G37

[positiverake1]

Anybody use a G37 on a puma with a mits control? , looks like a auto tool set, how do you use it?

[M-man]

Have tried it on a puma with Fanuc...It prob works the same with mits. On fanuc it is called automatic tool offset.. It could be used to check tool determine tool condition..

This is how it works on a puma lathe.
swing presetterarm down
(X-axis).
Position tool in The Z axis and X-axis, 2" above sensor(so it will hit the sensor when reading X-axis).
Launch G-code for automatic tool comp. U-2" (THe tool is expected to hit the sensor when moving this amount).
(half of the distance (1") are in Rapid and the other half is on parameter preset speed.
if no contact are done within a certain overtravel of expected contactpoint an alarm will be generated. If everything works as planned a new offset value will be loaded into the wear offset page). With some macro this could be used for ex. checking out critical tools, or just compensating for tool wear.

I think Fanuc uses G36/G37 for X and z axis, (this I am not completley sure of, without checking the g-code list)... Any way, it looks quite cool to the arm being swinged down and the tool are rushed toward the presetter in quite high speed.

[positiverake1]

So do you have to manualy bring the arm down and position the tool ? I know I used a same type of thing on a mazak years ago and how that worked is the tool had to be already set, and then run the program and the machine would drop the arm, rapid to position set both x and z and return home and send the arm back, like you said, it would be useful for a close diameter or spare tool on a long run, what I would like to use it for is for changing inserts, I always use the same tooling, so it would be nice to change a insert, call the G37 in M.D.I. and let it set it self, if you have to bring it to the probe manualy, I dont see the use? I think your saying it is automatic, like you said its cool to wacth, on that mazak, once I knew how to use it, I scared the hell out of my boss with it (rapids on that machine were 1800 in. per min) like to do the same thing to this boss . anyway Ill have to look at the settings, seems like I seen somthing about the rapid setting distance, dont want to rip the arm off! thanks for the info, any more would be great.

[M-man]

I have only used it during automatic operation. And I drop the arm with a M code.. On fanuc I think I could be able to assaign a M code to execute a tool setting macro, called from Mdi.. Ex M110 T1 (OD). And use M111 for ID or use a variable to set if it is an Id or OD tool...Mabe the right way is to determind wich switch that are going to do the messuring.. Ex M110 T1 P1..

The distance wich uses Rapid is 50% of your incremental command.. (On my machine it is).

Any ideas?

[positiverake1]

Hi m-man, hows it going over there in sweden? anyway Ill do some digging when I get some time, were ramping up to 50 hrs a week, but maybe Ill write a macro if I cant get the G37 to do what I want, probley go off machine scale (G53) and use some variables like you said for O./D I./D. , I'll have to find the sensor numbers or maybe it will set the numbers in the tool set page just like it does when I do it in manual, probley need some dwells and things, anyway good yaking at ya, I'll let you know if I figure it out.

paul from minnesota U.S.A.

[M-man]

(OD tool messuring/1)
#1=#4014
G53
G28U0
G28W0
G0T#20#20
M__ Code for pre-setter-arm down.
G0Z____
X_____
G36U-0.5"
G0U0.5"
Z______
X______
G37W-0.5"
W0.5"
G0W0.5"
G28U0
G28W0
M__ Code for pre-setter-arm up.
G#1 --- Return to G54,G55 etc.
M30

[positiverake1]

Looks good, Is this from a fanuc? have you ran this?

[M-man]

OD tools/Right side cutting.


This macro works for Puma 300 with Fanuc 16/18/21iT (Tried it today)
Control must support MAcroB,Workcoordinate system and quick setter options.

Set parameter 6080 to 110 and the macro will be called with M110, etc. (macro must be placed at O9020 for this to work.)

The macro is designed to work with tools that have already been set and got their insert replaced, etc. The position of the messure sensor position must set on each machine.(Set g54 to O in all axis, call a tool and do a messure, read the value in your coordinate system, this is the pos of sensor).

Anyway: In MDI.... M110 T0404 – will launch messuring of tool number four.
M110 T0505 will messure tool number five, etc.

All use of the macro is on your own risk.



%
O9020(PRE-SET OD)
IF[#20EQ#0]GOTO51
GOTO50
N0001
#1=#4014 ; Read and save work coordinate, G54,G55 etc.
#2=#5221 ; Read and save G54 X....
#3=#5222 ; Read and save G54 Z....
G28U0
G28W0
#5221=#0 ; Set G54 X to Zero
#5222=#0 ; Set G54 Z to Zero
G54
G0T#20 ;
M80 ; Swing pre setter arm down.
G0Z372 ; Move into z-pos to read X-axis
X187 ; Move X-axis into Pos.
G36X181 ; Launch X- axis messuring, X181 EQ expected contact pos.
G0U10 ; Retract 10mm
Z400 ; Move into z-pos for reading Z-axis
X140 : Move z axis in pos for reading Z-axis.
G37Z393 ; Launch z-axis messuring, Z393 EQ expected contct pos.
G0W10 : retract 10mm
G28U0
G28W0
M81 ; swing pre setter arm up
#5221=#2 ; Restoring G54 X to same value it had before calling macro
#5222=#3 ; Restoring G54 Z to same value it had before calling macro
G#1 ; Set work coordinate to same as befor macro call. G54,G55 etc.
M30
N50#3006=1(MESSURE OD) Skip this line if you don’t want to press cycle start twice.
GOTO1
N51
#3000=1(NO TOOL SELECTED) ; Launch alarm if no tool are selected.
M30
%


To set this macro on MIT, I am pretty sure it is just to change the varible number to read and set all coordinate values, and some m codes for setter arm...

Hopefully some one got any use of it...