Threadmilling 17-4PH

[rogkick]

Hi folks,

 

Has anyone got any good insight on threadwhirling 17-4PH Stainless (1350).

We were machining sizes 4-40 and 6-32 with .05mm over the recomended drill size, but we still getting very sticky or tight threads with the gage.

In settings we are:

2865 RPM

180 mm/min feed

and using overcut as recomended by tooling guy of .03

 

Its a 2 toothed Threadwhirl, and we are cutting right hand top to bottom...so its conventional milling.

To get close to thread size we are setting our wear offset at .07, but I think its rubbing more than cutting, and hence the inconsistencies.

 

Would appreciate some thoughts. Thanks

[EX-wccprogrammer]

My thoughts? TAP

 

Small threadmills are finicky. I would tap those sizes.

[JAMMAN]

We tap everything under 1/2"

[rogkick]

My thoughts as well, and my next recomendation to be honest.

I think management might be afraid if destroying parts becasue of worn or broken taps though.

[Brando]

if you're going to tap them and if its feasible, use castrol moly-dee tapping fluid its always extended tap life on tough stuff for me, but a warning it does stink!

[David Colin]

I had great results in 15-5 PH with Horn cutters 3 teeth (from CPT) and Widia cutters too (4 teeth if i remember). Better is to machine from top to bottom but you can choose left hand cutter for climb milling.

[The_kid]

if you have to mill it try bottom to top climb milling. coolant is your friend. if possible take it all in a single pass avoid "spring cuts" this will only dull the tool and make the next part worse. least in my experiance though I have only done 5/8 -18. let us know what you find works best.

[djstedman]

We have a job with 2-56 threads in 13-8 that we threadmill never could get them to tap to save our.. well anyhow..

 

We use Vardex threadmills and use thier free app to choose the threadmill and generate the code.. as well as feeds and speeds.. on that particular job we are getting 1000 holes or so out of one threadmill never have a broken tap either..

 

I beleive that job is a class 3 thread as well.. based on my experience in 13-8, 15-5 and 17-4 I would say definitly look into Vardex for threads ..

 

Just checked it out for a 4-40 thread btw and should be about

 

9664 RPM thats about 210 SFM

 

Helical lead in at about .88 IPM

 

Followed by the actual threadmill passes at 6.28IPM

 

We generally use two passes one at 70% of thread depth and one at finish since we get more consistent results that way and longer tool life..

 

Usually we see a bit of wear in the first few parts as the tool 'wears in' and then it settles in and cuts consistently for days..

[Rotary Ninja]

We are currently running hardened 17-4 PH and using 4-40 form taps with good results for the last three or four parts. I can't remember the hardness but it's some pretty tough chit. We snapped off a number of taps before getting it down. So far I think the form taps are winning over cut taps. We are using Guhring .104" diameter drills running at 1525 RPM and 3 IPM with a .050" peck. Then the tap is running .320" deep at 10 IPM/400 RPM. We are rigid tapping. I cannot remember the brand of tap right off hand, but I will let you know on Monday if interested.

 

I have never heard of the Vardex tools. Thanks for the info. I will look into it.

[Redfire427]

Vardex threadmills work great in 17-4 PH. I always cut bottom to top ( climb milling ) with multiple light cuts on small thread sizes. Flood coolant will help.

 

Carmen

[The_kid]

its probably a baladex form tap. they're very nice for parts that require getting close to poking through the bottom. they do tend to pull up the lead thread.

[Rotary Ninja]

I am not sure what he put in the machine today. I was busy with another pain in the butt part.

[rogkick]

Thanks for all the suggestions.

I did reference the ISCAR thread-milling program...it gave ridiculous speeds and feeds haha, but at the $$$ cost of threadwhirls, we toned it down a bit for the sake of a few seconds on a long cycle time.

Running it too slow reduced the chip load so we settled on:

5000 rpm

440 mm/min

arcing on at about 120 mm/min

2 Passes - 75% and 25% for the finish

It was critical to maintain the shortest overhang possible, so to do this we used two tools depending on what reach we need. The tool with the longer overhang however does cut undersize, but we reckon we can sort that with an improved backend tooling.

[MrFish]

Try slowing your feed rates a bit too. There is alot of engagement going on with small threadmills in small hole diameters.