Tapping Titanium

[jeff]

I have some #4-40 blind holes to tap .300" deep or so and it's been years since I worked with this crap.

Any tips, suggestions, things to look out for?

I'm going to be using the Guhring series 2912 modified bottoming tap, running at 15sfpm.

http://www.guhring.com/Documents/Catalog/Tools/2912.pdf

 

 

[crazy^millman]

Use a Moly Tap-Lube and not coolant on the holes. I did thread form Ti many years ago, but it is frowned upon by most since it does have some embrittlement issues. I was never able to have some test done on parts to see if like other metals the threads were stronger and not weaker. Boeing and Mil-Specs don't allow it so I suggest you tap it. At that size I worry more about RPM and syncing the spindle to the motion. I have even used floating tap holders on smaller tapes to allow for any machine deviations to not break a tap off. If you do break one you can burn it out as long as you don't burn the Ti doing so.

[jeff]

Thanks! We have Moly-Dee and I might just start the tap in the mill, and finish tapping it by hand to be safe. We only have a half dozen parts or so to do.

[crazy^millman]

Thanks! We have Moly-Dee and I might just start the tap in the mill, and finish tapping it by hand to be safe. We only have a half dozen parts or so to do.

 

Have done that as well. Tap about .1 deep and then use a fresh tap on the by hand work. Tap starts getting dull just replace it.

[Goldorak]

OSG exo tap A series are wonderful in hi-temp alloys like TI and inconel

[gcode]

I have some #4-40 blind holes to tap .300" deep or so and it's been years since I worked with this crap.

Any tips, suggestions, things to look out for?

I'm going to be using the Guhring series 2912 modified bottoming tap, running at 15sfpm.

http://www.guhring.com/Documents/Catalog/Tools/2912.pdf

 

Carmex Hardcut thread mills

 

http://www.carmex.com/page.php?instance_id=4&actions=show&id=875

[jeff]

Hmm I forgot about threadmilling.

How would an AlTin coated threadmill work in Titanium?

I only have 18 holes.

[Matthew Hajicek - Singularity]

I've been threadmilling in 17-4 and Ti grade 5 with no issues down to 2-56 using Harvey's single-profile threadmills for hard steels:

 

http://www.harveytool.com/prod/Thread-Milling-Cutters/Holemaking---Threading/Browse-Our-Products_271/Thread-Milling-Cutters---Single-Form---For-Hardened-Steel_199.aspx

 

It does tend to roll a burr in Ti, so I find it helps to re-skim the countersink, minor, and thread in that order after initially cutting the feature.

[jeff]

Screw it, we're just going to tap them. And if we get an order for more we'll threadmill.

Thanks guys!

[Colin Gilchrist]

Hmm I forgot about threadmilling.

How would an AlTin coated threadmill work in Titanium?

I only have 18 holes.

 Take Matt's advice. Buy a Harvey or Micro 100 small single point thread mill, and be done quickly. Especially with only 18 holes, you'll be done in no time. If you get a decent tool, you should be able to use it for a range of pitches in the future. I'd recommend buying a couple in different sizes, just to have them on hand when needed. I'd always prefer to thread mill when possible, it sure beats burning out a broken tap. And when a thread mill tool wears out, you can pop another one in, touch it off, and re-cut the same thread. (As long as the tools are consistent in how they are ground...)

[Pilot Plant Supervisor]

+1, or 10, on the Micro100 single point thread mills. We worked with Guhring on a bunch of modified taps for Ti, and it just didn't work out. The uncoated Micro100 tools last a LONG time, and I usually program my threadmills to conventional mill, because I like to start at the top.

[M Horton]

It's been awhile since i've machined titanium, But if i recall tapping 4-40 with a 3flute osg exo with ridgid dark tap goo. 200rpm, .025ipr and would feed down .100 and reverse out, blast chips from hole and tap then reapply goo to hole and tap then feed z-.200, etc etc. Could probably do it in 2 whacks if tap drill was stepped up a size bigger. Giving the tap a easy start with a lead chamfer to suit.

[lowcountrycamo]

I thread milled hardened 15-5 stainless 3/8 2" deep couple weeks ago with carmex.   Had to back grind the shank to  get it down the hole.  We almost never tap in machines anymore.  Carmex makes it so easy with there code app.

[METALMERKER]

+1000 on the Carmex threadmills! I used some to mill #0-80 X .250 dp in aged A-286, made 16 holes with no signs of wear. I've found it's ALWAYS best to go uncoated when it comes to Ti..

 

Sent from my SM-S902L using Tapatalk

 

 

[Guest]

Threadmill and be done with it.

 

Did some 2-56 @ .310 Deep (using a single point thread mill) and got hundreds of holes out of most threadmills. 2fl.

 

10,000 RPM @ 2.25 IPM (Tool diameter was .065) were the cutting specifics.

 

IN addition, WHEN a tool broke, we were able to remove the broken carbide touch off a new tool and get on with it again. Tapping, not so much.

 

JM2CFWIW

 

[oneyankfan1]

Threadmill and be done with it.

 

Did some 2-56 @ .310 Deep (using a single point thread mill) and got hundreds of holes out of most threadmills. 2fl.

 

10,000 RPM @ 2.25 IPM (Tool diameter was .065) were the cutting specifics.

 

IN addition, WHEN a tool broke, we were able to remove the broken carbide touch off a new tool and get on with it again. Tapping, not so much.

 

JM2CFWIW

 

Wise words.

[gcode]

The Carmex HardCut line works really well for tough thread milling apps

They are left hand cutters so a right hand thread is M04, G42 spiraling down top to bottom

[oneyankfan1]

Walter has some ba tm's. http://www.walter-tools.com/en-gb/tools/standard_products/threading/overview/threading_milling_cutter/tmo_hrc/Pages/default.aspx

[jeff]

I tapped them with a Guhring tap and all went fine, no issues. 

[Matthew Hajicek - Singularity]

What kind of surface finish did the tap leave?

[jeff]

What kind of surface finish did the tap leave?

It was a couple of weeks ago, and I can hardly remember what I had for breakfast yesterday.

I know it wasn't bad because it has to be good in order for a certain robotics company to accept it.

[crazy^millman]

Jeff you should have said it was a 4 finish. :laughing: