stainless steel

[Marty A]

afternoon everyone

 

i have a big ring of stainlee steel to cut.

i have'nt machined this in many many moons.

it's a big ring 33.00 ins. in dia. i have

some pockets and large holes to put in some

tapped hole etc, etc.before i call our cutter

guy i am coming here first.it is 304 ss

thats all i know about it. i will be using a 1.5 dia 3 inserted dyna shear. the inserts are coated

and they work really well on reg. steel a2,d2,s7

and so on.i run that cutter at 2300 rpm at a

feed of 230.i would like some input on the

speeds and feeds for this job.any ideas are

always appreciated.this job should only take

around 6 hours to do.the operator says it

will take him 8 to ten. well i know this

operator and yea it will take him that long.

the owner bet us a lunch that it will take that

long to do.cause my big mouth said it won't take

that long. so i want to have everything set

for the operator.well thanks in advance.

going home now and wait for all the freezing rain

have a good day all.

 

marty

[jeff]

Don't say freezing rain!!!

noooooo!

 

 

304 ss is nasty.

Depending on how deep the pockets are,we run our facemills dry with airblast whenever possible.

I would say a starting point of 1700 rpm maybe 20 ipm.The depth of cut might change that though if you are really hoggin.

I'm not familiar with Dyna Shear,we use Sandvik and Dapra facemills.

As for drilling,treat it like a 45 Rc material and you should be fine.HSS drills with coolant will do the job.

HTH

[mayday]

Motty, we run Z-carbs whenever possible in 304. they work well. I know old scool tells you HSS,no carbide but these work with the S/F right out of the book. Allied Spade bits for the big holes

[MCam Newbie]

Marty,

 

Mayday and Jeff are both +1, 660 SFM, maybe a little faster with copious air blast. I think I would raise the chip load to about .006 IPT though, or 30 IPM @ 1700 RPM, even a bit higher feedrate if face mill has a chip thinning lead angle, and if facing DOC is .150 or less. (Assumming a rigid machine. If your tool is an insert endmill, I'd slow to 440/500 SFM @ .003/.004 IPT, 25% of cutter diameter DOC radialy, maximum)

You want a slick coated insert, with a positive rake, as 300 series if prone to creating BUE on negative rake inserts, uncoated inserts, or inserts with a T or K land. Enough velocity to keep as much heat in the chip as possible. Watch you entry angle insuring the chip starts to form with force directed into the body of the insert, to avoid flaking along the upsharp edge.

You didn't say what size hole. I reccomend Guhring series 5510 or 5514, with the Firex coating. If you have through tool coolant, especially if you have some pressure to the coolant, they are the KIND. No centerdrilling, and size control to .002. I have drilled .618 diameter holes at 195 SFM @ .01 IPR. (1200 rpm @ 12 IPM) with high pressure coolant through the tool, into 316 SST w/Bhn 265, 4.5 diameters deep without pecking. After 240 holes, drill showed only about a .004 to .006 wear land. The 316 is much nastier than 304 SST IMHO.

Just keep in mind, whatever tooling you're using, 300 series will work harded, if given a chance to do so, and LOVES to stick to the cutting edge.

BUE is common cause of tool failure, if you have trouble Cermets work quite well at avoiding that, although the correct coatings on carbide work very well at avoiding it.

Well, there's my 2 cents worth! (More like a nickle, volumn-wise.)

Hope this helps somebody out there, if not you Marty, 'cause I type purley with my index fingers, occasionally hitting with a thumb, to highlight my digital dexterity.

[Marty A]

morning guys.

thanks for the advice guys. i have printed

this out for a ref. when we get the job.

again thanks for the help. oh by the way

jeff we didn,t get the freezing rain, just

the rain, still raining now.sheesh

 

marty