Grooving stainless steel 304. I know, more stainless...

SmlG54 · Apr 5, 2018

Hey all, first post.
Let's dive in.
304 stainless tubing, .250 wall thickness 3in od
Chucked in soft jaws 4.5 in sticking out 6inOAL
New to shop, parts have been ran before at 80sfm .004 in/rev
Problem:Chipping corner and cutting face of insert in 2 parts time
Insert- .125 Tool Flo AC3 grade held good in tool holder.
Cut: groove width of .3, radial of .1, plunge a few times diff to make width, save .001 on side walls Z and .01 dia X.

Solution so far, upped sfm to 550 and feed .008 .
Result: corners and face of insert hold well but side of inserts chip 1st pass. Dimensions are held but back wall where first pass of full engagement happens is gummy and and leaves step as though corner is broken.

Please help, 2nd week there, how in the heck can I solve this. Tried everything and changing feed/speed last. Solid setup I believe.

Sparky961 · Apr 5, 2018

I'd be trying 150 to 250 SFM and 0.001" to 0.002"/REV.

When plunging, keep your depth cuts to less than 1x insert width, width of subsequent plunges about 75 to 95 percent of width. Everything must be rigid and well flooded with coolant, preferably a little on the rich side but not necessary.

This has worked well for me on a SKT21 (turning centre), though it is less DOC than most are likely to claim possible.

SmlG54 · Apr 5, 2018

Many thanks for response. Much appreciated.
-Coolant is flooding but maybe hindered by shaving collection around tool. Insert has no chip breaker. ,002 radius on edge.
-called tool Flo today and looked at sfm chart for application, 250-700 for grooving with grade of insert. Pretty wide range huh? Also said less than .003/rev may cause work hardening???? I have no clue.
-total plunge radially is less than width of insert.

brian.pallas · Apr 5, 2018

So, make your first pass in the middle of the groove? Work your way out. Instead of plunging full width a thou from your finish size. I think .01 on X is heavy. I assume you are side turning with the groover on the finish? .001 or .002 per side is good IME.

Also, does the tool come down each wall, or is it down one wall, across the groove and then up against other wall and up? Change it to coming down both walls if it isn't.

Sparky's feeds and speeds are the range I'd be in to start.

Sparky961 · Apr 5, 2018

As long as it isn't getting hot and you're removing material, you aren't hardening it. I've run up to 350 SFM and found tool life suffers. That's my two cents. I'd bet on widely varying opinions on this.

SmlG54 · Apr 5, 2018

Thank you.
Yeah, it's programmed for finish front side wall, final dia, groove width and then back wall and up cutting.

You said middle of groove..? What should change.

BTW, aside from first pass, sounds clean for stainless on non full engagement passes at current sfm......although tooling rep was surprised at speed I said I attempted. He said 200-300sfm.

SmlG54 · Apr 5, 2018

From what I've seen Sparky, not many people agree on 304

Sparky961 · Apr 5, 2018

Brian raises two good points for finishing. Plunge the walls, and don't leave much on the diameter for finishing.

Most grooving tools don't do well with side loading but end loads are ok. That said you can use the deflection to your advantage and get a "wiper" effect for a really nice chatter-free finish. But that's another topic entirely.

Sparky961 · Apr 5, 2018

SmlG54 said:
From what I've seen Sparky, not many people agree on 304

Agreed.

cyanidekid · Apr 5, 2018

Well,there isn’t much to agree on! “304” is a shitbasket of unknowns. It’s all over the place in machinability and actual analisys.

SmlG54 · Apr 5, 2018

So .01 is to much? Ok no problem.
But wiper effect, do you care to briefly descirbe???

SmlG54 · Apr 5, 2018

cyanidekid said:
Well,there isn’t much to agree on! “304” is a shitbasket of unknowns! It is all over the place in machinability and actual analisys.

Well shit, how to people economically go from one batch of 304 after all the problems have been solved to another batch. Bleh

Sparky961 · Apr 5, 2018

Think about how the insert would be engaging the material if you are feeding to the left and the tool bends in the opposite direction due to cutting force. Just the leading corner is touching and then a very slight wedge shaped gap that serves to clean up the cut made by the corner. At least, that's how I understand what's happening. Feed too slow and you get chatter due to lots of tool engagement area, feed too fast and bad things happen.

Sparky961 · Apr 5, 2018

Sure, there's some variability in the material. But if you keep numbers conservative you shouldn't have big problems. With the right cutting parameters, carbide tools, and LOTS of coolant, it shouldn't be much harder to work with than mild steel.... But a lot easier to get a nice finish. I like working with 304 and 316.

Bobw · Apr 5, 2018

SmlG54 said:
Well shit, how to people economically go from one batch of 304 after all the problems have been solved to another batch. Bleh

I've been trying to figure that out for years.. It goes from shitty, to crappy, to miserable, and then back to just shitty.

And that is all in the same bar...

304 sucks... Inconel sucks too, but at least you know how much its going to suck EVERY TIME..
Its going to suck "X" amount today, its going to suck "X" amount at the other end of the bar, its
going to suck "X" amount next week, and even next month and even next decade.. No such consistency
with 304.

They really should just rename 304 as "Shiny Shitty Mystery Metal".

SmlG54 · Apr 5, 2018

Haha. It's funny, 1st two weeks on job I've had to gun drill 7in deep hastalloy, monel and work with 304. What a start?; At least it gets all the B's out of the way... I guess 4140 are for "Fridays'

But seriously.... Plunge to final depth on groove walls or leave a hair?? Drop sfm to 209......I did that. 400sfm plus soundest cleanest buy Chipping flank of insert. I'm gonna get fired....

Sparky961 · Apr 5, 2018

Any chance you can use a narrower tool? Even if you need to take multiple depth passes, it may work out better for you. I stand by the feeds/speeds I suggested though.

SmlG54 · Apr 5, 2018

Nah, boss wants this tools and grade.

I suggested grooving inserts with chip breakers but said chip chip breaking doesn't matter. I Dunn

Sparky961 · Apr 5, 2018

Plunge within 0.002 of finish, assuming you have everything dialed in and you know you actually have that left. Leave 0.001 on the walls. When you finish, come down one wall plunging, turn the corner and feed a bit past half way on the diameter. Retract and repeat coming down the other wall.

Sparky961 · Apr 5, 2018

Never had the chance to work with Hasteloy, Monel, Inconel, or Titanium yet.... But 4140 (A or HT) is a pleasure to machine.

Grooving stainless steel 304. I know, more stainless...

Aluminum

Cast Iron

Aluminum

Hot Rolled

Cast Iron

Aluminum

Aluminum

Cast Iron

Cast Iron

Titanium

Aluminum

Aluminum

Cast Iron

Cast Iron

Diamond

Aluminum

Cast Iron

Aluminum

Cast Iron

Cast Iron

Similar threads