shell mill on 316 stainless

yoozer · Jul 23, 2018

I'm apprehensive to run a program to face off over .350 stainless with a 5 tooth shell.
Rarely run stainless, so I just want to be sure I don't ruin the part, (or the tool) as this is the last op and got many many hours into it. The mitsubishi tool sales rep recommended the following:
400 SFM
.080 DOC
.006 FPT
Run Dry

Then the finish cut is 600 sfm, .003 fpt, .025 DOC

I don't have a lot of experience, but running .080 DOC dry seems scary. I envision seeing sparks.
So I'm going to hold off until I get some knowledgeable input. Thanks

Krovvax · Jul 23, 2018

Running 0.080 dry in ss 316 is fine. The most i ever took was 0.236 (max of my tool) dry with similar parameter. 3" wide.

You want to aim for gold chips. On the finish cut just spray a bit of cutting oil on the part so the insert wont let any small chips stick to the back of the facemill where it just rub.

Envoyé de mon SM-G920W8 en utilisant Tapatalk

Milland · Jul 23, 2018

More of an issue, will this facing be on just one side? Heat, rubbing, and release of stress in the material can warp a part, so pay attention to this aspect while cutting if flatness matters.

If the part is fairly thin it might be safer to use a smaller cutting tool, like a 1/2" endmill, and take the trade-off of longer cut time for lower unit stress into the part. But you could cut near full depth as a roughing pass, saving ~.020 to face the bottom. Or, if surface smoothness isn't critical, just cut to final depth with a ~.08 stepover.

I would do two passes, and use a .02 corner radius EM for the final pass.

yoozer · Jul 23, 2018

Krovvax, thanks for the info, esp the tip about spraying the cutting oil.
Milland, yes just facing one side, and flatness just has to be within .005 with for .250 thickness, I'm guessing
that is thick enough to not have to worry about warping?

This place is amazing....I did not expect to get replies so fast. I really appreciate the help!

Krovvax · Jul 23, 2018

yoozer said:
Krovvax, thanks for the info, esp the tip about spraying the cutting oil.
Milland, yes just facing one side, and flatness just has to be within .005 with for .250 thickness, I'm guessing
that is thick enough to not have to worry about warping?

This place is amazing....I did not expect to get replies so fast. I really appreciate the help!

I would rought half of it on one side. Flip it over rought second half. Flip it again to remove the stress and finish first side. Same thing fornthe last one.

Always take note how it wrap because its going to wrap. You might have to flip it more than this watch out.

Envoyé de mon SM-G920W8 en utilisant Tapatalk

evilusions · Jul 23, 2018

The speed and feed are fine, but if you are taking .350” off and only have 1/4” left, you will very likely have warping.

Hazzert · Jul 23, 2018

In our experiences with 304SS (different beast) indexable tools cause a lot of warping due to surface stress. I would be looking at finishing this part with a 1/2 Niagara 440 STR 2.0 endmill with .03" corner rads. I would probably HSM off the material for roughing as well rather than hitting it with a facemill if it was something I cared about. 500 SFM, .005 FPT, 8% stepover.

Milland · Jul 23, 2018

Hazzert said:
In our experiences with 304SS (different beast) indexable tools cause a lot of warping due to surface stress. I would be looking at finishing this part with a 1/2 Niagara 440 STR 2.0 endmill with .03" corner rads. I would probably HSM off the material for roughing as well rather than hitting it with a facemill if it was something I cared about. 500 SFM, .005 FPT, 8% stepover.

We're on the same wavelength, but I suspect you're not accounting enough for chip thinning with the .005"/tooth.

Milland · Jul 23, 2018

yoozer said:
Milland, yes just facing one side, and flatness just has to be within .005 with for .250 thickness, I'm guessing
that is thick enough to not have to worry about warping?

No, the part will almost certainly want to warp with the amount you're removing and the fairly thin final part thickness. Most wrought materials have a surprising amount of residual stress left in them, and cutting just one side is an easy way of having it show.

This place is amazing....I did not expect to get replies so fast. I really appreciate the help!

Only when we're not being collectively grumpy. And at least you asked a "real" machining question.

Hazzert · Jul 23, 2018

Milland said:
We're on the same wavelength, but I suspect you're not accounting enough for chip thinning with the .005"/tooth.

Too hard or too soft? OP can do the adjusted chipload to get to .005 per tooth. Those Niagara tools can be run hard

mhajicek · Jul 23, 2018

Milland said:
Only when we're not being collectively grumpy. And at least you asked a "real" machining question.

What OP didn't tell you is he'll be making the cut on a Harbor Freight bench-top mill converted for CNC.

Milland · Jul 23, 2018

Hazzert said:
Too hard or too soft? OP can do the adjusted chipload to get to .005 per tooth. Those Niagara tools can be run hard

Too soft, with the .040" stepover, .005"/Tooth is more like .003"/T (roughly), so the OP could double your suggested feed rate.

Milland · Jul 23, 2018

mhajicek said:
What OP didn't tell you is he'll be making the cut on a Harbor Freight bench-top mill converted for CNC.

Actually, I don't really have any beef with what he's doing, it's just that he would be better served on a forum oriented to that sort of small project. Heck, I have about 40 tons (not an exaggeration) of industrial spindles, profile rail, servo motors, etc. here that I want to use to make specialty machines tools with, y'all can make fun of me when I start asking dumb questions about making the damn things work...

yoozer · Jul 24, 2018

Milland said:
Actually, I don't really have any beef with what he's doing, it's just that he would be better served on a forum oriented to that sort of small project.

Am I in the wrong place? Anyway, I took the advice here and used 1/2" instead of shell, and it came out great. Thanks to everybody that chipped in advice. :cheers:

yoozer · Jul 24, 2018

mhajicek said:
What OP didn't tell you is he'll be making the cut on a Harbor Freight bench-top mill converted for CNC.

I didn't understand this until now... I just discovered the thread. Now I have a much better understanding of PM. I didn't do any lurking prior to posting.

plastikdreams · Jul 24, 2018

yoozer said:
Thanks to everybody that chipped in advice.

I see what you did there

Search

Largest Manufacturing Technology Community on the Web

Search

shell mill on 316 stainless

yoozer

Plastic

Krovvax

Hot Rolled

Milland

Diamond

yoozer

Plastic

Krovvax

Hot Rolled

evilusions

Plastic

Hazzert

Stainless

Milland

Diamond

Milland

Diamond

Hazzert

Stainless

mhajicek

Diamond

Milland

Diamond

Milland

Diamond

yoozer

Plastic

yoozer

Plastic

plastikdreams

Diamond

Similar threads