[superalitos]

:drowning:

Hi, I hope someone can help me with this problem.

When I use CSS (G96) my spindle runs automatically to maximum rpm programmed with G50 so it not accelerates as it reach the X0.0 corrdinate or low rpm as X coordinate increment.

I have programmed G96 at HOME position and before cutting movement near the stock and does the same thing.

G97 works as expected. I have no problem to select spindle gear range (G40,G41).

The whole lathe it's working well and precisely but this feature it's not working well.

Wasino L5-J, 1982

Unfortunatelly, I don't have parameters manual for this machine. I have only a maintenance & troubleshoot pdf donwloaded from the web for 6T Model-B but parameters don't match.

Best regards

:drowning:

[dcoupar]

Has it ever worked on this machine?

[underthetire]

I remember something about using a G50 to tell where to start the diameter on css from on the old controls.

Sent from my SM-T813 using Tapatalk

[superalitos]

I really don't know. Programming manual of the machine has indicated G97/G97 (rpm/css) as standard codes and options in the machine. Also I use G98/G99 (fpm/fpr). If I use G97 Sxxxx, rpms do what it suposed to do but if I use G96 Sxxx, automatically turns spindle to max rpm set by G50 Sxxxx. This is a problem because if I'm running a large part diameter inserts goes to very high temp and life expectancy turns down for every tool.

My machine is like the one you can see at https://www.youtube.com/watch?v=_RCx_DqMKVM, but mine moves and do tool change a little bit faster.

It's been a big problem to get parmeter, users and maintenance manual for Fanuc 6T-Model A.

[superalitos]

I have tried to do stuff like this:

(Facing 100 mm dia)

O0001
G21 G40
G28 U0 W0 T0 (Return to machine 0 with offset cancellation)
G50 X___ Z____ S1000 (Tool Zero Point Offset, setting Max RPM during G96 operation)
M41 Txx00 (Spindle speed range high, tool index)
G96 M4 S160 (turn on spindle and CSS mode)
G0 X105.0 Z-1.0 M8 (Aproach)
G99 G1 X-1.6 F0.18 (Feed Per Revolution, Feed)
G0 Z5.
X110.0 (safe pos)
G97 S400 M9
G28 U0 W0 T0 M5
.
.
.

Also:

O0001
G21 G40
G28 U0 W0 T0 (Return to machine 0 with offset cancellation)
G50 X___ Z____ S1000 (Tool Zero Point Offset, setting Max RPM during G96 operation)
M41 Txx00 (Spindle speed range high, tool index)
G97 M4 S400 (turn on spindle and CSS mode)
G0 X105.0 Z-1.0 M8 (Aproach)
G96 S160
G99 G1 X-1.6 F0.18 (Feed Per Revolution, Feed)
G0 Z5.
X110.0 (safe pos)
G97 S400 M9
G28 U0 W0 T0 M5

=> No matter the place I put the G96 code, as soon as control reads it it turns spindle to max rpm (1,000 rpm).

[sinha_nsit]

Use G50 without X/Z addresses.

[superalitos]

Already done sinha_nsit and still do the same.

[sinha_nsit]

Try G96 S10 and observe what happens.

[superalitos]

Try G96 S10 and observe what happens.

Still do the same. No rpm increment/decrement. :'(

[sinha_nsit]

No idea really.
Maybe a parameter has disabled G96???

Is it necessary to use M41 on this machine?

[superalitos]

No idea really.
Maybe a parameter has disabled G96???

Is it necessary to use M41 on this machine?

===
Yes,

M40 =Low Range [8 ~ 850 rpm]
M41 = High RPM [30~3,000 rpm]

For a AISI/SAE H13, 150 mm Diameter, Iscar WNMG-432-GN, I'm working in the low rage.

- SMM: 160 m/min
- G97 S330
- G96 S160
- G50 S750

I always use X0.0 as my reference for G50 tool offset setup.

Thank you all guys

[dcoupar]

When you execute the G50 X_ Z_ S1000 block, does the X absolute position display the same value as X_?

[superalitos]

:cheers:

Problem solved guys,

It was a parameter problem. (chair)

Parameter #0132 [LOWSP] - "Least spindle revolution number in CSS (G96)"

Setting was 1,010 rpm, I just change it to 100 rpm and started to work.

Anyway, thank you very much for your suggestions dcuopar, sinha_nsit and underthetire.

Best regards

:cheers: