What's new
What's new

0-80 treadmill tool deflection

claya

Cast Iron
Joined
Aug 6, 2006
Location
california
Cutting some 0-80 threads in Inconel 718. 0.145" deep. Using a Harvey Single cut coated T-mill, 3/16 cut length. Narrow shank is only 0.028". How much tool deflection should I expect to comp for? Hole is cutting undersize, and not sure if we are getting work hardening or tool delection.
 
Coated = rounded edges, effect goes up (relatively) as cutter shrinks. Stiffness (of shank/connector to cutter) goes down exponentially with smaller diameter.

Use the shortest possible shank length of the largest diameter possible for the job, and I'd suggest here that you use an uncoated cutter. If you have the time, get custom threadmills made with a .150 cut length and a shaft OD maxed to within .001" of nominal minor diameter when at final size (but don't allow rubbing), UNCOATED.

It might be worth factoring in as large a minor diameter starting hole as will meet spec, while (again) increasing shank size to suit.

Yes, you'll go through more, but the robustness and freer cutting aspect will give you a more reliable outcome. Just figure out what your replacement schedule has to be. Oh, and be damn sure your coolant flow and pressure is as high as possible and aimed right to ensure constant chip flushing. Recutting 718 chips with small tools is insta-death to cutter edges!
 
Cutting some 0-80 threads in Inconel 718. 0.145" deep. Using a Harvey Single cut coated T-mill, 3/16 cut length. Narrow shank is only 0.028". How much tool deflection should I expect to comp for? Hole is cutting undersize, and not sure if we are getting work hardening or tool delection.

What Milland said on coated.

doing a job right now in SS using a harvey t slot cutter to do a counter bore as the bottom of a 4-40 thread .170 deep the cutter is .078 dia x .039 tall/width, the shank is around .032dia and 250 long I'm deflecting about .0005,
your thread mill shouldnt deflect that much in a 0-80 ive done 2-56 with single cuts on inco and I didnt get any deflection that I am remember, I got wear issues usually about every 2-3 parts.

if your running non coated carbide I would start at 60 SF you may have to goto 40
 
These parts needed to be done last Monday, so I don't really have the option of new tools. I have to use what I have. We are using the shortest shank possible. Harvey suggests 3-4 passes in Inco 718. At that many passes, the chips are basically dust.

Is the advantage of a single pass to eliminate work hardening? Scares me to be that agressive on such a tiny 0.028 shank. At a single pass are you running at 40sfm? What chipload? Climb or conventional cut?

Sent from my SM-G975U using Tapatalk
 
Last edited:
These parts needed to be done last Monday, so I don't really have the option of new tools. I have to use what I have. We are using the shortest shank possible. Harvey suggests 3-4 passes in Inco 718. At that many passes, the chips are basically dust.

Is the advantage of a single pass to eliminate work hardening? Scares me to be that agressive on such a tiny 0.028 shank. At a single pass are you running at 40sfm? What chipload? Climb or conventional cut?

Sent from my SM-G975U using Tapatalk

Does Mitsubishi or anyone else make a thread mill for this where it mills the hole from scratch (no pre drill). The end cutting helps stabilize the tool from deflecting and I've had very good luck in Titanium / similar in small holes
 
I hope you have near Zero run-out on your holder/tool assembly. I always seem to have to run much lower SFPM with small threadmills.
Have you attempted tapping it with real tapping fluid?
 
Does Mitsubishi or anyone else make a thread mill for this where it mills the hole from scratch (no pre drill). The end cutting helps stabilize the tool from deflecting and I've had very good luck in Titanium / similar in small holes

Mits has the Epoch D line that does this, but I doubt they make 'em this small.
 
What Milland said on coated.

doing a job right now in SS using a harvey t slot cutter to do a counter bore as the bottom of a 4-40 thread .170 deep the cutter is .078 dia x .039 tall/width, the shank is around .032dia and 250 long I'm deflecting about .0005,
your thread mill shouldnt deflect that much in a 0-80 ive done 2-56 with single cuts on inco and I didnt get any deflection that I am remember, I got wear issues usually about every 2-3 parts.

if your running non coated carbide I would start at 60 SF you may have to goto 40
Harvey engineering strongly suggested coated tools, and sent me 2 replacements. Supposedly better than the style >Rc28 we were using.

They also recommended trying 50% the recommended 70sfm to start. IF that does not work then use 25% sfm.. Since I only have 2 tools to destroy, and past zero time to get more, should I just START at 25%sfm? That would be 17.5sfm.. (~1519rpm @ 0.11ipm) So thats: ~18.9minutes per hole, single pass. We have 30 holes to do. (Be faster? to roll tap by hand, as some of the old schoolers have suggested)[emoji51][emoji19]. What would you suggest, given the above. I gotta get these parts off the machine.

Sent from my SM-G975U using Tapatalk
 








 
Back
Top