PDA

View Full Version : Thread Milling ???



Mike Hunter
08-24-2009, 03:55 PM
Ok …Thread milling, can someone explain this to me, how is it done?

tattoomike68
08-24-2009, 04:15 PM
A cnc mill will mill a helix. some times with a single v type cutting tool that will cut more pitches. A larger tool with multi points but it will only cut the one thread pitch. You can threadmill and OD or an ID.

here are some videos. with two different types of cutters.

http://www.youtube.com/watch?v=ti_1OHMFCtI&NR=1

http://www.youtube.com/watch?v=_OlfyvRU67o&feature=related

Mcgyver
08-24-2009, 04:21 PM
great vids, nothing more to add to that!

tattoomike68
08-24-2009, 04:32 PM
great vids, nothing more to add to that!

Somebody will need to say that the cutters cost a hell of a lot of money for the trick ones, like 5 to 10 times the price of a tap.

Taps are cheap, cheap, cheap, and you dont need a CNC.

Bguns
08-24-2009, 05:23 PM
The Barrel is put on a lathe and threads milled with a Live tool on crossslide. Like a Versamill attachment, canted for thread helix angle..

Due to blind end of thread, probably not spinning too fast, :) but done in one pass, faster and cheaper for production than single pointing.

Much easier for square threads also...

lazlo
08-24-2009, 05:42 PM
A cnc mill will mill a helix. some times with a single v type cutting tool that will cut more pitches.
here are some videos. with two different types of cutters.

http://www.youtube.com/watch?v=ti_1OHMFCtI&NR=1

What's especially remarkable about that video is that it's running on a converted round-column mill/drill! :)

motorworks
08-24-2009, 07:21 PM
"Somebody will need to say that the cutters cost a hell of a lot of money for the trick ones, like 5 to 10 times the price of a tap.
Taps are cheap, cheap, cheap, and you dont need a CNC.''

That's true, they are $$ But:

I had a job 3 weeks ago where I had to make 32 parts
from 304 stainless.
I had to 'drill n tap' a M24-3 thread 45mm deep
Bit hard on the arms even at 55 %
Did the TDS in the lathe and set each part up on
a jig in the turbo cnc mill and thread milled them.
Approx 3 mins each including set up.

e2die :)

Mcruff
08-24-2009, 07:25 PM
We mill large threads at work with a boring bar and a lathe bit after we drill or bore the proper tap drill size. Works great and you can't get much cheaper than that. We have cut quite a few 1-1/2"-2" threads that way. We use Bobcad to draw the helix and program the mill with.

DR
08-24-2009, 07:57 PM
Threads can also be milled on a conventional (non-CNC) lathe.

Rig up a rotating tool on the cross slide. Set the thread pitch in the gearbox, engage feed and cut a deep, coarse thread in one pass.

Of course, the lathe spindle has to be slowed down considerably. You could conceivably mill threads by hand cranking the spindle. I did that to cut large threads in wood using a router to hold the cutter.

Years ago I saw a special fixture to mill threads on a conventional vertical mill. It was like a rotary table, plus the chuck moved upward corresponding to the thread pitch as the part rotated.

There are dozens of way to mill threads besides using CNC machines. Automatic screw machines were milling threads long before anybody envisioned CNC. Old horizontal/vertical mills did it using a gear driven indexing head off the X axis screw.

The primary advantage of milling large threads is the cutting ease compared to single pointing or tapping.

Thread grinding in hardened material is similar to milling.

rklopp
08-24-2009, 08:21 PM
It is interesting that in the guhring vid, they are conventional as opposed to climb milling. I wonder why. Usually surface finish is much better when climb milling.

SGW
08-24-2009, 08:28 PM
A friend of mine, Ron Ginger, milled a 2 1/2" taper pipe thread on his CNC'd mill using a single-point V tool programmed with MACH3. It was in a thousand-dollar casting, so he was sweating while the program was running. It took something like 3 hours to run and came out fine.

Ron's website is http://pleasantcovemodels.com/ .

drof34
08-24-2009, 11:25 PM
Here's another form of thread milling on a manual lathe.

http://i56.photobucket.com/albums/g171/drof34/2006_1219thread-milling0001.jpg

That's a bridgeport head mounted on a 56" swing lathe with a creep speed option.

That's two screws mounted on an arbor and they are about 8" in dia with a double lead.

oldtiffie
08-25-2009, 08:22 AM
Thanks drof34.

That will be an entirely different approach to many - but its not new and the principles are very sound.

And this will really upset the anti-"3-in-1" brigade who never miss an opportunity to "rubbish" 3-in-1 machines - the more so if thet are "Chinese" which most - mine included - are.

My lathe is a 3-in-1 and provided I get the spindle speed down, it would "eat" that sort of a job - provided that it was in the capacity of my change-gears and lead-screw!!! A lot of lathes seem to be limited to about the lead of their lead-screw or not much more than double it. So I would be limited to my lead (3mm) or at most double it (6mm).

http://i200.photobucket.com/albums/aa294/oldtiffie/Lathe_misc/Lathe1.jpg

It should be an easy job for a CNC-ed mill with a 4th. axis (dividing-head or rotary table). If it had a tilting head it could use straight cutters -as in your pic - and that includes my 3-in-1 machine.

My (yet to be-CNC-ed) Sieg X3 mill does not have a tilting head so I would need to make a tapered cutter to suit the thread form.

I will post the details of a cross-slide mounted tilt-able milling head attachment for the lathe that has ER-16 collets and 4 speeds tomorrow as it will mill both internal and external threads in lieu of a screwing tool in a lathe tool-post. Otherwise its the same.

hornluv
08-25-2009, 08:44 AM
Somebody will need to say that the cutters cost a hell of a lot of money for the trick ones, like 5 to 10 times the price of a tap.

Taps are cheap, cheap, cheap, and you dont need a CNC.

Yeah, but you've gotta see from that second video how they are worth that cost. It drilled the hole, counter sunk it, and thread milled in 10 seconds per hole. Pretty damn slick if you ask me. Eliminating tool changes needed to make the part is a big time saver and therefore money maker. It probably pays for itself in just a couple of parts, and does so many times over it's life.

DR
08-25-2009, 12:49 PM
.......................................

It drilled the hole, counter sunk it, and thread milled in 10 seconds per hole. Pretty damn slick if you ask me. Eliminating tool changes needed to make the part is a big time saver and therefore money maker. It probably pays for itself in just a couple of parts, and does so many times over it's life.

You certainly would have to have a horrendously large production run to justify those type tools.

They aren't general purpose tools. Presumably you would have to have the tool custom made to each hole spec. Probably bringing the price up to as much as 25 or more times the cost of more conventional tooling.

Allowed depth of hole, style of countersink and specs of countersink would all have to be taken into consideration for blind holes. For through holes it wouldn't be such an issue though.

lazlo
08-25-2009, 12:54 PM
They aren't general purpose tools. Presumably you would have to have the tool custom made to each hole spec.

Why couldn't you use that thread mill for a different hole sizes? It looks like a threaded drill mill.

I use ordinary drill mills to chamfer, slot, and drill.

DR
08-25-2009, 01:20 PM
Why couldn't you use that thread mill for a different hole sizes? It looks like a threaded drill mill.

I use ordinary drill mills to chamfer, slot, and drill.


For instance, if you had the same thread spec'd for multiple holes in a part, but the max allowed drill depths were different (a very real situation). The tool that did the deepest holes could not go deep enough to do the countersink on the shallow holes.

oldtiffie
08-25-2009, 08:57 PM
Machinery's Handbook addresses the issues with thread milling pretty well.

I will dig it out and post it later.

There are quire some issues with thread milling which I will cover ina later post.

It is quite practical for the HSM-er - but needs a bit of thought.

hornluv
08-26-2009, 12:17 AM
I can't see how that tool could be used with anything but through holes. If you look at the tool, the first little bit doesn't have threads, although I guess you'd just have a relief groove at the bottom of a blind hole. I can see how they could be standard sizes though. The diameter would have to be the tap drill size for whatever hole would be called for. The countersink diameter really only needs to be a bit larger than the nominal major diameter. Maybe .050 just to give plenty of wiggle room. Then it just needs to have the right pitch on it.

oldtiffie
08-26-2009, 08:22 AM
Machinery's Handbook addresses the issues with thread milling pretty well.

I will dig it out and post it later.

There are quite some issues with thread milling which I will cover in a later post.

It is quite practical for the HSM-er - but needs a bit of thought.

Here are the relevant pages from Machinery's Handbook 27 - which are a very good read as they address all of the issues:
http://i200.photobucket.com/albums/aa294/oldtiffie/Machinery_HB27/MHB27_P1962.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/Machinery_HB27/MHB27_P1963.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/Machinery_HB27/MHB27_P1964.jpg

I am thinking about thread-milling as an exercise on my lathe and the Hemingway Kits "Quick-step Mill" seems to provide all the answers I need to get going. Its not cheap but should do the job for threads with larger helix angles and/or large amounts to be milled out instead of boring them out.
http://www.hemingwaykits.com/acatalog/The_Quick_Step_Mill__.html

Hemingway's catalogue is a good read as well:
http://www.hemingwaykits.com/products.html

It should be quite possible and practical to mill internal and external threads with a "stubby" tap of the correct pitch - or a single point tool.

The QSM would need to be mounted in the lathe tool-post and the lead-screw set for the matching pitch thread and the half-nuts engaged as for normal screw-cutting.

The lathe spindle must be stopped before the half-nuts are disengaged if the cutter cannot be withdrawn from the cut first.

I have to think a bit more about the idea as well as the costs involved. I need to email Hemingway Kits for more info before I decide either way.

Following on with the logic, it seems quite feasible to rig a tool-post grinder up with the grinding wheel set up as a "single point cutter" for threading (internal and external)finer finishes and harder materials.

Tilting the QSM will be required for larger helix angles (say in excess of 3>5 degrees).

The outside diameter of (HHS) cutters or grinding wheels does not seem to be an issue, but it probably will be for internal threads as the cutter/wheel will need to be able to be withdrawn from the thread bore (aka root diameter) plus clearance.

I have the grinders for the job:
http://i200.photobucket.com/albums/aa294/oldtiffie/Med_Speed_Spindles/Bosch_HS_Grinder7.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/Med_Speed_Spindles/Bosch_HS_Grinder8.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/Med_Speed_Spindles/Bosch_HS_grinder1.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/Med_Speed_Spindles/Proxxon_small1.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/Med_Speed_Spindles/Bosch_HS_Grinder13.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/Med_Speed_Spindles/Bosch_HS_Grinder14.jpg

DR
08-26-2009, 10:49 AM
.................................................. .......................

It should be quite possible and practical to mill internal and external threads with a "stubby" tap of the correct pitch - or a single point tool.

.................................................. .......................





Shank type 60 degree milling cutters work well.

Taps don't work well at all, in spite of the conventional wisdom that they do. The helical grind of the teeth causes rubbing on one side. In other words, there's no relief on one flank of the tap's teeth.

lazlo
08-26-2009, 10:50 AM
The diameter would have to be the tap drill size for whatever hole would be called for.

That Ghuring endmill is a thread mill, not a tap. So if you watch when it cuts the threads, it's orbiting around the hole, just like the single-row thread mill in Mike's first video (on the Mill/Drill).

But DR has a good point about the limitations w.r.t. to the depth, and the clearance at the bottom of the hole necessary because of the drill/countersink section of the thread mill.

oldtiffie
08-26-2009, 08:59 PM
Originally Posted by oldtiffie

.................................................. .......................

It should be quite possible and practical to mill internal and external threads with a "stubby" tap of the correct pitch - or a single point tool.

.................................................. .......................


Shank type 60 degree milling cutters work well.

Taps don't work well at all, in spite of the conventional wisdom that they do. The helical grind of the teeth causes rubbing on one side. In other words, there's no relief on one flank of the tap's teeth.

Thanks for the correction and "heads up" DR as it is appreciated.

It was silly of me to have made the mistake that I did.

You are quite correct as it is very clear in the first of the pics (MHB page 1962) that I posted - see "Multiple Cutter Method"- where it clearly says that the multiple cutter should have no lead.
http://i200.photobucket.com/albums/aa294/oldtiffie/Machinery_HB27/MHB27_P1962.jpg

I should have thought that through better than I did before I posted it.

I thought I had that covered by - but not saying/posting - that that would have been largely alleviated by tilting the single cutter spindle by an angle equal to the thread helix angle.

If - particularly when "zero tilt" is applied - the side clearance on the "trailing" side of the "teeth is less than the helix angle that will certainly be the case as it will "rub" or "foul". But as you say/infer, any reduction due to the helix angle will reduce that clearance angle to (or past?) the point where it is useful or practical.

It had crossed my mind when I read it that I'd have to grind the additional clearance angle on the trailing flank to make it positive. I had had it in mind to only use a "stub" of a couple of teeth - or just a single tooth - as I intended to grind off all but one "row of teeth" as they were helical.

The "tap" is effectively being used as a form cutter the speed (RPM) of which is irrelevant to the thread as it is acting as a formed thread-grinding wheel or milling cutter would, in that the thread is formed/cut by the carriage being driven by the lead-screw as in any screw-threading operation.

That can be done on a conventional lathe as in the "Single Cutter Method".

The "orbital" method as shown in the videos would need to be done on a thread-mill/lathe and/or a CNC-ed mill.

DR
08-26-2009, 11:43 PM
Tiff',

The tap- as-thread-mill is interesting. Ask a bunch of machinists and I swear half will claim it works perfectly, the other half will say no way.

Being stubborn I had to try it for myself.

As I recall I took a 3/8-16 tap and ground all but one flute off. Then I ground back relief until there was only about .010" left on the OD at the tips.

I tried to mill a 3/4-16 internal thread in soft brass. It rubbed and squealed something awful.

Now, I suppose if you were to get something like a 2" diameter, 16 pitch tap and modify as I did then try an external thread it might work. There would so little helix on that large a tap diameter the rubbing might be tolerable.

oldtiffie
08-27-2009, 02:34 AM
Thanks DR.

I intended to remove/ease/relieve the trailing edge clearance angle on my T&C grinder.

It was only a thought to see if it was "do-able" as I'd prefer to use a HSS bit silver-soldered to the end of a bit of HSS round (as a boring bar) to keep it a short and as "stiff" as I could do it by grinding a single "tooth" onto the end HSS bit.

The main problem with using or modifying a HSS tap (single flute) is that I'd need as large a tap as I could get with the required screw pitch so as to minimise the helix angle.

MHB doesn't say as much, but I'd require the cutter/s to spin in as small a circle and arc as possible so as to minimise the "fouling" of the work by the spinning cutter. That of course leads to a possible compromise with the boring bar size and stiffness.

As MHB says, there is not much of a "thread-form distortion" problem until the helix angle gets close to 3>5 degrees as it starts to become significant then.

When the cutter is horizontal it is emulating a standard lathe screwing tool. But as it is tilted it starts to emulate a thread-grinding wheel where the included angle approaches or exceeds 61 degrees which will or may up-set the "Puritans" as regards thread form and errors when using the "three-wire" measurement method.

Franky, I doubt that a one degree error would either matter or be detected in a HSM environment.

While the "horizontal" (zero tilt) setting may be OK for most common "V" threads - which have relatively small helix angles, it is quite another matter for stuff like the relatively small diameter relatively deep and high-pitched helix angles on many of the acme lead-screw nuts that we see being done here.

The nuts would need to be relatively short and the boring bar tilted relatively highly. At those higher tilts in excess of say 5 degrees, the "form error" will be considerable and would need to be allowed for in the grinding of the "tilted" threading tool which will be wider and have "steeper" angles on the flanks of the thread/s and the milling cutter.

This sort of set-up makes threading larger threads for say back and face plates for lathes with a screwed spindle nose a whole lot easier.

Using a good high-speed die-grinder makes thread grinding a very distinct possibility.

The more I think about this, the more I am inclined to buy that "Quick Step Mill" I referred to in an earlier post.

hornluv
08-27-2009, 09:09 AM
Lazlo wrote:

"That Ghuring endmill is a thread mill, not a tap. So if you watch when it cuts the threads, it's orbiting around the hole, just like the single-row thread mill in Mike's first video (on the Mill/Drill)."


I didn't say it was a tap. In the quoted passage I was merely saying that the diameter of the portion of the tool that drilled the hole would have to be the diameter of the standard tap drill for that size thread, i.e. for a thread mill designed to make 1/2-13 the diameter would be 27/64". It would then drill the hole, move in again to countersink, then come down, move over and circle the drain to make the threads.