Milling a helix

Discussion on all milling machines vertical & horizontal, including but not limited to Bridgeports, Hardinge, South Bend, Clausing, Van Norman, including imports.

Moderators: Harold_V, GlennW

hanermo
Posts: 44
Joined: Tue Oct 01, 2013 5:47 am

Re: Milling a helix

Post by hanermo » Thu Jun 14, 2018 1:31 pm

So the feed rotates the blank, via gearing, thus making the feed/rev constant, no ?
While the feed advances at a given steady rate.

Excellent job. Imo.

You mentioned full-depth cutting.
Did you actually cut the full depth of the helix in one pass ?? !! ??

At what speed in rpm if I might ask..

Harold_V
Posts: 17199
Joined: Fri Dec 20, 2002 11:02 pm
Location: Onalaska, WA USA

Re: Milling a helix

Post by Harold_V » Thu Jun 14, 2018 3:52 pm

hanermo wrote:
Thu Jun 14, 2018 1:31 pm
So the feed rotates the blank, via gearing, thus making the feed/rev constant, no ?
While the feed advances at a given steady rate.
Correct!
You mentioned full-depth cutting.
Did you actually cut the full depth of the helix in one pass ?? !! ??
Finish cut will be full depth, yes, but note that this part has yet to be machined, as I'm still building the setup. It's rather involved, and I'm building something that will be useful for other projects, assuming I ever have need.

My plan is to use a 3/16" end mill for the cuts. By tilting the head of the mill I can establish the proper angles, so while I will take full depth cuts, that's only after having roughed the thread to full depth, which will be done in multiple passes, each ever deeper. First pass, at this point, is intended to be with the head vertical. I'll rough to full depth, than begin the process of forming the 14°30' flank on one face, likely the trailing edge. The last setup will be the opposite flank. As I will be fitting the thread to the worm, which displays a small amount of wear, the resulting thread (worm) form will be somewhat wider than the original. I'll post again when I have the entire setup made, including the worm machined to fit the setup. I intend to leave material for finish cuts after the form has been machined, to ensure I have the bearings concentric with the worm.
At what speed in rpm if I might ask..
At this point I can't answer that. In regards to spindle speed, I will likely rough with a HSS end mill, but I have a few new 3/16" carbide, which I will use for finish passes. I want to use a new cutter so I can generate the best possible finish on the worm, to limit future wear. I'll likely polish the worm before installing, to improve surface finish, which should be quite good. In regards to feed rate, I may never be able to provide useful information, as there's no indicator of speed, just a dial with marks 0-10. I'll pick a speed that provides a light cut, and yields the best finish. Being trained as a manual machinist, speeds and feeds are generally selected by instinct, then fine tuned by observing chip color and other characteristics. It's a little different from CNC, where one must enter hard numbers.

H
Wise people talk because they have something to say. Fools talk because they have to say something.

User avatar
NP317
Posts: 1493
Joined: Tue Jun 24, 2014 2:57 pm
Location: Northern Oregon

Re: Milling a helix

Post by NP317 » Thu Jun 14, 2018 10:20 pm

Using a roughing cutter for that first set of cuts?
Might make the process go faster and easier.
~RN

Harold_V
Posts: 17199
Joined: Fri Dec 20, 2002 11:02 pm
Location: Onalaska, WA USA

Re: Milling a helix

Post by Harold_V » Wed Jun 20, 2018 1:30 am

I finally have the setup made, and will now turn my attention to a procedure that will allow me to mount the gear (100 tooth) to the resulting part in such a way that it won't interfere with the final machining (after the worm is machined). if you're interested, here's a few pictures.

I'll begin with the right side of the setup. As table movement results in rotating the worm, one loses the ability to feed in either direction on that axis. To allow feeding, I made a ½"-20 screw which attaches to the base plate of the indexing head, which, in turn, is firmly bolted to the main base plate. By loosening the hold down bolts for the main base plate, the screw can be turned to advance or retract the entire setup, which becomes the feed mechanism. As the base is keyed to the table, it doesn't lose registration. If a fine movement is required, I'll simply use a long travel indicator placed against the setup so I can make precise movements. The 20 pitch thread allows for a reasonably fine adjustment without much effort.
Worm machining setup1.JPG


I wanted to ensure that the resulting setup would be useable for other projects, so I made the drive shaft telescopic. A short section of a 5/16" square hole sleeve was faced, then a bore created to locate the sleeve inside a short piece of 3/8" black pipe. A quick silver solder job and it was ready to accept the 5/16" square C1018 shaft I cut from a length of material I had on hand.

Had to drill and tap set screws in the flex sockets on each end of the drive, which proved to be rather challenging for the right side. It was hardened much deeper than the opposite end socket, and difficult to tap as a result. Broke one tap, but finally achieved success by persistence. Entering the hole was no problem, but the breakout side was impossible, so I machined a dog point on the set screw, then drilled a matching hole in the piece of pipe. Turns out to have been a good thing, as the set screw binds nicely as the dog point seats. Where the flex socket attached to the gear, I simply relieved the hole with a small mounted wheel (3/8" diameter) before tapping, to eliminate the hard surface. Worked a charm!
Worm machining setup2.JPG

This is how the setup will look, aside from not having the gear mounted yet, when the worm is machined. I'll take a picture of that when I start the process, and report on my success (or failure) after I make the attempt to machine the worm. Not being cocky (I've been away from my machines for a longer time than I was on them when I ran them for a living), I purchased enough material to make two worms. I'm hoping I don't need the extra piece.
Worm machining setup3.JPG
H
Wise people talk because they have something to say. Fools talk because they have to say something.

User avatar
Dave_C
Posts: 955
Joined: Mon Apr 21, 2008 10:34 am
Location: Springfield. MO.

Re: Milling a helix

Post by Dave_C » Wed Jun 20, 2018 2:32 pm

I purchased enough material to make two worms. I'm hoping I don't need the extra piece.
You'll only need it when you don't order the extra piece! :wink: At least that is how it works for me.

Owesome project, looking forward to seeing the finished product.

Dave C.
I learn something new every day! Problem is I forget two.

dorin
Posts: 533
Joined: Thu Nov 28, 2002 5:24 am

Re: Milling a helix

Post by dorin » Thu Jun 21, 2018 9:07 am

This looks really really cool.
I hope one day to have a tiny percent of the skill required to do cool things like this.
www.chaski.com

Harold_V
Posts: 17199
Joined: Fri Dec 20, 2002 11:02 pm
Location: Onalaska, WA USA

Re: Milling a helix

Post by Harold_V » Fri Jun 22, 2018 3:06 am

Thanks, Mike. I appreciate your comment.
I can't see any reason why you can't achieve similar results. If you have a good imagination and have the equipment, all it takes is the desire.

Much of the issue of building most projects is having the ability to see, in the mind's eye, what you want to accomplish. From there, you simply make what it takes to get it done. This entire project was built that way---starting with a base plate that would fit the table and provide the necessary features of keying (so it self locates) and registering the proper location for the main gear. Once that was solved, the rest was easy.

Harold
Wise people talk because they have something to say. Fools talk because they have to say something.

RSG
Posts: 963
Joined: Fri Feb 04, 2011 9:59 am
Location: Ontario, Canada

Re: Milling a helix

Post by RSG » Fri Jun 22, 2018 9:53 am

Hell of a lot of work but brilliant Harold. It seems many things are that way in the shop, were you spend more time making the fixture than the actual part.

I agree on the "minds eye" ability. It seems a lot of guys I know don't have it. It's vital to the work I do.....
Vision is not seeing things as they are, but as they will be.

User avatar
warmstrong1955
Posts: 3146
Joined: Thu Mar 18, 2010 2:05 pm
Location: Northern Nevada

Re: Milling a helix

Post by warmstrong1955 » Sat Jun 23, 2018 10:31 am

I'm looking forward to seeing this set up in action! Extremely clever!

As far as fixtures, I find that designing & making all the jigs and fixtures to build something, more fun than actually building the parts. Sure....the first one, or few is fun, but after that, making more & more is booooooorrrrrrring!

:)
Bill
Today's solutions are tomorrow's problems.

Harold_V
Posts: 17199
Joined: Fri Dec 20, 2002 11:02 pm
Location: Onalaska, WA USA

Re: Milling a helix

Post by Harold_V » Sun Jun 24, 2018 4:42 am

With the helix milling fixture completed, I turned my attention to the raw stock (Stressproof) from which I would make the needed worm. The ends of the resulting shaft provide the bearing surfaces on which the worm is supported, so concentricity was important, not only the ends with one another, but with the worm. The long end was fitted to a soft collet bored to 1.040" diameter, which allows for finish machining after the worm is machined. The short end was turned to 1.125", which allowed for the 100 tooth gear to be mounted. This end was supported by the tailstock while the worm was machined, so it was center drilled. To mount the gear, It was bored accordingly, then a couple 1/4"-20 holes drilled and tapped to match the holes in the flanged adapter, which was also bored to the same diameter. A 3/8"-16 square head set screw was used to affix the flange to the shaft, clamping on a small flat machined to assure positive drive and to prevent issues in removing the flange after the helix was machined. It all performed as expected.

Because the gears that drove the worm were near the cutter, a simple shield made of some scrap aluminum fascia material was made, to prevent chips from entering the gears. It served admirably well, and took just a couple minutes to fabricate. It was fastened to the gear bracket with a pair of small C clamps.

While the flanged adapter is mounted on the opposite face, the large gear (100 tooth) and the 32 tooth driver gear are seen here, mounted on the end of the worm shaft:
Worm4.JPG
You can see the chip deflector in this picture:
Worm3.JPG
The helix was roughed with various end mills, each progressively smaller. For roughing, the mill head was kept vertical. I started with a 5/16" three flute and ended up with a 3/16" with a small corner radius, to avoid sharp corners in the helix. It was taken to full depth, but narrow, allowing for finish cuts at the proper angle. Here's a picture of the helix being roughed. Sorry for the slightly blurry picture. I could have taken another had I known.
Worm2.JPG
Once roughed, the head of the mill was tilted to 14° 30", the angle checked with a vernier protractor. One side was roughed at the angle using the 3/16" HSS end mill, then finished with a solid carbide end mill, which also had a small radius applied to the corners. With the angle cleaned up, the head was tilted to the opposite side and the worm taken to finished width.

Here's a picture of the finish cut, taken while in motion:
Worm5.JPG
The end result was better than I had hoped, as the carbide end mill performed well beyond my expectation. The finish is very acceptable, and I'm well satisfied with the performance of the entire setup. I am pronouncing the concept a complete success.

The shaft will now be finish machined, to fit the bearings. I'll post another picture when it's finished.

H
Note: By left clicking on the images, a larger picture is shown. An even larger one can be displayed by RIGHT clicking on the images.
Wise people talk because they have something to say. Fools talk because they have to say something.

User avatar
GlennW
Posts: 6657
Joined: Sun Apr 15, 2007 9:23 am
Location: Florida

Re: Milling a helix

Post by GlennW » Sun Jun 24, 2018 5:56 am

Harold_V wrote:
Sun Jun 24, 2018 4:42 am
The end result was better than I had hoped

I had no doubts!
Harold_V wrote:
Sun Jun 24, 2018 4:42 am
...as the carbide end mill performed well beyond my expectation.
I'm curious as to why you had concerns about the carbide end mill. I find them to be much sharper and provide a much better finish than HSS end mills.
Glenn

Operating machines is perfectly safe......until you forget how dangerous it really is!

User avatar
Dave_C
Posts: 955
Joined: Mon Apr 21, 2008 10:34 am
Location: Springfield. MO.

Re: Milling a helix

Post by Dave_C » Sun Jun 24, 2018 1:37 pm

I find them to be much sharper and provide a much better finish than HSS end mills.
I'll have to agree with Glenn, I've gone to all carbide end mills which are all made for specific purposes. 3 flute with special coatings for aluminum and 4 flute and a different coating for steels.

I had some .200" slots to cut .500" deep in aluminum. Made with .125" carbide end mill, 2700 RPM, a little WD and shes good to go.

Not intended to get the thread side tracked so congrats Harold on the setup and the finished product. That's some pretty out of the box thinking! (The differance between a machine operator and a real machinist)

Dave C.
I learn something new every day! Problem is I forget two.

Post Reply