1st attempt at threadmilling. Any advice?

[RMagnusson]

I'm about to threadmill something for the first time and I'm kinda nervous. I'm always nervous trying new stuff on our mill, the spindle is SOOOO fragile.

 

My part verifies well, I will be cutting 5/16-18 threads .406 deep in 2024 aluminum w/ a 3fl 9 tooth threadmill. It kinda weirds me out that the .250 predrill hole is only .005 larger than the threadmill

 

I have the threadmill set to do 3 .02 spaced roughing passes, and starting at the top so it doesnt engage the whole tool at once. Feed set to 10ipm plunge @ 5ipm. My mill only has 3.5 hp and spindle speeds between 10k and 50k so I set the spindle at 25k to generate some power. Flood coolant is on.

 

Any advice?? I dont want to break a $150 threadmill, or a $1000 part, or a $10,000 spindle, or...

[Guest]

If it is an internal right hand thread it starts at the bottom and works up.

 

I alos would have opted for a smaller diameter tool for the 18 pitch thread, I like a "little" roominside of the part.

[Rick Henrickson 65]

you should be good to go! I usualy just do contour to control my lead in from the center of hole. and add a z to the G3 line = to the pitch

but either way should be good to go.

[Jaz]

I would mill it in one pass and from the bottom up. Maybe a flex pass if I saw any taper. 25,000rpm is plenty fast, 10ipm is OK for plunge if you have only a couple of holes to do, 5ipm is way slow. I would probably start with something like 12,000rpm and 30ipm (way conservative) and figure on cranking it up from there. If this is your first thread milling experience it can be scary. Dry run it, then run it in some wax or model board and finally in a piece of scrap aluminum to build confidence in the machine and cycle. You will like thread milling once you get comfortable with it. Good luck.

[?Mark]

For 5/16-18 you can go up to .265 hole dia (depending on the class...), so changing that could help.

Other than that, double check your numbers...

[connormac]

I'm with Mark. Take you ID out to .265. Cut your threads till there right by comp on thread mill. Then bring minor dia. closer to .257 till you start having trouble with gage.

[machtek]

I like to threadmill from the top down on right hand thread (G2) engaging only one tooth but I mostly cut hard steel. If you only have .005 clearance and you use 5 or 10 ipm the hole will be cut supersonic might only look like it wiggles a little and will take a super acurate machine to make a complete thread. Also if you engage all of the tool (bottom up) where are the chips of the initial cut going to go? just my .02

[TOOLMAN]

You need to start with at least a Ø.257 hole, this will decrease tool pressure. You will also need to get a smaller diameter threadmill for this hole. Ø.236 is max recommended for Ø5/16 thread regardless of pitch. Threadmill diameter is typically 75% of the major thread diameter or .3125 x .75 = .236. If you use a larger diameter tool your thread form will not be correct due to tool drag, although it is hard to see. Bottom up milling will wear the tool evenly across the teeth verses wearing out the first tooth with Top down. But, Top down can be fed much faster due to less tool pressure and deflection. For a RH thread its climb mill for Bottom up and conventional mill for Top down. We try to do without spring passes to lessen cycle time and tool wear.

[RMagnusson]

Wow, so many good replies.

 

So far I've:

Increased feed to 30IPM,

going to redo my predrill holes to .257-.265,

will inquire about another threadmill.

 

I'll try to mill it top down this time and if the mill doesnt load up too badly I'll try it from the bottom up.

 

..And going to tripple-check my numbers.

[Kelly Burns]

quote:

---

..And going to tripple-check my numbers.

---

Just smash the go button.

[Storkman]

Rman, send me your email addy. I might have some info you would be interested in.

[RMagnusson]

quote:

---

Just smash the go button.

---

Lol,

 

Terry, sent. Thanks.

[Storkman]

Ryan, you gots mail

[RMagnusson]

Replied.

[RMagnusson]

So I finally "smashed the start button."

 

It went ok I guess, for a first try anyway. Bolt wouldn't thread until I ran a hand tap through the 'threads.' Works fine afterwards, but I'm not really trying to just 'pre-tap' the holes.

 

The threads are too tight diameter wise. I am using .3125 for my major dia. Should I make it larger by a few thou?

[Guest]

use cutter comp and adjust it for proper size.

 

On an ID thread I draw the major diameter and chain that, then the operators use comp to dial it in

[Rick Henrickson 65]

comp the tool!

[Storkman]

Rerun it man, as many times as you need till it is dialed in.

[Storkman]

Ryan, I get with ya tomorrow on that info.

[Storkman]

you have mail again.

[RMagnusson]

Storkman, forgot to thank you for the threadmilling sheets. They have been a real time-saver. Thanks very much.

[Storkman]

My pleasure Ryan.

[dolphin1]

cut your feed to 19./20. IPM.

[RMagnusson]

I did that right before I ran it the first time (20 ipm). Pussed out I guess, haha, but I like how it sounded so I left it.

 

Thanks everybody.

[Randy Morton @ Clem Industrial]

How'd the cutter comp work for ya? The should always be the first bet. I would put comp in there even if you knew it worked....just in case. =]

 

Just curious why you can't just use a tap? Seems like an easy enough hole....