What's new
What's new

Cutting 316L with long tools

QNelson18

Plastic
Joined
Nov 28, 2023
Hello, this is my first time posting. I am currently trying to machine 316L in an older (late 90's early 2000's-ish) Fadal VMC 4525 that has a cat40 spindle. I am trying to machine a total depth of 3.27 inches deep. I have broken 4 300$ cutters already in my attempts at doing this. I have gone through Helical trying to do this using their 5 flute 4" LOC endmill which broke after pulling out of an ER collet holder running 800sfm and .0027 FPT which before pulling out was actually cutting pretty well. Switched to a 7 Flute chip breaker tool from helical and used their recommended feeds and speeds. On the first tool it broke immediately when it touched material, called an apps engineer from helical and tried his recommendation and still broke after about 10 seconds in the cut. I was using an endmill holder for those tools. I currently have a kennametal kor5ds .750 dia. 5 flute 3.75 flute length and am now facing extreme chatter while cutting the part. I have tried 450sfm with .0045 FPT at a .037 RDOC, then down to 350sfm and .003 FPT at .05 RDOC, then after talking to tech support went to 450sfm and .0035 FPT at a .075 RDOC and still lots of chatter. I am using the 2d dynamic roughing toolpath in mastercam.

Any help will be extremely appreciated. I am at my wits end with this job.
 
Just wow. Where did you get those numbers? I used the Haas tooling website because I knew I could quickly come up with a stainless-tailored end mill somewhat matching your parameters. The longest 3/4" endmill they have for stainless is a 2.5 LOC 5-flute. It says 200-230 SFM at 0.0025" FPT. You're trying to take another 3/4" deeper than that?

Also: your radial engagement is so low that the cutter is going to do nothing but try to climb on top of the material. 10-15% radial is where you need to be to get it to cut instead of just rubbing and chattering like crazy. But this is going to have considerable forces involved and with 5-7 flutes engaged, the whole thing is going to be a giant screw, trying to pull the work up and the cutter down. In an ER holder, you're going to need to torque the thing to value and make sure the shank and collet are spotless clean. I'd be looking at shrink fit or hydraulic holders. That cutter is going to have a lot of loads going on.
 
are all these tools you're referencing .750" diameter? I assume these speeds and feeds are your roughing passes?

800 SFM on 316L in a collet holder is straight up bananas LOL unless you were trying some sad version of high efficiency milling.
I agree about radial with Donkey, you're running 5% stepover and that may not be enough.

Depending on part quantity and how important cycle time is, I would be temped to get multiple .75 dia tools with minimal LOC and varying necked back clearance. I have ran a lot of 316L on haas' and I prefer high radial, low axial passes for roughing. With the decreased load I can at least get decent feed without tossing a part out/pulling a tool.
 
Just wow. Where did you get those numbers? I used the Haas tooling website because I knew I could quickly come up with a stainless-tailored end mill somewhat matching your parameters. The longest 3/4" endmill they have for stainless is a 2.5 LOC 5-flute. It says 200-230 SFM at 0.0025" FPT. You're trying to take another 3/4" deeper than that?

Also: your radial engagement is so low that the cutter is going to do nothing but try to climb on top of the material. 10-15% radial is where you need to be to get it to cut instead of just rubbing and chattering like crazy. But this is going to have considerable forces involved and with 5-7 flutes engaged, the whole thing is going to be a giant screw, trying to pull the work up and the cutter down. In an ER holder, you're going to need to torque the thing to value and make sure the shank and collet are spotless clean. I'd be looking at shrink fit or hydraulic holders. That cutter is going to have a lot of loads going on.

I have been getting my numbers from the manufacturer of the tools and calling the tech support lines. I don't really care at this point how I get there just need to cut 3.27" deep. My latest attempt was at .075 (10%) radial but the part has been stopped mid cycle from other attempts so I was thinking the chatter was because it didn't make it to its full radial yet just sounded so bad that I was afraid it wouldn't last long enough to get there. I was considering hydraulic but we have already spent so much on tooling that on this job not sure if the boss will buy off on buying a new expensive holder. After that first tool pulled out we switch to an endmill side locking holder but honestly had more success with the collet than now other than the whole pulling out problem.

are all these tools you're referencing .750" diameter? I assume these speeds and feeds are your roughing passes?

800 SFM on 316L in a collet holder is straight up bananas LOL unless you were trying some sad version of high efficiency milling.
I agree about radial with Donkey, you're running 5% stepover and that may not be enough.

Depending on part quantity and how important cycle time is, I would be temped to get multiple .75 dia tools with minimal LOC and varying necked back clearance. I have ran a lot of 316L on haas' and I prefer high radial, low axial passes for roughing. With the decreased load I can at least get decent feed without tossing a part out/pulling a tool.

Yes, all the tools have been .750 diameter. It is my roughing passes. I also thought 800 sfm was crazy but that cutter at those feeds and speeds was cutting really nice, had a good sound and finish until it pulled out. Boss just bought these current tools and I know he is going to want me to make them work but push comes to shove he will probably agree to switching tooling. Do you have a recommendation for who to get the long reach cutters from?

Have you thought of plunge milling most of the material out and then running a rougher and finish tool through it?

I have not given that much thought I have little experience with plunge milling.



I appreciate all the quick responses thank you guys!
 
Okay, on that Kennametal KOR 5 is supposed to be a badass rougher. I know the Titans of CNC channel has pimped that whole line. Most of their videos I found were in aluminum but, this is the KOR 6 in stainless. Looks a lot like what you're trying to do. I'd probably start with their recipe and see if the machine can take it. Man, I don't know if I'd rather have an ER32 cranked to 100 ft/lbs or a solid holder with a retaining screw. I like the rigidity of a solid holder but, you're fighting a lot of pull-out load.

 
Yes, all the tools have been .750 diameter. It is my roughing passes. I also thought 800 sfm was crazy but that cutter at those feeds and speeds was cutting really nice, had a good sound and finish until it pulled out. Boss just bought these current tools and I know he is going to want me to make them work but push comes to shove he will probably agree to switching tooling. Do you have a recommendation for who to get the long reach cutters from?
Out of all of your options, I would probably prefer to run in a side-lock holder. When running speeds and feeds from manufacturer recommendations (like a chart) it's always good to keep in mind your tool stickout. When they give a range of SFM and IPT that usually isn't for over 4.25xD stickout like what you are trying to achieve. The longer my tool is hanging out the lower I'll run the SFM and chip load.

with all that being said, I really don't run long ass LOC endmills. Never had great performance from them, at least with the spindles/toolholding I was working with at the time.
 
I'd whistle notch the shit out of that endmill if I was running it in a side lock. I personally like hydraulics for an app like this.
SFM sounds crazy for 316L and I agree with the low radial engagement as donkey brought up. Plunge rough might not be a bad idea, get as much of that crap out of the way as possible. I do a fair amount of deep cavity work in H13 and my go to is a helical 5 flute that has just 3/4" flute length at the end and a slightly undercut shank. They are WAY stiffer and much less prone to breakage when they re-cut a chip.
 
This is also in a 40-taper machine. Small taper + skinny cutter (relative to length) + ER-32 stickout = floppy as cooked spaghetti.

2 options I'd try for roughing (depending on exactly what you're attacking):

- Corncob rougher (even an HSS one would work). Slow, but easy-cutting and not prone to chatter

- Insert cutter (like a WEZ from Sumitomo). Take full width, low axial cuts like the Radical Kyle said above.

Someone mentioned a sidelock - if you can get a sidelock or a hydraulic holder that'll swallow the shank all the way to the gage line, you'll be ahead of the game vs. ER-32. As I hinted above, you're running near the rigidity limit of a Fadal with a 40-taper.
 
Another factor is taper wear on a machine that old. Probably lots of it.

It sounds like you are taking the full depth at one shot. That's a ton of side force working on a marginal spindle taper. Step it down. Sure it'll take longer but not as long a breaking every cutter you buy.
 
I'm trying some 1/2" YG PM60 "only one" serrated cutters on my '97 vintage Feeler FV-800 with a BT-40 taper in 304L and have had good luck for the price. At $70ish CAD and running a 50% step over and 10mm DOC I was very impressed. Cutter was in good shape and looked as new after roughing for 20 min straight. This was using straight flood coolant. Often, slow and steady is worth it on low volume jobs.
 








 
Back
Top