Inside turning problem

Hi people!
Long time i did not had such a part i could not machine on a easy way... I need to machine 10000parts, brass material.
So, i have this part, look inside it... first i tougth it would be easy and i made a carbide custom tool... 1500 rpm, F0.04mm/rot, it made 1038 parts, exactly. Then i taugth, maybe, hss custom tool could do it better on brass...no, not a single part,it destroyd it at first part. Then, i used a 2 flute carbide 4mm diameter long mill: 47 parts and very very slowly. I used a 2nd one with double feed, 500m/min, only 7 parts...so, i changed again to the custom tool, coated carbide this time... as you can see on the photo, did not last long, using 1000rpm and feed 0.04 mm/rot,
83parts...now i am tinking about using a 10mm mill,pasma cuted at center,
4mm diameter and try again...problem is i have to send the mill out to another shop,
pay for it and have no idea if it will work or not. Can you give some advice? Thank you! Best regards!
T

Chips are going to be the biggest issue here. Then you compound that with interrupted cut. (Assuming you are milling the slots first.) Although, milling the slots first might help with the chip issue.

I think I'd make a tubular tool with the inside and the outside relieved for clearance except for a couple of mm right at the end. Carefully taper the end to provide a slight amount of relief immediately behind the cutting edge. Saw slots to create 4 cutting faces. Relieve the end to give clearance. Peck drill with it.

Take a look at Rotabroach style cutters. A cutter like that is very robust. 10mm are available,but I doubt you'd be so lucky that the core they leave is the right size. it would probably need to be modified for a more neutral cutting angle.

Hmm these parts are just my cup of tea.

I would use HuFD's advice about using a peck Drilling method to get the chips out if you need to use a Static tool. Also I would try something with more rigidity up close, as opposed to holding along tool, hold a short Perpendicular tool. I found picture of what I mean (not exactly what you need, but get the idea). And who to ask.




BUT if it were me, I would use a 2,5mm-2 flute Endmill in a live Axial (Z axis) holder to Rough and Finish. 2,5mm is 8 times diameter, but you should be okay going slow. And the Endmills that size aren't going to break the bank.

R

Horn mini face grooving tool or similar from another manufacturer. You’ll get through coolant right to the cutting edge and then just peck away.


Sent from my iPhone using Tapatalk

Try using the sandvick CXS line of tooling. Contact your rep and have a talk. This line of tooling has changed everything in our shop and we have done some crazy small and deep face grooving with it.

Seriously you don't want to send this out to another guy, have it fail and cost you money. Contact Sandvik,,, I take a .118 wide CXS insert and go 1.300 deep in 6061 aluminum one pass. I have made over 100 parts with that insert. We had a little learning curve with it and had to modify the inset just a little to get that deep but it works.

Make Chips Boys !

Ron

Dupa3872 said:

Try using the sandvick CXS line of tooling. Contact your rep and have a talk. This line of tooling has changed everything in our shop and we have done some crazy small and deep face grooving with it.

Seriously you don't want to send this out to another guy, have it fail and cost you money. Contact Sandvik,,, I take a .118 wide CXS insert and go 1.300 deep in 6061 aluminum one pass. I have made over 100 parts with that insert. We had a little learning curve with it and had to modify the inset just a little to get that deep but it works.

Make Chips Boys !

Ron

Click to expand...

Thank you sir!
It was that solution but from another brand, WTO from Germany.

Is this leaded brass that you are having trouble with?
Or newer non-leaded?


---------------------

Think Snow Eh!
Ox

Ox said:

Is this leaded brass that you are having trouble with?
Or newer non-leaded?


---------------------

Think Snow Eh!
Ox

Click to expand...

alloy type matters. aluminum bronze often some might think its brass but it diffidently dont machine the same
.
actual brass likes to grab and usually negative rake is used. many a apprentice has had a twist drill pull its self out of chuck and get stuck in a hole. vibration and chatter can break off cutting edges

Ox said:

Is this leaded brass that you are having trouble with?
Or newer non-leaded?


---------------------

Think Snow Eh!
Ox

Click to expand...

Non leaded brass.

ricardo_gt said:

Non leaded brass.

Click to expand...

Well there's 90% of your problem.

BTW - what you are trying to doo there is known as "Trepaning". (not 100% sure on the spelling)



You could roll your own "hole saw" to make that feature.
I did that many years ago. Mine was a lot smaller and in leaded screw stock, but the principal is the same.

Just make a sleeve that would be the same size as your groove is to be, but extra long.
Try to put some tapered relief in it both inside and out. (on purpose)
Then put it on the rotary in your VMC and take a 3/16" (?) mill and cut something that looks like a saw tooth into it.
Index 120* (or whatever it takes to make it look like a hole saw) and repeat.

You could either grind in clearance when done by hand, or you could program an A/X move to produce the needed clearance on the face of the tool.

Heat treat


Now you would want to figure out how you would prefer to hold it.
On mine - I just went up and put a heavier shoulder up above my cutting portion and had the inside bored through, and I put a 1/4" bolt through to pin mine to a shank.

For as deep as you need to go tho - you would need to peck drill it to clear the ships out of your gullets.


You would also need to use whatever tip hook desired...


By going with shallow gullets over full depth single flute like you have, you gain rigidity in the tool it'self.



I would provide a pic of it, but that was before film was invented, so ...



-----------------

Think Snow Eh!
Ox