Speed, Feed and Tip tool selection

[Andren]

I need assistance in the theory of machining shafts (or hollow bars) with relative small diameters compared to its length. I need to profile the OD of a stainless steel rifle barrel with OD 32mm and ID 7.62mm and length 780mm on a CNC lathe. I'm not sure of the exact type of stainless in use and hope that anyone knowledgable in this field could comment on the appropriate machine tips, speeds and feeds required to turn down such a barrel to its profile.
What is the theory behind maching long shafts without getting chatter in the middle section? The one end is clamped in the chuck with the other guided in the hydraulic centre. the profile gradually tapers down from 32mm (130mm from one end) to 21mm (over the remaining of the 650mm length)

 

[Carthius]

Rifle barrel making is a very in depth process, and requires special tooling, processes, and materials. Whoever made this barrel put much time into the manufacture, and engineered it to be what it is.
Besides using extremely specialized equipment, and holding exacting tolerances, this barrel likely underwent some sort of heat treat, or temperment hardening. If you were to re-machine this part, you would not only risk mishaping, and damaging it, but also possible heat and stress damage from the machining process....which could be very bad for a firearm, and a marksman. Maybe a gunsmith could point you in the right direction. My advice would be to leave gun manufacuring to the pros. That's why they make the big bucks anyway....and also why that type of thing is so damn expensive.

 

[gbent]

Which side are you on?

 

[steveh]

I will agree with Carthius that barrel turning is a somewhat specialized type of process. It is done daily, however, by gunsmiths - many of whom have little formal training.
The typical grade for stainless barrels is 440C. The barrel is stress-relieved after gundrilling and rifling. It often needs straightening as well. As Carthius points out, you must be very careful or you will produce a useless barrel.
In general, what you want for turning barrels is the same thing you want for other parts with a similar slenderness ratio. You will need a small tool nose radius, lower then normal SFM, and as high a feedrate as you can manage that gives an acceptable finish. You also will have to use a tool with pretty good positive rake - if using inserts, buy something with a micrograin carbide and an upsharp shape.
Many people use some sort of adjustable rest to resist the tool's cutting pressure. This is not always easy since barrels are typically turned between centers (concentricity betwee I.D. and O.D. is a must).
Some people have had success on CNC lathes by more or less continuously varying the feed rate and RPM.
Overll, I would recommend that, if you are only turning an occasional barrel, that you buy pre-turned blanks from the manufacturer.
I hope this is of some help.
Steve

 

[Carthius]

I don't mean to tell anyone what they should, or should not do. I have been machining for some years now, and I love to tackle a challenge. I also own a few firearms, and I love nothing more than the customization and fine tuning of things I enjoy. However, a friend of mine lost half his hand and 60% of his hearing after performing a modification to the works of a high power falling block rifle. If he had consulted any gunsmith first, they would have told him not to. I gave him advice on fastening, and machine work. I don't want to give anyone bad advice. I do not mean to offend.

But if you choose to machine this barrel, here is my advice.
Use a lathe with a live center, or sub spindle. Before starting, put an indicator on the OD and turn it by hand to make sure it is true. Do this at both ends, and in the middle. If not true, softly 'bonk' it with a dead blow, while rotating it until it is true. Concentricity is important, as it will compound over such a length. Make sure the piece is tight and secure. I would use a carbide T&F tool of about 80 deg. with a .016 TNR. Smaller the nose, the less deflection youll have. But the 80 deg. will leave enough beef to get the job done. TiN coated is the way to go. If the barrel is stainless, you want your rpms and feeds a bit different than if it were some other form of steel. Machinery's handbook can give appropriate feeds and speeds for turning mtl's at specific diameters. Some tooling manufacturers also give recommended feeds and speeds for their cutters. Youll want to calculate a bit slower and lower. To avoid chatter, take off more per pass, at a slower rate. Work hardening will make cutting miserable. If possbile, use flood coolant. If not, brush cutting oil or soluble oil on while cutting, in front of tool path. There will be much deflection, so you will want to make several passes. You might need to add taper to the program to compensate for deflection. You might also need to change feeds and speeds part way through like steveh said. It would better if you had a setup part to try. I don't know if any of this helps, but if you want to talk CNC programming, drop me an email and maybe I can help.
Carthius@galaxy5.com