[Gundawg]

Can someone tell me how this works and how you generate the toolpath for it? Does the spindle actually reverse direction or stop and the spring loaded head unwinds I have never used one or seen it used.

Thanks Mike

[txcncman]

There are two types. There is the compression/tension tap holder (mill or lathe). Then there is a tapping head (mill only). With the tap holder, it allows the tap some wiggle room to align with the hole and to allow for variations in the feed rate to spindle RPM ratio. This type would be programmed for the spindle to reverse direction and the infeed feed rate to be slightly less than the tap pitch and withdraw at the same rate as the pitch (works best). With a tapping head, the spindle runs constantly the same direction (normally clockwise). As the spindle feeds toward the work, the gears in the tapping head cause the tap to rotate in the same direction. As long as infeed is maintained, the tap continues to rotate in the same direction. When infeed stops and then reverses for withdrawing the tap, the tap rotation reverses. This would be programmed with the tap pitch as the feed rate for infeed and withdrawal.

[SCzEngrgGroup]

There are two types. There is the compression/tension tap holder (mill or lathe). Then there is a tapping head (mill only). With the tap holder, it allows the tap some wiggle room to align with the hole and to allow for variations in the feed rate to spindle RPM ratio. This type would be programmed for the spindle to reverse direction and the infeed feed rate to be slightly less than the tap pitch and withdraw at the same rate as the pitch (works best). With a tapping head, the spindle runs constantly the same direction (normally clockwise). As the spindle feeds toward the work, the gears in the tapping head cause the tap to rotate in the same direction. As long as infeed is maintained, the tap continues to rotate in the same direction. When infeed stops and then reverses for withdrawing the tap, the tap rotation reverses. This would be programmed with the tap pitch as the feed rate for infeed and withdrawal.

I assume the tapping heads also include essentially a tension/compression feature, in case the mills feed is not a perfect match to the screws pitch?

Regards,
Ray L.

[txcncman]

I assume the tapping heads also include essentially a tension/compression feature, in case the mills feed is not a perfect match to the screws pitch?

Regards,
Ray L.

This is the idea, yes. "...to allow for variations in the feed rate to spindle RPM ratio."

[txcncman]

"Newer" machines with C axis encoders can actually use rigid tapping (usually M29). In this operation, the machine will match the C axis position with the tap position during acceleration/deceleration of the spindle, so a compression/tension tap holder or a tapping head is not really needed (or even usually wanted).

[Geof]

I assume the tapping heads also include essentially a tension/compression feature, in case the mills feed is not a perfect match to the screws pitch?

Regards,
Ray L.

Yes. This is inherent in the design. A tapping head has a reversing gear train inside and provided the feed is forward the forward gear train is engaged and the tap rotates at the same speed as the spindle. When the feed is reversed the reverse gear train is engaged as the tap runs ahead of the feed and the tap is reversed out of the hole.

A tapping head has a radius arm that has to bear against a fixed point and be able to slide down and up as the spindle moves. This arm is needed so the direction reversal can occur in the internal gear box.

A tapping head can also be used in a drill press just using hand feed.

[Gundawg]

I understand the concept I think, so the tapping head Tormach sells with their mills as an option does not require the spindle to change directions correct? The feed and speed would be a formula of the thread pitch correct? Is there a wizard that calculates this by entering the parameters tap size & depth to give the proper spindle speed?

I ask these questions because I own a 3D cad/cam program now that is designed more towards cabinet & sign makers IMO Aspire by Vetric one of the things I want to be able to do is tap holes so I am wondering how this toolpath gets generated? I do not want to have to buy Alibre or Sprutcam if I do not need too. I am used to using this other Cad system and it has a cam feature built in. I am trying to figure out what I need before ordering a machine. The cad program has a drilling toolpath that allows for peck drilling and you can enter your feed and speed but you would have to know those numbers, and I am not sure how to figure that out.

Thanks Mike

[txcncman]

I understand the concept I think, so the tapping head Tormach sells with their mills as an option does not require the spindle to change directions correct?

Tormach seems to have both available. Tormach Tooling System - Tapping Heads and Collets | Tormach LLC | We provide personal small CNC machines, CNC tooling, and many more CNC items

The feed and speed would be a formula of the thread pitch correct?

Speed is determined by both a chart and a formula. The chart would reveal a "Cutting Speed" in "Surface Feet per Minute". That number would be placed in a formula along with the diameter of the tool. This would give the RPM "recommended" for this specific situation. The feed would be determined by the pitch of the tap (1 divided by the number of threads per inch). For lathes, feed rate is usually expressed in inches per revolution. For every 1 revolution of the spindle the tool would advance the inches expressed in the feed rate. For a 1/4-20 tap, the pitch is 1 inch divided by 20 threads per inch which is 0.050 inches per thread, or 0.050 inches for each time the spindle rotates. This is a feed rate that would usually be expressed in G-code as F0.05.

Is there a wizard that calculates this by entering the parameters tap size & depth to give the proper spindle speed?

There are formulas, wizards, calculators, and programs that will do most of the calculations for you if you know what information to input.

I ask these questions because I own a 3D cad/cam program now that is designed more towards cabinet & sign makers IMO Aspire by Vetric one of the things I want to be able to do is tap holes so I am wondering how this toolpath gets generated?

Well, the "best" thing to do is to go to school and learn. But I am sure you are not going to do that. So, you have to figure out a way to take short cuts. Have you read the Machinery Handbook? Do you even have a copy? Which books do you have for machining and CNC? Have you read them? Have you searched for online videos that demonstrate these different techniques and watched them? Does your software support tapping operations? Have you asked the software maker?

A new Tapmatic tapping head will run you in the $500 to $900 range.

A new tension compression tap holder will run from $50 to over $200.

Which one has Tormach advised to use with the machine you intend to order?

How the toolpath is generated is specific to the machine. You have not specified a machine. You hinted that it would be a mill. On a mill for a 1/4-20 tap, it might be as simple as:

T01 M6
M3 S500
G0 G54 X0. Y0.
G0 Z0.3
G1 Z-0.75 F24.99
M5
M4 S500
G1 Z0.3 F25.

Or, the mill might have an option to use a G84 tapping cycle.

[MichaelHenry]

I assume the tapping heads also include essentially a tension/compression feature, in case the mills feed is not a perfect match to the screws pitch?

Regards,
Ray L.

If Tormach's tapping head is like the Procunier design, there is a clutch inside the head that allows the tap to "slip" if the spindle down speed is too slow for the tap. At least that's how I understand it. You stop down speed alltogether with the spindle rotating and the tap will not rotate at all. On Z reverse the gear train inside the head spins the tap at 2x spindle speed (or thereabouts). That system works a treat and I've used it to thread a bunch of 0-80 and 4-40 through holes in aluminum without one failure.

I've got a Procunier 1E, which goes up to 5/16" or so, but have not yet modified it for my Tormach. When it gets done, I'll probably copy the approach that Don here developed for his. In the mean time, I'm waiting for delivery of one of Tormach's compression/tension heads and will try that out.

Mike

[Don Clement]

The Tormach does not have a servo controlled spindle and therefore the spindle cannot quickly stop and or reverse. This means that for blind holes tapping with a tension-compression type head will have to be done at slower speeds to allow for the spindle to stop and reverse. The advantage of a reversing type tapping head with the Tormach is that tapping blind holes can be done at high speed. My Procunier tapping head has a cushioned double-cone clutch that allows the tap to disengage within 1/3 revolution. That is perfect for tapping blind holes at high speed. With the Procunier I feed at 100%, no dwell, and retract at twice the downfeed. So with my 3 digit Tormach I am only limited by the maximum feed rate for retraction which is 65 IPM.

Don

[Gundawg]

After reading all of this and watching YouTube videos on tapping heads I have a question would it not be easiest to just buy an auto reversing tapping head and just run a simple drilling toolpath and set the speed and feed and depth to a value that would allow the head to work properly? I am not understanding the advantage of these other head types? I am reading some of these automatic heads have adjustment for depth for blind holes. I saw several YouTube videos of auto reversing heads in use and it seems fairly straight forward. I also would not need new software maybe I am missing something. The project I need a tapping head for is not a blind hole it is for four 1/4-20 holes in 1" 6061 T-6 Al.

Mike

Here is an example [ame="http://www.youtube.com/watch?v=dgd6x2oF9Xk"]Tapping Head - taps 40 holes in two minutes. - YouTube[/ame]

[MichaelHenry]

So with my 3 digit Tormach I am only limited by the maximum feed rate for retraction which is 65 IPM.

Don

Have you considered upgrading to the new Series III drives and steppers when the upgrade kit is available? Seems like a good idea for me and you probably use your mill far more than I use mine, so the payoff should be better.

Mike

[Scott_M]

I have been using this supplier for over a year now. They make absolutely top notch stuff at a fraction of the cost of anyone else. I even special ordered 4-48 threadmills from them. Really good stuff. I would put their endmills up against OSG and Niagara any day.

Online Carbide

Scott

[SCzEngrgGroup]

I have been using this supplier for over a year now. They make absolutely top notch stuff at a fraction of the cost of anyone else. I even special ordered 4-48 threadmills from them. Really good stuff. I would put their endmills up against OSG and Niagara any day.

Online Carbide

Scott

OK, now we're talkin'! Those are pretty reasonable.

Am I correct in understanding the correct usage is:

1) Plunge into the center of the hole
2) Move out to the side
3) Helical cut upwards one thread
4) Back to center and retract

Regards,
Ray L.

[txcncman]

One thing we did not mention, with a thread mill, you can cut OD threads also. 2 tools in 1. Try to do that with a tap.

[Don Clement]

One thing we did not mention, with a thread mill, you can cut OD threads also. 2 tools in 1. Try to do that with a tap.

BUMP I show videos of both internal and external thread milling on my Tormach. I just change the insert from internal to external.

Don

[SCzEngrgGroup]

That Vardex insert tool is very cool, but I rarely do anything bigger than 3/8", and most is smaller, so I guess I'm stuck with solid cutters. I'll have to get some and give it a try.

Thanks for all the info, guys! I have REALLY hated to have to do all my tapping by hand, and a tapping head won't really help once I get a tool-changer going. I think this should be the solution I've been looking for.

Regards,
Ray L.

[David Bord]

There are these types of threadmills as well that I believe you can cut different size thread/diam with a single tool.

If this is the case, anyone have any info or good sources for them?

Scott, does online carbide make these?

[ame=http://www.youtube.com/watch?v=pQ83XRgRCyg&feature=related]Thread milling - YouTube[/ame]

Another video that was produced by tormach that gives some great detail using the same type of cutter. He says you can cut different pitch, metric and standard, all with the same thread mill.

[ame="http://www.youtube.com/watch?v=T4ZVoHei1uE&feature=related"]External Thread Milling with a Tormach PCNC 1100 - YouTube[/ame]

David

[David Bord]

Damn, this is cool... Thread milling with a modified tap!

[ame=http://www.youtube.com/watch?v=-J_Xrkrs1Xc&feature=related]Thread milling with a modified tap - YouTube[/ame]

Any reason this wouldnt work well for a hobbyst if you are willing to go slow?

HSS taps are a dime a dozen. If this works well it might be perfect if you dont want to drop the money on real thread mills.

Let me know what you think.

David

[mick.w]

almost definently multi tooth threadmilling is quicker and far more cost effective than single pointing. we are currently cutting a lot of 8un pitch threads of various diameters and depths and in different materials using just 1 style of tool and tip, we do however find it easier to start the theading cycles from the top of the hole allowing a guage check after the initial pass,
seco, kennametal,maxcut and stellram and others are all good threadmill tool manufacturers,
threads we have cut in the past using these tools include m370 * 6mm pitch at a depth of around 400mm and sized in one pass to guages with a surface finish of 3.2um or better,

cheers

mick w