[RussMachine]

Has TORMACH, or anyone come up with a recommended Tapping RPM chart to coincide with the 1-HP Low Torque/ Low RPM spindle motor?
I've discovered that at low speeds, the motor loses ALOT of torque.
I tried tapping a 3/8-16 hole today in 1018, 3/8 deep, thru hole, 500 RPM... and the motor stalled.
GOOD GRIEF!!
A 1-HP motor SHOULD be able to drive a 3/8 tap.
Maybe not.

[SCzEngrgGroup]

Not as much torque as you seem to think....

HP = RPM * Torque(ft-lbs) / 5252 or Torque = HP * 5252 / RPM

I believe the spindle motor is rated at 1.5HP, but that's at it's base speed, which is most likely 1800 RPM. At that speed, it will have barely 4 ft-lbs of torque. It is the nature of VFDs, that torque falls off as you either increase, or decrease RPM form base speed. Above base speed, power is more or less constant, which means torque falls off linearly with increasing RPM. At 3600 RPM, you'll have less than 2 ft-lbs.of torque. Below base speed, some VFDs can maintain constant torque down to maybe 30% of base speed, but it will fall off below that. So, at 500 RPM, you're below 30%, and losing torque. You can try increasing RPM - Some people do tap at 1000-1200 RPM, but I've never been brave enough to try it. Bottom line - anything over 1/4" in steel, you'll probably want to do by hand. I'd suggest getting a hand tapping fixture - they're inexpensive (about $80), and work really well. I use mine almost every day.

Regards,
Ray L.

[mountaindew]

Anything over a 1/4 I would consider thread milling with my expensive cnc machine. I like to use my machine for everything
You have great deal more control over threading process. So I read in cnc programing pg 434 , no personal experience with this at the moment.
It is next on my learning plan.
Sandvik Cormant has extensive information and formulas for milling and threading also.
I am taking their course on machining and I can say its very complete and explains most feed, speed, power, material relationships.

md

[Steve Seebold]

You could also try drilling your hole one side larger.

[mountaindew]

You could also try drilling your hole one side larger.

I was going to mention this and ask what size hole and what thread contact or tolerance he was working with or wanted.
Its going to get real tight at 75% contact like aluminum tap hole spec. verses steel at a 50% contact maximum.
Easy to look at chart so I figured he had this at or a larger size!
md

[RussMachine]

Next time I'll try 65% thread.
It would be nice if there was a third pulley to let the VFD run at 60HZ, while going 300 RPM, and a 2HP motor.
But I understand, we can't have everything. Gotta keep costs down.

[Don Clement]

Time for a paradigm shift with CNC. Even large holes are easily done on the Tormach by thread milling. Don't need those brute force methods one had to use with manual mills. I thread mill everything over 1/4" so no need for more torque or more HP. Here is my Tormach thread milling a 102mm -1mm hole:
Thread Milling M102-1mm Tormach Video by miltons_stuff | Photobucket


Don Clement

[mountaindew]

Next time I'll try 65% thread.
It would be nice if there was a third pulley to let the VFD run at 60HZ, while going 300 RPM, and a 2HP motor.
But I understand, we can't have everything. Gotta keep costs down.

No reason you cant change every part of your mill to meet or exceed your specifications!

From an engineering point of view, I go back to my jeep modification days! You add larger tires you need lower gears. Change gears you need larger motor. Swap motor and now suspension is overloaded......hard to find a point to stop.
And many years of off road experience has shown me the stock jeep with a experienced driver will go on 98% of all the trails. And the other 2% of jeep roads are so bad they almost require the jeep to be hauled on a trailer to and from anyway! And chances of Damage are almost 100% when used this way so trailer is good idea?

My point is! I purchased a tool or machine because of the complete design not the power rating or some other feature.
I did this knowing that the operator is 98% of the power of the machine not the motor.
As don below shows and I mentioned above there are a number of ways around every obstacle. Modern machines, tools and methods make all this imho easy to research, setup and perform. And do this a number of different ways based on the material, machines power, fixture, tool and tool holder.

Just an opinion from a new user that enjoys the challenge of learning this stuff!

Time for a paradigm shift with CNC. Even large holes are easily done on the Tormach by thread milling. Don't need those brute force methods one had to use with manual mills. I thread mill everything over 1/4" so no need for more torque or more HP. Here is my Tormach thread milling a 102mm -1mm hole:
Thread Milling M102-1mm Tormach Video by miltons_stuff | Photobucket


Don Clement

Nice video don,
Been shopping around for some thread mills, not many choices!
Would like to pick up a couple thread mills and 1 single point unit, any recommendations or good experiences, sizes / brand that you use most or like?
Thanks for any info
md

[RussMachine]

Does anyone know a (relatively) cheap place to purchase threadmills?
I looked on Ebay, and threadmills are going for $65 EACH!!
YIKES!!

[Geof]

That is cheap for a threadmill.

[Don Clement]

For the indexable threadmill shown in the video I used a 3/4" shaft Vardex thread mill toolholder KBC Tools & Machinery, Inc. modified for TTS use. To make the TTS modification a groove was turned in the 3/4" shaft to accommodate a circlip using a Nikcole Mini-systems insert grooving tool. http://www.niko-nikcole.com/mini_system.htm I then loctited a turned TTS ring adjacent to the circlip followed by chucking the modified Toolholder in a 5C 3/4" collet in a lathe and finish facing the ring TTS mating surface. See two photos below. The Vardex 3/8" TM carbide inserts cost ~$30 each but one must have an insert for each thread pitch, external and internal. KBC Tools & Machinery, Inc.

Don Clement

[LeeWay]

I happen to agree with Don in this case. Brute force may not actually be the way a tap was designed. Hand tapping, especially in harder materials require you to reverse the drive to break the chips. That is not required when using rigid tapping on a machine. A machine provides better constant torque once engaged in the thread. That is to say one that is setup up to rigid tap. Other taping methods work basically the same during the threading process.

I tap a lot in sizes from 6/32 to 3/8 16 every week with rigid tapping using a servo motor. My spindle speed is 100 RPM. For those tap sizes, it is economical to use a tap and tap holder. Anything larger and I would be looking at a thread mill as well. One size will make a lot of threads with those, whereas rigid tapping requires a different tap, collet and ER holder for each. Auto reversing tapping heads require that you change the collet and tap with each different size, but are very usable and economically viable if you rarely tap stuff and tap different sizes. No servo needed in that case. A small reversing head tapper would probably be ideal on your setup . I am not familiar with how the tension compression tapping holders work, but might be worth investigating.

[SCzEngrgGroup]

A tension-compression holder will work fine on a machine with a VFD spindle, provided you have a braking resistor to stop the spindle quickly, and have the acceleration ramp set pretty fast. But you have to be very careful on blind holes, as you don't have tight control over the maximum depth, unless your spindle stops VERY quickly. But, for most needs, it works just fine, and is a good compromise between a tapping head or hand-tapping and rigid tapping, which requires a servo spindle with Mach3. With either tension/compression or rigid tapping, you can periodically reverse direction to break chips, just as you do when hand-tapping. But, you have to be careful not to exceed the range of the tension/compression holder. Not an issue with rigid tapping.

Threadmilling is great, especially for rarely used or odd-sized larger threads. I have a single--point tool I've used for cutting threads from under 1/2" to over 2", both internal and external, Metric and Imperial, straight and tapered. After doing hundreds of threads, the tool still cuts like new. They are incredibly versatile tools, and the programming is almost trivial, despite how it appears. Threadmills also allow you to get exactly the thread fit you want, from very loose, to very tight, And the surface finish on threadmilled threads is hard to beat. A single single-point threadmill tool can cut almost any thread, with makes the $50-60 cost of the tool easier to accept. But, the downside of threadmilling is that it is MUCH slower than a tap, unless you use $$$$ multi-point tools, like the one Don shows in his photos. And, of course, a mistake with a tap breaks a $5 tap. A mistake with a threadmill can break a $100+ threadmill.

If you're doing a lot of holes, up to around 3/8-1/2", you probably want to use a tap, unless you don't have enough torque to do the job. Above that, thread-milling starts making a lot more sense, unless you're doing a LOT of parts, and want to get them done in a hurry. Then, you either need to invest in a $$$$ multi-point threadmill, or just hand-tap using a tapping fixture, which is also very fast, accurate, and easy. It's also not difficult to "power" a tapping fixture, using a stepper motor and belt/gear reducer.

Regards,
Ray L.

[LeeWay]

Hand tapping in my tapper is fast when I do it, but not when my employees do it. No matter how many times they do it on the same type part, they are glacially slow at it. Probably 3 times slower than what I do and a helluvalot slower than the rigid tapping. I have asked them why so slow and it is always that they do not want to break the tool. That they have done a few times and I have not ever broken one. I rake the tap over a candle before every hole. I cannot get them to do that. As a Boss, I apparently do not have enough leverage or teaching skills to make them do as I wish. Another plus for rigid tapping in my case.

[Don Clement]

I tap a lot in sizes from 6/32 to 3/8 16 every week with rigid tapping using a servo motor. My spindle speed is 100 RPM.

The Tormach does not do rigid tapping nor has a servo spindle that's why I use a Procunier reversing tapping head for taps under 1/4" (especially on blind holes which I do lots of) and use thread milling for threading over 1/4" on my Tormach.

Don Clement

[X35 Design]

I am a relative noob here, but I have been using a carbide one flute threadmill on my 1100. It has a 1/2" shank,, .488 diameter cutter, and can make threads from 11-32tpi up to 1.36" deep. MSC Part # 40232951

I use it in 3/8NPT and larger.

I also have a 1/4" shank from the same mfg that can do 16-48tpi with a .240 diameter, which will do 5/16 NC up to .8 deep.

I like the versatility that I can do so many threads with just these two tools. Not the most speedy method, but they work well for me.

[LeeWay]

Oh I am aware of that. But the economy kicks in for larger size threads.That is when you can start to realize benefits of thread milling.
It was a conscious decision on my part to get a machine that could rigid tap. I do a lot of it. Before this machine purchase, I did buy a Shars reversible tapping head to use in my manual mill for tapping. After the purchase, I sold it unused to a Member of the Zone.
I think the head I had could do from 6/32 to 1/2". Came with the collets. Quite economical.

[TurboStep]

...as you don't have tight control over the maximum depth, unless your spindle stops VERY quickly...

Its not a question of how fast but how constant. The brake on my 1100 stops the spindle in RPM*0.24 seconds. For example: it stops in 0.12 secons from 500 RPM, roughly one rotation. This is fairly constant and could simply be subtracted from the total depth of the thread - if it weren't for the other delays
Between the end of the feed and the start of the spindle deceleration there is a delay of between 100ms and 300ms. A constant delay would have been easy to compensate for, but this large variation makes the resulting depth rather unpredictable.
Another point to be aware of is that if I program a delay e.g. G04 P0.4, the actual delay that I measure is 200ms longer! In this example the actual delay would be 600ms.
I have no idea how these values vary between controllers but this is a good enough reason for me to stick with thread milling for all thread sizes.
The milling process with single point thread mills is slower but there's no need to play around to get if right first, and no risk of a tapping to the wrong depth. When I consider the whole process from CAM to the end product(s) I'm much faster, even with single point mills, but everyone's jobs will be different. A multi-point thread mill on the other hand is just as fast, if not faster than using a T/C head. When using a T/C head the spindle has to reverse directions twice per thread, and the feed into and out of the hole is slower. A thread mill can rapid down to the bottom, mill one rotation and rapid out.
Total cost depends on the whole process - not just on the price of the mills. I have 6 thread mills permanently set up in ER20 holders - time is not money for hobby use but that's still a considerable convenience. I wouldn't want to purchase 6 T/C holders! I don't have an ATC but it may be a consideration at some point so I can't justify the best part of $1000 for the non-ATC compatible Tormach Procunier. I can buy a lot of thread mills for that money.
Step

[Don Clement]

The Procunier stops within 1/3 revolution repeatably. BTW I have upgraded the spindle on the 1100 with the VFD brake. For me in tapping 10s of thousands of blind 4-40 holes using a roll tap and the Procunier works extremely well on my 1100. YMMV.

Don Clement

[Don Clement]

A big advantage for me in using a roll tap in tapping 4-40 blind holes is no chips are produced. Plus with the Procunier I tap @1200rpm with a feed of 30ipm down and retract @ 60ipm. Pretty fast for blind holes on my non rigid tapping Tormach 1100.

Don Clement