Cut tap, form tap or threadmill??

implmex · Aug 7, 2020

Good morning All:
I have a project I've been working on and some of the parts are 17-4 PH.
Attached is a picture of two of the parts, and I have quite a few more to make.
They will eventually be heat treated to condition H900...the stock is currently solution annealed (condition A).

The problem is with the tapped holes; they are M1.6 x 0.35 and they were put in with a cut tap.
They were the Devil's very own to tap...3 mm deep full threads because a shoulder bolt threads into these and is located by the recessed pocket you see.
So all has to be concentric (as good as I can realistically make it).

Since I'm gonna need to make these in respectable quantities (dozens) I need to find a better way that doesn't clinch my sphincter quite so hard as these ones did.
The cut taps (I tried two different brands...no name from McMaster and Taylor taps) did not run in easily...I had to squeak them in an eighth of a turn at a time and it took forever as you can imagine.
I helical milled the bores first (after pre-drilling them) so I'm down to 65% of thread already which is my lower acceptable limit.

So all you production threading gurus...what say ye?
How many will I have to trash to dial in the process?
Can I realistically threadmill that deep? Can I do it on a 20 year old beater Haas Minimill with a 6 K spindle?
Should I try to get forming taps?
Should I get better cut taps like Natchis or Guhrings?
Is this amount of pain just what I need to live with tapping condition A 17-4 PH?

Thanks in advance.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

DanASM · Aug 7, 2020

I have had great luck with TiCN for taps. I tried Ghuring. 5-40 taps .300 deep all day long 20k so far.

I have machined that same material in condition A quite a bit years ago. Still have some on the shelf.

Dont dwell anywhere when drilling and go all the way down in 1 pass. I tried tapping the hole twice with cut taps and was still reaking them due to them being so thin. too much torque. Watch for work hardening.

Do not "re-cut" anything. try not to peck drill unless you can do it without any dwelling. Might be able to get away with 1 rev dwell.

Condition A will be gummy and form tapping should work great. It will harden as soon as it is formed and the threads get stronger even with 60% threads

ChipSplitter · Aug 7, 2020

BALNH · Aug 7, 2020

I would lean to form tap. I’d drill with OSG gold drill. Annealed is pretty soft and gummy like 304.

Booze Daily · Aug 7, 2020

I always form tap 17-4.

Mike1974 · Aug 7, 2020

Can't speak to 17-4, but we form tap 0-80 in brass and aluminum, we only break taps when someone has flubbed a touch off or drill size... . 0-80 would be about the equivalent of the M1.6 diameter.

edit: If you haven't looked yet, Harvey makes a thread mill that will do that small and deep, but only single point.

Winterfalke · Aug 7, 2020

I did one job tapping in 17-4 annealed with a cut tap, I would look for any other possible option including CBN dentures on a tiny beaver before I tried it again.

Delw · Aug 7, 2020

implmex said:
Good morning All:
I have a project I've been working on and some of the parts are 17-4 PH.
Attached is a picture of two of the parts, and I have quite a few more to make.
They will eventually be heat treated to condition H900...the stock is currently solution annealed (condition A).

The problem is with the tapped holes; they are M1.6 x 0.35 and they were put in with a cut tap.
They were the Devil's very own to tap...3 mm deep full threads because a shoulder bolt threads into these and is located by the recessed pocket you see.
So all has to be concentric (as good as I can realistically make it).

Since I'm gonna need to make these in respectable quantities (dozens) I need to find a better way that doesn't clinch my sphincter quite so hard as these ones did.
The cut taps (I tried two different brands...no name from McMaster and Taylor taps) did not run in easily...I had to squeak them in an eighth of a turn at a time and it took forever as you can imagine.
I helical milled the bores first (after pre-drilling them) so I'm down to 65% of thread already which is my lower acceptable limit.

So all you production threading gurus...what say ye?
How many will I have to trash to dial in the process?
Can I realistically threadmill that deep? Can I do it on a 20 year old beater Haas Minimill with a 6 K spindle?
Should I try to get forming taps?
Should I get better cut taps like Natchis or Guhrings?
Is this amount of pain just what I need to live with tapping condition A 17-4 PH?

Thanks in advance.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Thats a tough hole to do in 17-4
the minor is max 1.321 mm or .052 - 1.221mm or .0481 its about the size of an 0-80 american.
I use yamawa YMW or emuge cut taps. I never did one that small in 17-4 or 15-5 materials smallest I went was 2-56. make sure you use lots of tapping fluid union butter field works best then the emuge stuff. the other popular shit dont work near as good.
that minor will need to be as close to max as you can go and the it must be perfectly straight.
form tap might work better in that small of thread, I use cut taps in 0-80s for steels alum with no issues but I dont know about the 17-4 as its a tad gunny before heat treat.

on the 2-56 ones I did in 17-4 peck tapping does help but your taps need to be sharp. we use spiral flute ones.
if you can find a thread mill that small I would try it out your old haas with 6k will be fine. Harvey tool may had one they have some great small tooling. we use the small key cutters for reliefs on the bottom of some blind holes(.055 dia) and they work and last a very long time.

1953chevB · Aug 7, 2020

what style of taps are you using? plug tap , starting tap,
also add two more suggestions,
part of the issue it's annealed condition, heat treat raw stock before machining to H1150 24-30HRc hardness, perfect machinability hardness.
anneal and soft parts gummy and don't cut well, then reheat treat after final machining to H900

second is to use tapping oil,

2outof3 · Aug 7, 2020

Machine the H900 material and then it is a matter of the right machine for the job. If the taps are not working, you can thread mill.

gregormarwick · Aug 7, 2020

I also pretty much exclusively form tap 17-4.

I also go to great lengths to avoid machining it in condition A - it's horrible shit to machine. Machining your parts in H900 should pose no problem, it form taps just fine even though it's a bit harder to drill.

1953chevB · Aug 7, 2020

I don't agree for something this small
Will be Breaking drills and taps
At My first post. This was was taught to me by the owner of ACR, he is gone now 40 years ago. ACR is now triumph gear. Go figure.
I be doing exactly that for ever job.
Cost heat treating is cheap.
Machining will pay for it.
edit:
FYI H900 = 40-47 HRc if it gets above 44 your going to have a rough time of it

mhajicek · Aug 7, 2020

I always cut my 17-4 in the hard, and threadmill everything, but my parts are always low quantities. 30 pc is a long run.

1953chevB · Aug 7, 2020

mhajicek said:
I always cut my 17-4 in the hard, and threadmill everything, but my parts are always low quantities. 30 pc is a long run.

but how big of parts? these are tiny, small drills and taps snap easily, just look at it and it will pop.
bigger parts where reasonable beefy tooling that is rigid, yes it can be done, but these are tiny.
but hey that's why we are here and we learn from each other, so any thing is possible , with the right
tooling and procedures.

litlerob1 · Aug 7, 2020

Roll them. I build a lot of small parts in 17-4. In a lot of different conditions. And 90% of the time I'm good with it. The exception to it is when I'm dealing with small chips. Small hard chips in 17-4 is a killer. So I would roll them.

R

mhajicek · Aug 7, 2020

1953chevB said:
but how big of parts? these are tiny, small drills and taps snap easily, just look at it and it will pop.
bigger parts where reasonable beefy tooling that is rigid, yes it can be done, but these are tiny.
but hey that's why we are here and we learn from each other, so any thing is possible , with the right
tooling and procedures.

Threads down to 0-80. Some parts tiny, some just small. Tight cutter runout is key.

litlerob1 · Aug 7, 2020

Don't take it wrong, I'll Threadmill basically everything. The problem I see, is that tiny Threadmills are single point, so you'll end up with stringers down in your hole. And tiny chips from 17-4 can lick nuts. It'll be a battle.

R

DanASM · Aug 7, 2020

litlerob1 said:
Don't take it wrong, I'll Threadmill basically everything. The problem I see, is that tiny Threadmills are single point, so you'll end up with stringers down in your hole. And tiny chips from 17-4 can lick nuts. It'll be a battle.

R

I just discovered form taps this past year. My dad says the ones he used to see years ago and the old ones in our tool crib dont have a relief channel ground in. The small ones were hard to grind a relief yourself and they had a hydraulic effect when used. Holes had to be much deeper to compensate for this.

I can see chips being a problem. The chips will workharden and then you will re-cut them. breaking cut taps. I run these form taps in screw machines with oil and I can run thousands. I usually break the taps on accident from bumping them (operator error). I have gotten about 15000 parts with 3 form taps. The 3rd is still in it now.

Condition A or annealed is what most of my material is. Its what my machines like. I use HSS tooling, Sharp. Bigger cuts to get the heat out. Dont tap a hole that got work hardened. I broke a form tap that way one time as well.

I find 316L and 17-4 Cond. A cuts nice but has a long stringy ship that needs attention at all times. The harder heat treated versions can be machined with carbide better and hold tighter tolerances and get better finishes.

303 is harder than 304-316 and thats why it can break a chip. I can walk away from 303 jobs but not 304-316-17-4.

I hope this helps.

Cut tap, form tap or threadmill??

Diamond

Attachments

Hot Rolled

Titanium

Cast Iron

Titanium

Diamond

Stainless

Stainless

Cast Iron

Titanium

Diamond

Cast Iron

Diamond

Cast Iron

Diamond

Diamond

Diamond

Hot Rolled

Similar threads