What's new
What's new

Follower rests, and turning DOM tube

Scott70

Plastic
Joined
Sep 22, 2017
Hello all.
Im getting beat to hell on a job and could use some input.
My project is turning down 82" of 1.625 OD x 0.875 ID DOM tube. Final size is 1.577" Tolerance is roller +/- 0.0015. This is a turndown prior to final sizing on a grinder and hard chrome plating (at a different shop). Final product is a hollow hydraulic cylinder rod. I am running a TOS SN50c and I have about 60" between centers to work with. I have a follower rest and a fixed steady, as well as live center and a 3 jaw tailstock chuck. This is my first attempt running a follower rest. I have to mount my follower on the LHS of the carriage because my DRO scale is mounted on the RHS and it interferes. I can reach just past the follower if I use my compound. Im cutting the material in halves, about 45" from chuck to tailstock.
I tried using roller tips in the follower rest and as soon as I get about 8 inches away from the tailstock it sets up a chatter that I cannot get control over. My feed is 0.005 ipr, 0.01 DOC, 180rpm.

I bailed on that setup, and attempted to do it in thirds, about 30" from chuck to tailstock, with similar chatter issues. I bailed on the follower rest and managed to cut that section without chatter, but the surface finish is poor, I assume due to the low RPM, soft material and tiny DOC, but it will probably get the job done.

I have a set of solid (steel...? ) tips I may try, and I am considering ordering some bearing bronze to make solid tips out of.
I have read up on box tools, I like the idea and may attempt to build one, but the way i was set up was pretty much like a box tool, so I wonder if its a waste of time.
Any advice or insight would be appreciated.
Regards, Scott.
 
It is unclear if +- .0015 ia what you are trying to turn or the final grind dimension. If you are turning to +-.0015 over 80" in two or three shots you have your hands full. Getting the separate turns coaxial is a tough thing to do. I've no advice other than to say "ouch".
 
I made a tool to turn small dia but the same thing would work for larger dia stock.
I mounted a piece of plate on left of crosslide drilled and bored a bore true to spindle and pinned it so I could remove and replace keeping it true. Moved plate to mill and worked off of that bore to mount 3 bearings true to spindle. No chatter as long a bar as you want that fits machine. Zero chatter as tool is only 1/4 inch behind cut.
 

Attachments

  • IMG_0811.png
    IMG_0811.png
    4.8 MB · Views: 91
It is unclear if +- .0015 ia what you are trying to turn or the final grind dimension. If you are turning to +-.0015 over 80" in two or three shots you have your hands full. Getting the separate turns coaxial is a tough thing to do. I've no advice other than to say "ouch".
1.577" +/- 0.0015 is the size I am looking to hit. I am unsure of the final grind size. I'll be making a few calls today to see what I can learn.
 
We used to take steel shot and fill a inner tube closed off on the ends. Slip down in the pipe and get after it. With the follower rest in place, it does make a difference the position of the jaws. Some of the follower rest I've seen they don't place the jaws where they need to be. Don't tighten the tailstock so tight, just barely where you can turn the center by hand with drag.
 
I made a tool to turn small dia but the same thing would work for larger dia stock.
I mounted a piece of plate on left of crosslide drilled and bored a bore true to spindle and pinned it so I could remove and replace keeping it true. Moved plate to mill and worked off of that bore to mount 3 bearings true to spindle. No chatter as long a bar as you want that fits machine. Zero chatter as tool is only 1/4 inch behind cut.
Thats pretty cool, thanks for the inspiration.
 
Like previous posts, thats a centerless job. Yes, you can try all the helpers like several hundred dollars of low melting alloys, lead shot, sand, mix in scrap carbide inserts, and, at best, its still going to suck. DOM often turns poorly no matter how you do it. And the chrome shop probably wants to put the minimium chrome on the tube, so surface finish matters. You don't want any steel sticking through after final grind. I'd guess the final dimension is something just over 40mm so there is not much to work with.

If I really had to machine this part, I'd look at roller box tools for inspiration. All the really cool help methods depend on dead straight stock for starters.
 
Yeah, the chrome shop generally wants it a ground surface. The few shafts I've had chromed or re-chrome, they always wanted it ground before applying chrome.

Years ago, I used to send out tubing of various sizes we used for drill bars and had the OD ground down by a 1/32" before we did anything else to it.
 
Thanks for all the replies. It is appreciated. Gbent you are correct, final size is 40mm. It does need to be reasonably straight. I know thats a crap line, but theres a bit of guesswork going on with this one. The chrome shop is going to do a finish polish, they said they would take a few thou off, so the finish doesn't have to be a 16ra or anything. We're going to put about .008 worth of chrome on this shaft. I'm still hunting for a centerless grinder in western Canada, preferably Edmonton or Calgary if anyone knows anybody. The chrome shop doesn't want to grind all that material off so I'm looking for help with this one.
Regards
Scott
 
Hey Scott, I haven't had this exact combination of parameters, but I've turned lots of DOM and I find I need a small nose rad (.008) high rpm (I'd be trying for 750-1000 rpm for that dia) and a good cut. If possible, do it all in one pass. Also you might try feeding it up a bit. I find .007-.012 will get the chip to break usually. If you can't get it to break, that adds another layer of problems.
With a good insert, it's very possible. However. The length is the problem. I had a job recently which I posted here, long shafts in brass. I found bronze tips wear far too much. Constantly chasing the correct pressure. If you have three fingers on your follower, try bronze on the top one and roller bearings on the other two. As the others have stated, it's a bugger of a job. I would try both ways, steady in front and behind the cut. Although DOM is fairly round, you might find it works better with a freshly turned diameter.
Good luck
 
Hey Scott, I haven't had this exact combination of parameters, but I've turned lots of DOM and I find I need a small nose rad (.008) high rpm (I'd be trying for 750-1000 rpm for that dia) and a good cut. If possible, do it all in one pass. Also you might try feeding it up a bit. I find .007-.012 will get the chip to break usually. If you can't get it to break, that adds another layer of problems.
With a good insert, it's very possible. However. The length is the problem. I had a job recently which I posted here, long shafts in brass. I found bronze tips wear far too much. Constantly chasing the correct pressure. If you have three fingers on your follower, try bronze on the top one and roller bearings on the other two. As the others have stated, it's a bugger of a job. I would try both ways, steady in front and behind the cut. Although DOM is fairly round, you might find it works better with a freshly turned diameter.
Good luck
Some good information here, thankyou. I managed to get an acceptable pass last night, it held size quite well, finish was good enough the grinder shouldnt complain.
 








 
Back
Top