[cjchands]

I am in a shop with several CNC Mills and Lathes.
We sold FANUC 6M Drill mate Pratt& whitney and Hundai Fanuc 21T CNC lathe.
People always ask: does it do RIGID tapping??

I searched in the internet and found the definition as:

A rigid tapping cycle synchronizes the machine spindle rotation and feed to match a specific thread pitch!!

My question is: DOESN'T MOST FANUC controller, Haas, Okuma, or major brand HAS "RIGID TAPPING" as standardize?

The only reason that it wouldn't come with Rigid tapping is if you have INVERTER and regular induction motor....ANy COMMENT??????
Thank you.

[toastydeath]

Older machines, and some less expensive/midpriced VMCs do not have rigid tapping. So, no, it isn't standard, and is usually a 1500-2000 dollar option on a lot of machines shops buy in quantity.

Rigid tapping is popular in the industry because there are certain high speed/high performance form taps that will not start in a floating tap holder. You must have a machine that does rigid tapping to use them.

Additionally, higher practical tapping speeds are possible on a rigid tapping cycle. On floating taps, the spindle and Z axes deceleration aren't completely synced, so at higher speeds, the floating tapholder sometimes winds out completely and breaks the tap off. With rigid tapping, the deceleration of the spindle and the Z axis are in sync all the way from full speed to dead stop, keeping the tap from breaking no matter how fast you try to tap.

[aussie28]

I am not a fan of taping on the machine but Rigid taping allow u hold the tap in u er collet same as u end mill. no floating holder require. my understand Rigid taping is u machine motor capable of spining CW and CCW with out any back flashe and synchronized with feed in Z match u input of pitch. Most importance thing is u tap still in one piece after taping cycle.

[Al_The_Man]

My question is: DOESN'T MOST FANUC controller, Haas, Okuma, or major brand HAS "RIGID TAPPING" as standardize?.

Not neccesarilly, with Fanuc and some others, the option is in the control but not turned on unless paid for, also the spindle motor has to have feed back encoder on the spindle.

The only reason that it wouldn't come with Rigid tapping is if you have INVERTER and regular induction motor....ANy COMMENT??????

With the right inverter/VFD, a regular induction motor can be made suitable for rigid tapping, if a pulse generator is fitted to the motor and an encoder on the spindle shaft.
The method used is called electronic gearing, where the Z axis is electronically geared off the spindle encoder.
This is also required for helical milling.
The similar functions performed on a Lathe would be threading and CSF.
Al.

[Geof]

......The method used is called electronic gearing, where the Z axis is electronically geared off the spindle encoder.
This is also required for helical milling.....Al.

Phrased as meekly as possible ...no not needed for helical milling.

Helical milling involves the X, Y and Z axes moving in synchrony but the spindle rpm is not related to any axis movement.

[Al_The_Man]

Geof, My understanding of helical milling is similar to rigid tapping or lathe threading where the Z axis for e.g. would spiral down a bored hole to create a 'Helix'? If so this would require sync to the spindle, no?
I will have to dig out my manual for the canned shape description.
Al.

[Geof]

Geof, My understanding of helical milling is similar to rigid tapping or lathe threading where the Z axis for e.g. would spiral down a bored hole to create a 'Helix'? If so this would require sync to the spindle, no?
I will have to dig out my manual for the canned shape description.
Al.

The Z axis does spiral down, or up, a hole but it is only axis motion involved.

You program a G02/G03 with a Z increment:

G91 G03 I0. J-.5 Z.125 F(something) L10

Will produce an upward moving helix of ten revolutions, actually 1"-8 NC thread with the correct tool. Your spindle rpm is not related to the axis motion.

[Al_The_Man]

I Think I was Probabaly confusing the G33 (constant lead) which I have seen a helix cut with a boring tool.
Al.

[Eurisko]

Geof,

I'm sure you're right, but I still have a hard time wrapping my head around that one. So in thread milling, you could actually press the feed hold button or override the spindle rpms without damaging the thread form?

[cjchands]

So if you were to buy a used CNC VMC or LATHE machine, how would you know or to look for if the machine does or doesn't have RIGID TAPPING function? Check for the encoder on the spindle?

[Caprirs]

Geof,

I'm sure you're right, but I still have a hard time wrapping my head around that one. So in thread milling, you could actually press the feed hold button or override the spindle rpms without damaging the thread form?

Yes, that is correct.

Rigid tapping requires an encoder on the spindle (or motor). This allows precise position control of the spindle motor similar to the X, Y, & Z axes. When the rigid tap cycle is commanded, the control changes how it controls the speed of the spindle motor. On such machines, the spindle can be treated like a rotary 4th axis and given specific position commands using G01.

During normal milling/drilling, the spindle is run with the strategy of maintaining rpm while sacrificing "rotation position". During rigid tapping, the strategy is to sacrifice rpm for position accuracy. So, the actual command inside the control typically looks like:

G01 Vv Zz Ff

Thus, the control treats the spindle and Z axis the same way it treats the X & Y axes.

During thread milling, the motion is just a helix with the spindle running at constant speed. The thread precision is controlled by the diameter of the helix (pitch diameter) and the slope of the helix (thread pitch).

[Caprirs]

So if you were to buy a used CNC VMC or LATHE machine, how would you know or to look for if the machine does or doesn't have RIGID TAPPING function? Check for the encoder on the spindle?

The encoder indicates the ability to do rigid tapping. However, as mentioned above some older machines have the rigid tapping function as an option that must be enabled by parameter. Most machines have it enabled. The control manufacturer can probably look up the serial number and tell you if the option should be functioning.

If the machine is under power, the easy check is to try the command.

[Geof]

I Think I was Probabaly confusing the G33 (constant lead) which I have seen a helix cut with a boring tool.
Al.

That must be a tedious process. Bore one cut, stop spindle, move X or Y, back up to top, advance tool in boring head manually, take second cut, etc, etc, forever. Or am I looking at it wrong?

Eurisko; Yes. You can Single Block through the entire sequence and use the over-rides. You can also choose to start the thread exactly where you want it to start and do Higbee cuts at either end.

cjchands; It has to be an encoder with what I think is called the Z channel signal. This is the one that gives the absolute position of the spindle once every revolution as well as the encoder count giving the precise rpm.

When tapping with a floating head it is okay if the control only knows how fast the spindle is running so it can control the Z feed to match. It does not matter if things get a bit out of synch during decceleration and acceleration at the bottom of the hole because the floating head absorbs this. Also a small accumulative error can be absorbed by the floating head.

With rigid tapping perfect synch has to be maintained at all times and even very small errors per revolution must not accumulate. The Z pulse gives a confirmation every spindle revolution that things are in synch.

When rigid tapping is possible repeat rigid tapping is also possible if the machines stores the starting condition, i.e. the precise Z position for a precise spindle position. Then you can go into the same thread several times.

[Al_The_Man]

That must be a tedious process. Bore one cut, stop spindle, move X or Y, back up to top, advance tool in boring head manually, take second cut, etc, etc, forever. Or am I looking at it wrong?

An example application where locomotive car wheels are press fit on to the axle.
The boring mill must bore a spiral groove in one shot through the wheel bore.
The tool on the boring bar has a convex shape that results in a concave groove.
Also some boring bars of this type have indexable tools by a servo mechanism through the bar. That can take advantage of the constant lead G33 and pick up the start point again, if required.

The spindle in a lathe or mill with syncronized feed is kept at the commanded speed by a pulse generator (tach) on the motor (an encoder can be used) , the Z axis is then synched to the 1/turn marker pulse on the Spindle Shaft encoder, the Z Servo is then geared to the spindle encoder/ not vice-versa.
The spindle is not used in a servo fashion, sync is done by the Z axis that monitors the actual spindle speed.
Al.

[Geof]

An example application where locomotive car wheels are press fit on to the axle.

The boring mill must bore a spiral groove in one shot through the wheel bore.
The tool on the boring bar has a convex shape that results in a concave groove......Al.

What is the function of the spiral groove? I could understand it for an oil groove but I doubt whether the wheel is intended to spin on the axle .

Lubrication during a multi-hundred ton press fit to prevent galling?

[M30]

Wouldn't they just do a shrink fit instead of a press fit for something like that?

[Al_The_Man]

Lubrication during a multi-hundred ton press fit to prevent galling?

Yep, they are lubed with linseed oil, the tonnage must conform to a certain range, for acceptance.
To achieve this each axle seat is measured and the wheel bored to suit.
Al.

[tobyaxis]

In Short Rigid Tapping is mainly used for Blind Hole Tapping.

To add to the Helical Interpolation Off Thread Topic LOL I have always had a hard time rapping my brain around this one.

It was questioned earlier in this thread, "What If you were to hit the Feed Hold during Helical Thread Milling???" I assume that the Thread would be damaged a little, but not too much. I have never done any Thread Milling and have to ask, "What would really Happen if you did hit the Feed Hold during Helical Interpolation ". Has anyone here done this before??? If so, what were the results?

[Geof]

...It was questioned earlier in this thread, "What If you were to hit the Feed Hold during Helical Thread Milling???" I assume that the Thread would be damaged a little, but not too much. I have never done any Thread Milling and have to ask, "What would really Happen if you did hit the Feed Hold during Helical Interpolation ". Has anyone here done this before??? If so, what were the results?

The same thing that happens whenever you hit Feedhold; the cutter relaxes back to an un-deflected state so it leaves a little witness make on the part.

If you were running a 3 axis contoured surface with simultaneous motion in X, Y and Z you would not worry about hitting Feedhold. Helical interpolation whether it is cutting a thread or simply interpolating a hole is merely a 3 axis contoured surface wrapped around inside a hole.

Google 'topology' and do a bit of reading.

[sinha_nsit]

The Z axis does spiral down, or up, a hole but it is only axis motion involved.

What type of tool is used for thread milling in this fashion. It should be able to cut in the radial direction as well as in the axial direction, otherwise Z movement is not possible. Am I correct?

Second question:
Is it true that rework on a tapped hole is not possible if we are using floating tap holder. With rigid tapping, rework is possible provided the workpiece can be kept exactly in the same original position, and Z position of the tap is also exactly same when tapping is started.

It is a good forum for learning interesting things.