Best turning method regarding stress relief

[RSG]

Another question for the more experienced guys.....

I am turning some aluminum parts that require a large dia through hole and was thinking of trying a short cut where I mount the billets of aluminum on a rotab in the mil first and rough cut the center out using a 1/4" endmill, then mount it in the lathe to do the work as shown in the drawing.

My question is of a stress concern. In doing this will it distort the material prior to putting it in the lathe or will it be ok or should I just chuck up a standard billet and go the traditional way using a boring bar.

Let me know your thoughts.

[Russ Hanscom]

A hole saw or trepanning would be options; regardless, it makes sense to save the center slug and not turn it all into chips. Leave a little allowance for the finishing passes.

I would not expect any difference in stress regardless of how the center is removed.

[Harold_V]

Key to success in this scenario is to rough before doing any finishing. Even a very slender object can be held without distortion if pie soft jaws are incorporated.

I agree with Russ----it makes little sense to reduce the core to chips. However, trepanning would be far faster than using a rotab, which, under just the wrong condition, can result in a broken end mill when the cut meets the beginning end.

A robust trepanning tool should permit removing the core in a minute of cutting, or less. Sound will dictate when the cut is about to break through. Alternately, one can use a long travel indicator to determine depth. Stopping the cut and a tap with a hammer will generally remove the core without breaking the trepanning tool. A hole saw would not be the best choice, only because it lacks the ability to discharge chips adequately. Solve that riddle and they work just fine.

Harold

[RSG]

Thanks for the tip! So how do I make a trepan tool? Can I use a boring head and if so what type of cutter would I put in?

Thanks
RG

[ctwo]

I read the question somewhat different. I wondered if internal material stresses were of concern, such as if you final machine the OD, then hog out all the material in the center, will the piece distort because of those stresses and move the OD, for example?

[johnfreese]

I see an entirely different issue. It is very difficult to hold such a thin walled part without distorting it.

I think I would look at annular cutters to rough out the hole.

[ctwo]

Silly me, I just realized that Mr. Crispen recently machined almost this same part. Check out his youtube channel on how he did it. He used trepanning for the center. Apparently Mr. Crispen is a studying apprentice machinist at Rolls Royce.

[Harold_V]

I wondered if internal material stresses were of concern, such as if you final machine the OD, then hog out all the material in the center, will the piece distort because of those stresses and move the OD, for example?

How the part changes in your scenario may not be predictable, but it is almost certain the part WILL change. That's why parts that are critical should be roughed fully before any finishing cuts are taken.

I've experienced one incident whereby I had to rough, semi-finish, then finish before I could eliminate noticeable movement. The material in question was Delrin. It has a serious amount of internal stress, generally not uniform in nature.

The roughing operation should remove the vast majority of material, leaving only enough for finish cuts to permit total cleanup. With that in mind, it's important that roughed parts be held properly, so all features are in proper relationship with one another. If attention to that is not exercised, it's not uncommon for parts to not clean up.

Harold

[Harold_V]

I see an entirely different issue. It is very difficult to hold such a thin walled part without distorting it.

Not with proper soft jaws.

Harold

[Harold_V]

Thanks for the tip! So how do I make a trepan tool? Can I use a boring head and if so what type of cutter would I put in?

Thanks
RG

Regardless of one's choice of machine (lathe or mill), the tool geometry will be virtually identical, as the part relates to the tool the same way.

Think of such a tool as a parting tool. The chief difference is that you must address the right hand side of the tool, as it creates a radius in the part. Relief must address that radius. Because the tool is ground with a diminishing thickness due to the required geometry, one must start with a rather broad tool.

Chip control is critical. Extreme positive rake performs exceedingly well. The rake (in my instance) was created by grinding a deep, uniform chip breaker, allowing the chips to flow from the resulting groove easily. Best they are not directed back to the cut.

Early in my apprenticeship I had literally hundreds of pieces in which I had to remove the core. Aluminum, 1" thick, with a roughly 4" diameter finished bore. We started with approximately 6" square pieces of material, held in a four jaw chuck. Because the machine in use was robust (a 15" or 16" Monarch), I was able to remove the core in about a minute. The tool used was made of HSS, relatively wide, as it must be strong to withstand the heavy feed involved.

I recommend using a lathe, not a mill, unless you have a heavy mill at your disposal. The typical drop spindle mill doesn't provide the needed rigidity, assuming you're hoping to remove the core quickly. If you're not in a hurry and can tolerate lighter feeds, it certainly can work. I've done it with a boring head, cutting 300 series stainless with acceptable results. Lubrication was extremely important.

Harold

[RSG]

Thanks guys, this is why I love this site.....

Harold, after asking the question about lathe or mill earlier today I got thinking of some HSS I ground for a facing pocket on the lathe years ago. I pulled the tooling off the shelf tonight and with a bit of grinding did just what you mention. The blank is .75" x .75" so it's robust enough. I ground enough relief on the sides to accommodate the curve in the pocket. I just don't have enough rake though based on your post above so I will go back fix that. I'm not at that stage yet anyway but when ready I have 12 parts to do the same.

btw, you know I will be using my soft jaws

[Harold_V]

Nice to hear soft jaws are to be used. However, do take note that the cross section of your part is rather slender, so wide jaws may be required in order to eliminate crushing. You may have to make wide jaws that will clamp on 300° or more of the part to avoid distortion, but, rest assured, if you make the jaws large enough, you can hold the parts without ANY distortion. Piece of cake!

When grinding this tool, don't provide much relief on the left hand side. That limits the loss of support, and it isn't necessary, as the generated groove will provide the needed clearance. I'd suggest you limit it to a degree, maybe two, no more. Finish width of the tool? Depends a great deal on the rigidity of the machine. No more than ¼", and you may need to reduce it to less. Keep the over-all length as short as you can, to retain strength.

Harold