milling stainless steel

[peaceandcalm]

hi..
I have Okuma CNC machine pretty rigid with cat 40 holders
I am using sanvik T390 4 insert holder with inserts 2030 whch is recomended for s/s material, the material is s/s 316, and the dia of cutter is 25mm 4 inserts
using 2mm depth of cut 3000rpm and 1600mm/m the insers are breaking like after 1 hour of work which is about 6 pecies of work which isnt much
using coolant as well i tried 2030 seems little bit better but still breaking
any recomendations?

[Cmailco]

Wow, that's nearly 800 sfm for that cutter; a bit fast for 316.

Try slowing the sfm to 450-600 and follow these parameters:

450 sfm when radial depth of cut (rDOC) = .75-1.0D, at .1016-.0762 mm per tooth, respectively.

That's at an axial depth no greater than 3mm.

525 sfm when rDOC = .6D, at .152 mm per tooth

575-600 sfm when rDOC = .2-.3D, at .2032 mm per tooth

As axial and radial DOC increases, sfm decreases and vice versa. Light peripheral milling <.2D, and you really need to start compensating for radial chip thinning to keep the heat out of the part.

Best regards,
Chuck

[peaceandcalm]

according to the packet of insert:

260m/min and 0.13 avarge per tooth
so in my calculations:

318 (constant right?) so 318x260 then devide cutter size which is 25mm
comes to 3307 rpm, as for the tooth feed i do this:

0.13x4x3307 comes to 1719mm/m
am i right to use those conditions?
ahh as i said erlier depth of cut is 2mm
the inserts break totally after few pecies i am not familiar with the sfm calculations not sure how to do one..how to calc from sfm to mm/min?
thanks for help

[Cmailco]

Originally Posted by peaceandcalm according to the packet of insert: 260m/min and 0.13 avarge per tooth so in my calculations: 318 (constant right?) so 318x260 then devide cutter size which is 25mm comes to 3307 rpm, as for the tooth feed i do this: 0.13x4x3307 comes to 1719mm/m am i right to use those conditions? ahh as i said erlier depth of cut is 2mm the inserts break totally after few pecies i am not familiar with the sfm calculations not sure how to do one..how to calc from sfm to mm/min? thanks for help

peace,

I don't see a problem with your calculations at all.

What type of cutting are you doing at these speeds? Would you best categorize it as:

a) slotting – rDOC = .9-1D
b) pocketing - rDOC = .65-.7D
c) peripheral; light to heavy - rDOC = .1-.3D

axial = 2mm

I had to download Sandvik's catalog as I'm not very familiar with their end milling cutters. It's a long download but from what I gathered from one .pdf, their recommended range is 215-260 m/min. Which of course would suggest a general starting point of 215 for slotting and 260 for light peripheral milling.

You mentioned cutting to 2mm depth, so I assumed a slotting or .65-.7D radial cutting situation. Everything changes as the radial depth of cut decreases because a numerically low tool engagement angle means; less time in the cut and a need to compensate for radial chip thinning.

We routinely mill 408 stainless (a bit different animal) at speeds in excess of 900 sfm, at better than 100 inch/min for this very reason. So, speed is always relative to the type of cutting condition and the material's properties. That's why 'general' advice is so difficult.

A few other things to think about are:

1) Type of toolholder

A quality milling chuck or preferably a tool-holder/cutter-body type arrangement, but never an ER or TG collet chuck.

2) What length/diameter ratio?

Long L/D ratios require a reduction in sfm & mm/tooth. A ratio of 5-6:1, typically achieves stability at 85-90%. 6:1-7:1, 75-85%. So it's something to consider, and again, these are very general guidelines.

3) Entry and exit

50% reduction in speed on entry and exit when slotting or cutting with >.5D, or better yet, enter with a roll-in technique. I'll add a diagram later that explains the way 'I' do it, though everyone has their own preference.

Lots of entry & exit is extremely hard on inserts, especially if you don't compensate the feed and/or technique.

Regards,
Chuck

[peaceandcalm]

ok, i will try to make a video of the cam i am using and post it here..
but for now i am using 12.5 which is 1/2 of the cutter as radial cutting
but i will post a small video later when got time...
your info very helpful by the way
thanks

[Cmailco]

Look forward to your video and glad I could be of at least some assistance.

[peaceandcalm]

here it is, simple its 70 mil long the who part the maching part is only about 50 mil long and its round bar been machined as you see only doing the flats on both sides using collet 40mm and using collant..

http://www.mediafire.com/?aocdwq4qdcsa77m

finished the job about 120 pecies lost about 20 to 25 inserts
was using 3000 rpm 1000 to 1200 mm/min by 2mm axial cut by 12.5 radial cut with 25mm 4 insert holder..
machining time for both sides 12 to 14 min.
let me know if that sounds normal.

[Cmailco]

Lots of entry/exit, so you have to minimize the shock loads on the inserts using a roll-in.



I typically pick a distance ~2.5mm from edge of the part and enter at a 10º angle. Rounding the corner moves the cutter into the cut in a more ideal situation; producing a chip that is thick-to-thin on exit.

I'd also run it dry to avoid thermal shock. Lots of entry/exit only exacerbates this problem.

Use the largest radii insert available, that or round inserts if the setup has the rigidity for it.

The key is to achieve a predictable cutting process where you know exactly when the insert needs to be indexed. Once you get the processing nailed down and can observe something approaching 'normal' tool wear, you're pretty much "good to go".

[peaceandcalm]

dry on 316 S/S material? wont that just burn the inserts striaght away?

[Cmailco]

Straight from the Sandvik Technical Catalog page 35; "Application Hints" for stainless steels:

Roughing • Use high cutting speeds (vc = 150-250 m/min) to avoid built-up edge. • In roughing, always run dry, without cutting fluid, to minimize problems with thermal cracks.

That said, the only real problem that coolant helps with is built-up edge which, according to Sandvik, is alleviated with higher cutting speeds while the PVD coating handles the lubricating chores.

I've never run coolant for roughing operations in 316 SS unless slotting and even then, I'll use trochoidal toolpaths with no coolant. If I had no trochoidal option, I'd be tempted to flood with coolant in a slot though, otherwise machine dry with air blast or use minimum quantity lubricants; ie, air blast with vegetable oil.

YouTube- Emuge HPC 316 SS Milling
Best regards