[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.

[Gundawg]

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?

School is not an option for me I wish it was. I work rotating shifts in job number 1 and job number 2 is running this business I need the machinery for. Rotating shifts nights to days and differing days off make a school schedule impossible. I have read several text books on machining manual machine work but I am self taught I have learned what I know from reading books and internet forums like this one. I do not have any books on CNC. What I have done was read through the tutorials on the software I have and learned to draw in cad and make toolpaths for my CNC router. The system I use now does not use Gcode but as I have learned to run the router I am sure I will learn to run the mill. I do not believe the software I have now supports tapping. Your explanation has helped me to understand that.



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

I have talked with Tormach a couple times on the phone trying to figure out just what I need to order. They have not advised me on a tapping head. I have just started really getting serious about this and I am trying to figure out what to order. I am looking at the PCNC 1100 I have been playing with the options list and on the deluxe package I noticed it listed a tapping head. Sorry for some of my dumb questions but I am picking up some knowledge by asking these questions.

[txcncman]

Questions themselves are not dumb. What is important is that you use the information to make improvements.

To change from an apprentice status machinist to a journeyman machinist it is recommended to take 576 hours of classroom training and over 8000 hours of on-the-job training (about 4 years). If you neglect the classroom training and only rely on the on-the-job training, that number of hours increases to 10304 (about 5 years). And remember, this is 4-5 years of serious, dedicated study and work. Doing it part time will take much longer.

[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]

[Don Clement]

[QUOTE=Gundawg;1001634] 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

The Procunier has no adjustment for depth for blind holes. The clutch simply disengages within 1/3 spindle revolution. I just measure the z-axis height on surface plate and enter into tool table. http://i72.photobucket.com/albums/i1...HeightMeas.jpg Set the depth and write four lines of Gcode.

BTW If I was just tapping 4 holes, I would just use a Fisher micro tap guide with T-handle tap wrench and tap manually. Fisher Machine Shop Pee Dee Wires and Tap Guide
http://i72.photobucket.com/albums/i1...tap-holder.jpg

Don

[Gundawg]

That is 4 holes per part times 100 parts I have manual tap handles and guides. The whole idea for me having a CNC is not doing a bunch of manual operations. I plan to build a fixture to hold multiple parts to use the full travel of the machine. These particular parts are 2.25" wide x 5" long x 1" thick I will buy bar stock and cut into blanks and fixture the parts to get the largest amount to fit per setup.

In my shop I will not work for less than $50 an hour and try to make $100 an hour anything less than $50 an hour gets outsourced or the product is scrapped. I do not machine for other people only the products I sell are made in my shop. I build as the demand calls for the products sometimes I am real busy but this time of the year is slow and allows for prototyping and bringing in new equipment to learn to use. I have to justify the cost of the machine if I need to purchase new software I will to do the tapping but if I don't need it I would rather put the $1100 towards something else. I have several other projects planned that I will need to tap 1/4 - 20 holes in .500" Al.

I am thinking I can draw the part and make the tool path for tapping using a drill tool path and edit the code if that is the only thing my present software won't do.

Thanks for helping work through this stuff.

Mike

[dbrija]

I just ordered one of these (ER20 3/4 Floating Tap Tool Holder MariTool). The price was much more reasonable than the Tormach version. Hopefully it works out well. I have a TTS adapter to glue on, or I may just turn the face near the shank to clear the collet like I did for my facemill.

[txcncman]

@Gundawg - Maybe now you understand that there is not just one answer and none of the answers is simple. There is one problem I see with going with a tapping head. For all the tapping heads I have used or see used, you have to have an anchor point, or a stop to hold the head from actually spinning around so that the internal clutches can do their job. For most applications, this means that you cannot use an automatic tool change and just continue machining. The operator will have to manually attach this stop each time the tapping operation comes up and then remove it before proceeding. Also, the tapping heads are more expensive then the compression/tension tap holders by about 10X or more.

An alternative is to put a tapping head on a drill press or manual mill nearby and let the same operator power tap the parts after they have been drilled on a previous operation.

[Don Clement]

In my shop I will not work for less than $50 an hour and try to make $100 an hour anything less than $50 an hour gets outsourced or the product is scrapped. .

Thanks for helping work through this stuff.

Mike

You got the advice you paid for then.

Don

[Gundawg]

You got the advice you paid for then.

Don

What is that supposed to mean?

I appreciate all the sugestions I am just trying to work through all of this so I don't purchase things I don't need. I did that last time when I bought my CNC router not knowing and now I own a $2000 indexer I have never used. I am asking for advice some I will use and some I won't.

I belong to several forums and always help when I can to try and pay back for good advise I have been given. I am sure after I have used a CNC mill for a while I will be able to help other people with the experience I gain.

I am a hobby machinist of sorts but I sell the stuff I make I don't try and hide that. I do make things and tools for myself but I would never buy a machine like this to tinker with for me it is too large an investment. Sorry if my questions are not recieved well.

Mike

[SCzEngrgGroup]

So..... Seems to me all of these would *require* a spindle encoder if running CNC, to be able to set the feedrate with sufficient accuracy, no? If the downfeed is too fast, looks like very had things will happen, no? *Slighty* slow is OK, if not preferred, as long as it's not TOO slow, right?

Regards,
Ray L.