What's new
What's new

Where does SFM number come from?

Cooperstock

Aluminum
Joined
Apr 13, 2015
Hello,
So I have been reading through posts on feeds and speeds. I know it is ALWAYS a reoccurring question. I am attempting to understand the underlying concept.

I have specifically been looking at 304SS which I see everything from 250SFM to 700SFM, and chip loading from .0015 IPT to .005

Lets just assume carbide as the cutter, Im not interested in HSS.

Q1. do carbide inserted tools need to be calculated differently than solid carbide?

I know for SS constant cutting engagement, (no slow feeds, or pauses which could cause work hardening)

I know that manufacturers of endmills provide suggested Feeds and speeds for their endmills. I believe this is driven by flute grind, Helix angle and quality of carbide material itself.

Q2. But why does SFM vary so greatly depending on machining method? Isn't SFM a property of the material itself and the heat the cutter can take (i.e. property of the cutting material)?

Someone mentioned that 40 taper machines should be run a 30%-40% less of the specs of those of 50 taper. This concept makes sense due to rigidity of the holder, but I rarely see this mentioned or asked. Is it assumed 50 taper for most posts?

I also see little comment on type of tool holder. It seems milling chucks and hydraulic chucks would allow for 'better numbers' due to their rigidity and runout. It seems like using a standard 'end mill holder' (with the set screw(s) on the side) would be a less ideal choice especially when in harder materials.

Q3. Does the SFM used in calculations depend on HP of the machine?
I thought the HP (or more specifically the RPM at which 'good' torque is produced) was the driving number for MRR. But RPM is SFM when combined with the tool diameter...so?

Since this topic does come up so often, feel free to direct me to posts that address these questions.

I just get tired of reading
"I don't machine this material much, but I tried this.... and it seemed to work ok"
 

litlerob1

Diamond
Joined
Nov 4, 2013
Location
Utah, USA
I'm not going to answer all your questions. You've actually answered a lot of your own up there. MRR and SFM have nothing to do with each other.

SFM (in Machining) is the rate of rotation at which neither the Tool or Material fails to be Machined. It was easier for me to understand in the context of Turning. I can't run the same RPM on 12" as 1" and expect my Tools to survive. The reason there is a range, is the additional conditions. (Increased Rigidity, better holders, better melt, better coolant, HSM paths, coatings, density, etc...) If I'm at the low end of applied SFM, rigidity isn't even an issue, it's when I want to push it. Thus, increasing my ability to get more MRR. But fundamentally, they are unrelated.

R
 

Cooperstock

Aluminum
Joined
Apr 13, 2015
I'm not going to answer all your questions. You've actually answered a lot of your own up there. MRR and SFM have nothing to do with each other.

SFM (in Machining) is the rate of rotation at which neither the Tool or Material fails to be Machined. It was easier for me to understand in the context of Turning. I can't run the same RPM on 12" as 1" and expect my Tools to survive. The reason there is a range, is the additional conditions. (Increased Rigidity, better holders, better melt, better coolant, HSM paths, coatings, density, etc...) If I'm at the low end of applied SFM, rigidity isn't even an issue, it's when I want to push it. Thus, increasing my ability to get more MRR. But fundamentally, they are unrelated.

R

Yes, I understand SFM is rotational surface speed (either the material in a lathe or the cutter on a mill). I was just unclear why the SFM for a given material seems dependent on the process chosen. If someone is running 700SFM for 304SS then either that is the cutter or the material limiting that, but when do I know the transition between material limitation and cutter limitation? I keep reading 125 - 250 SFM for stainless but clearly people are running much higher SFM based on their posts.

So is there a lower bound to SFM for a material?
Other than just slow cutting, if the end mill is spinning a 1/2" EM at 500 RPM -> 65SFM Then for 4 flute at .005 IPT is 10IPM. Is there a fundamental issue with increasing the load on the cutter (i.e. increasing the IPM)?
Is there a benefit? (more heat into the chip so less heat in bulk material?) obviously if I can make bigger chips then the MMR goes up.

My mill has a load meter.
If I I engage a sharp 1/2" Carbide endmill (5 flute) in a hydraulic holder and increase the feed until the load is 20% (or 50%) is there a problem with this principal? a 250SFM for Stainless and 1/2" - 5 flute at .0015"IPT calculates to 1910RPM at 14 IPM, this seems slow, but if I I am cutting at .5" Axial-DOC and and .25% stepover (.125" Radial DOC), That .93 in3/min.

(of course this assumes material is well clamped/confined)

I have a matsuura with a 40 taper, limited to 4500RPM max but peak torque is way lower.
 

exkenna

Stainless
Joined
Nov 29, 2007
Location
North Alabama
The question.
SFM, Feed rate, depth of cut, where do I start?.

Answer. First and foremost: material group dictates surface footage, that's your starting point.
From there you can surmise feed rate for a given tool based on the type of cut and the tool maker's data.
Use feed rate and SFM to solve for RPM.
A good rule of thumb for traditional indexable milling cutters (not feed mills of course) is .004 feed per tooth in steels and stainless. Typically increase that by 30% in aluminum. Some exceptions for aluminum are Hi Performance niche tools for aluminum, like the Ripper Mill or such.

After getting the starting numbers you can adjust feed rate. If slotting, try increasing DOC in Z and watch the load meter to use up available torque. If profiling increase feed incrementally and watch the load meter and wall finish. Be aware of radial chip thinning when profiling at less than 50% step over.
Guhring has a handy calculator for this: Milling Performance Optimizer - GUHRING

The short answer is: Material dictates surface footage because heat is always and forever the killer of carbide.
Cutting metal causes heat. Excessive SFM causes more heat.

The only acceptable mode of failure is abrasive wear. Maintaining the proper SFM allows the carbide and coating to do their job, so when you've found your sweet spot the load meter and visual inspection of the tool will (in theory) let you get the most out of it before catastrophic failure.
 

Orange Vise

Stainless
Joined
Feb 10, 2012
Location
California
It's all about heat.

Tools will cut metal at virtually 0 SFM. Think of a hand tap. But the finish can be pretty bad and they're not very efficient.

So let's take turning a piece of 1018 steel as an example. A fairly gummy material because it has a relatively low tensile strength (compared to other steels), it's unalloyed, has no free-machining additives like sulfur or lead, and has a pretty high yield strength as a percentage of its tensile strength. Turn this stuff at low speed and you get a cloudy, smeared finish. The material is tearing rather than shearing. Crank up the SFM and at some point you get a polished finished that looks like it came off an OD grinder. What's happening is that right at the (microscopic) cutting edge, the heat is weakening the material, and the material is being sheared off cleanly from the base material, which has not heated as much and retains its strength.

Carbide inserts have heat-resistant and in some cases heat activated (AlTiN) coatings that give significantly higher heat resistance than the material it's cutting. By heat resistant I mean it keeps its strength at high temperatures.

However, keep cranking up the SFM and now you've gone past the limits of the insert. Too much heat. The edge literally burns up and things snowball. The now-blunt edge causes heat to increase even more and now you have sparks flying off the workpiece.

If you're roughing on a lathe, you can take deeper cuts and slow down the SFM. Surface finish is less important. This is a safety measure because you don't want an insert to blow up while taking a 0.200" DOC. Save the high speeds for finishing. If a finishing insert blows up, your part comes out oversized, but you don't crash your machine.

Turning SFMs don't directly translate to milling SFMs, primarily because of the interrupted nature of milling which create vibrations. Higher speeds generally exacerbate the effects of vibrations, because of both increased energy and getting up close to resonant frequencies, so speeds need to be reduced.
 

Cooperstock

Aluminum
Joined
Apr 13, 2015
The question.
SFM, Feed rate, depth of cut, where do I start?.

Answer. First and foremost: material group dictates surface footage, that's your starting point.
From there you can surmise feed rate for a given tool based on the type of cut and the tool maker's data.
Use feed rate and SFM to solve for RPM.
A good rule of thumb for traditional indexable milling cutters (not feed mills of course) is .004 feed per tooth in steels and stainless. Typically increase that by 30% in aluminum. Some exceptions for aluminum are Hi Performance niche tools for aluminum, like the Ripper Mill or such.

After getting the starting numbers you can adjust feed rate. If slotting, try increasing DOC in Z and watch the load meter to use up available torque. If profiling increase feed incrementally and watch the load meter and wall finish. Be aware of radial chip thinning when profiling at less than 50% step over.
Guhring has a handy calculator for this: Milling Performance Optimizer - GUHRING

The short answer is: Material dictates surface footage because heat is always and forever the killer of carbide.
Cutting metal causes heat. Excessive SFM causes more heat.

The only acceptable mode of failure is abrasive wear. Maintaining the proper SFM allows the carbide and coating to do their job, so when you've found your sweet spot the load meter and visual inspection of the tool will (in theory) let you get the most out of it before catastrophic failure.

With chip thinning the problem is still heat management?
Why is chip thinning only a concern at less than 50% step over?
That makes sense about slotting and profiling with adjusting Depth or speed to take advantage of the machine load capability.
 

Cooperstock

Aluminum
Joined
Apr 13, 2015
It's all about heat.

Tools will cut metal at virtually 0 SFM. Think of a hand tap. But the finish can be pretty bad and they're not very efficient.

So let's take turning a piece of 1018 steel as an example. A fairly gummy material because it has a relatively low tensile strength (compared to other steels), it's unalloyed, has no free-machining additives like sulfur or lead, and has a pretty high yield strength as a percentage of its tensile strength. Turn this stuff at low speed and you get a cloudy, smeared finish. The material is tearing rather than shearing. Crank up the SFM and at some point you get a polished finished that looks like it came off an OD grinder. What's happening is that right at the (microscopic) cutting edge, the heat is weakening the material, and the material is being sheared off cleanly from the base material, which has not heated as much and retains its strength.

Carbide inserts have heat-resistant and in some cases heat activated (AlTiN) coatings that give significantly higher heat resistance than the material it's cutting. By heat resistant I mean it keeps its strength at high temperatures.

However, keep cranking up the SFM and now you've gone past the limits of the insert. Too much heat. The edge literally burns up and things snowball. The now-blunt edge causes heat to increase even more and now you have sparks flying off the workpiece.

If you're roughing on a lathe, you can take deeper cuts and slow down the SFM. Surface finish is less important. This is a safety measure because you don't want an insert to blow up while taking a 0.200" DOC. Save the high speeds for finishing. If a finishing insert blows up, your part comes out oversized, but you don't crash your machine.

Turning SFMs don't directly translate to milling SFMs, primarily because of the interrupted nature of milling which create vibrations. Higher speeds generally exacerbate the effects of vibrations, because of both increased energy and getting up close to resonant frequencies, so speeds need to be reduced.

That is a good point with the 1018, So when there are different SFM given for HSS vs Carbide, thats really taking into account the properties of the cutter (ie the heat it is capable of handling).

So how are some people claiming they cut 304SS at 700SFM? or does HSM allow for heat to be more reasonably dealt with so higher SFM are possible?
 

exkenna

Stainless
Joined
Nov 29, 2007
Location
North Alabama
I've seen 304 cut at 700sfm using HSM methods.. trochoidal machining.
The tool is not in the cut long enough to retain heat, and because of radial chip thinning most of the heat is carried out in the chip.
 

Cooperstock

Aluminum
Joined
Apr 13, 2015
I've seen 304 cut at 700sfm using HSM methods.. trochoidal machining.
The tool is not in the cut long enough to retain heat, and because of radial chip thinning most of the heat is carried out in the chip.

Ah, thanks for sharing. That was my guess but wasn't certain.
 

CarbideBob

Diamond
Joined
Jan 14, 2007
Location
Flushing/Flint, Michigan
...
Why is chip thinning only a concern at less than 50% step over?
Because there is no chip thinning at 50 percent and above.
You are not understanding how this works, lay it out in a CAD.
SFM numbers in a catalog are way guesses. Too many variables and sometimes done by people with not a lot of chips in their shoes. Call this local experience in some cases and a wide range in others.

Milling is different from turning due to the impacts and tool time in the air. Air time good, impact bad.
Turning splines is sort of like milling.
Depth of cut has a very small influence. You just use more edge length.

The questions you ask are very good, any answers very complicated.
It would be so nice if it was straightforward. The devil lives in the details and if someone could kill that it would be better for my life.
All good, follow me down the rabbit holes. You think life has driven you mad in the past, now you dive into my world......

It is physics, the rules apply but so many ifs and or and buts and twists. Those melt your brain and you go with this or that works.
Bob
 

cyanidekid

Titanium
Joined
Jun 4, 2016
Location
Brooklyn NYC
basic stuff, but still excellent thread. some real experience speaking here! yes, all the above, but one super-obvious thing not brought up is the variation in the material you are working.

"304" in particular is a total shitbucket of unknowns.
even alloys that are less "all over the place" like 4140, can vary greatly from piece to piece.

an interrupted roughing cut in a nasty piece, VS. a light finishing cut in a nicely machining chunk, well it really could be WAY more different than the spread that had you troubled to begin with. :D
 

mmurray70

Hot Rolled
Joined
Jan 11, 2003
So how are some people claiming they cut 304SS at 700SFM? or does HSM allow for heat to be more reasonably dealt with so higher SFM are possible?

Yes its all about time in the cut. Think of it like a duty cycle. Look at a traditional tool path cutting a slot. 50% of the time your cutting and heating, and 50% of the time its cooling. If your doing HSM with a 10% stepover that works out to only a 7% duty cycle. Huge difference. Everyone knows how plunging is hard on tools, you can look at this the same way too. Things heat up because the tool is engaged and cutting 100% of the time, same with drilling, SFM is generally much lower drilling due to 100% time engaged in cut.
 

ChipSplitter

Titanium
Joined
May 23, 2019
Location
Maybe
SFM (in Machining) is the rate of rotation at which neither the Tool or Material fails to be Machined. It was easier for me to understand in the context of Turning. I can't run the same RPM on 12" as 1" and expect my Tools to survive. The reason there is a range, is the additional conditions. (Increased Rigidity, better holders, better melt, better coolant, HSM paths, coatings, density, etc...) If I'm at the low end of applied SFM, rigidity isn't even an issue, it's when I want to push it. Thus, increasing my ability to get more MRR. But fundamentally, they are unrelated.

R

Exactly.
One reason for SFM recommendations to vary wildly is because some applications need long tool life and don't care that much about cycle time (think mold-making), while others need super fast cycle time and tool life is calculated at 30 min. in cut or even less (think high-production automotive). With any material there is a "sweet spot" where tool life and cycle time begin to balance the scales. Eg.- Milling A-36 with a 1/2" 4 flute coated EM at .350" RDOC, up to 1" ADOC, .0025 ipt at 650 SFM gives me a life of 25-40 min. depending on the endmill manufacturer and material conditions. Dropping to 400 SFM may increase that to 80-100 min., but you have to decide how important cycle time is vs. tool life.

Clear as mud, eh?
 

5 axis Fidia guy

Stainless
Joined
Aug 17, 2006
Location
Wisconsin
The SFM varies huge in the tool recommendations from the manufactures as you have found out. I am a mold maker doing mostly hard milling. My usual go-to method is, use the lower values for roughing, and the higher values for finishing. Sure you can use the higer values for everything depending on how often you feel like changing tools. For a night run I usually stay conservative to make it thru the night.
 

Cooperstock

Aluminum
Joined
Apr 13, 2015
Whoosh

Thank you all,
Yes i see how all of the conditions connect. And my understanding has improved. I got the parts done i needed.
Heres what i learned (and i know there is much more to learn)
1. End mill makes a huge difference. I started with a 5 flute 1/2" coated carbide, kroycera. Would cut ok, but couldnt take much depth. When i changed to a different supplier it cut soo much cleaner.
2. I stuck with 200 -ish sfm for milling 304 and things went well. Used 20 sfm for drilling with HSS drills. 35sfm for carbide drills. Feed about .001" per rev.
3. I was milling a 8" x 14" plate starting at .25" thick, so stabilit was an issue. Where possible i drilled through and then cut full plate thickness with a .004" RDOC. No issues.
4. Tapped 2-56 holes by hand
5. For small features i was able to take .001" ADOC with onlinecarbide 3/8" 4fl carbide. I was amazed it didnt rub, but cut very cleanly (i made sure i had close clamps to make plate as stable as possible)
6. I know its not recomended, but i did use high pressure coolant (3 nozzles). Since all my cuts were light it seemed to go ok. I will experiment with no coolant soon.

So i agree with those experienced posters above...it is very much dependent on the specifics of the machine, material, holding, features, access to part, and cutter.

I did try a trochoidal path, but it was with the kroycera, it did ok, but wasnt happy with the result, will try it again with the onlinecarbide endmill. I wasnt sure how to best calculate the feed rate. It seems even with climb milling the chip thickness is pretty thin unless i travel fast, or take heavier overlaps. But thats a different topic.

Ill try to post pics of the parts. Not sure i can do it from phone app
 

ARB

Titanium
Joined
Dec 7, 2002
Location
Granville,NY,USA
I've seen 304 cut at 700sfm using HSM methods.. trochoidal machining.
The tool is not in the cut long enough to retain heat, and because of radial chip thinning most of the heat is carried out in the chip.

I've been doing this with staggering results. In the old days you would have been nuts to run a 1/2" mill at 5K in 304. Let alone get High MRR and long life. Modern tools and cutting paths have changed the game.:cheers:
 








 
Top