Low tool life when turning 316L stainless steel

soyasaus · May 23, 2018

Hello! I'm new on this forum. Glad to see there is an active machinist forum here.

I'm wondering if you could give me some tips for improving tool life when turning stainless steel (usually 316, sometimes 904)

The tool starts to chip/wear out after like 10 cuts, it still works but the finishing is worse and it makes more noise.

So the insert I'm using is KNUX 16 04 05R11 2025
Cutting speed is usually around 80-100m/min with a feedrate of around 0.25mm/rev
Tend to take 2mm deep cuts, can do 2.5-3mm but it seems to work alot better at 2mm
This is manual turning with a pretty old lathe (Colchester Triumph 2000 if I recall)

So yeah, I don't know if its actually that bad but I tought I'd ask cuz I feel like I might be doing something wrong.
Any ideas?

Kbdutson · May 23, 2018

I ran into this same problem on my last job. Same mat. I was getting longer life out of molded thread ins. over ground. I called tool company and they recomend increasing rpm speed. It worked great. Call your rep and ask what the specs for that mat and tool are. A simple change in feed and speed was all I needed. I went about 30% faster actually. Was nice bonus to cut cycle time too

Mechanola · May 23, 2018

You want a negative geometry tool, not such a positive one. Then less depth but more feed at roughing. One millimeter max., double feed rate. Try to make hot tiny curly chips. Don’t cut, scrape. It goes even further in that direction with nickel alloys.

Kbdutson · May 23, 2018

Oh, and went from about 6 parts to about 60 on tool life

HuFlungDung · May 23, 2018

The insert coating is of great importance, too. I like the Sandvik grade 1125. Proper chip breaker is also important to create the proper chip curl and to avoid having the chip erode away the insert under the cutting edge. Also a negative lead angle attitude (instead of square on) of the insert toolholder can help direct the chip to break against the shoulder of the cut instead of breaking against the insert.

DMF_TomB · May 23, 2018

soyasaus said:
Hello! I'm new on this forum. Glad to see there is an active machinist forum here.

I'm wondering if you could give me some tips for improving tool life when turning stainless steel (usually 316, sometimes 904)

The tool starts to chip/wear out after like 10 cuts, it still works but the finishing is worse and it makes more noise.

So the insert I'm using is KNUX 16 04 05R11 2025
Cutting speed is usually around 80-100m/min with a feedrate of around 0.25mm/rev
Tend to take 2mm deep cuts, can do 2.5-3mm but it seems to work alot better at 2mm
This is manual turning with a pretty old lathe (Colchester Triumph 2000 if I recall)

So yeah, I don't know if its actually that bad but I tought I'd ask cuz I feel like I might be doing something wrong.
Any ideas?

.
1) tool life with stainless is normally less than 30 minutes. sure maybe 60 minutes in some cases but an abrasive alloy will always wear faster. some bars or batches of metal can be full of slag or hard spots and tool life can be 10x shorter. hit a piece of slag size of grain of rice i have seen 60 inserts totally destroyed trying 10 times and failing all 10 times even with different feeds and speeds tried. ground out slag piece and then machined first time without slightest problem
.
2) vibration can destroy cutting edges fast. same feeds and speeds can easily work on one machine and part but not on another machine and part
.
3) coolant ? some alloys really cut better with longer tool life if not done dry
.
4) feeds and speeds. what is cutting tool manufacturer recommendations ?? remember free advice from some and your cutting tool might be white hot and melted in less than 5 minutes. obvious got to consider cost of failure and scrapping part and damaging tool holder
.
5) if all else fails i would read what cutting tool manufacturer recommends and normally they list maximum and normally got to reduce a bit for reasonable tool life

soyasaus · May 23, 2018

Thanks all for the replies.
So from what I've gathered I should maybe try upping the RPM and/or feed and try smaller cuts?
I also understand a negative-angled insert should be more ideal for SS? I think this 2025 insert I'm using is positive, I'll see what else I can try.

HuFlungDung said:
The insert coating is of great importance, too. I like the Sandvik grade 1125. Proper chip breaker is also important to create the proper chip curl and to avoid having the chip erode away the insert under the cutting edge. Also a negative lead angle attitude (instead of square on) of the insert toolholder can help direct the chip to break against the shoulder of the cut instead of breaking against the insert.

I think I we got some 1125 (in black) lying around that I will try.

Mechanola said:
You want a negative geometry tool, not such a positive one. Then less depth but more feed at roughing. One millimeter max., double feed rate. Try to make hot tiny curly chips. Don’t cut, scrape. It goes even further in that direction with nickel alloys.

Don't cut, scrape? I've always thought that for SS alloys ur supposed to cut continually to not wear out the tool

DMF_TomB said:
.
1) tool life with stainless is normally less than 30 minutes. sure maybe 60 minutes in some cases but an abrasive alloy will always wear faster. some bars or batches of metal can be full of slag or hard spots and tool life can be 10x shorter. hit a piece of slag size of grain of rice i have seen 60 inserts totally destroyed trying 10 times and failing all 10 times even with different feeds and speeds tried. ground out slag piece and then machined first time without slightest problem
.
2) vibration can destroy cutting edges fast. same feeds and speeds can easily work on one machine and part but not on another machine and part
.
3) coolant ? some alloys really cut better with longer tool life if not done dry
.
4) feeds and speeds. what is cutting tool manufacturer recommendations ?? remember free advice from some and your cutting tool might be white hot and melted in less than 5 minutes. obvious got to consider cost of failure and scrapping part and damaging tool holder
.
5) if all else fails i would read what cutting tool manufacturer recommends and normally they list maximum and normally got to reduce a bit for reasonable tool life

1) Well that means my setup might not actually be too shabby as they usually last 30 min or more when I only do 2mm deep cuts. Sometimes they wear out really fast though... Does turning a "used" steel shaft matter, because of tension in the material or something?

2) I actually think vibration is less of a problem in this setup. Feels rather stable this old lathe

3) Always use coolant

4) I usually just go by the book and try small changes in feedrate and cut depth now and then.

5) Where do you even find manufacturer recommendations? If I go to:
knux 16 4 5r11 225
it shows me the different values of this cutting insert but not any recommendations to speed/feed/depth of cut. I see they got a calculator but I'm not advanced enough to use that stuff

Mike C. · May 23, 2018

Are you running any kind of coolant or cutting oil? I do a lot of modified 304 and 316 pipe flanges on a Pacemaker. I just hose it down with Tap Magic and it definitely extends cutter life. I try to run about 100f-150ft/min and get plenty tool life. Problem with stainless is that it is a poor conductor of heat. Heat tends to run back into the cutter rather than into the work or chip. If it's just burning up the edge, you may have to slow down instead of speeding up.

soyasaus · May 24, 2018

Mike C. said:
Are you running any kind of coolant or cutting oil? I do a lot of modified 304 and 316 pipe flanges on a Pacemaker. I just hose it down with Tap Magic and it definitely extends cutter life. I try to run about 100f-150ft/min and get plenty tool life. Problem with stainless is that it is a poor conductor of heat. Heat tends to run back into the cutter rather than into the work or chip. If it's just burning up the edge, you may have to slow down instead of speeding up.

Yeah I use coolant running from a pump aimed straight at the cut. If I don't use coolant it starts glowing hot red "in" the cut. So yeah I've noticed SS is a pretty shit conductor of heat :P

But I actually run at quite a bit higher cutting speed than u at around 260-330ft/min. So yeah I might be pushing it a bit hard for the tool to handle.

What tool insert do you use for SS and how long does it usually last for you?

eKretz · May 24, 2018

For certain stainless steels, you want higher speed and SLIGHTLY lower feed. If you go too low on the feed you will run into the work hardening problem. For others, lower speed and higher feed works better. Usually the former is for some of the difficult and the latter for more common stainless steels. If you're experienced, you ought to be able to see generally what parameters need to be adjusted and which way just by looking at the worn tool's cutting edge. (I.E. if there's cratering, built up edge, etc. Examine the edge as you go, don't wait for the tool to break. Optimal coating and geometry are key for best tool life as well. It does sound as though your speed may be a little high, but just to clarify, is the edge wearing or chipping out? The vast majority of stainless steel roughing work I did was at cutting speeds around 250ft/min. With full food coolant. It can also help a LOT when roughing to increase the tool's lead angle (or use a different tool with greater lead angle) and thin the chip out.

soyasaus · May 24, 2018

Mike C. said:
Are you running any kind of coolant or cutting oil? I do a lot of modified 304 and 316 pipe flanges on a Pacemaker. I just hose it down with Tap Magic and it definitely extends cutter life. I try to run about 100f-150ft/min and get plenty tool life. Problem with stainless is that it is a poor conductor of heat. Heat tends to run back into the cutter rather than into the work or chip. If it's just burning up the edge, you may have to slow down instead of speeding up.

eKretz said:
For certain stainless steels, you want higher speed and SLIGHTLY lower feed. If you go too low on the feed you will run into the work hardening problem. For others, lower speed and higher feed works better. Usually the former is for some of the difficult and the latter for more common stainless steels. If you're experienced, you ought to be able to see generally what parameters need to be adjusted and which way just by looking at the worn tool's cutting edge. (I.E. if there's cratering, built up edge, etc. Examine the edge as you go, don't wait for the tool to break. Optimal coating and geometry are key for best tool life as well. It does sound as though your speed may be a little high, but just to clarify, is the edge wearing or chipping out? The vast majority of stainless steel roughing work I did was at cutting speeds around 250ft/min. With full food coolant. It can also help a LOT when roughing to increase the tool's lead angle (or use a different tool with greater lead angle) and thin the chip out.

Seems like cratering is whats mostly happening. Has also had a small part of the tip break off sometimes but that's when I've pushed it too hard.

I'm using Sandvik 2025 insert which from what I've read is supposed to be decent at SS. Geometry might be less than ideal on the one I use though.

Is there any feedrate you would consider "default" when turning SS? This is 316L I'm turning now.

Didn't get to test anything today as I was busy with other things but I'll experiment with some other inserts and different feedrates tomorrow

eKretz · May 24, 2018

I would first try switching to something that has a larger lead angle. If you can get away with it use a square insert set at 45° - as far as geometry I always had good luck with the old school method on tougher stainless - a flat square positive insert with a chip breaker. You should be able to get both feed and depth of cut up this way. Maximizing tool life was necessary on a lot of our jobs because we'd have cuts 10 feet long on a pretty large diameter (10"+). For cratering or notching it can help to vary depth of cut on consecutive cuts also. A lot of times cratering (assuming behind the edge) is too much speed/heat.

As far as feedrate, no default. Take the max you can get away with. The job is best done with maximum work in minimum time. Thinner inserts will require less feed, thicker inserts can take more. The rigidity of the part and machine will also play a large role.

soyasaus · May 25, 2018

eKretz said:
I would first try switching to something that has a larger lead angle. If you can get away with it use a square insert set at 45° - as far as geometry I always had good luck with the old school method on tougher stainless - a flat square positive insert with a chip breaker. You should be able to get both feed and depth of cut up this way. Maximizing tool life was necessary on a lot of our jobs because we'd have cuts 10 feet long on a pretty large diameter (10"+). For cratering or notching it can help to vary depth of cut on consecutive cuts also. A lot of times cratering (assuming behind the edge) is too much speed/heat.

As far as feedrate, no default. Take the max you can get away with. The job is best done with maximum work in minimum time. Thinner inserts will require less feed, thicker inserts can take more. The rigidity of the part and machine will also play a large role.

Nice! Do you mean a lead angle something like this: http://www.superprecision.com/images/cutting_forces_g2.jpg
At the bottom right corner?

Was busy today as well so didn't get to mess around with anything today either though

DMF_TomB · May 25, 2018

i would read what the cutting tool manufacturer recommends. remember at maximum tool life might be 10 minutes. better places offer a recommended range of sfpm and ipt
.
you always going to hear from somebody claiming they machine at 2000 sfpm at .050 ipt get great mirror finish and tool lasts 15 years machining 8000 tons of parts
.
i remember trying a feed and speed recommendation from internet and tool got white hot and melted in less than 5 minutes. just saying at least with cutting tool manufacturer recommendations they tend to give reasonable max limits or a reasonable recommended range of settings to try.
.
tool life i would write down feed and speeds settings with standard tools made to precise sizes (tool stick out amounts, etc) and record your data results. as you try different settings you will record sudden tool failures and tool life data and can make your own feed and speed charts

eKretz · May 25, 2018

Lol, cutting tool manufacturer recommendations are a starting point only. Not sure if I should be insulted at this point Tom. I don't think I made any outrageous claims at all, and I assure you I have had plenty of experience machining difficult materials and parts. Have you ever tried differing lead angle tools in difficult materials? I think by the sound of your comment you would be very surprised. Anyone who has any experience should already have a general idea where to start with speeds and feeds. New coatings and geometries are great and all, but they aren't going to make a seismic shift in tool abilities. They are good and they do help increase productivity, every little bit helps, but the final arbiter should always be the cutting edge. SEE what is going on for yourself and adjust from there. There are too many variables in machining to just grab some numbers out of a book or data sheet and expect that to do better than your own optimization.

eKretz · May 25, 2018

soyasaus said:
Nice! Do you mean a lead angle something like this: http://www.superprecision.com/images/cutting_forces_g2.jpg
At the bottom right corner?

Was busy today as well so didn't get to mess around with anything today either though

Yes, exactly. The higher lead angle will often cut better in difficult to cut materials. The downside is you can't cut to a square shoulder.

DMF_TomB · May 25, 2018

i not saying you will not get different results with a different tool or tool orientation
.
my experience is cutting tool manufacturer recommendations are the best starting point but if they are max recommendations they usually are reduce 10% to 50%
.
keeping your own notes on results you get with tools and feeds and speeds is best. many long skinny tools vibrate or long skinny parts vibrate and feeds and speeds need a lot of adjustment from normal recommendations

soyasaus · May 26, 2018

eKretz said:
Yes, exactly. The higher lead angle will often cut better in difficult to cut materials. The downside is you can't cut to a square shoulder.

That is good to know!

It is a bit annoying that it leaves a tapered shoulder but that can always be fixed after

RC Mech · May 26, 2018

Some good suggestions in this thread (except for Tom's, but that's par for the course) but only Mechanola touched on it in Post #2: cut the DOC. You're cutting at 0.080"-0.018". I just finished some 304 reaction vessels on the same Colchester- that cut is a bit much for these machines in 316. Cut your DOC in half and kick up the feed to at least 0.012"/rev from the 0.009"/rev. Follow the suggestions regarding rake angle and you should be laughing.

Low tool life when turning 316L stainless steel

Plastic

Plastic

Stainless

Plastic

Diamond

Diamond

Plastic

Diamond

Plastic

Diamond; Mod Squad

Plastic

Diamond; Mod Squad

Plastic

Diamond

Diamond; Mod Squad

Diamond; Mod Squad

Diamond

Plastic

Stainless

Similar threads