[sluggo]

I have a 15M control and the manual talks about using G84.2 and G84.3 to rigid tap. I know that my machine needs a spindle encoder to do this, how do I tell if my machine is equipped with one? I tried just calling up a G84.2 using the example in the manual but I got a "Invalid G code" alarm, does this mean it can't do it, or that maybe the subroutine is missing?

[sluggo]

Thanks I'll check it. The other thing I'm thinking but have not had a chance to check is that maybe the normal G84 might sync the spindle with the feed every time. Is that possible?

[cncwhiz]

With any Fanuc that I have ever worked with, G84 will not do rigid tap. On "some" of the 0M controls, they used an M29 before the "G84" to make rigid tap. I have never seen a 15M control that works that way. I have 3 15 controls in my shop and the all use "G84.2". You can still use "floating" tapping. It will not run as fast and you will need to mess with the depth.

[cnc-king]

you must bear in mind that rigid tapping is an option on most machine with fanuc controls. the 18Im will rigid tap with a G84 with no preparatory statements. the kitamuras and makinos work this way
on all the 15M that i have worked on G84.2 is preceded by G95 for rigid tapping
G98
G95
G84.2 X**** Y***** Z*** R****F**
STUFF

G80
G94

F = PITCH

[codyst]

G95 is setting it up for feed per revolution. I've never tapped on a 15M, but if the parameter sets are comparable to a 16M there is a parameter specifying whether or not a rigid tap M code is needed, or whether the G84 initializes rigid tapping.

[cncwhiz]

I have never seen a 15M use an M code for tapping. I have some different vintage 15 controllers and they all use "G84.2" if they have rigid tap. OM uses an "M29" before the tap cycle "G84" for rigid tap.

[sluggo]

I checked the parm. that cncwhiz suggested, and it was not on. I'm not sure why that post was removed? Can I just enable PWE and then turn it on? I tried with g95 in front, that didn't do it, I got that Idea from some where resiliently and I think I will program all my tapping that way from now on. What can I do to be sure my spindle has an encoder? I am running a mid to early 90's Toyoda FH-60.

[Leblondmakino]

Its just a case of checking the name badge on your spindle motor then getting in touch with Fanuc so they can give you the motor spec and tell you which type of spindle encoder is mounted.

Some machines have the encoder or resolver running off a belt from the spindle shaft but this is mostly seen on lathes and is rarley seen on machining centres.

My Bridgeport horizontal only uses the encoder for positioning the spindle for a tool change with M19 and the encoder runs off a belt from the spindle shaft.
It will not do rigid tap.
John.

[cnc-king]

G95 is setting it up for feed per revolution. I've never tapped on a 15M, but if the parameter sets are comparable to a 16M there is a parameter specifying whether or not a rigid tap M code is needed, or whether the G84 initializes rigid tapping.

i indicated that the F is the pitch of the thread being cut

[cncwhiz]

Codyst,
A 16M is way a much newer than a 15M. If the machine is setup to even do rigid tap then you have to program it. There is no parameter to specify an "M" code. As far as the "G95", "G94", this is a standard for all feed parameters in "most" fanuc controls. G95 allows for more variations then G94. For the most older controls "G84.2" is for rigid tap and "G84" is for floating tap. When they went to "0M", they added an "M" code for rigid tap. You need to add a "M29" in a line before the tap cycle. This machine uses a "G84" for both tapping cycle types.

[codyst]

And if you would've read my post you would see that I indicated that I have not tapped on a 15M, and that I wasn't sure if the parameter sets were close to a 16M as I've never had any reason to dive into the parameters on a 15.

On newer controls there is indeed a parameter that specifies whether an M code is issued before rigid tap is initialized, or if G84 causes it to rigid tap. If this parameter is set, you can not use a floating tap holder.

As for the G95 comment: by the context of cnc-king's post it appeared as though he was saying that G95 was needed to initialize rigid tapping ".....on all the 15M that i have worked on G84.2 is preceded by G95 for rigid tapping....."

I was just pointing out that G95 was Feed/Rev and not necessarily needed to rigid tap.

[Greaseball]

The operator of our Kitamura H500 15m control is telling me that he cannot rigid tap below 400 rpm. Can anyone tell me if this could be true or is he blowing smoke?

[angelw]

The operator of our Kitamura H500 15m control is telling me that he cannot rigid tap below 400 rpm. Can anyone tell me if this could be true or is he blowing smoke?

The only issue that could occur with using slow spindle speeds is if the spindle was direct drive, ie, no gear ranges involved for high and low spindle speeds, and if taping a large diameter thread in tough material. The reason being that the spindle speed may vary through lack of torque at a low spindle speed. Other than that, its smoke.

Regards,

Bill

[stevo1]

The operator of our Kitamura H500 15m control is telling me that he cannot rigid tap below 400 rpm. Can anyone tell me if this could be true or is he blowing smoke?

Other then what Bill has stated the only issue that I have had is if we set our feed on one of our 15series at 1 IPM it has issues but this is a very slow feedrate which is not near 400rpm no matter what pitch.

IMO it is definitely smoke.

Stevo

[angelw]

Thanks I'll check it. The other thing I'm thinking but have not had a chance to check is that maybe the normal G84 might sync the spindle with the feed every time. Is that possible?

The other thing I'm thinking but have not had a chance to check is that maybe the normal G84 might sync the spindle with the feed every time.

I don't understand what you mean by the above. Post the code thats being used to invoke Rigid Tapping.

Regards,

Bill

[sinha_nsit]

On 0i M, if 5200#0 is set to 1, G74/G84 do rigid tapping, provided the machine is capable of rigid tapping. No M29 would be needed. This parameter selects between standard mode and rigid mode for G74/G84.