 ... D32000 (max. 1500 numbers dep. on memory configuration)
Addressing the Parameters: $TC_DP1 [Dn] . .. $TC_DP25 [Dn]
Delete "Flat" Tool $TC_DP1 [6] =0 Deletes D6
Offsets $TC_DP1 [0] =0 Deletes complete tool memory
SITRAIN
1/2008
Read/Change Tool Offsets in the NC Program
Programming exercise:
N10 R1=$TC_DP3[4,1] reads L1 from T4 D1
N20 $TC_DP12[4,1]= $TC_DP12[4,1]-0.051 changes L1 wear
Active tool radius overall$O_TOOLR
Active tool length overall
m: length 1…3
$P_TOOLL[m]
Active correction
n: parameter number 1…25
$P_AD[n]
Active cutting edge (D- No.)$P_TOOL
Active tool number (T- No.)$P_TOOLNO
Content of system variablesName

NC-84D-HP
Comparing the Possible Tool Data Management Types
To software V.3 only "deep" structures: offset call with "T123"
From software V.4 in addition "flat direct" structure is possible: offset call with "D32000"
From software V.5 in addition "flat indirect" structure is possible: offset call of D123 with "D5"
9 D numbers in PLC DBB...
From software V.5 with "deep" structure max. 12 cutting edges per tool, where D number and
cutting edge number CE= are separated. You can check the D numbers are uniquely assigned
via the CHKDNO command.
T3 D1
T123 D1 D2
T4711 D1
T32000 D1
D2 D3 D4 D5 D6 D7 D8 D9
T3 T135 T1358 T1359 T12345678
D2 D33 D100 D120 D121 D122 D123 D124 D125 D32
000
T3 T135 T1358 T1359 T12345678
D2 D33 D100 D120 D121 D122 D123 D124 D125 D32
000
1
100
2
124
3
2
4
33
5
123
6
125
7
66
8
4711
9
122
D5
T3 CE=1
D345
T123 CE=1
D11
CE=2
D1
T4711 CE=1
D471
T32000 CE=1
CE=2
D1
CE=3
D1
CE=4
D2
CE=5 CE=6 CE=7 CE=8
D17
CE=9
D18
CE=1
0

NC-84D-HP
For fine offsetting of the tool influence on the machining (e.g. a heavy tool the
gantry bends particularly at a specific machining position) location-dependent fine
offsets are introduced in software V.5. They are additive to the normal offsets.
SITRAIN
1/2008
Fine Offsets Relative to Location
DL1 ... 6 (per D No. max. 6 dep. on MD18108)
with D selection, DL1 is automatically active
Per DL offset 2 values: Wear value $TC_SCPxy[t,d]
Setup value $TC_ECPxy[t,d]
DL No. 1 ... 6 Parameter No. 1 ... 24
state = DELDL[t,d] Deletes all additive offsets for the cutting edge of the tool
state = DELDL[t] Deletes all additive offsets for all cutting edges of the tool
state = DELDL Deletes all additive offsets for all cutting edges of all tools
successful if state =0

NC-84D-HP
Up until software V.4 it was necessary to create a new data set (new D No.) to
generate a mirrored tool length.
Example for reading and changing tool offsets
Task A new data set D2 is to be created and selected for a rotatable tool (machining
"from below") with negative tool length L1 in a subroutine for the active tool.
Sample Solution NEGL1_SPF
STOPRE
$TC_DP1[$P_TOOLNO,2]= $TC_DP1[$P_TOOLNO,1]
$TC_DP3[$P_TOOLNO,2]= $P_TOOLL[1]
$TC_DP6[$P_TOOLNO,2]= $TC_DP6[$P_TOOLNO,1]
D2 M17
From Software V. 5 Mirroring of the tool lengths and base values automatically becomes effective with
$SC_MIRROR_TOOL_LENGTH=1 when the appropriate geometry axis is
mirrored.
$SC_MIRROR_TOOL_WEAR=1 activates the mirroring for the wear data incl. the
DL values.
SITRAIN
1/2008
Mirroring the Tool Geometry
SD42900 $SC_MIRROR_TOOL_LENGTH =1 Mirrors tool lengths and tool base dimensions
SD42910 $SC_MIRROR_TOOL_WEAR =1 Mirrors tool length wear values incl. DL
Mirroring is effective when the associated axis is
mirrored
SD42920 $SC_WEAR_SIGN_CUTPOS Wear +/- signs dep. on cutting edge position
SD42930 $SC_WEAR_SIGN =1 Inverts the sign for all wear dimensions
SD42940 $SC_TOOL_LENGTH_CONST =0 Assignment of tool lengths dep. on G17 ...
17 ... 19 indep. of G17 ... G19 in these planes
-17 ...-19 the same but with swapped axes of the
respective machining plane
Cutting edge L1 mirr. L2 mirr.
position
1
2 invert
3 invert invert
4 invert
5
6
7 invert
8 invert
9

NC-84D-HP
...= NEWT (...) Create new tool The function returns the automatically generated internal T
number as return parameter. If no duplo number is specified, this is generated
automatically by the tool management.
Example: DEF INT T_NO, DUPLO_NO = 7
T_NO=NEWT("DRILL", DUPLO_NO)
DELT(...) Delete tool The DELT function can be used to delete a tool without referring to
the T number.
Example: DELT("MYTOOL",DUPLO_NR)
...=GETT(...) Read T No. The GETT function returns the T number required to set the tool
data for a tool. If there are several tools with the specified identifier, the T number
of the first possible tool of these tools is returned. - 1: No tool found.
Example: R10=GETT("DRILL", DUPLO_NO)
$TC_DP1[GETT("DRILL, DUPLO_NO),1]=100
SETPIECE(...) Preset workpiece counter number of units is decremented by the specified
number as set in $A_MONIFACT. (Spindle spec. optional)
(Timer or count) = 10 1 min. machining = 10 min. operating life
= 0 No wear
Example: SETPIECE(1) Workpiece counter of main spindle is decr. by 1
SETPIECE(4,2)Workpiece counter of 2nd spindle is decr. by 4
Control of wear time as set in MD20310 bit 17
= 0 Timer is running if G0 is not used for traversing
= 1 Timer ON/OFF via PLC (DB x 1.3)
GETSELT(...) Read the selected T No. For accessing the compensation data for the next tool
already before M6.
Example:GETSELT (R1) Get No. of the (pre)activated tool of main spindle
GETSELT (R2,2) No. of the (pre)activated tool of 2nd spindle
SITRAIN
1/2008
Program Commands for Tool Management
Find out preselected tool No. (t- No.)GETSELT(x)
Decrement number of pieces
(for how many, spindel- No.)
SETPIECE (x,y)
Find out T- Number… GETT (“WZ“,DUPLO_NR)
delete tool, duplo number optionalDELT (“WZ“,DUPLO_NR)
Create new tool, duplo number optional… =NEWT (“WZ“,DUPLO_NR)
Used symbols
spindel- No.x
Find out T- Number… GETT (“WZ“,DUPLO_NR)
Tool parter No.DUPLO_NR
Tool name“WZ“

NC-84D-HP
Information on the program runtime and the part count is provided to assist the
machine tool operator. The functions defined for this purpose are not identical to
the functions of tool management and are intended primarily for systems
without tool management.
The desired information must be specified in defined machine data and can be
manipulated via system variables in the NC and/or PLC program. The information
is available to the MMC via the operator panel/PLC interface.
A dedicated display screen for the SINUMERIK 802D control is provided for
program runtime and workpiece counter.
Exercise Program a circle with diameter= 75 mm and traverse it with F350. How many
minutes does the machining take?
(theoretically π × 75 / 350 = 0.673 min)
R1= $AN_POWERON_TIME
G3 G91 I= 75/2 F350
MSG ("Runtime= "<< R1- $AN_POWERON_TIME)
M30
SITRAIN
1/2008
Program Runtime (from Software V.6)
$AN_SETUP_TIME Time since last INITIAL.INI or series start-up [min]
$AN_POWERON_TIME Time since last Power ON or last POR [min]
$AC_OPERATING_TIME Sum of machining times since Power ON [s]
$AC_CYCLE_TIME Runtime of active program until now [s]
$AC_CUTTING_TIME Tool cutting time (machining feed) since PO [s]
MD 27860 $MC_PROCESSTIMER_MODE
Bit 0=1 $AC_OPERATING_TIME active
Bit 1=1 $AC_CYCLE_TIME active
Bit 2=1 $AC_CUTTING_TIME active
Bit 4=1 Measurement also with DRY
Bit 5=1 Measurement also with PRT

NC-84D-HP
Another machine data is required for configuration of the workpiece counter:
MD 27880 $MC_PART_COUNTER
Bit 0=1 $AC_REQUIRED_PARTS is monitored
Bit 1=0 Alarm/VDI output if equal to $AC_ACTUAL_PARTS
Bit 1=1 Alarm/VDI output if equal to $AC_SPECIAL_PARTS
Bit 4=1 Counter $AC_TOTAL_PARTS active
Bit 5=0 Counter $AC_TOTAL_PARTS is incremented with M2/M30
Bit 5=1 Counter $AC_TOTAL_PARTS incremented at M command specified in
MD 27882
$MC_PART_COUNTER_MODE[0]
Bit 8=1 Counter $AC_ACTUAL_PARTS active
Bit 9=0 Counter $AC_ACTUAL_PARTS is incremented with M2/M30
Bit 9=1 Counter $AC_ACTUAL_PARTS incremented at M command specified
in MD 27882
Bit 12=1 Counter $AC_SPECIAL_PARTS active
Bit 13=0 Counter $AC_SPECIAL_PARTS is incremented with M2/M30
Bit 13=1 Counter $AC_SPECIAL_PARTS incremented at M command specified
in MD 27882
All workpiece counters are declared as inactive in the default machine data set.
The counters are activated by default for the SINUMERIK 802D.
SITRAIN
1/2008
Workpiece Counter (From Software V.6)
$AC_REQUIRED_PARTS Setpoint count (alarm output and $AC_ACTUAL_PARTS=0)
$AC_TOTAL_PARTS Part count since Power ON
$AC_ACTUAL_PARTS Part count since last reset
$AC_SPECIAL_PARTS Part count since last reset (user-defined)
like $AC_ACTUAL_PARTS, but without automatic reset
MD 27882 $MC_PART_COUNTER_MCODE[0...2]
M function which triggers the counting process:
[0] for $AC_TOTAL_PARTS
[1] for $AC_ACTUAL_PARTS
[2] for $AC_SPECIAL_PARTS

NC-84D-HP
MEAS MEAW The measurement (with or without delete distance-to-go) is performed in a path
motion (e.g. with G1). The positions are captured for all geometry axes at the
switching edge of the measuring probe and written to:
$AA_MM[axis] in machine coordinate system
$AA_MW[axis] in workpiece coordinate system
When this variable is read, from software V.4.3 an implicit preprocessing stop is
generated. With earlier versions it was necessary to program a preprocessing
stop with STOPRE.
Measuring Success You can query the measuring success until the next measurement command by
means of the status variable $AC_MEA[n] (n= number of the measuring probe):
1= Measurement successful 0= Probe not deflected
Switching status The current output state of the probe is written in $A_PROBE[n]
Stopping Path The stopping path after delete distance-to-go corresponds to the following error
plus deceleration distance. Feedforward control FFWON is absolutely necessary!
Following error at KV=1(MD 32200) and F1000 = 1mm
Deceleration distance at a=10m/s2 (MD 32300) s=v2/2a = ca. 0.015mm
Determine stopping path experimentally: $AA_MM[axis]–$AA_IM[axis]
CAUTION: Measuring probes often have a delay that can be activated!
GEOAX The measurement does not work with simulated geometry axes as often found as
Z axis on our training units. Deactivate:
N1 GEOAX ( )
N2 GEOAX (0, Z1)
...
N99 GEOAX ( )
Here Z1 is the channel axis name. When using GEOAX it must not be identical
with the geometry axis name (change alarm 14414 MD20080).
SITRAIN
1/2008
Measurement, MEAS, MEAW
N10 FFWON
N20 MEAS=+1 G1 F1000
X100
N30 STOPRE
N40 R1= $AA_MM [X]
Measurement with delete
distance-to-go at deflection of
measuring probe at 1st
measuring input
Measurement with delete
distance-to-go at deflection of
measuring probe at 1st
measuring input
Polarity of measuring probe used:
MD13200 MEAS_PROBE_LOW_ACTIVE[n]

NC-84D-HP
Programming Exercise - Measuring
Determine the center point of a hole/slot (carry out two measurements in X
direction and form the mean value) and make this position available in R0
rounded to three decimal places.
Solution: N1 GEOAX ( )
N2 GEOAX ( 0, Z1 )
N3 G0 G90 X100
N4 MEAS=1 G1 X0 . ..
N5 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
N6 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
N7 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
N8 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
N9 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
N10 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
N11 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
N12 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
SITRAIN
1/2008
Exercise - Measuring
0 approx. X100 X200

NC-84D-HP
With MEASA, MEAWA per movement up to 4 measurements are possible;
with MEASA delete distance-to-go is performed after the last trigger pulse.
The measurement results are found in
$AA_MM1...4[axis] for event 1...4 in the MCS
$AA_MW1...4[axis] for event 1...4 in the WCS
Example MEAWA
Two light barriers are to monitor direction and speed of the workpiece flow on a
remote controlled axis in the following expected form:
MEAWA [U]= (02,1,2,-1,-2)
STOPRE
R1=$AA_MM1[U] R2=$AA_MM2[U]
R3=$AA_MM3[U] R4=$AA_MM4[U]
SITRAIN
1/2008
Axial Measurement Functions MEASA, MEAWA
Measuring with delete distance-to-
go within up to 4 trigger pulses
Measuring without delete
distance-to-go within up to 4
trigger pulses
Mode is using a two digit number:
left.: used encodernumber
right: measuring procedure
Active encoder 0
encoder 1 1
encoder 2 2
both encoders 3
Terminate measuring 0
mesure in order of trigger pulses 1
Measure in order of programmed sequence 2
MEAWA[ax]= [mode, ±n, ±n, ±n, ±n) G1 X…
MEASA[ax]= [mode, ±n, ±n, ±n, ±n) G1 X…

NC-84D-HP
MEAC (from Software V.4) Allows continuous measurement of data sequences in up
to 10 FIFO buffers $AC_FIFO1[n] ... $AC_FIFO10[n] (number in
$MC_NUM_AC_FIFO). The measured values are available as machine
coordinates.
The max. FIFO length is defined in $MC_LEN_AC_FIFO. If the FIFO is full,
measurement is automatically terminated. The FIFO can only be read out once, it
is then empty. Endless measurement is possible by cyclically reading out the
FIFO.
Mode 0 Cancel measuring job
1 to max. 4 trigger events that can be activated simultaneously
2 to max. 4 trigger events that can be activated in succession
3 to max. 4 trigger events that can be activated in succession , but no
monitoring of trigger event 1 at START
Example At axis motion of the X axis a measurement sequence is to be created in FIFO1
and stored in an array VALUE.
The falling edge of probe 1 is evaluated.
DEF REAL VALUE [100]
$AC_FIFO1[4]=0 ;Delete FIFO
G0 X0
MEAC[X]= (1,1,-1) G1 X100 F300
MEAC[X]= (0) ;Cancel measurement
WHILE $AC_FIFO1[4] <>0
VALUE[$AC_FIFO1[4]-1]= $AC_FIFO1[0] ;Relocate measured values
ENDWHILE
M0
STOPRE
M30
SITRAIN
1/2008
Continuous measurement MEAC in the FIFO
Continuously measuring
into FIFO (without delete
dist.-to-go)
MEAC[ax]= [mode, FIFO_No, ±n, ±n, ±n, ±n) G1 X…
The measurement results are in the FIFO.
At access the index specifies the function:
The FIFO is deleted by resetting the
number of elements:
e.g.: $AC_FIFO2[4]=0
Optional
Act. write indexn = 5
Number of valuesn = 4
Summary of values (read only)n = 3
Read/ overwrite last valuen = 2
R/W value 1…N= 6
Read/ overwrite oldest valuen = 1
Writing a new value or
read and delete oldest value
n = 0

SITRAIN Training for Tool Offset and Measuring

Recommended

Recommended

More Related Content

Similar to SITRAIN Training for Tool Offset and Measuring

Similar to SITRAIN Training for Tool Offset and Measuring (20)

Recently uploaded

Recently uploaded (20)

SITRAIN Training for Tool Offset and Measuring