What's new
What's new

Help with a Lathe tapping cycle

elcar903

Plastic
Joined
May 5, 2022
Hi I am trying to get a tapping cycle to work on my
Daewoo Lynx 210
Year: 2002
Fanuc controller Oi-T ( no other letters after it)

I am using Mastercam 2018 with the default lathe post
and I am only having issues with the tapping cycle,
The other code such as turning or OD threading works fine

The code I have seems to run, its just that the spindle ramps the RPM up to fast and changing the S85 in the code doesn't seem to effect it.
the lathe shows the RPM going to around 680 when running this operation and its to fast for this tap.

Tap is a 12MM-1.75

Here is the code I am using:

%
O0100 (SHAFT P1)
(DATE=3/28/2023)

G20

(TOOL - 8 OFFSET - 8)

(12X1.75 TAP)
T808
G97 S85 M03
G0 G54 X0. Z.1
M29
G84 Z-1.25 F.0689
G80
G00 X9. Z5. M05
T800
M30
%

Thanks for any help on this I can get
 
As suggested by Ox, but also delete G97 S85 M03, M29 S85 and the Tapping Cycle will start the spindle. It depends on the implementation of Rigid Tapping by the MTB as to whether starting the spindle prior to calling the rigid tapping will affect the operation, so having the spindle started from stopped by M29 S_ _ and the cycle is the safest method.

Your example code shows the tapping operation being the whole program. If the tapping operation were to follow a drilling operation, for example, where the spindle was already running for that previous operation, its also better to stop the spindle (M05) before the tapping operation for the same reason as previously stated regarding not having the spindle running with G97 S85 M03 prior to the rigid tapping cycle.

Regards,

Bill
 
I was finally able to get it to run correctly and not have an alarm on it.

Based on the suggestions here and what my machine likes apparently I was able to get it to work.
Other variants gave an alarm or would feed incorrectly.

(TOOL - 8 OFFSET - 8)

(12X1.75 TAP)
T808
G0 G54 G99 X0. Z.1
G97 S85 M29
G84 Z-1.25 F.0689
G80
G00 X9. Z5. M05
T800
M30

The controller is an "Fanuc Oi-Ta from what Doosan told me today after waiting 2 days on a reply.
and it apparently is picky on certain cycles, Other operations don't have any issues with the code that Mastercam posts.

Thanks for the help with this.
 
On a side note, a combined XYZ positioning move can be risky, due to a possible interference with clamps, for example. I prefer XY positioning, followed by Z positioning. This may take a second or two extra, but is safer.
 
When the tool is at G28 position, rapid in Z, followed by rapid in X, to approach the workpiece OD is safer.
 
Former Daewoo/Doosan/DN A/E here.

For Rigid tapping on lathe we always recommended "G97 S100 M29;" on a line by itself, immediately followed by - "G84 Zxxxx Fxxxx;" then a "G80" to cancel both the G84 cycle AND the M29 rigid tap mode.
I believe that minimum speed for the Lynx is 100 rpm so try not to ask for anything lower than that.

Also, your Fanuc is a Fanuc 0iT-C.

@sinha is correct, a Z position followed by X is recommended for clearing the tailstock when approaching from a G28 home position tool change.
 








 
Back
Top