303 Stainless Bore Feeds and speeds

Dupa3872 · Mar 24, 2018

Guys

I have been doing this job four times a year for ever. Over the years Ive fussed with this bore and always settle for less. The material is 303 the bore size is .594 +-.001 and its 1.220 deep in a blind .563 hole that goes another .750 deep. My machine is a HAAS Sl-20 I am using a Sandvik solid carbide 3/8 bar and TCGX coated insert with a .015 Rad.

My customer is looking for as close to an 8 finish as I can get. I always end up spending a few hours polishing the bores after, I'm tired of it. They don't want them honed or ground.

What would you guy run for RPM and feed rate ?

Make Chips Boys !

Ron

Karl_T · Mar 24, 2018

Never done this. My calculator gives 1350 RPM, .008 IPR or 10.7 IPM for a start trial. In other words, slow speeds, hi feeds. I would use cutting oil.

If you are no where close to this, try it. You will know far more than anyone else. its your machine and you have done it before.

ricardo_gt · Mar 24, 2018

Why don´t you bore at full speed and use a reamer after?
I would buy Kennametal drill, by far the best price/quality option.
1000rpm and around 30ipm/min should be fine to bore.

litlerob1 · Mar 24, 2018

How are you/they checking a 8rms Finish? I get that it's a Bearing fit, but are you/they checking it with a Profilometer or is it a Shiny look they are after?

Either way I would run the Finish pass at least double what the above recommendations are, (200 SFM and less). So I would try probably 375 SFM and F.002", I would also make sure there is plenty of material for a finish pass, more than the radius of the Tool-at least.

R

Dupa3872 · Mar 24, 2018

The bore is actually a sealing surface. A liquid gel is inside the part and a shaft with a sandwich of aluminum washer type parts and an O-ring fit inside. They are not using anything other than eyeballs to check the finish.

I am running at 1350 RPM 740 SFM and a feed rate of .004 I am leaving .005 for finishing. If i leave too much the chips build up and leave marks, I don't have high pressure coolant to blow the chips out, but I'm getting a good jet through the tool.

Karl T was pretty damn close, better than what I was getting. I was at 2600RPM with a .001 feed rate and it was not bad, Karls numbers were better. I just know that the magic combination is out there.

Thanks for the help so far guys

Make Chips Boys !

Ron

precisionmetal · Mar 24, 2018

Ron,

Can you obtain/make a larger boring bar?

I'd be inclined to go up to maybe .425/.450 in diameter, and possibly even get the bar gun-drilled so you can make a connection on the back end and pump coolant through the bar to really help flush the chips out.

Just thinking out loud...

PM

djm77 · Mar 24, 2018

Slow it down to around 150rpm and maybe 0.004” feed per rev. It’ll take a bit longer per part, but you won’t be spending hours polishing it afterwards.

Should take around 2mins for the finish pass. How long do you spend polishing?

Sent from my iPhone using Tapatalk

litlerob1 · Mar 24, 2018

Dupa3872 said:
The bore is actually a sealing surface. A liquid gel is inside the part and a shaft with a sandwich of aluminum washer type parts and an O-ring fit inside. They are not using anything other than eyeballs to check the finish.

I am running at 1350 RPM 740 SFM and a feed rate of .004 I am leaving .005 for finishing. If i leave too much the chips build up and leave marks, I don't have high pressure coolant to blow the chips out, but I'm getting a good jet through the tool.

1350 RPM is not 740 SFM in .594" bore. Good you are getting coolant through the Tool.

But hey if the results are there, go for it. A Profilometer is going to pick up a little bit worse than a 4 with .0156" TNR and .004" feed. But that doesn't get you Shiny.

Dupa3872 · Mar 24, 2018

litlerob1 said:
1350 RPM is not 740 SFM in .594" bore. Good you are getting coolant through the Tool.

But hey if the results are there, go for it. A Profilometer is going to pick up a little bit worse than a 4 with .0156" TNR and .004" feed. But that doesn't get you Shiny.

RPM is not 740 SFM in .594" bore

Man I know....You know Ive been doing this a long time and need to at some point LEARN things. My G50 is 1350 RPM and my G96 (CSS) is 740 I have never got a good solid grasp of this and it's almost embarrassing, I just haven't taken the time. I get mixed up with the terms used FSM, IPM, IPR, TNR People use different terms to describe the same thing at times and I get mixed up over it.

I need to take an hour and learn this crap, I had a good grasp in the beginning and today I just grab numbers that I know worked for me in the past. Tools and insets have advanced and my numbers from the past are probably not as good as they should be.

Ron

NodecoMachine · Mar 24, 2018

litlerob1 said:
1350 RPM is not 740 SFM in .594" bore. Good you are getting coolant through the Tool.

But hey if the results are there, go for it. A Profilometer is going to pick up a little bit worse than a 4 with .0156" TNR and .004" feed. But that doesn't get you Shiny.

.0156R and .004IPR comes to a 43Ra finish in theory.

1350RPM at .594 dia. Is 210SFM.

In smaller bores like this I would be using a.0078R insert and a small finish pass (.002-.004 DOC). This should allow higher spindle speed without chatter (400SFM+?) and no tearing from large chips rubbing between the bar and bore. Of course a slower feed rate is needed because of the smaller TNR, so .001-.002IPR.

Dupa3872 · Mar 24, 2018

djm77 said:
Slow it down to around 150rpm and maybe 0.004” feed per rev. It’ll take a bit longer per part, but you won’t be spending hours polishing it afterwards.

Should take around 2mins for the finish pass. How long do you spend polishing?

Sent from my iPhone using Tapatalk

I'm not feeling it man 150 RPM ?? I might try it. I am spending 2-3 min depending on how it looks to start. I use a cloth pad coated with lapping compound mounted to a handle. I move in a honing pattern then draw the pad out in one motion.

Ron

litlerob1 · Mar 24, 2018

NodecoMachine said:
.0156R and .004IPR comes to a 43Ra finish in theory.

1350RPM at .594 dia. Is 210SFM.

Sorry missed a "3" you are right.

@ Ron forget about the acronyms ABC FNG, RCH, SFM, RPM blah blah. Regardless of what your G96 is set to the RPM you are running determines the Surface Feet, so 3.14 X Diameter X RPM / 12 = SFM

R

djm77 · Mar 24, 2018

Dupa3872 said:
I'm not feeling it man 150 RPM ?? I might try it. I am spending 2-3 min depending on how it looks to start. I use a cloth pad coated with lapping compound mounted to a handle. I move in a honing pattern then draw the pad out in one motion.

Ron

Any time I get a poor finish/vibration etc I’ll slow it right down and just let the machine gently remove the material. It’s an old manual lathe thing I was taught. Works just as well on a CNC lathe.

Sent from my iPhone using Tapatalk

Dupa3872 · Mar 24, 2018

djm77 said:
Any time I get a poor finish/vibration etc I’ll slow it right down and just let the machine gently remove the material. It’s an old manual lathe thing I was taught. Works just as well on a CNC lathe.

Sent from my iPhone using Tapatalk

Got ya....we are on the same page and think alike, Thanks

Ron

litlerob1 · Mar 24, 2018

djm77 said:
Slow it down to around 150rpm

I would not do this until after I tried using a Garden Rake and Chisel and fixturing it to a Dewalt with duct tape. There is no reason to be running that slow. I'm sorry, that is not what Modern Machinery is for. I can't even imagine doing that on a Manual either to be honest. That is painfully slow. 150 RPM = 23 SFM. I run parts in high temp/ Alloys faster than that. 303 is barely even Stainless as it is. Inconel 718 runs at 30 SFM.

There is no good reason to run that slow IMNSHO.

R

dpolseno41 · Mar 24, 2018

Feed: .0017 IPR
G50: 4,000 RPM
G96: 300

bigjon61 · Mar 24, 2018

400 SFM (2600ish RPM) with .002-.004 IPR using a 1/64 corner radius. Drill as big as you can and leave .005 per side to keep the chips to a minimum on tbe finish pass. If you want shiny you are going to have to spin it fast.

djm77 · Mar 25, 2018

litlerob1 said:
I would not do this until after I tried using a Garden Rake and Chisel and fixturing it to a Dewalt with duct tape. There is no reason to be running that slow. I'm sorry, that is not what Modern Machinery is for. I can't even imagine doing that on a Manual either to be honest. That is painfully slow. 150 RPM = 23 SFM. I run parts in high temp/ Alloys faster than that. 303 is barely even Stainless as it is. Inconel 718 runs at 30 SFM.

There is no good reason to run that slow IMNSHO.

R

Yet it works pretty much every time. I’d love to run all my jobs as fast as I should with much higher feeds and speeds, but it doesn’t always work like that. We can’t have the correct tooling for every job, so I do get a job that has a deep bore with a small diameter then I’ll push it as hard as possible and if it doesn’t work my go to option is always to slow it down. Not a problem on 1 offs really when you just have to get the job done. Rip out the bulk of the material at normal speeds and feeds them slow it right down for the finish pass to hit size and finish.

Sent from my iPhone using Tapatalk

TRussell · Mar 25, 2018

djm77 said:
Yet it works pretty much every time. I’d love to run all my jobs as fast as I should with much higher feeds and speeds, but it doesn’t always work like that. We can’t have the correct tooling for every job, so I do get a job that has a deep bore with a small diameter then I’ll push it as hard as possible and if it doesn’t work my go to option is always to slow it down. Not a problem on 1 offs really when you just have to get the job done. Rip out the bulk of the material at normal speeds and feeds them slow it right down for the finish pass to hit size and finish.

Sent from my iPhone using Tapatalk

If you are checking it with a profilometer, I don't think it's possible to turn an 8 microinch finish. I have spent quite a bit of time with a Mitsubishi rep trying to hit a 16 microinch finish in 17-4. I know the numbers can work out, with tnr, and ipr, but in practice, and checked with a profilometer I don't think it's possible. The bore I was working on was spherical, and interupted by grease holes, so it's not quite the same thing, but after a bunch of fucking around, I still ended up polishing. Good luck.

TRussell · Mar 25, 2018

I guess I should say that if you need something that looks like glass, but tests in the low 20s with a profilometer, you're good. If you really need an 8 microinch finish, I'm sorry, I don't think thats possible turning.

303 Stainless Bore Feeds and speeds

Stainless

Cast Iron

Aluminum

Diamond

Stainless

Stainless

Aluminum

Diamond

Stainless

Cast Iron

Stainless

Diamond

Aluminum

Stainless

Diamond

Aluminum

Hot Rolled

Aluminum

Aluminum

Aluminum

Similar threads