316 stainless steels

[ken wong]

how do you guys recommend feed and speed to cut .75 with slot on 316 stainless steels and drill 1/2 dia hole i never machine this material before

please help

[Dave.L]

Ken,

 

1st, you need to select tools well suited for stainless steel.

 

2nd, the manufacture of those tools will provide starting feeds and speeds.

 

That is the best method to use.

 

Garr tool makes some very good and afordable solid carbide endmills and drills that will work with SS. Give them a call.

 

HTH

[Guest CNC Apps Guy 1]

A rigid setup will allow you to run at the higher end of the scale.

[Colin Gilchrist]

Hanita, Duramill, SGS, Dataflute, Ghuring, Titex, and Helical tools all make good cutters for Stainless.

 

As a general rule, 316 is usually cut pretty slowly. I'd start around 35 sfm.

 

Is it 316L or 316LVM by any chance? I used to do some chemical fluid manifolds out of 316L. Ugly stuff.

[Dave.L]

quote:

---

I'd start around 35 sfm.

---

Kennametal makes some nice 5 flute endmills. These tools are very high performance. We use all sizes and run very high feed rates.

 

As you will see, the SFM for these tools in 316SS is 190-260.

 

So, that's why I say you need to get the info from the tool manufactures since this is very different than Colin's 35 SFM which BTW I am not saying is wrong, I'm saying it's totally dependent on the tool.

 

http://www.kennametal.com/images/repositor...YPCFEVMCQFBYIV0

[jeff]

quote:

---

So, that's why I say you need to get the info from the tool manufactures since this is very different than Colin's 35 SFM which BTW I am not saying is wrong, I'm saying it's totally dependent on the tool.

---

^^^ this

[K2csq7]

Are you doing it now???

 

I have cut quite a bit of 304 & 316, Dave is right on, the window of workable feeds and speeds is pretty small, and very tool specific.

Coolant thru no peck carbide drill is the way to go. The coolant needs to get to the tip of the drill (lots of it).

[Jayson Kramer]

Also look at Hanita Varimill. they work great in 304 and 316ss. Start off at 200 sfm.

[Dave.L]

quote:

---

Also look at Hanita Varimill

---

I believe this is the same as the Kennametal Harvi II since Kennametal owns Hanita now (I think)

[Zoober]

Peel mill will get you up above 300 SFM and a much larger chip load due to chip thinning.

Looky here

[Justin Beebe at Folsom Tool]

Without seeing your part it is hard to know for sure but for the slot I would use one tool to rough and another to finish

 

T1 .500 diameter Niagra Stabilizer TIALN coated

RPM = 400SFM = 3056

Feed = .0017 per tooth = 20.8 ipm

Toolpath = contour ramp leaving .007 on walls and .007 on floors if the slot is not through

 

T2 .500 diameter Niagra Stabilizer TIALN coated

RPM 3800

FEED 24 ipm

Toolpath 2D contour may need to slow down the feed in the corners

 

These are the feeds and speeds suggested by the manufacturer for 316 and 304. I used this method with the exact same feeds and speeds in 304 with great success. Make the endmills as stubby as possible and hold them in milling chucks. Make your setup as rigid as possible. It would help if we had more information about the part for example the slot depth and length etc.

 

For the drilling I would use a Guhring Series 5514 drill or its equivelant with through the spindle coolant. Do not use a spot drill. If you must peck use a G73 chip break cycle not a G83. I would only run it at about 1/2 the speed and feed as Guhring suggests.

[MotorCityMinion]

Bull$h1t carbide 4 flute .25 ball at $16.00, 304SS, aprx. 460 SFM, 60.IMP all day, roughing with the SF Blend toolpath in a weak set-up.

Tool holds up nicely even at 1.10 outof the holder.

 

Standard el cheapo .50 carbide Em, same situation, I'm 2d contouring around 155 SFM. with good results.

[ken wong]

thanks all you guys

[Colin Gilchrist]

 

My bad. I missed a zero.

 

Should have been 350 sfm.