Parting off aluminum dia ~1.5" (38mm) fast and flat

[TauRunUm]

Guys we are doing part which require to be very flat after parting. Lathe don't have secondary spindle, so we would need to do second operation and that take additional time, so are doing slow part off.

RPM is 600, and first couple of mm I use only 0.01mm/rev, then 0.02 and at 20mm diameter it goes to 0.03mm/rev

This give very flat surface but it is slow, if I play with RPM and feeds, parting is fast but surface finish isn't good at all.

I am using part off insert (TT9080 I think) 3mm wide, holder is taegutec tter 2525-3.

It there some better part off insert primary for aluminum which could allow faster parting but with good surface finish?

Also it doesn't need to taegutec because we need need to buy one more holder

 

[atex57]

Are you using an aluminum specific insert?
Is the corner radius helping? Smaller and sharp are your friends.

Ed.

 

[TauRunUm]

Are you using an aluminum specific insert?
Is the corner radius helping? Smaller and sharp are your friends.

Ed

Nope this is universal for steel, and it is flat (zero rake I think it is called). I used it because that is what what we had and because it was essential to start making parts to see can we cut it flat without second op.

Now when we can, I decided to ask for advice about insert. I will write mail to iscar and tt folks to see what they proposed.

 

[atex57]

Yah, a steel insert can be trouble in aluminum. Take a diamond file and dust off the top to get rid of the coating and produce a sharp edge.

Ed.

 

[Ox]

Start at Z-.025 and take it down to .100" and then go back up and reset to Z0 and take a skim cut and finish it off.

You should be able to feed at least .1mm on both passes.

Depending on tit allowance, you would want to edit your tip angle.
Some inserts will hook up to 18* for this.


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

Think Snow Eh!
Ox

 

[TauRunUm]

Thanks for advances, we are ordering inserts for aluminum from TT (K10 grade) and Iscar (IC08 grade).

If we have still problems with surface quality I will try what Ox proposed to do skim cut.

Btw right now we are cutting with 600 RPM, with inserts for Al how fast to go for 1.5" dia? Or to stay with 600RPM only increase feed rate to 0.1mm/rev?

 

[david n]

I part at 2-3k rippems……006-.008 feed…….when the cut gits down to.200 or so, I slow down the rpms and feed so parts don’t fly all over when they drop……I’ll do the skim cut if the part surface is a finished surface.

 

[Ox]

Yeah, you can bump the speed up quite a bit, but you may want to edit the finish speed if your part flies around much.
It may, or may not.


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

Think Snow Eh!
Ox