What's new
What's new

316 pocket milling help

tay2daizzo8

Hot Rolled
Joined
Nov 8, 2013
Location
north of Bean town
hey all, need some recommendations on endmills and speeds/feeds

the job is 316 plate
pocket depth is .277
part is 4"x18X with some islands in the middle

right now im running a garr vrx 4 flute stub at 2000 rpm and 15ipm

Im only getting 4 or 5 parts from the endmill...the flutes are all chipped above the end then it finally looses a flute or two


im ramping down at 1.5 degree angle to the full .277 depth
any ideas?

thanks
 
What's your stepover? And does it do a full width initial cut at the final depth? If you're using a narrow stepover but hitting the first cuts full, may want to use a small pocket program where you're stepping down until you can start the stepover cuts.

I'm not a fan of Garr endmills, I've had a sense that their carbide is more brittle than others I've used. Not sure if that's a fair assessment, just my impression.
 
The other thing I'd recommend is using stub length endmills, and as short a toolholder projection as you can. If using a collet holder, make sure it's in good shape, and a larger series so you can be sure it's gripping well.

Are you using flood coolant? May want to confirm with whoever makes the endmills that it's not a thermal stress issue.

This is presupposing that the mill is a proper 40 taper VMC in good shape, and you're not trying to do this on a converted Bridgeport...
 
cat 40 okuma mill..very rigid machine, im using flood coolant to get the chips out of the pocket. everything is stubbed up.
stepover is .100
there is only about 10 inches where is doing a "full slot" everything else is peripheral

ive tried imco...not very good imho

i got my tool rep looking again, but it seems this company pushes garr products. everytime i need something he brings the garr rep along with him..like jeez ive gone thru the garr book a hundred times already

I would have likes to do trochoidal cuts but i cant fit it in the memory
 
Try reprogramming the full width cut to a series of steps, maybe three. I would also consider the SGS Z-Carbs, I did a fair amount of 17-4SS and Gr2 Ti with good results.
 
A Guess based on the part size....

Probably 3/8”.........

more then likely rubbing the part to size, instead of making a chip...

15 / 2000 = .0075

.0075 / 4 = .001875 per cutting edge.....

If I’m using a carbide End Mill in 316.

My preference is a 3 flute AlTiN coated for a lot of materials...

And 160 SFM as a starting point for 316....
 
Go with a 5 or 6 flute bullnose, lighten up the depth of cut and go with substantially higher speeds and feeds.
316 isn't bad,but it can be a p.i.t.a. at times.
 
hey all, need some recommendations on endmills and speeds/feeds

the job is 316 plate
pocket depth is .277
part is 4"x18X with some islands in the middle

right now im running a garr vrx 4 flute stub at 2000 rpm and 15ipm

Im only getting 4 or 5 parts from the endmill...the flutes are all chipped above the end then it finally looses a flute or two


im ramping down at 1.5 degree angle to the full .277 depth
any ideas?

thanks

I cut 316 plate which is 3mm in depth with either 3 or 4mm end mills quite often. (mostly 3mm)
I profile out the parts, and only go as wide around it as the end mill itself.
I bought some of the 3mm Imco M924 bits some time back for approx $20 USD each and ran them at speeds recommended by Imco on their site. So a 3mm end mill and 7000 rpm or so and 220mm per minute ramping down at 0.2mm max ,at a 2 degree angle to 3.01mm depth with a little tab to keep it in place with full flood coolant.
My parts are approx 24mm long and 5mm high, so that cutter needs to cut 58mm in length or so to get around it each step.
I am not in a job shop, so no hurry, but I got from those Imco mills 400 parts cut before the coating started to wear with very minimal wear on the diameter. Those mills are still usable though, for cutting with the full length on other parts and ROI on those plates was great.
I do these parts all the time and I do not get chipped flutes at those speeds on any cutters I use, but those Imco M924 cutters are worth every cent.
I have found that I no longer run it by ear, but start with the manufacturer recommended feeds and speeds in 316 every time. I did have a lot of mis drilled holes and drills breaking on those parts ( they have drilled holes as well) until I used the Sutton Tools feeds and speeds for their 1.8mm bits.
They plunge in 225mm at 7500 rpm and I now get 800 holes a bit since I used that, where I was lucky to get 50 before one broke previously and that was plunging at 25mm! and with a spot drill to each hole, I no longer have any scrap as everything drills true.

I ran Sandvick cutters in the same material and the results were the same, if I followed their recommended speeds and feeds, though their site is more complicated to get those and of course their cutters are quite a bit more to buy

I would suggest buying one of those Imco cutters , as their prices are good and they have the correct info right there on their site.
 
Abandon the ramp. You'll need 3 tools instead of one. First drill a hole at least 25% larger than the diameter if your endmill, .01 above the depth of your pocket. Drop into your drilled hole with a center cutting 3 flute end mill (slowly) .002 above the floor depth of your pocket and open up that drilled hole just enough to cut out the angle left by the drill point. The finally get in there with your standard 4 to 7 flute endmill to finish the job. I find with 316 all the damage is done when your tool gets into non-ideal cutting situations, 316 is very unforgiving.
 
thanks everyone, i think im going to do what kingbob said, drill and plunge, should save my endmill some.
3 flute in 316 tho? i got some new alumapower bright and shiny 3 fluters i guess i could give a try, but my feed would be reduced 25 percent.
i am a job shop and right now im looking at a 3hr cycle(most of that is 44" of dovetail oring groove, which is another diaster all in itself)
 
So your still going with hardly any chip load at all?

I'm going to disagree with that... I know the "consensus" in Stainless is to FEED IT!!! FEED IT HARD!!
or it'll work harden on you..

Though if you go and look at ANY manufacturers feed and speed #'s, the stainless #'s are always the lightest feeds.

Quite a few years ago, I had to mess with some A286, and for some reason I decided to call IMCO's tech line.. And he
gave me some #s (lower feed per tooth than I thought) and we got talking about some other stuff I was working on..
TONS of 13-8.. I was running a lot of 1/2" endmills.. .003 per tooth.. 100sfm would give me very good tool life,
120 was the absolute tops, hit 130 and I might as well have just hit them with a hammer and tossed them in the scrap
bucket..

So, the recommendation was 200sfm... BUT only .0015 per tooth, on a 1/2".... Really??? REALLY!!! I ran out the rest of
that 13-8, I had 2 1/2" endmills in there.. When the job was done, one had 24 hours on it, and one had 26.. And I could
have put them back in the container and sold them as new... I was also able to run deeper, wider, and eliminate finish
passes.. Lighter chip load, less tool pressure, I could dig much deeper and much wider, and double my surface speed.
It sounded a LOT better too..

When pulling a BIG THICK chip on a work hardening material.. You are trying to curl that chip, and it gets Freeken HARD..
Its not the material you are going to be cutting you have to worry about, its the material you are trying to curl into the
flute..

Years ago there was an ad on the back MMS, I don't remember the brand, but it was a 304 cutting comparison.. If
you actually looked at the #'s.. 1/2" endmill, in 304.. They had some competitor #'s and "their" #'s..
The "WOO-HOO awesome" endmill was able to run deeper and faster, the difference?? they backed the
feed WAY down to .0014 per tooth...

I'm completely cool with less than .002" a tooth on a 1/2"er.
 
I would experiment and see how hard I could push the cutter.

316ss less then 28 RHc

full slot 190 sfm .0018 fpt

heavy roughing 235 sfm .0023 fpt

light roughing 305 sfm .0028 fpt

finishing 390 sfm .0052 fpt
 








 
Back
Top