[deanmachine]

Hi, I have a question about a old 6t control on a takasawa lathe that I have been teaching
myself . We are programming using g50s i set u0 and w0 in my tool change position and always
return my tool to the same position at the end of the program using the same g50 #s from the begining.
thats the only way i can get to run properly. However if I need to comp a tool in i put the comp number in the
offset page and it runs fine but always ends up off in the u the same amount that i used to offset tool. Then
if i just run it again it will take it off again like in a inc. mode. This seems like i am doing somthing wrong
is there a easier way to control this comp. I have only ran 90s and up controls and this issue seems like
I am doing somthing wrong?????? Any sugestions

Thanx
DMACHINE

[angelw]

Hi, I have a question about a old 6t control on a takasawa lathe that I have been teaching
myself . We are programming using g50s i set u0 and w0 in my tool change position and always
return my tool to the same position at the end of the program using the same g50 #s from the begining.
thats the only way i can get to run properly. However if I need to comp a tool in i put the comp number in the
offset page and it runs fine but always ends up off in the u the same amount that i used to offset tool. Then
if i just run it again it will take it off again like in a inc. mode. This seems like i am doing somthing wrong
is there a easier way to control this comp. I have only ran 90s and up controls and this issue seems like
I am doing somthing wrong?????? Any sugestions

Thanx
DMACHINE

I suspect that you're not cancelling the Tool Offset when returning the X, Z slides to the position where the G50 was specified. In the following example:

G50 X350.0 Z250.0
G50 T0100 S3000
G96 S200 M03
G00 X_ _ Z_ _ T0101 M08
_ _ _ _ _ _ _ _
_ _ _ _ _ _ _ _
_ _ _ _ _ _ _ _
_ _ _ _ _ _ _ _
G00 X350.0 Z250.0 M09
M01

if the X Tool Offset 01 was -0.250, the X slide will return to a position -0.250 of where the G50 was originally specified. Accordingly, the return to Tool Change position should be as follows for the above code snippet:

G00 X350.0 Z250.0 T0100 M09

Regards,

Bill

[deanmachine]

many thanks thst sounds right i will try it
thank you

[bertus.nl]

hi try the next prog it wil work i had the same problems but if jou read the yello book well ,there are 2 ways to do this and i think that the way you are doing this is screaming for epic failure.

G01 PROGRAM

Example2)
O0002 :
N10 G50 S2000 T0100 :
G96 S180 M03 :
G00 X70.5 Z5.0 T0101 M08 :
G01 Z-100.0 F0.25 :
G00 U2.0 Z0.5 :
G01 X-1.6 F0.23 :
G00 X65.0 W1.0 :
G01 Z-54.5 F0.25 :
G00 U2.0 Z1.0 :
X60.0 :
G01 Z-54.5 :
G00 U2.0 Z1.0 :
X55.0 :
G01 Z-30.0 :
X60.0 Z-54.5 :
G00 U2.0 Z1.0 :
X50.5 :
G01 Z-30.0 :
X60.3 Z-54.7 :
X72.0
G00 X150.0 Z200.0 T0100 :
M01 :
N20 G50 S2300 T0300 :
G96 S200 M03 :
G00 X55.0 Z5.0 T0303 M08 :
Z0 :
G01 X-1.6 F0.2 :
G00 X46.0 Z3.0 :
G42 Z1.0 :
G01 X50.0 Z-1.0 F0.15 :
Z-30.0 :
X60.0 Z-55.0 :
X68.0 :
X70.0 W-1.0 :
Z-100.0 :
G40 U2.0 W1.0
G00 X150.0 Z200.0 M09 T0300 :
M30 :

program is from this link page 14 enjoy http://www.cnc.info.pl//files/fanuc_...aining_588.pdf


i put in a very good atachment with the explanation

Maximum Spindle Speed Limit in CSS-mode
G50 S--- (Sets the Spindle RPM Limit in G96-mode)
NOTE: G50 must not be commanded inadvertently on the same line together with any X or Z coordinates, otherwise a new work coordinate system will be set. The G50 command remains modal, so there is no need to repeat it within the same program unless a new speed limit needs to be set.


greetings bertus

[angelw]

i put in a very good atachment with the explanation

Maximum Spindle Speed Limit in CSS-mode
G50 S--- (Sets the Spindle RPM Limit in G96-mode)
NOTE: G50 must not be commanded inadvertently on the same line together with any X or Z coordinates, otherwise a new work coordinate system will be set. The G50 command remains modal, so there is no need to repeat it within the same program unless a new speed limit needs to be set.


greetings bertus

Deanmachine's control is a Series 6. G50 is the way in which the Coordinate System is set with this control; there are no WorkShift or Tool Geometry Offsets available as is the case with the DOOSAN example.

Regards,

Bill

[bertus.nl]

hi

i have had a takisawa lathe with fanuc 6t from 1984 or 85

i sold it a few years ago but i can ask the guy to take a picture from the machine and control.

and the program how its done .


greetings bertus

[fordav11]

for a 6T, the way Bill explained it in post#2 is "how it's done"

[L98FIERO]

Listen to Bill and Fordav11, they got me working on my 6T! Thanks again guys!