What's new
What's new

VMC 650 (chinese machine NEW) Metrol toolsetter

williedl78

Plastic
Joined
Mar 28, 2024
Location
5Rachelenansn_
Issues with getting the Machine setup,

Machine was delivered with tool setting probe on top of the 4 axis. I have relocated it to the table. about a 9" difference. The machine is running Fanuc OI MF.

Macro program works and I have relocated the X&Y for the new probe position.

Issue 1 when I set the tool lengths for my tools, it loads the length offsets into the Wear offset of each tool not the geometry. Not sure how to change this?

Issue 2 I set all my tools then setup up my part I brought my master tool down and touch the top of the part and save that location in G54 for z. When I run a program from Fusion it puts (G43 H##) and the moves to z location, My distance to go is several inches below the table.

I wrote in MDI to select several tools and go to G54 Z0 and it is good on location.

I went back to program that fusion outputs and removed the line with G43 and the program runs correctly.

I am not sure if this has to do with where the location of z is for the new probe location, and if so where do I change that, or if I am going to have to change the program every time to and manually remove every G43?.
 
For issue 2, it sounds like are you not accounting for the master tool length when you touch off the master tool on the top of the part. When I touch off on 0i-Mf+, my master tool is my Haimer probe and G43 is not active. The G54 Z value is gotten by entering Z6.9970 and pressing "measure" while the G54 Z box is highlighted. Z6.997 is the known length of my Haimer probe from the gauge line. All my tool lengths are positive relative to the gauge line.

Issue 1 must be an issue in the probing macro.
 
Thank you for all the help, I think that will help with issue 1. Here is the macro supplied, and I cannot make sense of it. thank you for any help It is greatly appreciated.

O9020(Metrol AUTO-TOOL-LENGTH-MEASUREMENT For Mitsubishi)

#510=596.750(X-axis Machine Coordinate)
#511=-140.50(Y-axis Machine Coordinate)
#100=3000(FIRST FEED)
#101=1200(SECOND FEED & "Don't exceed 1200")
#102=505.(Z MAX TRAVEL)


#103=4(RE MEASUREMENT ERROR)
#104=0.05(TOOL MAX WEAR)
#105=50(MAX DIAMETER)
#106=15(OVER TOOL DIAMETER Y OFFSET)


#513=0(OFFSET)


(#3003=1)
(SINGLE BLOCK DISABLE)
IF[#7GT0]GOTO2(D)
(TOOL-DIAMETER<=0)
IF[#7NE#0]GOTO2(D)
(TOOL-DIAMETER-MISSED)
IF[#7GT#105]GOTO81(D)
(TOOL-DIAMETER>MAX DIAMETER)
#7=1

N2
IF[#11GT0]GOTO4(H)
(TOOL-OFFSET-NO.<=0)
IF[#11NE#0]GOTO4(H)
(TOOL-OFFSET-NO.MISSED)
IF[#4111EQ0]GOTO3(H)
#11=#4111(H CODE)
GOTO4

N3
#11=#4120(T CODE)

N4
IF[#11LE0]GOTO82
(TOOL-OFFSET-NO.<=0)
IF[#9NE#0]GOTO6(F)
IF[#9GT0]GOTO6(F)
#9=#101

N6
IF[#23EQ0]GOTO10
IF[#23EQ#0]GOTO10
IF[#23GE1]GOTO10
#104=#23

N10
#112=#4003
(G-GROUP3-MEMORY)
#113=#5021
(X-COORDINATE-MEMORY)
#114=#5022
(Y-COORDINATE-MEMORY)
#115=#5023
(Z-COORDINATE-MEMORY)
#116=#4119
(S-CODE-MEMORY)

N20
G00G91G28Z0
(M06T#11)
(Automatic tool change "H" code)

M05

IF[#7LE#106]GOTO30
#107=FIX[#7/2.]
GOTO40

N30
#107=0

N40(Offset +Y)
#108=#511+#107
G90G53X#510Y#108
(Offset +Y: #108=#511+#107,G90G53X#510Y#108)
(Offset -Y: #108=#511-#107,G90G53X#510Y#108)
(Offset +X: #108=#510+#107,G90G53X#108Y#511)
(Offset -X: #108=#510-#107,G90G53X#108Y#511)


M33(AIR BLAST ON)


IF[#512GT0]GOTO42
IF[#512LT0]GOTO42


#512=-140.(#100 FIRST FEED Drop distance)


N42
G91G31Z-[ABS[#512]]F#100
G31Z-[#102-ABS[#512]]F#9

N44
#121=#5023
#111=#5023+0.2
(#111=#5023,Not installed the tool protection)
IF[#111LE-#102]GOTO84
G91G01Z5.F5000
(#3004=2)
(Second measure feed switch to no avail,default electricity=0)
G31Z-7.F40.
#120=#5023


M34(AIR-BLAST-OFF)


G04X0.1
(#3004=0)
(Second measure feed switch to valid,default electricity=0)
#111=ABS[#120-#121]
IF[#111GT#103]GOTO85
(RE MEASUREMENT ERROR)
#110=#[2000+#11]-#513
IF[#110EQ0]GOTO46
IF[#23GT0]GOTO50

N46
#[2200+#11]=0
#[2000+#11]=#120+#513
#516=#120
GOTO52

N50
#515=#120-#110
#109=ABS[#515]
IF[#109GT#104]GOTO86
#[2200+#11]=#515(#104,"W" code,Measure wear extent & add to tool wear offset)

N52


M34(AIR-BLAST-OFF)


(#3004=0)
(Second measure feed switch to valid,default electricity=0)
G28Z0
G90G00G53X#113Y#114
(G91G30X0.Y0.)
(Back to tool change location)
G#112
GOTO100

N81
#3000=1(ATM-TOOL-DIAMETER-ERROR,D Error)
GOTO100

N82
#3000=2(ATM-TOOL-OFFSET-NO.ERROR,H Error)
GOTO100

N83
#3000=3(ATM-OFFSET-LEVEL-ERROR,Nothing)
GOTO100

N84
G91G28Z0.
#3000=4(ATM-INCORRECT-TOOL,#102 or Fanuc 1321 parameter)
GOTO100

N85
G91G28Z0.
#3000=5(ATM-RE-MEASUREMENT ERROR,W Error or Fanuc 6200 parameter #1 SK0 Error)
GOTO100

N86
G91G28Z0.
#3000=6(ATLM-TOOL-WAS-BROKEN)

N100(FINISH)

(#3003=0)(SINGLE BLOCK ENABLE)

M99
%
 
It doesn't look like there is a calibration routine, this program is stand alone.
You could alter this line to calibrate it yourself "#513=0(OFFSET)"

It looks like this should be called by a command like G65P9020Dxxx.Fxxx.Hxxx.Wxxx. correct?
D = DIAMETER OF TOOL
F = FEED RATE
H = HEIGHT OFFSET
W = MAX ALLOWED WEAR OFFSET

This program doesn't rotate the tool during touch off so there is no way for it to know if it will hit a tooth.
According to the parameters set in the program it has a wide 50mm touch pad.
When the D is greater than 50mm it will shift the Y to touch off the tool.

It shouldn't be setting the wear offset unless you specify Wxxx. in the command.
I have a Kitamura that has the D offset geometry and wear macro numbers backwards, I wonder if your machine is the same for H offsets.
A simple test would be this:

O1
#2001=1.
#2201=2.
M30

If this runs correctly tool 1 H offset Geometry should be set to 1. and Wear should be set to 2.
 
Correct in MDI "G65P9020H1" for example. The machine comes down touches probe, up, slower feed and touches probe a second time, then back to tool change position or Home. I check offsets and is entering the number in wear. I will try your suggestion and see what happens. Thank you
 
It doesn't look like there is a calibration routine, this program is stand alone.
You could alter this line to calibrate it yourself "#513=0(OFFSET)"

It looks like this should be called by a command like G65P9020Dxxx.Fxxx.Hxxx.Wxxx. correct?
D = DIAMETER OF TOOL
F = FEED RATE
H = HEIGHT OFFSET
W = MAX ALLOWED WEAR OFFSET

This program doesn't rotate the tool during touch off so there is no way for it to know if it will hit a tooth.
According to the parameters set in the program it has a wide 50mm touch pad.
When the D is greater than 50mm it will shift the Y to touch off the tool.

It shouldn't be setting the wear offset unless you specify Wxxx. in the command.
I have a Kitamura that has the D offset geometry and wear macro numbers backwards, I wonder if your machine is the same for H offsets.
A simple test would be this:

O1
#2001=1.
#2201=2.
M30

If this runs correctly tool 1 H offset Geometry should be set to 1. and Wear should be set to 2.
another issue is I am fairly new to these macro programming, I am unfamiliar with the #2001 #2201. In the program above I was trying to make sense of these numbers and what they are referencing same with #5023
 
Unfortunately this is a typical example when execution of basic task demands the intervention of macro wizard. Shameful lack of information (operating manual, instructions ???).
The program itself seems to me very cumbersome to fulfill this simple job. Metrol tool setters are meant to be used in Z axis only.
I suggest to use the program which I wrote and is used in many applications. The operating instructions are attached. Seems to me to be shorter and clearer to follow and understand.
To use the air blow M33/M34 (tool setters harshest enemy), edit the program accordingly.
%
O9555( SNR AUTOMATIC LENGTH MEASURMENT TLS FANUC)
(REV. 25.03.2022)
(G65 P9555 I.. I.. I.. - MEASURE TOOL)
(G65 P9555 C123.456 - CALIBRATE TOOL SETTER, C - CALIBRATION TOOL LENGTH)
(G65 P9555 A0.1 - TOOL BREAKAGE, A - TOLERANCE)
G5.1Q0
#120=520 (BASE NUMBER)
#121=1500 (FAST APPROACH FEED)
#122=30 (MEASURING FEED)
#123=2. (BACK OFF)
#124=20. (CALIBRATION MOVE)
#125=10000 (LENGTH WEAR MACRO)
#126=11000 (LENGTH GEOM MACRO)
#127=0.01 (MEASURING DISTANCE)
#129=100 (TIME DELAY)
#130=600. (Z AXIS STROKE)
#131=300. (MAXIMUM TOOL LENGTH)
(##################################)
IF[#3NE#0]GOTO2000
IF[#1NE#0]GOTO3000
G28G91G0Z0
#3004=0
#1=0
N10
IF[#[4+#1]EQ#0]GOTO9999
M6T#[4+#1]
N20
G91
G0X[#[#120+3]-#5021]Y[#[#120+4]-#5022]
N50
G31Z[#[#120]+#131-#5023]F[#121*2]
G53
(*****************)
#14=#5023
G31Z[2*#127]F[#127*600]
G53
#15=#5023
G0Z[#14-#5023]
IF[ABS[#14-#15]GT#127]GOTO60
(*****************)
#3000=91 (PROBE OPEN)
N60
M0 (STOP BEFORE MOVING TOWARDS TS)
G91
#3004=2
G31Z[-0.99*#130-#5023]F#121
G53
(*****************)
#14=#5023
G31Z[2*#127]F[#127*600]
G53
#15=#5023
G0Z[#14-#5023]
IF[ABS[#14-#15]LT#127]GOTO70
(*****************)
#3000=92 (PROBE FAIL)
N70
G0Z#123
G31Z[-0.99*#130-#5023]F#122
G53
#3004=0
#[#125+#[4+#1]]=0
N80
#[#126+#[4+#1]]=#5063-#5043+#5023-#[#120](SET TOOL OFFSET)
G91G28G0Z0
#1=#1+3
GOTO10

N2000 (CALIBRATE TOOL SETTER)
#3004=2
G91
G31Z-#124F#121
G53
(*****************)
#14=#5023
G31Z[2*#127]F[#127*600]
G53
#15=#5023
G0Z[#14-#5023]
IF[ABS[#14-#15]LT#127]GOTO2010
(*****************)
#3000=92 (PROBE FAIL)
N2010
G0Z#123
G31Z[-2*#123]F#122
G53
#[#120]=#5063-#5043+#5023-#3
#[#120+3]=#5021
#[#120+4]=#5022
GOTO9999

N3000
G91G28G0Z0
IF[#4111EQ#0]GOTO3005
IF[#4111NE0]GOTO3010
N3005
#3000=97 (NO ACTIVE H)
N3010
X[#[#120+3]-#5021]Y[#[#120+4]-#5022]
N3020
G0Z[#[#120]+[#124+#[#126+#4111]+#[#125+#4111]]-#5023]
N3030
G31Z[-[#124+#1]]F[#121]
G53
(*****************)
#14=#5023
G31Z[2*#127]F[#127*600]
G53
#15=#5023
G0Z[#14-#5023]
IF[ABS[#14-#15]LT#127]GOTO9999
(*****************)
#3000=98 (BROKEN TOOL)

N9999
#3004=0
G91G28Z0
M99
%

Stefan
Cogito Ergo Sum
 

Attachments

  • SNR TLS OPERATING INSTRUCTIONS.pdf
    412.1 KB · Views: 1
another issue is I am fairly new to these macro programming, I am unfamiliar with the #2001 #2201. In the program above I was trying to make sense of these numbers and what they are referencing same with #5023
#2001 should be H1 Geometry offset.
#2201 should be H1 Wear offset.
#5023 is the stored Z position when the sensor is tripped during a G31 move.
 
getting used to this machine, has been a bit more challenging than i remembered. i am also stuggling with getting z set in g54. the machine is metric machine coordinates, and my programs are Imperial units.
 
getting used to this machine, has been a bit more challenging than i remembered. i am also stuggling with getting z set in g54. the machine is metric machine coordinates, and my programs are Imperial units.
Check parameter 3104 bit 0. I expect it will be 0. If set to 1 your machine position display will be displayed in imperial if you are programming imperial.
 








 
Back
Top