Rigid tapping code questions for Mori CL-153 lathe

[tar356]

Looking for some code help for tapping on my lathe. It's a 2001 CL-153 with a Mistubishi controller.

Here's the code from Fusion 360 i'm trying to use for a 3/8-24 hole, but it alarms out:

T1111
G54
G98
G97 S200 M3
G0 X0. Z2.0147
G0 Z1.6147
M29 S200
G84 X0. Z0.5439 R1.4939 P0 F8.3
G80
Z2.0147
G28 U0.
G28 W0.
M30

(The M8 and M9 were deleted for testing)

I'd like to use the canned G84, but not opposed to using G32 and a floating head if needed.

Thoughts?

Thanks!

Todd
Orange, CA

 

[Fancuku]

What is the alarm?
And don't ever use inch per minute (G98) feed in a lathe. There is zero reason for that.

 

[tar356]

What is the alarm?
And don't ever use inch per minute (G98) feed in a lathe. There is zero reason form that/

Thanks for the reply Fancuku...

I didn't right down the alarm, but it was a few numbers and letters.

Ahhh, maybe the G98 is the problem?? Fusion posted the G98, maybe if I switch to G99 and change the feed to inches per revolution it might work??

 

[Vancbiker]

Mori mills with Mitsu controls do not use M29. The G84 is rigid tapping by default (selected by parameter). I suspect the lathe will be the same.

 

[tar356]

Mori mills with Mitsu controls do not use M29. The G84 is rigid tapping by default (selected by parameter). I suspect the lathe will be the same.

So remove the M29??

 

[Fancuku]

Thanks for the reply Fancuku...

I didn't right down the alarm, but it was a few numbers and letters.

Ahhh, maybe the G98 is the problem?? Fusion posted the G98, maybe if I switch to G99 and change the feed to inches per revolution it might work??

It will not alarm with G98 but it is not recommended to use IPM feeds in a lathe.

And like the other poster said, the M29 may be your problem. Remove the M29 line and try again.

 

[angelw]

Looking for some code help for tapping on my lathe. It's a 2001 CL-153 with a Mistubishi controller.

Here's the code from Fusion 360 i'm trying to use for a 3/8-24 hole, but it alarms out:

T1111
G54
G98
G97 S200 M3
G0 X0. Z2.0147
G0 Z1.6147
M29 S200
G84 X0. Z0.5439 R1.4939 P0 F8.3
G80
Z2.0147
G28 U0.
G28 W0.
M30

(The M8 and M9 were deleted for testing)

I'd like to use the canned G84, but not opposed to using G32 and a floating head if needed.

Thoughts?

Thanks!

Todd
Orange, CA

Hello Todd,
Irrespective of whether G99 or G98 is used to specify the feed mode, the Feed Rate should be specified as accurately as possible when using Rigid Tapping. A floating holder is forgiving, but not so with Rigid Tapping and a Rigid Tool Holder.

A feed per minute of 8.3" and a spindle speed of 200rpm will result in an error of 0.0017" per 10 revs or 0.4166". Not a mammoth error, but similar to never having seen a crack get any smaller, program errors never seem to improve situation. Particularly errors that are obvious and easily preventable.

Regards,

Bill

 

[TeachMePlease]

What is the alarm?
And don't ever use inch per minute (G98) feed in a lathe. There is zero reason for that.

Sure there is... Broaching with your lathe

 

[tar356]

Ok all..

Made the changes to post as follows and ran it in "air":

T1111
G54
G99
G97 S200 M3
G0 X0. Z2.0147
G0 Z1.6147
G84 X0. Z0.5439 R1.4939 P0 F0.04166
G80
Z2.0147

G28 U0.
G28 W0.
M30

The tool moved to position, "threaded" in, the spindle reversed, ramped up in rpm with the tool not backing out. Alarm showed "Spindle drive unit alarm" (G1035)

Thanks,

Todd
Orange, CA

 

[sinha]

I am not conversant with this control. However, there are some general comments:

1. Are you sure if rigid tapping option is enabled on your machine?
If so, the spindle should first stop and then again restart automatically at the R-point.
In fact, M03 is not needed. Only an S-word is needed. And, spindle override switch will become disabled.

2. Try specifying some dwell at the bottom, say, 500 milli-seconds.

 

[13engines]

What is the alarm?
And don't ever use inch per minute (G98) feed in a lathe. There is zero reason for that.

That's quite a statement. I have drilled all day long many a time on a lathe using G98, and find no problems with it. Being a mill guy who is sort of a newb on lathes I find it familiar and am comfortable with it. Besides that, the entire programming manual provided by Mori Seiki (Fanuc) uses G98 in all of the Hole Machining Canned Cycle examples. G97/G98 or G97/G99. Take your pick when drilling as far as I'm concerned. They both do the same thing in their own way.

And then there's Polar Coordinate Interpolation. Another G98 place to play.


2nd thoughts: Still not keen on blanket statements, but on a basic two axis lathe, I can see where that statement is not very far from the truth. Especially if you were trained in that way. As anyone knows, specifying FPM for a drill starts out as FPR anyway, plus some math. It's not hard to see where in a days work, G97 may never show up.Ever! As the statement goes. :-)

Even as a lathe newb, the joke mentioned about broaching on a lathe is not lost on me. Good one...

 

[angelw]

Ok all..

Made the changes to post as follows and ran it in "air":

T1111
G54
G99
G97 S200 M3
G0 X0. Z2.0147
G0 Z1.6147
G84 X0. Z0.5439 R1.4939 P0 F0.04166
G80
Z2.0147

G28 U0.
G28 W0.
M30

The tool moved to position, "threaded" in, the spindle reversed, ramped up in rpm with the tool not backing out. Alarm showed "Spindle drive unit alarm" (G1035)

Thanks,

Todd
Orange, CA

Hello Todd,
Whether synchronous (rigid) tapping is carried out with the G84 command is determined either by parameter setting, or by program command using R0/R1 to use asynchronous and synchronous respectively. The "R" address is also used in the command line to specify the Retract Plane. The "R" address for selecting Rigid Tapping is differentiated from the "R" plane address by preceding it with a comma at the end of the command line.

The control can also be set via parameter to use a custom "M" code to specify rigid tapping. Therefore, unless you know your control well, you need to check the parameter settings relating to Rigid Tapping.



Regards,

Bill