316SS Machining Characteristics

Have a challenging feature that is giving me fits at the moment.

I use a machinist calculator application on my phone for all drilling applications, and it is normally spot on. You plug in drill size, max rpm, material (w/ hardness), and drill size/material and it spits out the feed and speed.

This particular feature is a .070" hole to depth .425"

Calculator spits out 3077 RPM with a 2.039 IPM F/R at .006 IPR.

I've broken two drills now, both HSS, and it seems like I am hitting hard spots in the material. I've seen this before in stainless, but I'm confused because I drilled 4x .0625" holes within an inch of these and it seems like a localized hardness would've likely affected them as well. All drill bits are black oxide coated HSS and new so dullness shouldn't be the issue.

I also center drilled first, which although likely not necessary with this small of drill I prefer to do it in case the bit is "flailing" a little before it makes contact.

Any suggestions?

I recommend starting at about 45 sfm for HSS drill in 316SS...about 2,450 rpm. If it was a cobalt drill I'd go upwards of 50sfm but not much higher.
Feed rate needs to drop to less than .003 ipr for this small of a drill. I recommend starting at .002 and work your way up.

I run a lot of 316 but use almost all carbide drilling now days...been a long time since I used HSS and cobalt drills. The numbers above are what I used to use running 316 strain hardened barstock.

Not enough information. Are you peck drilling? What design is the Drill? Do you have coolant through? Why are you using a Center Drill on a Milling machine? What condition is the material? Is .006" feed per tool or per flute?

Either way .006" is more than double where you should be. BUT 2.039 IPM at 3077 RPM is .0006" so NOT .006" big difference, but it's hard to help if the info isn't correct. .0003" per lfute is way too light. I personally think your SFM is pretty good.

This is the problem with "APPS" that do this for you, you need to learn what SFM is, where it's appropriate and why it's used. RPM means nothing to me, except to figure out what the SFM is. And feedrate just means I need to figure out chipload for you. when working with Stainless Steel forget RPM and Feed start thinking in SFM and C.L.

R

Using a lathe I would never even dream of going over .001 IPR on 316 with that small a drill. I think you have misplaced a decimal point.

litlerob1 said:

Not enough information. Are you peck drilling? What design is the Drill? Do you have coolant through? Why are you using a Center Drill on a Milling machine? What condition is the material? Is .006" feed per tool or per flute?

Either way .006" is more than double where you should be. BUT 2.039 IPM at 3077 RPM is .0006" so NOT .006" big difference, but it's hard to help if the info isn't correct. .0003" per lfute is way too light. I personally think your SFM is pretty good.

This is the problem with "APPS" that do this for you, you need to learn what SFM is, where it's appropriate and why it's used. RPM means nothing to me, except to figure out what the SFM is. And feedrate just means I need to figure out chipload for you. when working with Stainless Steel forget RPM and Feed start thinking in SFM and C.L.

R

Click to expand...

Apologies on the typo but I did mean to type .0006" IPR instead of .006". I am peck drilling, with a .020" peck to try and avoid this issue. I was thinking by reducing the IPR and the peck size that I could avoid overloading the drill, which is not difficult as you well know with a drill this small.

The reason I use the application is because I have verified it against my own hand calculations numerous times. It is almost always spot on the hand calculation or very close to it. I do know what SFM is, I simply am not an expert in machining which is why I asked the question. It is much faster to use a calculator that I have verified than to do hand calculations every time which I am sure you can understand. The drills are 118° points.

As you said .0003" is way too light, what would you recommend? I am guessing that this is somewhere around .0015 IPR.

FWIW I used the .0625" drill with the same IPR albeit slightly different feed/speed and it drilled perfectly fine with no issues. Same drill material/coating/etc. and .0075" difference in drill diameter so what could've caused this. That drill also shows no signs of excessive dulling post cycle under a magnifying glass.

Center drill is purely to ensure location since it is much more rigid than a .0625" or .070" drill. No coolant through. Material is annealed to Rockwell B90.

I machine 316 all day long. I work in metric and would go with around 2100rpm, 0.02mm/Rev which is around 42mm/min feed. Something like 0.0008”/rev 1.6”/min feed. That’s where I’d start.


Sent from my iPhone using Tapatalk

My usual for 316 is lots of coolant. Through coolant is best and don't peck. 316 work hardens and too much heat blows up tools, same with chips getting in the way. Get a through coolant carbide and win every inch. If it were me on HSS I would go slower on HSS drills than what is called out for just to make sure things don't go bad, it likes feed more than speed. Likely what is happening is the depth is making the heat build up without coolant getting to the bottom, hardening the part and changing the working speeds and feeds. Are they getting destroyed nearing the bottom? Go slower or more pecking or more coolant, reduce the localized heat.

IMHO Coated 8% cobalt really helps in stainless, can make the difference between getting 1 hole to several per regrind. Thats a deep hole for the dia so you need a spot to start with and that means a small spotting drill so things locate - get off to a good start.

With stainless and problems, the best move is always to drastically cut back speed but keep a feed per tooth thats cutting not rubbing, your 6 tenths to me sounds about right. But i would not hesitate to half it or go a bit more.

gottb said:

Apologies on the typo but I did mean to type .0006" IPR instead of .006". I am peck drilling, with a .020" peck to try and avoid this issue. I was thinking by reducing the IPR and the peck size that I could avoid overloading the drill, which is not difficult as you well know with a drill this small.

The reason I use the application is because I have verified it against my own hand calculations numerous times. It is almost always spot on the hand calculation or very close to it. I do know what SFM is, I simply am not an expert in machining which is why I asked the question. It is much faster to use a calculator that I have verified than to do hand calculations every time which I am sure you can understand. The drills are 118° points.

As you said .0003" is way too light, what would you recommend? I am guessing that this is somewhere around .0015 IPR.

FWIW I used the .0625" drill with the same IPR albeit slightly different feed/speed and it drilled perfectly fine with no issues. Same drill material/coating/etc. and .0075" difference in drill diameter so what could've caused this. That drill also shows no signs of excessive dulling post cycle under a magnifying glass.

Center drill is purely to ensure location since it is much more rigid than a .0625" or .070" drill. No coolant through. Material is annealed to Rockwell B90.

Click to expand...

I'm doing you a favor in asking this; why do you think .0003" chip load per flute would equal about .0015" IPR?

Center drills are for Centers, Spot drill is for locating small Drills. Just a tiny tiny Spot on a .07" Drill maybe .01" deep with a dwell.- .02" peck for the Drill is a little light, but probably fine. I would use a chip load of .0005" per flute, so that would be 3.077 programmed IPM @ 3077 RPM. This is exactly what I am talking about with the calculator, you need to know what all those values are, to be efficient.

3.14*diameter*RPM/12=SFM
3.82*SFM=RPM
Feed in IPM/RPM/flutes=chipload per flute
chipload per flute*flutes*RPM=Feed in IPM

So if your chipload per flute with a 2 flute Drill is .0003" then for 2 flutes it would be .0006" right?

R

litlerob1 said:

I'm doing you a favor in asking this; why do you think .0003" chip load per flute would equal about .0015" IPR?

Center drills are for Centers, Spot drill is for locating small Drills. Just a tiny tiny Spot on a .07" Drill maybe .01" deep with a dwell.- .02" peck for the Drill is a little light, but probably fine. I would use a chip load of .0005" per flute, so that would be 3.077 programmed IPM @ 3077 RPM. This is exactly what I am talking about with the calculator, you need to know what all those values are, to be efficient.

3.14*diameter*RPM/12=SFM
3.82*SFM=RPM
Feed in IPM/RPM/flutes=chipload per flute
chipload per flute*flutes*RPM=Feed in IPM

So if your chipload per flute with a 2 flute Drill is .0003" then for 2 flutes it would be .0006" right?

R

Click to expand...

No, I was saying that .0003" was light. But I was guessing around .0015 IPR (.00075 chip load per flute) would be closer to where I wanted to be.

The thing is, I have used these exact calculations that you have listed above. There are a million different pieces of reference material that list them, and it is basic algebra that I am more than capable of performing manually. I have then verified this calculator using the aforementioned equations. Your assumption that I am so ignorant to have not double checked is misguided at best. That being said, I was asking for the chipload per tooth that you would recommend, which you listed at .0005 which is basically right in the middle of the low number I had spec'd (.0003") and the high number I suggested (.00075"), I assume you are capable of doing the arithmetic necessary to figure that out based on your overwhelming knowledge of mathematics.

I understand your concern when you think someone is too stupid to do anything but use a calculator, but you seem to be hung up on that subject and less understanding that I do indeed know how to use these equations. All essentially based on an admitted typo at the beginning of this post. Now, I am not sure why you persist on being such a curmudgeon, but hey man, its no skin off my back.

As far as the spot drill vs. center drill argument is concerned, I am fairly certain this has been beaten to a pulp by the rest of the internet, and the only comment that I have to make on the subject is that I have used center drills for this purpose repeatedly and never have had any issues with location, so IMHO they achieve the same end goal. While technically I would agree with you that a spot drill is the correct tool for the job, if this achieves a satisfactory result then its really neither here nor there. I have heard it stated before that "the right tool is whatever works" and that is basically my stance on this argument. When to Use a Spot Drill + 7 Useful Tips and Techniques - CNCCookbook: Be A Better CNC'er you can see from this article that I am not the only one who does this.

You are right, because of the wording I misunderstood. I thought you were "guessing" that .0003" was Equal to .0015".

R

I think your chipload is light I would just give it more to bite into. I was doing a job in 304L with the same size drill but .625 deep and used similar parameters. However I used good drills designed for 304 and spotted my holes first. Using a center drill in this case is not the correct tool. Unless your center drill has the same angle or larger than that of your drill. Dont start the hole make only a spot and you should have less trouble.

Whysosharp said:

I think your chipload is light I would just give it more to bite into. I was doing a job in 304L with the same size drill but .625 deep and used similar parameters. However I used good drills designed for 304 and spotted my holes first. Using a center drill in this case is not the correct tool. Unless your center drill has the same angle or larger than that of your drill. Dont start the hole make only a spot and you should have less trouble.

Click to expand...

I am only using just the tip of the drill and to be honest I don't know the angle of that drill point, we get them through McMaster and the page doesn't state.

At any rate this is a .108" end of the drill (#3 center drill) and I am only going down .040", and visibly doesn't look like a drastic angle difference from the drill that is actually drilling the hole.

One thing that could support your argument of using a spot drill is the lackluster cutting ability of the center drill. Could this be work hardening the stainless as it drills in? I have on flood coolant, but could see how that would be happening. Still doesn't make sense why the .0625" drill was fine with the same center drill/depth of center and similar specs speed/feed wise, but I could see this being a flaw.