4-40 threads in Ti

[gcode]

I've got some Ti parts I'm building that have 4-40 x .375 min depth hole callouts.

I'm looking for ideas to machine these holes.

I was thinking roll tap, but .375" is really deep for a 4-40 thread.

I'm not even sure I can buy a 4-40 roll tap that long

The other option is thread milling..

I can buy 4-40 single point thread hobs long enough, but that's all I've been able to come up with.

The parts are worth about $50k each and breaking taps is NOT an option

Any ideas out there TIA

[Guest MTB Technical Services]

I've got some Ti parts I'm building that have 4-40 x .375 min depth hole callouts.

I'm looking for ideas to machine these holes.

I was thinking roll tap, but .375" is really deep for a 4-40 thread.

I'm not even sure I can buy a 4-40 roll tap that long

The other option is thread milling..

I can buy 4-40 single point thread hobs long enough, but that's all I've been able to come up with.

The parts are worth about $50k each and breaking taps is NOT an option

Any ideas out there TIA

 

 

Rigid Peck Tapping with a high-spiral cut tap.

[gcode]

Rigid Peck Tapping with a high-spiral cut tap.

I'll have to see if I can buy taps long enough.

There are lots of places on the parts I can practice that

will be cut away later

[Matthew Hajicek - Singularity]

The main advantage of threadmilling would be that if you snap the tool you can get it out and cut again with a fresh tool without cross-threading.

[crazy^millman]

We use to roll form those kind of threads when we worked together many years ago. That deep will be tricky. I would use a Moly Thread Lube verse coolant. Follow the normal process of holding +/-.0005 by reaming the holes and you should be good. Still might break a tap. Have done the peck tapping with a HY-Pro as well .01 and let it take what ever it takes. Love it when a person quote 5 seconds a tapped hole and then wonders why a part with a 1000 tapped holes took so many hours to get done.

 

HTH

[Pilot Plant Supervisor]

We have done lots of these with Micro 100 solid carbide thread mills. Usually takes a couple of spring passes when you get that deep.

[gcode]

The B/P calls out a 3B thread..

I ran this through Sandvik's Coro 2.0 machining app and it recommended a thread mill

Looking through their catalogue, they don't offer any 4-40 3B taps

[cincy k]

Thread mill. On a part that expensive that's all I'd consider. Look at Harvey Tool. They have the exact length you need. It'll take a few passes but at least it's predictable. 

[Prodoggg]

We machine a lot of Ti. What I do is drill the hole with .0925 dia. drill (2.35 mm)and tap with YMW ZELX Ti LHS/RHC GH2 tap. Use Emuge tapping fluid while tapping. Blow out the hole to be free of coolant first. Drill HSS Co @ 40-50 SFM, Carbide drill @ 100-120 SFM. .0003/.0006 per tooth chip load. Tap @ 12-15 SFM. You can use a dwell in the G84 rigid tapping cycle by adding a P to the canned cycle, this helps cool the tap before retract. (P1000 = 1sec, P2000 = 2sec, ect.) We get hundreds of holes per tap. Hope this helps, If you go with a thread mill do yourself a favor and use a rough and a finish thread mill. Stay away .001/.002 with the rougher and the finisher will last much longer while most the abuse is taken by the rougher. Have Fun!

[robk]

Thread milling has not failed me yet. Personally I'm very nervous when it comes to tapping titanium. Usually the tap will break on retract. Therefore I wouldn't recommend peck tapping. None of our customers specs allow us to use a form tap.

We've had very good results using Emuge and Walter threadmills.

[Mic6]

Getting chills thinking about tapping that.  I can hear the creeak..snap or in the case of 4-40..TINK

 

Threadmill all day every day.

 

Any brand should be good.  I run Emuge, SCT, Accupro.

[Newbeeee™]

At 50k for the part, cycle time is not important.

I would threadmill without hesitation.

One thing to be aware with these threadmills, is the form maybe correct (60deg for instance) but the peak/tip of the form (ie the crest of the thread) is not necessarily correct.

We got caught out on this for Aerospace parts the other year as the threadmill was ground to a point with no rad.

 

 

edit: Rour at prodoggs comment of have fun!!!

[gcode]

this is getting even more challenging

4 of the holes are in the bottom of a 2.5" deep pocket with

.200" from C/L of the holes to the pocket walls.

There is no room for a tool holder and off the shelf thread hobs are too short.

I'm going to need a custom thread hob, ground out of a 5/16" carbide blank 

[Colin Gilchrist]

Oof. Gotta love the imagineer that designed that.

[Newbeeee™]

Oof. Gotta love the imagineer that designed that.

Cue the 'ol rolleyes...

 

 

G - ask the guy who quoted it 'what did you have in mind for these threads???'

[gcode]

OK,

I'm getting custom tools quoted from Carmex.. based on their HardCut line

They are left hand cutting so you can climb  a right hand thread from the top down.

They'll have to be ground on an 8mm x 6" long blank.. and I'll hold them in a Rego_Fix collet holder.

I've got lots of pockets and other spots that will get milled away, so I can prove out the process

before I take the money shot.

I feel better now.. at least I have a plan.

 

see attached screen shot

 

 

 

[gcode]

Cue the 'ol rolleyes...

 

 

G - ask the guy who quoted it 'what did you have in mind for these threads???'

If I had to guess, I'd say they are holding down a dust cover

[Mic6]

At 50k for the part, cycle time is not important.

I would threadmill without hesitation.

One thing to be aware with these threadmills, is the form maybe correct (60deg for instance) but the peak/tip of the form (ie the crest of the thread) is not necessarily correct.

We got caught out on this for Aerospace parts the other year as the threadmill was ground to a point with no rad.

 

UNJ?

[Newbeeee™]

UNJ?

Metric

[CADCAM3D5AXIS]

^^ Whitworth ^^