What's new
What's new

Trepanning a 7.500 inch hole in stock

Zahnrad Kopf

Diamond
Joined
Apr 5, 2010
Location
Tropic of Milwaukee
Have to cut some large bores in relatively thin cross section parts and am considering trepanning them. The issue is that I have never trepanned anything near that size so I don't even know if it is a feasible option at this point. Material is 9" OD 4150 ( 0.6" thick ) that needs to finish at 7-3/4" ID. I was thinking to trepan 7.65"-7.70" and finish with a boring bar.

Reasonable? Or no? Tooling recommendations? Would be doing this on a 15HP turning center with 8-1/4" chuck. Have oversized pie jaws for it already. Set up for 1" sticks and 1.5" ID blocks.

Thanks.
 
Have to cut some large bores in relatively thin cross section parts and am considering trepanning them. The issue is that I have never trepanned anything near that size so I don't even know if it is a feasible option at this point. Material is 9" OD 4150 ( 0.6" thick ) that needs to finish at 7-3/4" ID. I was thinking to trepan 7.65"-7.70" and finish with a boring bar.

Reasonable? Or no? Tooling recommendations? Would be doing this on a 15HP turning center with 8-1/4" chuck. Have oversized pie jaws for it already. Set up for 1" sticks and 1.5" ID blocks.

Thanks.

I know this isn't the answer you were looking for but throw it on your mill, clamp it down and slot it out :)
 
I have done something like that, except material as 1/4" CRS. I used a single point tool. The biggest problem was when the disk is cut away, it tended to fall into the chuck, jamb against the tool, and rip the work out and course messed up the tools. I solved the problem by placing a spring loaded rod against the center so that when the center was cut away, the rod would hold the disk to the chuck until I could retrieve it.

Tom

Edit:- As dstryr mentioned I did that before going to the lathe. The reason I changed was a problem was speed and short tool life. I had 100's of these parts to do.

T:-
 
Material is 9" OD 4150 ( 0.6" thick ) that needs to finish at 7-3/4" ID. I was thinking to trepan 7.65"-7.70" and finish with a boring bar.

Reasonable? Or no? Tooling recommendations? Would be doing this on a 15HP turning center with 8-1/4" chuck. Have oversized pie jaws for it already. Set up for 1" sticks and 1.5" ID blocks.
Sure, muy no problemo, babe. You didn't say how many but if it's less than 25, this cheapskate would grab a 1" square of high speed steel and hand grind the tool. Then I'd trepan the slugs out of all your blanks as a first op. In fact I'd probably trepan to about .005" away from breaking through then wack them out with a hammer. That's a touch safer for you, the machine, and the part than having a 6" chunk of steel clonking around in the lathe. Usually the center plug just falls down but all it takes is one ...

Instead of a totally blunt nose, I'd grind the front of the tool with a touch of an angle. That seems to work better for me ... gets the chip out of the way better, doesn't chatter as easy. And I use a bunch of top rake with a hook behind it to curl the chip. 4150 is not going to want to break, another reason to first op it - get all that boingy sproingy stuff out of the lathe.

If you decide to spend the big bucks instead, go Manchester. Good stuff.
 
I have done 6" disks out of 14mm steel plate on a small 11x24 kerry so i see no reason to shy away. Hss tool for one-offsies or grooving/trepanning insert tooling if you got more than a few.
 
Something like an Iscar HFAER 180C-6T32 with an HFPR insert on a stick tool, or a HFAIR on a 1.5" round bar would be my choice. There are other similar tools in the catalog for that application. The trick will be managing the slug to keep it from jamming. On manual machines we used to trepan until it was paper thin then stop the spindle and knock the slug out with a hammer. Maybe a drilled hole with a bolt to hold the slug in place? Does your lathe have a low gear or is it one speed?
 
I know this isn't the answer you were looking for but throw it on your mill, clamp it down and slot it out :)

Hey Deeno,

No way, no how. WAAAAaaaayyyyyy too slow, comparatively. You're just a hater on the roundy-round stuff, tho. :D

The biggest problem was when the disk is cut away, it tended to fall into the chuck, jamb against the tool, and rip the work out and course messed up the tools.

In fact I'd probably trepan to about .005" away from breaking through then wack them out with a hammer.

^^ That's what I would do... stay away .005-.010" and then whack em with a hammer or mallet.

Thanks boys. This is exactly what my plan was/is. We do this all the time with mill parts too so it's a natural thing for us. Keeps the heart rate much more agreeable.

I will admit that I've been vacillating between doing exactly what EG suggests and using a Manchester type. On the one hand, I've got the lump of HSS sitting right here.... on the other hand, I nice, ready insert would be kind of keen....

Decisions, decisions...

I'm guessing that at this size, something on the order of 50-100 RPM and 0.002" - 0.003" IPR would be the ticket?

Thanks, Gents. Grab a pint, on me.
 
I might be way off base but could you use a hole saw 7.5"? It should capture the slug as well
 
Last edited:
Sounds like this is worked out. Just to add that I have a trepan tool that I use on a 50 taper mill to cut out 10" slugs. About the same cycle time as it would be on the lathe.

FWIW

Bill
 
Sounds like this is worked out. Just to add that I have a trepan tool that I use on a 50 taper mill to cut out 10" slugs. About the same cycle time as it would be on the lathe.
FWIW
Bill

Deano ( Dstryr ) put you up to this. Didn't he?

Damn you...

thinking-emoji1.jpg
 
Their distribution in the US currently stinks, but the larger Valcut tools are ideal for this. Use the 6mm or 8mm tools, if you can find them.
 
Get them laser cut... :stirthepot:

Humor aside, I wouldn't simply for not wanting to deal with the HAZ left in the 4150. In short, eff that. However, I did consider w-jetting. The problem is that even at reasonable cost for either of those, they just cannot compete with the simplicity and cost effectiveness of trepanning them. As has been pointed out - even the meager HSS bit makes this simple enough. What do you think even laser or w-jetting 15 - 20 pieces would cost? And then, there is the lost time of back and forth transit, plus processing. Even at 0.002" IPR, that's only two hours for 20 of them. So two hours of electric and payroll, + tooling versus someone else's processing charge plus shipping ( x2 ). Makes trepanning look heroic.
 
I used a face plate instead of a chuck. I mounted the part with a 3/4" thick mdf for backing( medium density fiberboard) which is smooth and flat. Before mounting the work I brushed shellac on the mdf, this kept the piece from falling on the ways. Alcohol loosens the shellac when done. The waste was screwed to the mdf in 6 places.

The part was 6061 aluminum and 6.125 diameter .375 thick when done.
 
^^ That's what I would do... stay away .005-.010" and then whack em with a hammer or mallet.

Another way to solve that problem is to leave .010"-.015" (whatever you're comfortable with or what your stock thickness
allows) and then just flip the part in the chuck. When you make your facing cut the slug drops out without causing any
problems. Haven't done much trepanning lately but I have used a good Iscar insert style tool in the past and it worked
very well...
 
There's not going to be much HAZ on a nitrogen cut part with a modern 4000W fiber laser. Locally I would pay a $150 lot charge for cutting 20pcs but there are 5-6 shops I could job it to in my area under 15mi away. I mill the laser cut edge on 4130 parts all the time. For a lathe part you just need to use an insert with enough lead angle that the tip gets under the HAZ to peel it away from underneath. Your location may may not make the economics work.
 








 
Back
Top