Need Help!- G84 Z-1.250 R2000 P1000 F.0909

[PRINT_FX]

G84 Z-1.250 R2000 P1000 F.0909

what is the R and P?


this is a face tapping cycle on a TW-10 twin spindle...
I'm abit afraid of letting this program going into the shop, I don't know what R or P means, can't find information on that anywhere... would assume that R is starting point and P for pause,
but why 4 digits and why a pause?

we are setting up a 5/8 emuge tap with a collet.

thank you

[dcoupar]

You don't say what control you are using, but the explanation from the 18iT-B manual seems to agree with what you say.

The R value is the distance from the current Z position to the start of the tapping feed.

The P value is the dwell time, although I've never programmed a tap cycle with a dwell. It has 4 digits because P can't have a decimal point. P1000 would be a 1 second dwell (.001*1000)

R can have a decimal point.

I believe if you're going to use rigid tapping, you'll need an M29 S#### in the block immediately preceding the G84.

M29 S500
G84 Z-1.25 R.2 P1000 F0.0909

[PRINT_FX]

I’m using a TW-10 Nakamura-Tome Luck-Bei B104-18, but the programming style is the exact same as a TW-20 machine that we also have with Fanuc controls series 16-TT, I actually like theses types of controllers.

Below is the program that I’m about to try…

N4
(5/8-11 UNC TAP)
M00(BLOW OUT SHIPS)
G40
T0505G0
G97S175M03
G00X0Z1.
G84 Z-1. R.2 P1000 F0.0909
G0Z1.
G80
G28U0W0M09
M01

I could not find any info about M29, what is the exact explanation of M29?

Should I use M29 as you described with the same speed as the beginning of program or with different speed?

Thank you

ps. material 4140 bar

[dcoupar]

On the machines I work with, M29 is Rigid Tapping mode. If the program you posted works on your TW20, it should probably work on the TW10.

I believe R can be an absolute or incremental value based on a parameter setting. I'm used to R being incremental, so in your example I would program an R-0.8, but again your machine may be set up for absolute R.

I probably would include a G99 at some point befor the G84 to be sure IPR was active.

Good luck.

[PRINT_FX]

yes M29 works at least the machine does not give me an alarm...
and the R value is -.8, you were right, also G99...

tapping 1.75in deep in one shot is too much for the tap but it did not break yet, LOL

do you think is possible to retap it using the same section of the program?
going 1.250 during the first pass and 1.9 deep for the second pass?

example:
G84 Z-1.250 R-.8 F0.0909
G0 Z1.
G84 Z-1.9 R-.8 F0.0909
G0 Z1.

maybe a forming tap would do the job...

[dcoupar]

I've never tried going back into a hole while rigid tapping on a lathe, but I don't know why it wouldn't work.

[PRINT_FX]

dcoupar,
you were and are a great help, thank you

tomorrow I'll see how many parts can I make with one tap.

have a good day

[sinha_nsit]

If rigid tapping is enabled on your machine (possibly yes, because you are not using floating tap holder, still you are not breaking taps), you can also do peck rigid tapping. Just insert a Q-word, with peck-length (in mm or inch) as a decimal value. You also have the option of using G73- or G83-type pecks, through a parameter (5200#5 on 0i; 0 for G73 type, 1 for G83 type).

[dcoupar]

Originally Posted by sinha_nsit If rigid tapping is enabled on your machine (possibly yes, because you are not using floating tap holder, still you are not breaking taps), you can also do peck rigid tapping. Just insert a Q-word, with peck-length (in mm or inch) as a decimal value. You also have the option of using G73- or G83-type pecks, through a parameter (5200#5 on 0i; 0 for G73 type, 1 for G83 type).

Have you tried this yourself, sinha_nsit? According to the Parameter Manual for both the 16 and the 0, 5200 bit 5 is valid only on M controls, not T. And I see nothing in the Lathe Operator's Manual regarding peck tapping... it is explained in the Mill Operator's Manual, however.

[sinha_nsit]

Originally Posted by dcoupar Have you tried this yourself, sinha_nsit? According to the Parameter Manual for both the 16 and the 0, 5200 bit 5 is valid only on M controls, not T. And I see nothing in the Lathe Operator's Manual regarding peck tapping... it is explained in the Mill Operator's Manual, however.

No, I have not tried. I just referred to the manual.

On T-series, 5104#6 (PCT) is set to 1 for peck tapping cycle (with Q-word).
With this setting, according to parameter manual, 5200#5 (PCP) can now be used for selection between fast/regular pecking.
G84/G88 is to be used on T-series.

[dcoupar]

Originally Posted by sinha_nsit No, I have not tried. I just referred to the manual. On T-series, 5104#6 (PCT) is set to 1 for peck tapping cycle (with Q-word). With this setting, according to parameter manual, 5200#5 (PCP) can now be used for selection between fast/regular pecking. G84/G88 is to be used on T-series.

As far as I can tell, this is not available on the 16TT controls. There is no listing for parameter 5104, and the PCT determines the T-code displayed. It does appear in the 16i model B parameter manual, but PRINT_FX stated he has a 16-TT, NOT a 16i.

[sinha_nsit]

Maybe.
I was referring to 0i series.