Single point threading in 6063-t6

[Philcott]

Hi guys,

 

I'm trying to get a decent thread in 6063-t6 aluminum and I'm not being too successful. I'm getting torn threads.

 

It's an M10 x 1.25 thread (pitch dia. = .358)

 

I've used Kennametal top notch inserts and sandvik lay down inserts with RPM's of between 250 and 1000 (slower seems better).

 

Varying depth of cuts and varying last cuts and varying spring/clen up passes.

 

I've used soluble oil coolant and Oemeta hycut cutting oil.

 

I'm going to try a ground finish Iscar threading tool now and may try WD30, kerosene or any other friggin liquid (might try diet coke next, but not my Anjeo rum) to try and get a smooth thread.

 

Has anyone had success cutting this crap material? Help, please, help.

[Pilot Plant Supervisor]

I have ground geometry into the top of inserts to get the chip to flow, but it still leaves alot to be desired. I would probably roll with a Landis tool.

[Philcott]

Wish I had a Landis too to try. I'm getting so frustrated with this thread. I've tried just about everything I can think of short of freezing the part before machining.

 

We have a crazy_millman I need a crazy_threadman's help[ on this one.

[specv]

IMO you are running waaay to slow, i would not run less than 2500 if possible. also make sure the inserts you are using do not have an edge prep on them (it sounds like you are doing that now with a ground insert).

[Philcott]

Tried one at 2500. Just awful.

[Pilot Plant Supervisor]

If you have a tool & cutter grinder,take a diamond wheel with an 1/8" or 1/16" radius (size depending on insert size) and grind a slot parallel with the leading edge of the insert. You want to grind right up to the edge so there is only .001 - .002 land at the edge. The radius of the slot should be 15 to 20 degrees positive rake where it meets the edge. If you can do this, the chip will tend to flow down the radius and not pile up so bad on the insert. You still need to take very shallow cuts (.0005 or so) and use something like Acculube LB-2000. Like I said before, not perfect but you can get there.

[Philcott]

The problem I seem to be getting is the material lifting/pulling off the part and leaving torn out areas, It's not a build up on the threads.

[EX-wccprogrammer]

Slap me for being stupid, but might I suggest...

 

Modify a straight fluted tap by grinding all of the cutting teeth off except those of one flute.

 

Taps are sharp, and will shear gummy material better than any insert.

[Pilot Plant Supervisor]

I understand. It sticks to the insert then pulls chunks out of the material. The method I described is a pain in the butt, but we have machined threads this way on some NASTY refractory alloys that are soft and gummy. And, they are abrasive as well. You gotta love it.

[EX-wccprogrammer]

On second thought, what about a modified threadmill? A tap may not handle the radial stress very well.

[Philcott]

I understand. It sticks to the insert then pulls chunks out of the material. The method I described is a pain in the butt, but we have machined threads this way on some NASTY refractory alloys that are soft and gummy. And, they are abrasive as well. You gotta love it.

 

We don't have a way to grind that here anymore and my eyes aren't what they once were to hand grind the tool. I do appreciate the tip though.

[Philcott]

On second thought, what about a modified threadmill? A tap may not handle the radial stress very well.

 

This idea has me thinking. Hhhmmmmmm.

[Philcott]

I'm a little further ahead with this now. I am leaving more for my last pass .003, turning at 3000 rpm and using the coolant. So far I got one in a row. Yee frigin' Haw

[Rocketmachinist]

I would try getting a PCD threading tool. Diamond tools are wicked sharp and would cut through that stuff like butter. Also, how may passes are you taking? Lots of light cuts is going to be your best bet.

[Newbeeee™]

Phil - is it a released/aerospace part?

May be worth digging out the mtl cert and check it out as this shouldn't be a problem.

[Philcott]

I would try getting a PCD threading tool. Diamond tools are wicked sharp and would cut through that stuff like butter. Also, how may passes are you taking? Lots of light cuts is going to be your best bet.

 

It's cutting in 18 passes now and ran last night with no problems. What a day yesterday fighting this crap.

 

I really think the main solutions were getting the cutting speed up high enough and smaller passes. Sharp tool played a part for sure and I'll get a PCD insert if we get this job again.

[Philcott]

Thanks to all who gave me suggestions they all contributed to figuring this out.