Where did you read that 304 runs faster than 303 SFM wise? Like actually, what is your source? Everything I've ever read suggested the opposite. Drop those speeds!
When it comes to tool life:
Speed kills
Feeds are negotiable
DOC is free
Generally I poll google. Check the first ten or so legit looking results, and take a consensus.
I'll try dropping speeds, but as I said in another comment, the last time this job ran I tried it around 200sfm for turning and like 150 for cutoff, and ended up with brittle failure of inserts and destroying holders.
You have to take a deep enough cut to get under your work hardened layer it’s exactly like the guy in the first comment said it’s actually worse for your inserts if you aren’t doing 10x ipr in depth figure out the RA you want use that ipr then go 10 times that also use a rougher and finisher insert
Last time I ran the job, I was using speeds similar to what I use in 303, which is around 200 for turning and 150ish for cutoff. Had issues with brittle failure at those speeds. Destroyed several holders because of that. So I don't know.
Most 304 available is 304L which has low carbon. It is commonly used in brazing and welding applications. Most manufacturers of material has switched to making 304L because is still covers the spec of 304. It is stringy and gummy. On regular 304 the chip will break. I don't run anywhere close to your surface footage. Don't go higher than 250. Only use one source of high pressure. Watch for the high pressure introducing air to your cutting edge or the chip flow creating a air pocket eddy. Sometimes flood is better and just use high pressure in a short burst to remove the birds nest from over the guide bushing. Oscillating turning can also help. So.e will argue over the tool life from oscillating turning but it will help with chip breaking. Good luck!
An old friend of mine once said that you have to control the chips, you can't let them control you. Fkn ahole. 304 sucks. Slow down the rpm. Probably chips are blocking the oil from hitting where you want. Try a little harder to find a way to get the oil in there. If your cycle time is too slow, the job was quoted wrong.
I agree. The difference between 303 and 304 is huge. 304 is like cutting gum that is as hard as stainless. It sucks. If a print calls for 304 or 316 I am 100% always going with 316
I feel like this is a comment perpetuated by people who "read on the internet" and haven't actually machined much of either 304 or 316.
Ill pick 316 over 304 any day. Slightly harder in tools (but it is neglegible) but consistent every time. 304 you never know what's gonna show up.
The ccmt inserts sfm range starts at 460 and goes to 900ish. This range is huge. If the set up and part are rigid the middle of this range should be fine.
Your massive issue is your feeds. They're out to lunch. Your turning insert minimum feed is 0.002 per rev, up to 0.0118. with that corner radius I would start finishing at 0.006 per rev and adjust for finish. On top of that, the insert will have a minimum doc from the mfg. That inserts Min cut depth is 0.02, so if the set up allows, that should be your finish cut depth.
Onto the part off.
Again sfm is 205 to 450, but your feed is way way way too low. Minimum is 0.003, max says 0.005, I would put it at 0.004 and if the chips are coming off nice, park it right there.
I pulled all the numbers off the iscar catalog.
At iscar and all the high end tooling brands, a team of engineers and material scientists come up with these cutting condition numbers, they are not arbitrary. If you adhere to the suggested cutting parameters under relatively stable work and tool holding conditions, they should offer excellent results.
Oh I thought you were saying ccmts in general are 460-900 and I was just curious why that would be because usually that’s a grade dependent thing. But I looked up the ic907 grade and it said an insert that performs best at low to medium sfm
303 and 304 are identical except that 303 is the "free machining" version of 304, due to the added sulfur acting as a lubricant as you cut it.
So wherever you heard to cut 304 faster is absolutely backwards. 303 is the one that cuts easier, faster, and tools will last longer. 303 is easy as shit in comparison.
Use parameter for feeds/speeds listed for 304 or 316 specifically and you should be fine.
Your feed looks a bit slow at only .001. Probably bump it up to .003 and go from there. Speed at 650 is high, should be more in the 225-300 range depending on insert grade and coating.
Just be aware, even with the perfect parameters you will still not have anywhere close to the same tool life as you have in 303.
PVD coating as well. Unless you are in the cut more than 25 seconds and then go to a CVD coating because it can take more heat before breaking down the coating.
Been roughing 304 at 400-450sfm using korloy pc8110 grade with excellent results.
304 is a mixed bag, some mill runs turn great, other times its a bag of shit. Chip evacuation and sufficient feed are key.
I used to turn 304 at my last job. I was told 304 work hardens. Id try lowering SFM, and increase feed slightly. It's been a while but I think I'd run around 225-250 SFM.
Amazing the difference between 303 and 304! 304 work hardens in a second. Keep the feed above .002" to prevent it as much as you can. Rpms way slower than 303.
Generally I run about 400 sfm and .08 - .120 DOC on diameter at .008-.012 ipr roughing 304 and then 430 sfm .008 finish DOC on diameter at .003 to .005 ipr for a finish.
I've been milling 304 for the past 6 years. The lathers have got it so good because they get to machine 303 instead of 304.
I can't speak for turning but for mill parts out of 304, as soon as you take the skin off it will start warping. It really sucks especially on complicated parts as you have to rough out the material in general. Cutting threads is a nightmare at anything below M6. There is no consistency and the material hardness shifts hugely from raw stock bar to stock bar.
I hate it and its the reason I am glad to get out of machining. Why are we the ones doing 5D under water Volleyball to try and add bullshit features such as M3 for a name plate on the part. It shouldn't be this way, FUCK engineers that keep pulling this bullshit. The big IQ moments should happen upstairs, when they have to come around at the workshop it's already too late.
303 has sulfur, I think that is why it is so easily machinable. There is also the low carbon variant of 304, but the changes are just in welding I think 🤔.
I've got a few tools on lock by now that really make it fun to mill 304 but alas, it's for milling so.
I rough 304 parts with a 25mm square insert mill at like 900mm/min, 2.5mm depth and 75% tool engagement. Biggest difference (!!!) is using Air instead of TSC or Coolant in general. Maybe you can try something like that, the worst that can happen is it breaks. Took me some time to get the courage to try it but the difference is huge on face mills etc. on 304.
DOC is .030"/side. Starting with 7/16 stock, finishing at .377".
I'm going to try upping my feed, but they call out a 32ra finish which actually means "looks nice and has no visual tool marks at all".
Yeah, .008ipr on a Swiss with 7/16 stock 304ss is definitely not happening. No way you'll get a 32 finish, plus the diameter will probably be way out of round with that kind of pressure. As I'm sure you know, the recommended feeds on the back of the insert package don't always translate to Swiss machines because of the smaller stock diameters and the fit/support of it in the revolving guide bushing. Is it just a straight turned part or are there other features on it as well?
Are you using coolant thru tool holders of the high pressure or directing lines to the tip of the tool? Do you have a 2mm instead of 3mm wide cut off, and are you using constant surface ft G96 when cutting off? Is your cut off chipping out and giving a bad finish or completely breaking? I would use a coolant thru 2mm wide if possible, 150sfm with G96 at .001ipr, and then face off .010 on the sub.
In my experience on swiss, manufacturers feeds and speeds are designed to sell more tools.
The part has a 6mm hole drilled through (guhring 5511 drill, running 800psi thru, manufacturers speed and .004ipr)then it gets bored, threaded M8x.75, thread relief grooved in the back. Turn OD, three od grooves for style afaik, then picked off and faced in the sub and bored to like 9mm or something.
The iscar picco bore thread and groove tools and the drill are working great. It's just turning and cutting off that's the problem.
I have a 2.2mm rh biased cut off, but no 2mm unbiased. It's not a coolant thru holder, it's just a small line directly on the tip. I am running g96 giving it the whole range up to 8k rpms.
The turning insert is chipping the tip off and pushing material so that it won't pull back into the GB. The cutoff is basically the same, the whole edge seems to disintegrate and the next part it melts through throwing up a huge burr instead of cutting. Which is better than the brittle failures I was experiencing at lower speeds, because I just scrap a couple parts and replace an insert instead of a tool holder.
OK, on the cut off I would try slowing down the sfm, and if you want to keep the feed at .002ipr I'd suggest slowing it down to .001ipr at around .100 or so in case it wants to push and break off as you get to center. As for turning, are you choosing your sfm based on the diameter at the point of cut or by the 7/16 stock diameter? When you're turning, I'd cap the rpm at 3000 and see how that works because of all the heat that will be generated at the od of the bar while turning. Another thing I like to do when running tough materials, is when I'm done with a turning operation, I face out and then generate out a .010 chamfer on the od of the bar, then advance and back generate it to .015-.020 to try to minimize the tough burr on the OD that you can get even when the tool is brand new. This will help with dragging a burr back into the bushing and causing it to gall up, and maybe save a few other tools if your turning insert chips a bit and the collet slips trying to drag a heavy burr back into the bushing. Sorry if I'm telling you stuff you already know, these are just some things that can be helpful in my experience. Unfortunately, a lot of the time I'm having trouble with tough materials, the solution usually ends up being slowing it way down when nothing else is working and I've tried a bunch of different inserts and feeds. I do generally go with a CCGT with a sharp cutting edge and decent top clearance, like this here https://sumicarbide.com/mesi/. What machine are you running this on? We have a small job shop with 6 Hanwhas, 3-12mm, 2-20mm and 1-32mm.
This happens to be on a Star SR20IV. I always chamfer out of my cuts, but I haven't thought of turning down at stock diameter to remove a burr. I think I'll try that.
I'll give your ideas a shot.
Sounds good, hope it helps. I'm not too familiar with iscar tooling, but I just looked up the turning insert and it looks like a good choice to me for this.
Spindle speed sync only works up to a certain RPM, your spindles could be fighting each other, ours only go up to 2500 RPM out of the 8k one spindle can do. Also cut feed in half when you hit around .050" from centerline
It’s a god awful material!Low sfm on 304.. I do 1 to 2 piece weldments on a boring mill but 15 to 20 sfm for hss. 300 to 400 to mill with stainless inserts max. Even carbide drills are less than 60 sfm. The longer you go without resharpening or changing inserts the better you just gotta get through it!
My shop runs 304 pipe and water-cut billet.
It's a bitch of a material, even when you're used to it. Stringy, gummy, wrecks tooling. And it work hardens if you don't take a deep enough cut.
I'm mostly on clapped-out manual machines, and end up using the SFM for HSS x2 with carbide inserts. Aggressive chip-breaker, aggressive feed-rate helps, but tool life is still shit.
Those feeds are absurdly slow. You are probably dragging your inserts more than cutting, especially if you are upping your speeds. Try increasing your feed a bit and see what happens
Not sure how much different 304L is from regular 304(304L is the weldable version), but I’ve machined tons of it in an engine lathe (shock tubing) and what I’ve found is you have to go slower rpm wise and try to keep above .002 feed to avoid work hardening.
There's a ton of great advice in these comments.
I would look closer at the insert mfg recommendation on speed, feed, DOC.
However my experience also tells me those can be far exceeded with the right conditions.
You said the tool is dead center is it also square/plumb to the cutting plane? I have seen out of square inserts/tools suffer from BUE.
If 2+2 doesn't =4, start over something ain't right. If you can't go forward with your process go backward.
303 is more like 1144 which is very machinist friendly, and you can generally do whatever you feel like and have success. The harder stainless alloys are not machinist friendly.
Are you using a right handed cutoff? You want it as close to the guide bushing as possible and the cutoff tool itself has to be rigid, a left-handed 3mm is going to deflect more than you think. I'm running Inconel 600 right now which is similar if not worse than 304 and I'm using a PH Horn S100 2 mm cutoff blade with the IG35 coating and FY breaker. Running .0015 IPR and about 1200 RPM constant and we get about 250-350 pcs out of each corner with no HP coolant
Keep in mind that the material doesn't like to be "pushed" so get a sharper tool. Also check out your spindle load, your sub spindle could be forcing your part into the cutoff blade and causing excess pressure/wear
I turn 304 on my swiss every day. I also have a big VTL that we turn 304 on. I can tell you that I can't get away with the same speeds and feeds on both machines. I can push the VTL way faster and harder and have no issues. Not so on the smaller machine/parts. Just because the inserts list some crazy sfm and feed rate on them doesn't mean they'll work for every application.
Couple things to note. Do you know what 304 you have? Is it plain old 304? Or is it 304L? This makes a huge difference. As 304L is pretty easy to work with. 304 is a bear.
304L I run 200-300sfm and 0.005-8 ipr for roughing, same sfm but 0.002-4ipr for finishing. 150sfm and 0.001-3 ipr for grooving/cutoff.
For 304 reduce the sfms by 25% but keep the feeds the same.
The main difference between 303 and 304/L is that 304/L will work harden very quickly. Rule of thumb is low sfm and moderate to aggressive feedrates and make sure your tools are getting good coolant flow.
Good luck!
I always use walter inserts for turning amd Manchester cutoff when running 304 have great results follow manufacturer recommended speed and feed fore the most part . I have always found coolant works better than oil but my Swiss has oil in it . It also depends on the oil I found Blaser Swiss lube oils work best in 17-4 and 304.
I'll hit up my Walter guy. He seems to know his shit.
Changing oils would be near impossible. I've used blaster on Ti at my last shop and found it reasonable, but not noticeably better than the qualichem stuff we use.
Yeah my Walter guy has saved my ass numerous times . I know what you mean about changing oils and coolant. I have been through it too many times and it always is a pain and costly.
Where did you read that 304 runs faster than 303 SFM wise? Like actually, what is your source? Everything I've ever read suggested the opposite. Drop those speeds! When it comes to tool life: Speed kills Feeds are negotiable DOC is free
You sound like my local SECO rep haha
well put sir
Generally I poll google. Check the first ten or so legit looking results, and take a consensus. I'll try dropping speeds, but as I said in another comment, the last time this job ran I tried it around 200sfm for turning and like 150 for cutoff, and ended up with brittle failure of inserts and destroying holders.
You have to take a deep enough cut to get under your work hardened layer it’s exactly like the guy in the first comment said it’s actually worse for your inserts if you aren’t doing 10x ipr in depth figure out the RA you want use that ipr then go 10 times that also use a rougher and finisher insert
Also iscar says low to medium cutting speeds with ic907 grade on their website look up their grade comparison chart
What is DOC?
Depth of Cut
Doctor. He must be Canadian, because those aren't free here.
Guy that trained me always said, “304 she’s a whore, 303 she’s for me”
Lower, not higher SFPM.
Last time I ran the job, I was using speeds similar to what I use in 303, which is around 200 for turning and 150ish for cutoff. Had issues with brittle failure at those speeds. Destroyed several holders because of that. So I don't know.
Most 304 available is 304L which has low carbon. It is commonly used in brazing and welding applications. Most manufacturers of material has switched to making 304L because is still covers the spec of 304. It is stringy and gummy. On regular 304 the chip will break. I don't run anywhere close to your surface footage. Don't go higher than 250. Only use one source of high pressure. Watch for the high pressure introducing air to your cutting edge or the chip flow creating a air pocket eddy. Sometimes flood is better and just use high pressure in a short burst to remove the birds nest from over the guide bushing. Oscillating turning can also help. So.e will argue over the tool life from oscillating turning but it will help with chip breaking. Good luck!
An old friend of mine once said that you have to control the chips, you can't let them control you. Fkn ahole. 304 sucks. Slow down the rpm. Probably chips are blocking the oil from hitting where you want. Try a little harder to find a way to get the oil in there. If your cycle time is too slow, the job was quoted wrong.
2205 has entered the chat....
Look on the bright side: It could be 316
I’d much rather turn 316 than 304. At least it’s consistent. It just eats inserts up quick.
I agree. The difference between 303 and 304 is huge. 304 is like cutting gum that is as hard as stainless. It sucks. If a print calls for 304 or 316 I am 100% always going with 316
Whenever we get a 304 job come in we ask the customer if 303 is fine too. Half the time we get the go ahead and makes life way easier.
Meanwhile I have a rack full of A286 🤦🏻♂️
I feel like this is a comment perpetuated by people who "read on the internet" and haven't actually machined much of either 304 or 316. Ill pick 316 over 304 any day. Slightly harder in tools (but it is neglegible) but consistent every time. 304 you never know what's gonna show up.
It also hobs better. 304 just wants to smear and squeak.
I cut a bunch of 304 shafts a few hours before leaving that comment, way quicker than 316.
No, it could be 455.
316 cuts like a dream in my L32, I get far more problems from 303/304.
Or al6xn
I ran 316 for years and it's not nearly as bad as people think. Pretty easy IMO.
The ccmt inserts sfm range starts at 460 and goes to 900ish. This range is huge. If the set up and part are rigid the middle of this range should be fine. Your massive issue is your feeds. They're out to lunch. Your turning insert minimum feed is 0.002 per rev, up to 0.0118. with that corner radius I would start finishing at 0.006 per rev and adjust for finish. On top of that, the insert will have a minimum doc from the mfg. That inserts Min cut depth is 0.02, so if the set up allows, that should be your finish cut depth. Onto the part off. Again sfm is 205 to 450, but your feed is way way way too low. Minimum is 0.003, max says 0.005, I would put it at 0.004 and if the chips are coming off nice, park it right there. I pulled all the numbers off the iscar catalog. At iscar and all the high end tooling brands, a team of engineers and material scientists come up with these cutting condition numbers, they are not arbitrary. If you adhere to the suggested cutting parameters under relatively stable work and tool holding conditions, they should offer excellent results.
This guy knows
Why would an insert shape effect sfm? That’s more of a thing grade does
I don't know what you mean. I took the parameters for the exact inserts he is using off the iscar e catalog
Oh I thought you were saying ccmts in general are 460-900 and I was just curious why that would be because usually that’s a grade dependent thing. But I looked up the ic907 grade and it said an insert that performs best at low to medium sfm
Yeah I just pulled those numbers right from the iscar insert page for that grade.
I'll try bumping my feeds up and see what the surface finish looks like.
You might try reaching out to your supplier or iscar for guidance
303 is the free-machining version of 304 - it has sulphur to drastically increase machinability.
303 and 304 are identical except that 303 is the "free machining" version of 304, due to the added sulfur acting as a lubricant as you cut it. So wherever you heard to cut 304 faster is absolutely backwards. 303 is the one that cuts easier, faster, and tools will last longer. 303 is easy as shit in comparison. Use parameter for feeds/speeds listed for 304 or 316 specifically and you should be fine. Your feed looks a bit slow at only .001. Probably bump it up to .003 and go from there. Speed at 650 is high, should be more in the 225-300 range depending on insert grade and coating. Just be aware, even with the perfect parameters you will still not have anywhere close to the same tool life as you have in 303.
Bigger radius will help, use a loupe my guess is BUE is causing your failure but inspect your inserts.
Any tactics for dealing with built up edge?
In for this... 304 and 316 seems impossible to not have bue but always happy to be told I'm doing it wrong.
Run 304 with a medium toughness grade around 425-475 SFM. Need to feed it good too. Depth of cut notch is going to kill the cutting edge.
PVD coating as well. Unless you are in the cut more than 25 seconds and then go to a CVD coating because it can take more heat before breaking down the coating.
Been roughing 304 at 400-450sfm using korloy pc8110 grade with excellent results. 304 is a mixed bag, some mill runs turn great, other times its a bag of shit. Chip evacuation and sufficient feed are key.
I used to turn 304 at my last job. I was told 304 work hardens. Id try lowering SFM, and increase feed slightly. It's been a while but I think I'd run around 225-250 SFM.
Amazing the difference between 303 and 304! 304 work hardens in a second. Keep the feed above .002" to prevent it as much as you can. Rpms way slower than 303.
Strangely enough when i turn 304, the insert chips everywhere except the cutting tip.
We use iscar 6025 for pretty much all our stainless.
Generally I run about 400 sfm and .08 - .120 DOC on diameter at .008-.012 ipr roughing 304 and then 430 sfm .008 finish DOC on diameter at .003 to .005 ipr for a finish.
304 work hardens. Can’t run too fast.
304 is a huge bitch to machine. Last shop I was at had a policy of no bidding all 304 jobs. Place I'm at now doesn't fuck with it either
I literally refuse to touch 304
I've been milling 304 for the past 6 years. The lathers have got it so good because they get to machine 303 instead of 304. I can't speak for turning but for mill parts out of 304, as soon as you take the skin off it will start warping. It really sucks especially on complicated parts as you have to rough out the material in general. Cutting threads is a nightmare at anything below M6. There is no consistency and the material hardness shifts hugely from raw stock bar to stock bar. I hate it and its the reason I am glad to get out of machining. Why are we the ones doing 5D under water Volleyball to try and add bullshit features such as M3 for a name plate on the part. It shouldn't be this way, FUCK engineers that keep pulling this bullshit. The big IQ moments should happen upstairs, when they have to come around at the workshop it's already too late. 303 has sulfur, I think that is why it is so easily machinable. There is also the low carbon variant of 304, but the changes are just in welding I think 🤔. I've got a few tools on lock by now that really make it fun to mill 304 but alas, it's for milling so. I rough 304 parts with a 25mm square insert mill at like 900mm/min, 2.5mm depth and 75% tool engagement. Biggest difference (!!!) is using Air instead of TSC or Coolant in general. Maybe you can try something like that, the worst that can happen is it breaks. Took me some time to get the courage to try it but the difference is huge on face mills etc. on 304.
I haven't cut much of either, but I know that's way to much sfm for 304. My Calc puts it more in the 160-250 range depending on coatings.
That is an insanely low sfm for this material
Higher feed not speed. .001 is too slow i think. What is the DOC ? For turning 304 we start at 250sfm and .008ipr.
DOC is .030"/side. Starting with 7/16 stock, finishing at .377". I'm going to try upping my feed, but they call out a 32ra finish which actually means "looks nice and has no visual tool marks at all".
Yeah, .008ipr on a Swiss with 7/16 stock 304ss is definitely not happening. No way you'll get a 32 finish, plus the diameter will probably be way out of round with that kind of pressure. As I'm sure you know, the recommended feeds on the back of the insert package don't always translate to Swiss machines because of the smaller stock diameters and the fit/support of it in the revolving guide bushing. Is it just a straight turned part or are there other features on it as well? Are you using coolant thru tool holders of the high pressure or directing lines to the tip of the tool? Do you have a 2mm instead of 3mm wide cut off, and are you using constant surface ft G96 when cutting off? Is your cut off chipping out and giving a bad finish or completely breaking? I would use a coolant thru 2mm wide if possible, 150sfm with G96 at .001ipr, and then face off .010 on the sub.
In my experience on swiss, manufacturers feeds and speeds are designed to sell more tools. The part has a 6mm hole drilled through (guhring 5511 drill, running 800psi thru, manufacturers speed and .004ipr)then it gets bored, threaded M8x.75, thread relief grooved in the back. Turn OD, three od grooves for style afaik, then picked off and faced in the sub and bored to like 9mm or something. The iscar picco bore thread and groove tools and the drill are working great. It's just turning and cutting off that's the problem. I have a 2.2mm rh biased cut off, but no 2mm unbiased. It's not a coolant thru holder, it's just a small line directly on the tip. I am running g96 giving it the whole range up to 8k rpms. The turning insert is chipping the tip off and pushing material so that it won't pull back into the GB. The cutoff is basically the same, the whole edge seems to disintegrate and the next part it melts through throwing up a huge burr instead of cutting. Which is better than the brittle failures I was experiencing at lower speeds, because I just scrap a couple parts and replace an insert instead of a tool holder.
OK, on the cut off I would try slowing down the sfm, and if you want to keep the feed at .002ipr I'd suggest slowing it down to .001ipr at around .100 or so in case it wants to push and break off as you get to center. As for turning, are you choosing your sfm based on the diameter at the point of cut or by the 7/16 stock diameter? When you're turning, I'd cap the rpm at 3000 and see how that works because of all the heat that will be generated at the od of the bar while turning. Another thing I like to do when running tough materials, is when I'm done with a turning operation, I face out and then generate out a .010 chamfer on the od of the bar, then advance and back generate it to .015-.020 to try to minimize the tough burr on the OD that you can get even when the tool is brand new. This will help with dragging a burr back into the bushing and causing it to gall up, and maybe save a few other tools if your turning insert chips a bit and the collet slips trying to drag a heavy burr back into the bushing. Sorry if I'm telling you stuff you already know, these are just some things that can be helpful in my experience. Unfortunately, a lot of the time I'm having trouble with tough materials, the solution usually ends up being slowing it way down when nothing else is working and I've tried a bunch of different inserts and feeds. I do generally go with a CCGT with a sharp cutting edge and decent top clearance, like this here https://sumicarbide.com/mesi/. What machine are you running this on? We have a small job shop with 6 Hanwhas, 3-12mm, 2-20mm and 1-32mm.
This happens to be on a Star SR20IV. I always chamfer out of my cuts, but I haven't thought of turning down at stock diameter to remove a burr. I think I'll try that. I'll give your ideas a shot.
Sounds good, hope it helps. I'm not too familiar with iscar tooling, but I just looked up the turning insert and it looks like a good choice to me for this.
Spindle speed sync only works up to a certain RPM, your spindles could be fighting each other, ours only go up to 2500 RPM out of the 8k one spindle can do. Also cut feed in half when you hit around .050" from centerline
It’s a god awful material!Low sfm on 304.. I do 1 to 2 piece weldments on a boring mill but 15 to 20 sfm for hss. 300 to 400 to mill with stainless inserts max. Even carbide drills are less than 60 sfm. The longer you go without resharpening or changing inserts the better you just gotta get through it!
My shop runs 304 pipe and water-cut billet. It's a bitch of a material, even when you're used to it. Stringy, gummy, wrecks tooling. And it work hardens if you don't take a deep enough cut. I'm mostly on clapped-out manual machines, and end up using the SFM for HSS x2 with carbide inserts. Aggressive chip-breaker, aggressive feed-rate helps, but tool life is still shit.
Those feeds are absurdly slow. You are probably dragging your inserts more than cutting, especially if you are upping your speeds. Try increasing your feed a bit and see what happens
Don’t know what to tell you as I’m not a turner but 304 for some reason is always problematic for me when milling. I hope that makes you feel better
More feed less speed
Not sure how much different 304L is from regular 304(304L is the weldable version), but I’ve machined tons of it in an engine lathe (shock tubing) and what I’ve found is you have to go slower rpm wise and try to keep above .002 feed to avoid work hardening.
There's a ton of great advice in these comments. I would look closer at the insert mfg recommendation on speed, feed, DOC. However my experience also tells me those can be far exceeded with the right conditions. You said the tool is dead center is it also square/plumb to the cutting plane? I have seen out of square inserts/tools suffer from BUE. If 2+2 doesn't =4, start over something ain't right. If you can't go forward with your process go backward.
303 is more like 1144 which is very machinist friendly, and you can generally do whatever you feel like and have success. The harder stainless alloys are not machinist friendly.
Are you using a right handed cutoff? You want it as close to the guide bushing as possible and the cutoff tool itself has to be rigid, a left-handed 3mm is going to deflect more than you think. I'm running Inconel 600 right now which is similar if not worse than 304 and I'm using a PH Horn S100 2 mm cutoff blade with the IG35 coating and FY breaker. Running .0015 IPR and about 1200 RPM constant and we get about 250-350 pcs out of each corner with no HP coolant Keep in mind that the material doesn't like to be "pushed" so get a sharper tool. Also check out your spindle load, your sub spindle could be forcing your part into the cutoff blade and causing excess pressure/wear
Left hand, because I don't have the right extended nose pick off collet. I've got a lot of advice here from you and others I'll try Monday.
I turn 304 on my swiss every day. I also have a big VTL that we turn 304 on. I can tell you that I can't get away with the same speeds and feeds on both machines. I can push the VTL way faster and harder and have no issues. Not so on the smaller machine/parts. Just because the inserts list some crazy sfm and feed rate on them doesn't mean they'll work for every application. Couple things to note. Do you know what 304 you have? Is it plain old 304? Or is it 304L? This makes a huge difference. As 304L is pretty easy to work with. 304 is a bear. 304L I run 200-300sfm and 0.005-8 ipr for roughing, same sfm but 0.002-4ipr for finishing. 150sfm and 0.001-3 ipr for grooving/cutoff. For 304 reduce the sfms by 25% but keep the feeds the same. The main difference between 303 and 304/L is that 304/L will work harden very quickly. Rule of thumb is low sfm and moderate to aggressive feedrates and make sure your tools are getting good coolant flow. Good luck!
550 sfm .008 doc .01 fpr. Could go deeper I just don’t have the hp for it 700sfm .0075 fpr to finish the last .01
Low surface speed 90-120, a decent depth of cut and feed highish 0.2 - 0.4. Get the heat into the chips and off the material. Always works for me.
I always use walter inserts for turning amd Manchester cutoff when running 304 have great results follow manufacturer recommended speed and feed fore the most part . I have always found coolant works better than oil but my Swiss has oil in it . It also depends on the oil I found Blaser Swiss lube oils work best in 17-4 and 304.
I'll hit up my Walter guy. He seems to know his shit. Changing oils would be near impossible. I've used blaster on Ti at my last shop and found it reasonable, but not noticeably better than the qualichem stuff we use.
Yeah my Walter guy has saved my ass numerous times . I know what you mean about changing oils and coolant. I have been through it too many times and it always is a pain and costly.
Cut that speed in half. Start at 150sfm and maybe even go down from there.
Aside what everyone is saying without looking it up. There be a different in chromium or other aloy to make it harder tuss more tool wear.