What's new
What's new

Cutting Internal threads on Lathe, Production style in Titanium

jared.l24

Plastic
Joined
Jan 13, 2016
Hello all, thank you for the space.

I'm about to run a couple of production parts on my Haas ST25y with a Bar Feeder and am looking for some help to speed things along.

They're very simple straight forward parts. The tricky part is cutting the internal threads in GR-2 Ti. The threads are 3/8-16" & 1/2-20", about .500" deep. I was previously doing this, single point style with a Micro 100. But my quantities have risen, I do have a Bar Feeder, so I'm trying to keep this as hands off as possible.

One option, I could threadmill them since it's a Y-axis lathe. But that will require a new/custom post and Mastercam just doesn't talk to the Y-axis very well IMO.

Tapping seems out of the question for my quantities. Right now about 200, but those numbers will keep rising.

Is there a multipoint internal threading tool that will stand up to more abuse than a single point, and also cut down to a 3/8-16 I.D? What am I missing?

-j
 
Hi jared.124:
If you can find a way, threadmill it with a cutter that has as many points on it as you need for your thread depth.
One turn and done, and you'll have far less hassles than any other way.
If your control supports helical milling using spindle rotation and synchronous movement in Z, you can just mill them by rotating them rather than the usual threadmill routine where the tool moves in X, Y and Z and the part is stationary.
You might find it easier to program that way, if MasterScam is not doing it for you.
It might give you a better part too.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
MasterCam can easily do this without problem, not sure what issues you're having?
Y not get the thread milling code off the threadmill website? Most good companies will provide this.
Id be talking to my reseller if I couldn't threadmill a damn part in a Y-axis lathe....
 
One option, I could threadmill them since it's a Y-axis lathe. But that will require a new/custom post and Mastercam just doesn't talk to the Y-axis very well IMO.
Definitely threadmill that part. You do NOT need to use the Y-axis to threadmill. You can just use a C and Z motion and you can even hand code it. Not that big of a deal.

I threadmill parts on a 1986 Mazak CNC lathe with a C-axis. The machine was built way before Y-axis lathes were made.

Move the threadmill to X0, move in to depth in Z, G1 feed up in X to cut thread diameter, then G1 feed in C 360.0 with Z+ 1 thread pitch in same line (feedrate will be in degrees per minute), move to X0, and retract Z out of the part. Done.

You should be able to get 100+ plus parts per threadmill in Titanium. I get 100 parts per threadmill in Inconel 718 running about 100 SFM on the tool.
 








 
Back
Top