How Many Parts Are You Getting With Your Parting Tool?

Hi Everyone! I’m not sure we’re getting the most from our parting tools. Everything is low/med-alloy annealed steel (4140, 41L40, 1215, etc) between, say, 1/4” and 1-1/4” diameter. We’re using Iscar Tangs and getting maybe 500-1000 pcs in general with 2.4mm wide inserts. I even spring for the thru-tool coolant holders since our machines have HPC but still feel we should be getting more parts. I default to 400SFM and .003ipr with G96. It’s barfed work and the machines have sub spindles. Does that sound like reasonable tool life to you or way low? There’s not many variables I could change other than insert grade, speed and feed I suppose so just thought I would do a quick reality check. Thanks for any feedback!

What's the actual coolant, and the mix? Filtered or not? And is there any chance of converting to oil?

We were using Blaser Swisslube oil and we changed to something comparable but cheaper...still oil. There’s a filter bag in the high pressure pump, not sure what the mesh size is though.

I know it’s a very “general” question and we DO tend to get more pieces when running the smaller parts than the larger ones. Oh, and some of the machines use a larger 4mm cutoff that seems to last longer than the smaller 2.4mm. The machines that use the 2.4mm wide inserts are newer so maybe my problem is that I am comparing that life to the older machines that all use 4mm?

Edge life is still the same with the cheaper oil?

Can you post some close-up pics of damaged edges? Are all the machines wearing or failing inserts the same way? And are there parameters that are different between the machines using 2.4mm and 4mm inserts?

And no question that the inserts are correctly supported and at the right heights?

Just fishing, of course, but more info will help others interpret and make suggestions.

Your tool life seems a little low. What are the recommended cutting conditions for the insert you're using? I use 2 mm wide Tungaloy cutoff inserts and am usually at .005 ipr in steel, so your feed seems low to me, but I'm not familiar with your insert.

I think Milland asked very good questions. Can we assume that you're getting corner wear and changing the inserts due to poor surface finish?

Actually that is too many variables! 1 1/4 4140 I would be happy with 500 pcs per edge.
1/4 diameter 1215 30,000 pcs per sharpening with cutting oil and high speed blades would not impress me.

https://www.youtube.com/attribution...gzgpRdwyUIWBX0zQFV4AaABAg&feature=em-comments

Link is a screw machine running 11/32 12L14, the customer orders parts by the bucket fulls, I would guess 30 to 40 K per sharpening. Running filtered Mobilmet cutting oil, variable speed drives on the spindle and feed so I have no clue what the speed and feeds are.

I can try to get a close up on Monday.

I cannot commit to an answer regarding if tool life is been affected with the new oil because the new(er) Swiss machines that use the oil are largely running jobs for the first time or two so we don’t have much history to compare them to *on those machines*....just what life used to be on the older fixed headstock Hardinges that run water-soluble oil with the 4mm tang grips. I was expecting the Swiss machines to get much longer life since they’re running oil, and high-pressure oil thru the tool at that! I suppose it’s possible the thinner inserts are costing more life than is being saved with the thru-tool oil?

Regarding failure mode, it seems like the inserts are either in very good shape or they explode and melt the holder. I look at the insert at, say, 500 pcs and it looks great so I put it back in but before I check it again it’s gone (and the holder with it...) So I’ll set the tool life to, say, 500 pcs and just switch it out the next time even though the insert looks okay...(I don’t have ALL the time in the world to optimize exactly how many parts we can get out of each insert on every job) but I don’t think we have any used inserts that are showing any wear you can at least feel with your fingernail. So the bucket of used carbide has inserts in seemingly-good shape but swapped out out of fear of blowing up the holder. Maybe that’s just what you get with a 2.4? The 4mm seem to show wear more detectably before blowing up. The larger Swiss machine uses 3/4” tooling which allows for the same 4mm insert and that one behaves like they do in the Hardinges...pay reasonably close attention and you’ll SEE the failure coming over the course of 100 or more parts and have time to catch it and switch out the insert before failure.

The cutting parameters are pretty much the same..300-400 SFM and .003/.004 IPR G96, G50S3000 on the Hardinges and G50S5000 on the Tsugamis...we’ll reduce that if the bars rattle too much at top end RPMs. The insert box recommends something like 200-500 and .002-.007.

The insert height is perfect on the Tsugamis since Y is just a button press away but the Hardinges are all over the place (no Y) even though they have greater life...but maybe that’s entirely due to the 4mm width?

I almost always check for wear by dragging my finger along the cutting edge and the corner of the insert that faces away from the main spindle since THAT is the corner that always chamfers the back side of the part during cutoff so it SHOULD wear before the other corner. Maybe that’s not a good method for cutoffs?

I don’t want to turn this into a giant project to eek out another 10% or whatever if 500-1000 pcs seems reasonable. I just want to make sure everyone else isn’t getting like 5,000 parts when cutting off 1/2” 41L40!

Thanks for any input!

FredC said:

Actually that is too many variables! 1 1/4 4140 I would be happy with 500 pcs per edge.
1/4 diameter 1215 30,000 pcs per sharpening with cutting oil and high speed blades would not impress me.

https://www.youtube.com/attribution...gzgpRdwyUIWBX0zQFV4AaABAg&feature=em-comments

Link is a screw machine running 11/32 12L14, the customer orders parts by the bucket fulls, I would guess 30 to 40 K per sharpening. Running filtered Mobilmet cutting oil, variable speed drives on the spindle and feed so I have no clue what the speed and feeds are.

Click to expand...

Ha! Yeah, I know that’s quite a range of operating parameters I threw out there but what you said is VERY helpful...500ish pcs in 1–1/4”ish 4140ish not so bad but expecting tens of thousands of parts in 1/4”ish 1215ish.

God I love those old screw machines...like watching a lava lamp!

I use a lot more high speed drills than I used to because the carbide is so brittle it doesn’t always give you a lot of warning like the HSS does. I suppose the same effects could be present in cutoffs!

Thank you!

Nerdlinger said:

I use a lot more high speed drills than I used to because the carbide is so brittle it doesn’t always give you a lot of warning like the HSS does. I suppose the same effects could be present in cutoffs!

Thank you!

Click to expand...

That's one thing I wonder about - perhaps the machine's (relative) lack of rigidity is hurting you on carbide insert life?

Any way you could swap in a holder for "blade" style parting tools? I'd look at a cobalt steel or PM steel for the blade for good wear life, and perhaps going thinner (2mm or less) if you can keep the stiffness to stickout acceptable.

Cut the forces, get a little more toughness in the cutter, and after a little testing you might get a much more reliable parting.

But if testing time isn't warranted and you're OK with ~500pcs/edge, then I don't know what to say. To me, that seems really short lived, but I'm not a production expert. The last time I did real production was during Co-Op at tech HS, decades ago.

Teachmeplease does a lot of Swiss work, maybe you can pm him and ask what he'd doing for parting tooling. Maybe there's a better system you could look at.

Do not forget to ask the tool rep about recommended grades. Completely different inserts are needed for 4140 and mild steel.

Thanks, guys! I believe the machines are (relatively) tight for the work they do so I do not thing it is a rigidity problem. The stick out is at a minimum for the tools as they slide up to the “head” of the holder. Just from the last couple comments it seems like I’m probably operating at a “C” on my parting ops so I’ll look into it more closely. I hope I can get the Iscar Tang Grips to work as we’ve invested in a few holders, they work well for us in the 3/4” shank (4mm wide insert) version, they’re easy to change out inserts, and they were overwhelmingly popular on a recent PM thread titled something like, “What’s your favorite cutoff tool?”

I’ve been setting up a lot of new operations in those new machines but for the most part all those programs are written and have run once or twice. So they’re making parts but now it’s time to work out the kinks...like questionable cutoff tool life.

Thanks, again!

I loved these things, no idea if you have a way to hold the holders but might be worth a try

C & H Butt Brazed Cutoff Tools

I used the skinniest ones, 1/8". Saved material They hold the inserts so much more securely, might be the reason they work so well ?

So you're running soluble oil in the Hardinges?

I feel like that is important - just about every modern cut off is optimised for soluble oil in that the chip former relies on the extremely rapid cooling of the chip to work effectively. The deep spherical groove in the centre of just about every modern cut off insert on the market is there to form the chip to be narrower than the groove so that it ejects freely and doesn't jam. The function is heavily dependent on the chip being cool the instant it is separated from the material, and that is just not going to work so well with cutting oil as it does with soluble oil.

Note that this is just the theory as I have read/been told it and not something that I have observed in practice - I do not run cutting oil in any of my machines.

3

[rather a lot really]

Nerdlinger said:

I can try to get a close up on Monday.

I cannot commit to an answer regarding if tool life is been affected with the new oil because the new(er) Swiss machines that use the oil are largely running jobs for the first time or two so we don’t have much history to compare them to *on those machines*....just what life used to be on the older fixed headstock Hardinges that run water-soluble oil with the 4mm tang grips. I was expecting the Swiss machines to get much longer life since they’re running oil, and high-pressure oil thru the tool at that! I suppose it’s possible the thinner inserts are costing more life than is being saved with the thru-tool oil?

Regarding failure mode, it seems like the inserts are either in very good shape or they explode and melt the holder. I look at the insert at, say, 500 pcs and it looks great so I put it back in but before I check it again it’s gone (and the holder with it...) So I’ll set the tool life to, say, 500 pcs and just switch it out the next time even though the insert looks okay...(I don’t have ALL the time in the world to optimize exactly how many parts we can get out of each insert on every job) but I don’t think we have any used inserts that are showing any wear you can at least feel with your fingernail. So the bucket of used carbide has inserts in seemingly-good shape but swapped out out of fear of blowing up the holder. Maybe that’s just what you get with a 2.4? The 4mm seem to show wear more detectably before blowing up. The larger Swiss machine uses 3/4” tooling which allows for the same 4mm insert and that one behaves like they do in the Hardinges...pay reasonably close attention and you’ll SEE the failure coming over the course of 100 or more parts and have time to catch it and switch out the insert before failure.

The cutting parameters are pretty much the same..300-400 SFM and .003/.004 IPR G96, G50S3000 on the Hardinges and G50S5000 on the Tsugamis...we’ll reduce that if the bars rattle too much at top end RPMs. The insert box recommends something like 200-500 and .002-.007.

The insert height is perfect on the Tsugamis since Y is just a button press away but the Hardinges are all over the place (no Y) even though they have greater life...but maybe that’s entirely due to the 4mm width?

I almost always check for wear by dragging my finger along the cutting edge and the corner of the insert that faces away from the main spindle since THAT is the corner that always chamfers the back side of the part during cutoff so it SHOULD wear before the other corner. Maybe that’s not a good method for cutoffs?

I don’t want to turn this into a giant project to eek out another 10% or whatever if 500-1000 pcs seems reasonable. I just want to make sure everyone else isn’t getting like 5,000 parts when cutting off 1/2” 41L40!

Thanks for any input!

Click to expand...

I run screw machines with HSS cutoff tooling. I dont use carbide unless it is a ring or the tool doesnt have to go below .250: due to chipping the carbide.

If I have anything difficult to machine I use Tantung cutoff blades. I have had tremendous success with them over the years. Very easy to sharpen.

I use mostly HSS (M2, M42, T15). I would expect to get an easy 5000 parts of 41L40 at .500" Dia. Making sure the tool is on center can be the difference between 5000 parts and 500 part life span.

The Tantung I use has 46%ish Cobalt. It has very good red hardness and does not like to chip.

DanASM said:

I would expect to get an easy 5000 parts of 41L40 at .500" Dia. Making sure the tool is on center can be the difference between 5000 parts and 500 part life span.

Click to expand...

5,000 eh!? It sounds like I’m leaving money, parts, and time on the table....I’ll have to investigate this further. Thank you!

Just to be sure - I check my tool center height by 1) facing off less material than the width of the insert and check for a tit and/or 2) check the front of the bar and the back of the part after cutoff in production for a tit. Is that about right? One or twice I have pinched a 6” rule between the insert and the stock to see if it’s tilted and that worked surprisingly well.

Thanks, again!

That's a fine way of checking if your tool is below center, but it won't tell you if it's above center. After facing off with the cut off tool like you describe, I like to look at the face of the part with the tool at X0 to see if it looks too high. A little high is fine and usually recommended, but too high puts too much pressure on the tool at the end of the cut and can explode an insert. I'll have to try that trick with the steel rule. It sounds promising.

To set center height of tool, give it a negative Y offset and face with tool. Measure the post and adjust offset by the measured amount. You can add some to put the edge just above center.

Nerdlinger said:

5,000 eh!? It sounds like I’m leaving money, parts, and time on the table....I’ll have to investigate this further. Thank you!

Just to be sure - I check my tool center height by 1) facing off less material than the width of the insert and check for a tit and/or 2) check the front of the bar and the back of the part after cutoff in production for a tit. Is that about right? One or twice I have pinched a 6” rule between the insert and the stock to see if it’s tilted and that worked surprisingly well.

Thanks, again!

Click to expand...

I am not sure how to bring one on center on a swiss machine. I have mine on cross slides or a vertical slide. I can bring them in by hand and line it up with the face of the part by eye. Making sure it is below center a little bit so it will leave a small tit when I cut it off by hand.

I then have set screws with an egg shaped cam on my toolholder that I can turn to rise or lower the cutoff tool. Make minor adjustments until I get what I like.

I just ran 4000 .312" round 316 SS parts with 1 tool. It was still cutting good so I left it in on the next job. 5000 parts of .125" round 316 SS. It could use a sharpen now but it usually gets 2500-3500 parts on these jobs. I got over 7500 this time around with it.

Some of my long running 1215, 12L14 jobs that run all week long can get between 1-2 days per sharpening all the way to 5-6 days. Sometimes we run those jobs Monday - Saturday 7 hours a day and the cutoff/form tools last quite a while.

Just a little bit above center will cause faster tool failure than slightly under center.

I also ran 2500 parts in 440C SS and I used 1 cutoff the whole time and didnt re sharpen yet. It still looks good.

I have some material here that is 4140, 41XX (equivalent, JIS), and 440C SS. These are all in the mid 20's rockwell I believe. They cut nice and hold tolerance just fine with my HSS Tooling and slower speeds. They can be tough materials but if I let the tools cut and don't put too much pressure on things it seems to machine pretty decently. I would consider it free machining grade for the jobs I do. I can walk away from them for hours at a time.

I have seen some things on ebay that you can chuck up in the collet and use it to level your tools and get them on center. Don't know if that would work in the swiss world though.

Good Luck. 41L40 should be easy to machine. I haven't seen it in a while but its even easier than the 4140 I have been machining.

Knocking on wood, the Iscar Tang-Grip, 3mm width, IC808 grade is the only parting tool that I have yet to kill.

I've destroyed plenty of other parting tools including Iscar's Pentagrip and various two-sided inserts from Iscar, Mitsubishi, and Sandvik, usually by leaving them in there too long.

If your tool life is tied to number of parts rather than time-in-cut, that certainly suggests that the bulk of the wear/damage is happening in entry/exit. Maybe slow the feed for the last 0.100"?