What's new
What's new

Doosan lathe will it G84 Rigid tap?

yardbird

Titanium
Joined
Jul 3, 2013
Location
Indiana
I’m trying to see if this thing will Rigid tap. My day shift buddy hasn't ever done it but swears to me it will but his word is all I have, I’m not so sure. I think I had a dream where I went through this before and broke the very first tap and called it quits and gave up went back to the spring holder. All of this shit runs and without the risk of breaking more shit it looks to me like all of these have spindle drift at the end with no slide movement. The book I have calls the G84 a tapping cycle and no mention of M29. I see that in the G code list on the control they have a G84.2 listed as Rigid tap but when I try to run it the spindle comes on then pukes a PS0010 IMPROPER G-CODE. G32 is synchronized feed, isn’t that what rigid is? Is the only benefit to G32 tapping is that it disables the feed/spindle overrides? How can I tell for positive if this thing has Rigid tap or not?

Fanuc 0i-TC or D? Thanks....

Brent

:1111(RIGID TAP 1/2" - 13)
G0G99G40G54X14.Z10.T0
T0606
M41
G0X.0Z.15
G97S350M29M3
G84Z-1.55F.076923
G80G0Z.5
G0G40G54X14.Z10.T0
M30

:2222(TAP CYCLE 1/2"-13)
G0G99G40G54X14.Z10.T0
T0606
M41
G97S350M3
G0X.0Z.15
G84Z-1.55F.076923
G80G0Z.5
M9
G0G40G54X14.Z10.T0
M30

:3333(G32 TAP 1/2" - 13)
G0G99G40G54X14.Z10.T0
T0606
M41
G97S350M3
G0X0Z.5M8
G32Z-1.55F.076923
Z.5M4
M9
G0G40X14.Z10.T0
M30

20201018_045945.jpg
20201018_050210.jpg
 
IME on a Fanuc G84.2 and M29>G84 are the same thing and can be used interchangeably.

Did you try M29 and see what happens?

If it turns out it doesn't have rigid tapping (not impossible, my Doosan doesn't, uses E axis interpolation to rigid tap with the live tools), but it does have C axis control, then you can rigid tap at centreline with Z/C interpolation.
 
Hello Brent,
Its been my experience that on a lathe that doesn't have a "C" axis, if its Rigid Tapping ready, the spindle will respond to M19 to orientate the spindle. I've not seen it documented, just my observation.

Because of the mass of the spindle and chuck and hence the inertia involve, there is a relatively low max spindle speed for rigid tapping; 1000 rpm on all lathes I've seen with RT.

Regards,

Bill
 
Yes your lathe will rigid tap!

DO NOT put an M3/M4 on the rigid tap line. Rigid tapping MUST be done from a dead stopped spindle. This applies to main, live, and sub spindles.

So - tap like this

For the Main Spindle -

M5 P11(MAIN SPINDLE STOP);
G0 G54 G99 T0505(TAP)
X0 Z.25 M8(POSITION)
G97 S250 M29(RIGID TAP)
G84 Z-.75 F.05(TAP CYCLE)
G80 M9(CANCEL CYCLE)
G0 Z1.(CLEAR Z)
G28 U0(HOME X)
G28 W0(HOME Z)

ETC

Always tap in IPR mode. Thread lead is 1/#of thds per inch.
 
DO NOT put an M3/M4 on the rigid tap line. Rigid tapping MUST be done from a dead stopped spindle. This applies to main, live, and sub spindles

Douglas, do you know if this is a Doosan thing or does it apply to Fanuc machines universally?

If the latter it would explain some problems I've had trying to do this on some of our other machines (Our Doosan definitely doesn't have rigid tapping enabled, but that's another story). For whatever reason tapping on centre with the main spindle is something that I very rarely need to do so I always have worked around it.

Just a couple of weeks ago I rigid tapped a hole on our NTX using Z/C interpolation because the tap was too big to turn with the tool spindle and I couldn't get main spindle rigid tapping to work according to the instructions in the manual, which did not state that I had to start from a stopped spindle...
 
Douglas, do you know if this is a Doosan thing or does it apply to Fanuc machines universally?

If the latter it would explain some problems I've had trying to do this on some of our other machines (Our Doosan definitely doesn't have rigid tapping enabled, but that's another story). For whatever reason tapping on centre with the main spindle is something that I very rarely need to do so I always have worked around it.

Just a couple of weeks ago I rigid tapped a hole on our NTX using Z/C interpolation because the tap was too big to turn with the tool spindle and I couldn't get main spindle rigid tapping to work according to the instructions in the manual, which did not state that I had to start from a stopped spindle...

If your Doosan isn't rigid tapping there's some sort of other issue there. It should! I should know, I worked for them for years as their applications and training guy.

I believe it is a "Fanuc thing" as every time I needed to rigid tap - mill or lathe - it had to be done from a dead stopped spindle. In my pre-Doosan days I had a Takisawa V1 machining center with rigid tap and it had to be from a stopped spindle. In my post-Doosan days I've been on a myriad of CNCs and all of them had that in common.
 
If your Doosan isn't rigid tapping there's some sort of other issue there. It should! I should know, I worked for them for years as their applications and training guy.

I believe it is a "Fanuc thing" as every time I needed to rigid tap - mill or lathe - it had to be done from a dead stopped spindle. In my pre-Doosan days I had a Takisawa V1 machining center with rigid tap and it had to be from a stopped spindle. In my post-Doosan days I've been on a myriad of CNCs and all of them had that in common.

Thanks, like I said I've not run up against this often as tapping on centreline in a lathe is just not something I've needed to do often.

Regarding our Doosan, it's a bit of a black sheep - a 2006 inbetweener machine from right at the end of the Doosan Mecatec era. The live tools are an axis unto themselves so rigid tapping using them is done by interpolation and macros. The option for rigid tapping is not enabled because it's generally unnecessary - except of course for centreline tapping on the main spindle...
 
Thanks, like I said I've not run up against this often as tapping on centreline in a lathe is just not something I've needed to do often.

Regarding our Doosan, it's a bit of a black sheep - a 2006 inbetweener machine from right at the end of the Doosan Mecatec era. The live tools are an axis unto themselves so rigid tapping using them is done by interpolation and macros. The option for rigid tapping is not enabled because it's generally unnecessary - except of course for centreline tapping on the main spindle...

Understood. We had a file for those back in the office, not sure what's happened since then.
 
Douglas, do you know if this is a Doosan thing or does it apply to Fanuc machines universally?

Hello Gregor,
On the advice of my Fanuc colleagues, the spindle should be started for Rigid Tapping from a stopped condition and its universal relating to Fanuc Controls. It doesn't actually state that in any Fanuc manual, however, notwithstanding that Rigid tapping can be specified with G84 (rather than with an M code) via parameter setting, all examples of Rigid tapping in Fanuc manuals show a uniform syntax of M29 S_ _ _ _, with no M code (M03/M04) to start the spindle.

I took the matter up with a factory employed Fanuc Engineer quite some years ago, when I client was having trouble rigid tapping with a new Fadal VMC. He was quite emphatic that the spindle had to be started from stopped by the Tapping Cycle, by either specifying Rigid Tapping with an M code, or by G84 via parameter setting.

However, from the writing of a PMC program point of view, it would not be difficult for the spindle to be stopped and started again again when the Rigid Tapping M code is encountered.

Regards,

Bill
 
Bill

When I was at Doosan it was emphatic that rigid tapping (M29) ALWAYS be from a dead stopped spindle. So, I think much has to do with how the MTB writes the ladder and sets the control upon installation to the machine.
 
Bill

When I was at Doosan it was emphatic that rigid tapping (M29) ALWAYS be from a dead stopped spindle. So, I think much has to do with how the MTB writes the ladder and sets the control upon installation to the machine.

Hello Douglas,
You're preaching to the choir. That's the advice I had from Fanuc many years ago and confirmed recently. We didn't touch on control via the PMC during our discussion, but I can see no reason why the spindle couldn't be stopped by the PMC program and then allow the Tapping Cycle to restart it as a requirement of the Fanuc control.

I find it rather interesting that in Dry Run mode, the spindle still keeps pace with the axis move; slow or increase the feed rate and the spindle slows and speeds up according.

Regards,

Bill
 
....but I can see no reason why the spindle couldn't be stopped by the PMC program and then allow the Tapping Cycle to restart it as a requirement of the Fanuc control.

Absolutely the case. The CNC sends notice to the PMC by address F76.3 that rigid tapping is commanded. The builder's PMC ladder program at that time could stop spindle rotation in preparation of sync'ing Z and the spindle.
 
Not a lathe, but a Yasnac mill I ran years ago required an M29 Sxxx and IPR feed for tapping. Don't remember if it alarmed out or not with an additional Sxxx line or not...

Not sure if Yasnac, or just a parameter, but when I started with that same machine also used Hx for length offset, and Hxxx for D offset... but I changed it to H and D like "normal" :D
 
First off thank you to EVERYONE. As suggested I dropped the M3 and it run as should, I think? Appears there is a need to drill a half mile deeper or stay short on your Z tap depth?

Look at the CRT screen, watch the spindle speed after it reaches the Z depth. If you only had one shot how do you calculate the slide drift after the Z depth?

Even though this is probably fairly elementary to most of you. No matter how long I do this stuff I still get a little chubby when I learn how to make it do something new.

Thanks Again Folks!

Brent

Doosan Fanuc 0i-TD G84 Rigid Tapping Cycle 1 - YouTube

Doosan Fanuc 0i-TD G84 Rigid Tapping Cycle 2 - YouTube
 
I find it rather interesting that in Dry Run mode, the spindle still keeps pace with the axis move; slow or increase the feed rate and the spindle slows and speeds up according.

Regards,

Bill

Hello Bill,

Weather it be here nor there I'm disputing what you say and that is interesting. I'm not able to make this happen on this particular machine. Either in dry run or automatic mode.

In automatic when the feed rate is at zero the alarm light come on and the message is "feed rate at 0%" but it keeps right on keeping on.

That could be a desired feature in some cases.

Brent
 
Do these typically have a little slop to them? I can twist the tap a little bit. Seems like a no no for this kinda operation?

Brent

20201019_032811.jpg
20201019_032823.jpg
 








 
Back
Top