[deanmachine]

hi I have a older fanuc 6t control on a takasawa lathe we are having issues touching off tools please help we do not know this control

[BlueChip]

Kind of vague but here's some starters :

(1) Move the turret to where you want the tool change position to be ... if it's other than X / Z zero return position.
(2) Go to the position display ... flip to the U / W display ... U --> CAN W --> CAN ... this will zero out the display.
(3) Take 1st tool ... touch the face of the part ... let's say that's Z0 to make things simple ... record the W value that's in the position display.
(4) Touch or take a skim cut on the OD ... let's say that it now measures .500" ... take the U value in the position display and add the .500 to it .... record that.

You need to do this for every tool ... every tool will have different values of course because every tool is sticking out of the turret different dimensions.

Those U and W values are your G50 numbers.
The 6T control doesn't have Work Offsets or Geometry Offsets ... the program uses the G50 command to establish the relationship between the TOOL TIP AT TURRET INDEX POSITION AND THE X / Z ZERO POINT ON THE PART.

Your program looks like this :

G50 X ( the U value from the above ) Z ( the W value from the above ) ( no movement happens here ... just the X / Z position display is set to these values )
G00 T0101 ( or whatever tool # you used in the above )
-----
-----
----- do the work with the tool
-----
-----
G00 X ( the U value from the above ) Z ( the W value from the above ) ... physically move the tool back to the index position
THIS POSITION AND THE G50 VALUES MUST MATCH ... because you want the turret to physically be at the position from which the G50 numbers were recorded.
M01

( next tool )
G50 X ---- Z ---- ( values are whatever you obtained from touching off THIS tool using the procedure above )
G00 T0202
-----
-----
----- do the work with the tool
-----
-----
G00 X ---- Z ---- ... physically move the tool back to the index position ... this position MUST match the G50 values for this tool
M01

Hope this helps ... it'll start the discussions anyway.

Bluechip
Check out our Real World Machine Shop Software at Kentech Inc. - Real World Machine Shop and CNC Software

[deanmachine]

THANKS SO MUCH WE ARE GETTING GOING ON YOUR DIRECTIONS I WILL LET YOU KNOW HOW IT WORKS MANY THANKS

[deanmachine]

WE ARE N THE RIGHT TRACK I BELIEVE HOWEVER WE PUNCHED IN THE G50#S AS NEGATIVE BECAUSE THATS WHAT THEY WERE AND IT WAS CUTTING WAY BIGGER THAN IT SHOULD IN BOTH AXIS (BY MANY INCHES) WE TRYED MAKING THEM POSITIVE BUT HAD WEIRD RESULTS
ANT IDEAS? ALSO ON THE TOOL OFFSET SCREEN DOES IT NEED A VALUE IN THE XZ SPOTS FOR THE TTOL THAT WE ARE ALLING UP NOW THEY ARE ALL SET TO ZERO

[BlueChip]

The G50 numbers pre-set those values into the position display ... think of it as pre-setting a digital readout ... when the display is set that's where the machine "thinks" it is. So if G50 Z is 1.000 ... the machine knows it has to move in the negative direction 1.00 to get to zero. You may have to reverse the signs. Make sure the G50 values are measuring from the tool at index position ... with the display at zero ... to the part.

The offset on the 6T is for wear on the tool ... so if you command T0101 you are using Tool station #1 and offset #1. If you measure the part and it is .002 too long ... inputting an offset value of -.002 in the Z offset #01 will cause the tool to shift up -.002 as it cuts .... making the length correct. So the offsets are just for wear. Some people add values to purposely make the diameters big and the lengths long ... then adjust based on actual cut dimensions.

Hope this helps ...
Bluechip
Check out our Real World Machine Shop Software at Kentech Inc. - Real World Machine Shop and CNC Software

[fordav11]

if you dont know how to set G50s on a 6T (or any machine without geometry offsets) you should read up on that first.....
google has plenty of answers....
https://www.google.com.au/search?num...ls+on+fanuc+6t

Quick G50 Fanuc 6T question