[DLawrence]

I have an order now for 500 1/2-13 tapped through holes..... One inch deep........ in 12L14 steel , and the man is saying he wants them produced

ongoing at 4000 to 5000 a year.

In order to enjoy the benefits of straight tapping , instead of going to thread milling .......I am about to machine a (seven inch dia) #30 roller chain sprocket out to sit

right on top of the large (aprox 6.5 inches dia spindle pully ....there is clearance to do this........ and then just change out the motor pully to a drive sprocket .....probably about half

the diameter of the present small VEE pully

With a more than 2X increase in torque I think tapping 1/2- 13 with my large large reversing tap head will go well.

One of the beautys of roller chain is the easily adjustable length feature ....therefore to easily try different size input side drive sprockets.

IF the 3/4" TTS quickchange system begins to slip....... I want to try a drive dog clamped to the spindle nose and sticking down to push on a dog welded to the tapping head ,

creating a positive rotational drive while preserving the quickchange TTS ability.

Unless I get feedback from this post that changes my perspective......., I am going to move forward with this

I can balance the big sprocket if need be.

Thanks
Dave Lawrence

[Tormachmaster]

I have an order now for 500 1/2-13 tapped through holes..... One inch deep........ in 12L14 steel , and the man is saying he wants them produced

ongoing at 4000 to 5000 a year.

In order to enjoy the benefits of straight tapping , instead of going to thread milling .......I am about to machine a (seven inch dia) #30 roller chain sprocket out to sit

right on top of the large (aprox 6.5 inches dia spindle pully ....there is clearance to do this........ and then just change out the motor pully to a drive sprocket .....probably about half

the diameter of the present small VEE pully

With a more than 2X increase in torque I think tapping 1/2- 13 with my large large reversing tap head will go well.

One of the beautys of roller chain is the easily adjustable length feature ....therefore to easily try different size input side drive sprockets.

IF the 3/4" TTS quickchange system begins to slip....... I want to try a drive dog clamped to the spindle nose and sticking down to push on a dog welded to the tapping head ,

creating a positive rotational drive while preserving the quickchange TTS ability.

Unless I get feedback from this post that changes my perspective......., I am going to move forward with this

I can balance the big sprocket if need be.

Thanks
Dave Lawrence

Are you saying you cannot tap 12L14 1/2-13 tap with your machine? I believe in if it is not broken then don't fix it and you should have zero problems doing those tapping operations just get a really good tap. But 4000 to 5000 parts a year you may be working with the wrong machine.

[sin_arms]

I would get a different machine if you have room, an older VMC or a new smaller servo machine would make short work of that.

[Steve Seebold]

I seriously doubt your Tormach has the power to tap 1/3-13 holes in steel, even in 12L14.

This material has a lead content that makes it free machining but I just don't think you have the power required to do it.

[WOTDesigns]

Definitely not worth another machine unless you are billing a ridiculous amount for them. I purchased a Haas because of customer work and seriously miss being in my garage making money rather than payments. Now when you don't have time to make money doing other parts because the Tormach is tied up THEN buy another machine and leave the Tormach dedicated to this part. Less set up, time wasted and you have 2 machines.

As for the roller chain... it is likely to work but is likely to be a very bad idea. There is a reason no machine manufacturer I have ever seen uses roller chains on their spindles. They are inherently sloppy and will cause massive vibration due the the spinning mass of a chain with many constantly twisting and straightening links. That will definitely lead to a terrible finish on everything not requiring full torque. Timing belts are readily available in nearly any size. They transmit power well and with adjustment provide less slop than almost any other mechanism and is what MANY manufacturers or "real" VMCs use including my Haas. If you really want to get fancy use the QD (quick disconnect) pulleys and you can change your speed ratio back with the same belt left in place in about 5-10 minutes depending on set up.

I just ordered a couple timing pulleys and belt to convert my lathe feed drive to a DC reversible 24V motor so I can feed finer than .0047" per rev. SPI/SI has good pricing (less than McMaster) and a vast inventory on hand. They have a great distance calculator but it was down the other day so I found the one in the second link below. It lets you figure out the exact ratio, sizes and belt length based on your motor to spindle distance.


Timing Belt Pulleys for Small Power Transmission Applications- SDP/SI
Belt Length Calculator | B&B Manufacturing

P.S. using a full thread mill will likely be about the same time per hole since your straight tap has to turn much slower, pause, reverse, back out. The thread mill only has to make a few helixes or so at higher speed and rapid out... bet a nickle it is faster than tapping 1/2-13 on the Tormach. If the holes require a specific fit it will last longer than your standard tap as you can just change the offset to compensate for wear.

[Don Clement]

What wrong with thread milling on the Tormach?

[rowbare]

How many holes per part and how many parts are we talking about? Is there much other machining happening? It might be more efficient overall to do the tapping on a drill press with a suitably sized tapping head while the mill does the rest of the machining.

bob

[SCzEngrgGroup]

I think you are greatly under-estimating the difficulty of tapping 1/2-13 to 1" depth in steel, unless you can reduce the thread % considerably. Going to 1" depth without being able to back-up probably 2-3 times during the process, to break/clear chips, will be very difficult, and will probably result in either a stalled spindle and/or broken taps. If you're determined to do this, I think you'd need to do custom g-code to enable you to back the tap ALMOST out of the hole, and go back down several times. Without rigid tapping, if you ever pull the tap all the way out, even once, you won't be able to re-start it. A braking resistor on your VFD will be essential.

Given the low-ish volume, I would do it with a single-point thread-mill, and just find something else to do while the machine was doing the work. It will take a lot longer, but, end of the day, you'll have a MUCH better result, and should have NO broken tools. If time is an issue, use a multi-point threadmill. Or, get a machine capable of doing true rigid tapping, like a Novakon Pulsar. Then you don't even need a tapping head - you can put the tap right into an R8 or ER collet.

Regards,
Ray L.

[DLawrence]

Thanks for all the input Guys, Based on the collective consensus ....I will go with ...... for me....... the unknown ,......thread milling.

Thanks again all
Dave Lawrence

[WOTDesigns]

EASY stuff. take an air cut or two. Here is a cheap (yes this is CHEAP for thread mill) on ebay. Time wise you will be ahead. This will outlast 3 or 4 standard taps and end up being the same cost (minus all the money and time spent converting things)... just don't crash it and it will last several thousand holes easily.

Do a little googleing on thread milling. Lost of good info on speeds, feeds and strategies.

1 2 13 Carbide Thread Mill Brand New TiAlN Coated | eBay

[Steve Seebold]

Thanks for all the input Guys, Based on the collective consensus ....I will go with ...... for me....... the unknown ,......thread milling.

Thanks again all
Dave Lawrence

I think if I had thousands of 1/2-13 holes to tap, I would be looking at a good drill press and a suitable Tap Matic.

[bobeson]

I thread-milled a few dozen 1/2-13 holes in A36 with my 1100, and it worked well. I broke one tool by starting with the wrong speeds and feeds, for lack of thread-mill-specific recommendations. Lakeshore is now publishing recommended speeds and feeds for their line of full-form variable-flute carbide thread-mills: http://www.lakeshorecarbide.com/pdf/...HREADMILLS.pdf

I would recommend making two or more cut-depth passes, but it would probably work out OK to do it in a single pass if you're pressed for time. One good tip I found is to cut slightly more than a full revolution before returning to the hole center, to avoid a small line that can be formed in the thread at the entry/exit point from an incomplete leadin-leadout path. In addition, it helps to have your entry and exit take place along the helical thread path, and not on a plane. This may sound tricky, but once you get it coded into a working routine, it'll all be straightforward enough.

Making the full 1" of thread will be difficult with off-the-shelf full-form tooling, but perhaps you could just relieve the shank a bit and do it with multiple cuts. Lakeshore's 1/2-13 threadmill has a 0.875" DOC. The thread pitch is ~0.077", putting you at 0.952" thread depth after cutting one revolution, and >1" after two revolutions, but you first need to clear the tool's shank. Can you adjust the chamfer enough to make this tool fit as-is?

FWIW, I doubt that you would experience TTS slip while tapping. In my experience, this usually requires a combination of torque and vibration from uneven radial cutting forces. With evenly-distributed cutting forces such as in tapping, you are likely to stall the motor before you slip, assuming a properly-setup TTS collet.

I like threadmilling better than tapping because you never need to hassle with extracting broken taps from your workpiece. The sky-high price of the tooling is painful, though.

[TurboStep]

Lakeshore's 1/2-13 threadmill has a 0.875" DOC.

I missed that one! The Maritool 1/2-13 has a flute length of 1.0".
Step

[MichaelHenry]

HSMAdvisor claims that a 1/2-13 form tap in 12L14 at 500 rpm and would need 7.6 ft-lbs of torque. Does anyone have a rpm vs torgue curve for the 1100 mills?

[Zetopan]

HSMAdvisor claims that a 1/2-13 form tap in 12L14 at 500 rpm and would need 7.6 ft-lbs of torque. Does anyone have a rpm vs torgue curve for the 1100 mills?

No "curve" is necessary. At full speed with the drive belt set to the high speed range the 1.5 HP spindle motor is operating at 120 Hz. The 60 Hz power line frequency and above is where the motor is rated at 1.5 HP. Below the 60 Hz power line frequency the spindle motor is operating at constant torque since constant power would cause the drive currents to approach infinity at 0 RPM. So at 500 RPM on the high speed range the spindle motor is operating in the constant torque region and we can trivially compute that torque at 60 Hz by knowing that 1 HP is equal to 33,000 pound feet of energy per minute.

Power = Torque * RPM / 5252, where Power is in HP and Torque is in pound feet (this equation is trivially derivable).
1.5 = T * (5140 / 2) / 5252, where 5140 is the 120 Hz RPM and we divide by 2 to get 60 Hz RPM.
T = 3.065 pound feet.

Since the maximum RPM on the low speed range is 2,000 RPM, that results in 5140 / 2000 * 3.065 = 7.878 pound feet of torque on the low speed range.
Thus nearly a full 1.5 HP would be needed for the example tapping at 500 RPM. However, at 500 RPM on the low speed range only 0.75 HP is available.
This means that an additional 2:1 reduction would be required on the spindle to just reach the required tapping HP, even though the torque requirement
would be met without the additional reduction.

All of these calculations assume 100% efficiency in the motor to spindle coupling.

[zero_divide]

HSMAdvisor claims that a 1/2-13 form tap in 12L14 at 500 rpm and would need 7.6 ft-lbs of torque. Does anyone have a rpm vs torgue curve for the 1100 mills?

No. You can not tap 1/2-13 hole in any steel on tormach.
Unless you use oversized hole and can Iive with lesser thread engagemnt.

HSMAdvisor already has the machine definition for Tormach 1100 btw
It also warns that it will not work.