Why 29.5 degrees

All discussion about lathes including but not limited to: South Bend, Hardinge, Logan, Monarch, Clausing and other HSM lathes, including imports

Moderators: GlennW, Harold_V

JimGlass
Posts: 2281
Joined: Sat Jan 04, 2003 8:33 pm
Location: 40 Miles West of Chicago/near DeKalb
Contact:

Why 29.5 degrees

Post by JimGlass »

People often ask when threading why is the compound rest set at 29.5 degrees instead of 30 degrees? Well, the thinking is with the compound set at 30, it is possible for the right side of the tool to shave the right side of the thread.

With the compound set at 29.5 degrees, the right side of the tool shaves off the thread after each pass. Only the left side of the tool and very tip remove material. In shallow threads I don't think 29.5 degrees is an issue but that is what the "book" recomends. In my sketch the angle center line is shown at 25 degreesinstead of 29.5 to emphasize the point.

A quesion comes to my mind. What does a CNC lathe do about the 29.5 degrees. My guess a CNC lathe would plunge staight into the threads.
Maybe someone could explane that to me.

I did what I could with my infant knowledge of Solidworks to show what is happening with the 29.5 degree infeed. You actual result may vary.
Jim
Attachments
tool bit path when thread turning
tool bit path when thread turning
thread turning.jpg (33.16 KiB) Viewed 16212 times
Last edited by JimGlass on Sun Jan 01, 2006 5:02 pm, edited 2 times in total.
Tool & Die Maker/Electrician, Retired 2007

So much to learn and so little time.

www.outbackmachineshop.com
widlin1
Posts: 5
Joined: Thu Dec 22, 2005 8:22 pm

Post by widlin1 »

Jim I still think that if your tools is ground with no rake to an angle of 60 degrees and you feed the compound in at any angle less than 30 degrees your are pushing the right side of the tool into the work and causing it to cut on the right side more than if you fed in at 30 degrees where in principle it would just rub. If you were to make several spring cuts the final result with a 60 degree tool with no rake would be that both sides of the tool are touching the work forming a 60 degree thread. Now if you feed in at angle less than 30 degrees you are pushing the right side of the tool into the right side of the cut thread. Exaggerate the feed angle to 20 degrees and it is easier to see. If you feed in at an angle greater than 30 degrees your are pushing the right side the cutting tool away from the right side of the cut thread and the right side will have a stepped surface. I think that feeding in at 29.5 degrees just insures that both sides of the cutting tool are cutting and that one side is not dragging. A 29.5 degree or 20 degree or 15 degree feed all more closely approach feeding the tool in at a 0 degree (from the normal) feed which will evenly feed both sides into the work piece while a 30 degree feed will only feed the left side into the work piece.

Respectfully

Jeff
JimGlass
Posts: 2281
Joined: Sat Jan 04, 2003 8:33 pm
Location: 40 Miles West of Chicago/near DeKalb
Contact:

I stand corrected

Post by JimGlass »

Well Jeff:

It appears you are right. If the compound rest was set a "0", the tool would cut equally on both sides. Moving the compound rest toward the 30 degree withness mark, would remove progressively less material on the right side. At 30 degrees the right side of the tool would slide past the thread. Any angle greater than 30 degrees, the right side of the tool would move away from the right side of the thread with each infeed.

Therefore, at 29.5 degrees the right side to the tool would shave off a tad from the right side of the thread rather than clear the thread. Never really analysed this 29.5 degree thing before. Well Jeff maybe we both learned something today or should I say you taught me something.

Jim
Tool & Die Maker/Electrician, Retired 2007

So much to learn and so little time.

www.outbackmachineshop.com
Guest

Post by Guest »

Yes, Jim I agree, and thank you for your help as well.

Happy New Year.

Jeff
MikeC
Posts: 1613
Joined: Sun Sep 14, 2003 11:05 pm
Location: Birmingham, AL

Post by MikeC »

Back before I had even less of a clue about what i was doing than I do now, I tried cutting a few threads with the crossfeed. it would work, but chatter was usually a problem.
srgcraze

Post by srgcraze »

In CNC, the angles are pretty much irrelevant. The CNC lathe I use doesn't have a compound, of course. But the programming can make the tool do anything. Usually, the bit is progressed straight into the work, cutting both sides of the thread at the same time.

I've also tried to cut threads using the crossfeed only, just like a CNC machine does. Sharp cutter, small cuts, large tools, secure work-holding, usually not much of a problem. However, it works better for me using the compound set at 29.5. I think the problem has to do with rigidity and chatter.

One of the things about CNC is that everything is so rigid. In order to keep the tolerances where they need to be and to stand up to the rigors of moving large workpieces so quickly, the CNC machines are usually so very much more heavy and rigid than most manual machines you'll see. You can do so many things with a CNC that you couldn't attempt on a manual machine. Climb-milling, for example, is used so much more on CNC than a regular mill. You very seldom ever get any problems with chattering on a CNC lathe, but look at the size of the tooling and how secure they are held.

However, if you have an insert that's a little bit loose... you'll get the same choppy threads that you get on a manual machine that has a chattering bit.
Neilho
Posts: 69
Joined: Sun Jan 05, 2003 7:01 am
Location: Vermont,USA

Post by Neilho »

The CNC lathes I've used (2, to be exact, so I'm no expert) used a commercial thread cutting carbide insert, basically a form tool. Appropriate, when you think a bit about it, because the proper thread form has a rounded crest and root, which a plain 60deg V-tool can't make. So the commercial shop approach, as with other carbide tooling, is to buy the appropriate toolholder with a matching box of inserts, use the inserts and throw them away when they get dull. Very cost effective for making many parts with the same thread, but since nearly every thread series requires a different insert, a full range of threadcutting tooling quickly gets very expensive. Reading the appropriate section in the MSC catalog will give you a good idea how quickly! Fun reading, though.

neil
lees

Why 29.5 degrees

Post by lees »

Your question about CNC lathes is one that has many answers. For example, I own 2 CNC lathes that have programming with a threading statement (most languages do have a threading statement) that allows me to specify one of four different angles for infeed during successive threading passes. These different angles are used by the control to move the tool in the direction of the threading pass to simulate an actual angular move.
Whenever I program a 60 degree thread, I always choose the 29 degree option to perform the "wiping" action talked about in another post. The threads have been coming out fine using this angle.
D-R

Post by D-R »

I use a 30 degree infeed in my CNC's. The chips come off as nice short curls on the leading side of the cutter.

If possible a straight infeed should never be used. Straight infeed can give a slightly negative cutting angle on the trailing side of the tool.

Using the CNC's "canned" cycle for threading the amount of infeed for each succesive pass is automatically calculated. There're several options for this calculation. Number of passes to get to depth is one. My favorite is to specify depth of the first pass and the controller calculates each following path so the same amount of material is removed on each pass. There's an option for a final "spring" pass, just a repeat of the final pass with no infeed.

Incidently, I've noticed the recomended number of passes for each tpi of thread in carbide insert catalogs seem to be greater than hobby machinists might be inclined to use. One catalog I remember seeing a suggestion of using around 10 passes to cut a 20tpi thread.
Flim63

29.5 deg

Post by Flim63 »

The South Bend manual on thread cutting says this about the angle... If fed straight-in, the chips would not clear out well and tend to tear the bottom of the thread. Keeping the angle slightly less than 30 deg has the left edge doing the bulk of the cutting, but just shaving the right face for a very smooth surface, otherwise you risk having very small 'steps' on the right face.
NeilP
Posts: 2
Joined: Wed Jan 26, 2022 7:05 am

Re: Why 29.5 degrees

Post by NeilP »

I have always wondered about this angle business too, and have thought about it occasionally over the years, all the way back to my Ag Eng Colllege days in the mid 90's.

To plunge cut or go to the mythical 29.5 degrees etc..(for metric), why 29.5 and not 29 what happens if you go over 30..

I did know this , and every time I think about it..once every few years or so, I have to re learn it.

So seeing this thread and Jim's original sketch, I thought I'd follow his lead and draw a diagram with my infant knowledge of SketchUp :lol:

As soon as you see it, and see angles much greater than 30 degrees...IE 35 degrees and 75 degrees, it becomes blindingly obvious as to what is happening.

I now see it and will probably not forget it this time

As far as I see it now ANY ANGLE less than Half the thread angle is usable. All you are doing is moving more and more away from a plunge cut and cutting on the trailing edge less and less until you reach the half angle and push the toll down the face on each advancement, and 'stiff' the trailing face, and then get beyond the 'half angle' and then you start producing steps.

Blindingly obvious once seen in a picture.

I am leaving this picture here in case it helps it 'click' in someone else brain
Attachments
Screenshot 2022-01-26 at 12.37.28.jpg
Last edited by NeilP on Wed Jan 26, 2022 7:54 am, edited 1 time in total.
NeilP
Posts: 2
Joined: Wed Jan 26, 2022 7:05 am

Re: Why 29.5 degrees

Post by NeilP »

Zoomed in pics
Screenshot 2022-01-26 at 12.47.03.jpg
Screenshot 2022-01-26 at 12.48.35.jpg
Post Reply