A decent speed and feed chart

hello all i want to ask a question to some ppl that will be able to answer this question once and for all. does anyone know of a good reference guide or chart for speed and feed rates based on tooling and material??? also i wanted to know what everyone uses for this. most the time i start out with an experienced guess and go from there. theoretically i would like a chart or grid that i look at that would tell me the max speed and feed i can use for the tool and material combonation, or better yet when i choose the tool in mastercam it already loads it for me. any help on this is greatly appreciated!

Google CNC Cookbook or Gwizard. It has a comprehensive data base with materials and speeds and feeds and works well for most applications both turning and milling.

camscan said:

here we go again, must have fastest feeds and speeds. Fast is not in the least bit important, how many you have made at the end of the day is

Click to expand...

And most likely the only thing this guy has cut is his toe nails...
Have you ever CUT METAL??? worked in a Shop?? Served an APPRENTICESHIP????

My guess is nope... just another cad jockey turned into a programer
Is that how it's done these days???

This is why people on here stop asking questions and helping others because of comments like the above ........GROW UP

stephon0913 said:

hello all i want to ask a question to some ppl that will be able to answer this question once and for all. does anyone know of a good reference guide or chart for speed and feed rates based on tooling and material??? :

Click to expand...

Sheesh.... don't want much do you?

When you find the croc of gold at the end of the rainbow, grab the book next to it.

stephon0913 said:

hello all i want to ask a question to some ppl that will be able to answer this question once and for all. does anyone know of a good reference guide or chart for speed and feed rates based on tooling and material??? also i wanted to know what everyone uses for this. most the time i start out with an experienced guess and go from there. theoretically i would like a chart or grid that i look at that would tell me the max speed and feed i can use for the tool and material combonation, or better yet when i choose the tool in mastercam it already loads it for me. any help on this is greatly appreciated!

Click to expand...

Well your best bet is the insert guidelines, but be aware they are best case scenario. Depth of cut, coolant application, and machine rigidity / part setup all play a major factor ( almost as important as "speeds and feeds" )

When trying to get longevity out of your program and setup you need to factor in all these variables to get things right.

I could tell you that :

Mild steel (1018)/ C12L14 = 800 sfpm
4140 ANN / 8620 = 600 sfpm
4340 HT = 350 sfpm
4140 HT = 400 sfpm
304 / 316 SS = 275 sfpm
17-4PH900-1150 = 300 sfpm
6061/2011 AL = 3000 sfpm

all using a CNMG 432 PM 4225 insert from Sandvik. With the feeds and depths of cuts comes careful consideration of your setup.

With a Mori Seiki SL150 ( smaller machine ) the maximum depth of cut i can take is around 0.250" Diameter on mild steel, 0.200" on 4340 HT and i would never go more than 0.012 feedrate.

On our new NLX2500 i can take that same job and push 0.320" diameter or 0.018" feedrate on midsteel and easily do 0.250" at 0.014" on 4340 HT.

Now i would never run that when using a tailstock, or when im not holding on by the full jaw of the chuck, and i certainly wouldnt run those feeds/speeds on small diameter work.

Some materials are more forgiving than others and if you cant get coolant right where you need it, things can change in a hurry.

So like i said , basically follow the insert guidelines and remember that those are under perfect conditions, and you need to adjust from there.

David.

Gary E said:

And most likely the only thing this guy has cut is his toe nails...
Have you ever CUT METAL??? worked in a Shop?? Served an APPRENTICESHIP????........ yada yada....

Click to expand...

camscan said:

Come on Gary , give the lad a break, he is using his experience? blah blah...........

Click to expand...

Crap guys...... ain't no slack for nobody, huh?

You all don't know him, how can you toss the judgement up front? Sound like grumpy old farts to me.

In my case, I personally had 6 years in a shop, lots of experience with several things. What CNC experience I had was on a prototrak and self taught. I switched jobs and worked with a couple guys that knew what they were doing on the CNCs, so it was a whole new game. I asked the main CNC guy if there was a way to calculate speeds and such. I was use to guessing going by how it felt to me for 6 years of mostly manual machining. He was happy to help and gave me a straight up answer, not like some grumpy dried up old pecker

camscan said:

here we go again........ Fast is not in the least bit important, how many you have made at the end of the day is

Click to expand...

Actually, quality is far more important that quantity, or so many may agree.

stephon0913 said:

hello all i want to ask a question to some ppl that will be able to answer this question once and for all. does anyone know of a good reference guide or chart for speed and feed rates based on tooling and material??? also i wanted to know what everyone uses for this. most the time i start out with an experienced guess and go from there. theoretically i would like a chart or grid that i look at that would tell me the max speed and feed i can use for the tool and material combonation, or better yet when i choose the tool in mastercam it already loads it for me. any help on this is greatly appreciated!

Click to expand...

The only chart you need is a calculator.

Several years ago I was told, on steel:

100 SFM for high speed steel
200 SFM for plain carbide

I find with HSS, on tool steels and such, maybe as low as 80 SFM, mild steels, maybe as much as 120 SFM or so. Carbide can often run more than 200 SFM. Coated carbides might go for 300-600 SFM, you really just need to look for manufactures specs.

If you ask me, on aluminum, it's pretty much whatever the machine can handle. You can run 1000+ SFM easy with HSS endmills.

but you don't necessarily have to go as high as any of these speeds, or be constrained by them. Keep in mind that this is best with flood coolant.

To calculate RPM:

RPM=(3.82*SFM)/DIAMETER

say 1/2" HSS endmil on mild steel

(3.82)*(100)/(.5)= 764 RPM

Feeds are hard to be straight forward, way to many variables. It can range from less than .0005" per flute to more than .010" per flute. It is easy to start with around .002" per flute.

Calculate as:

FEED=(RPM)*(# of flutes)*(FEED PER FLUTE)

Say from the above speed....

(750)*(4)*(.002) = 6 IPM

And that should be fairly mild. And these are better for less than 50% width of cut.

But keep in mind that there are MANY variables. Spindle HP, machine rigidity, tool quality, coolant quality and depth of cut, width of cut. If spindle RPMs high and HP is low, cutting .008" per flute can turn into .012" per flute real quick as it bogs, and gets worse till it backs up on max torque or stalls.

Cutting full width you will likely need to back off a bit. Cutting deep you sure might need to. But these should get you a starting point. All just depends on machine, tool and material.

If you tell me this is on some little POS benchtop mill, I'll ringe your neck for wasting my time and tell you to burn it and throw it out in scrap. Just because they are shit and makes these calculations useless. Cause even a beat to piss, neglected, worn out 40yr old bridgeport still be 10x better than a worthless little benchtop

couldnt agree more .....grumpy old engineers that want to sit shooting people down should stay off this forum if there not going to help . we all start somewhere and get better with experience and HELP

David Colongioli said:

Well your best bet is the insert guidelines........... David.

Click to expand...

Crap, I just assumed he was looking at milling, you talking lathe?

Sorry if I missed something

annoying said:

Crap, I just assumed he was looking at milling, you talking lathe?

Sorry if I missed something

Click to expand...

It's ok man......you get an "A" for effort just the same!

Nicely done.


Later,
Russ

OK, for those that call out ''Grumpy old men'' perhaps you don't know what a contentious issue speed and feed ''charts'' can be.

Yes of course there are guidelines, but they are only that, a guide, most of the time, getting the best results is down to experience plus basic knowledge of the principles of metal cutting.

And no, us '' Grumpy Old Farts'' don't always get it right.

Limy Sami said:

OK, for those that call out ''Grumpy old men'' perhaps you don't know what a contentious issue speed and feed ''charts'' can be.

Yes of course there are guidelines, but they are only that, a guide, most of the time, getting the best results is down to experience plus basic knowledge of the principles of metal cutting.

And no, us '' Grumpy Old Farts'' don't always get it right.

Click to expand...

Thats a better answer ! more helpful and constructive

Use the manufacturer's speed/feed data as a starting point. Work from the low-end to high, dependent on the depth of cut.

Probably more useful than anything when you're trying to set a starting point, especially if you don't have a lot of experience.

My personal experience tells me that there is no set "answer" to this. A test is always worth a million theories, regardless the number crunching involved because there are just too many variables involved.

To give you an idea... we have two fairly identical machines in our shop, one being a Makino with HSK40 tooling, the other a Roeders. One likes a 12mm 6-flute tool at one gage length, while the other is only stable with the exact same tool in a slightly longer holder when running the exact same parameters!

We have had to develop two separate ranges of cutting parameters for these machines. Point being... there's a lot more to this than the tool and the workpiece. Some people like 'statics' though... easier to wrap the head around I guess....

GL

Well thanks for the mixed response sure shows the grumpy old machinists from the forward thinkers I'm just trying to get some info from people that have been doing this longer than I have.

stephon0913 said:

hello all i want to ask a question to some ppl that will be able to answer this question once and for all. does anyone know of a good reference guide or chart for speed and feed rates based on tooling and material???

Click to expand...

Nope.
To many variables for a simple chart.
As a simple example cutting 4140 with carbide.
Optimal SFM will be between 200 and 2000 SFM and optimal chipload will be from .0005 to .040.

You can nail down a tighter range if you restrict it to save full width slotting with 1/2 to 3/8 endmills with a TiN coating at 50% of dia. deep on 32Rc 4140 parts. 62Rc parts will need very different numbers.
Even then end mill grind and helix angles will change the numbers.
Then there is the machine itself...........
On top of that what is right for you for life may be way different for somebody making 5 million parts a year in continuous 24/7 production.

You learn by playing with pushing it or find a tool engineer that has busted up tons of stuff to help you. Even if you choose number two it will still be a guess.

This is why manufactures specify wide ranges, we don't know all the parameters of your cut and how tooling costs per hour affect your hourly rate.
The on-line calculators will give you a starting point.

I wish I could say yes, my life would be so much easier if there was a simple answer here.
After 35 years of testing tooling I still find things that send me back to the drawing board.
Bob

That chart would be a mile long.

One of the endmills I use for harder materials has like 9 recommended speeds based off the amount of engagement......for every different type of hard material. There is also increased chip load based on radial depth...


On a side note: Guessing can be fun.

Limy Sami said:

OK, for those that call out ''Grumpy old men'' perhaps you don't know what a contentious issue speed and feed ''charts'' can be.

Yes of course there are guidelines, but they are only that, a guide, most of the time, getting the best results is down to experience plus basic knowledge of the principles of metal cutting.

And no, us '' Grumpy Old Farts'' don't always get it right.

Click to expand...

Well, I started on my post before yours was posted.

I just thought the the whole purpose is sharing ideas and experiences and giving/receiving guidance. And some venting of course. Heck, take those elements away and all that is left is gossip. Be a bunch of clueless women and girls on here then.

lots of good knowledge on here though. I sure got some valuable help from schniedermachine a couple years ago.

Don't get me wrong, it's fun to read some of the BS on here too. I just thought guys was looking for help, not insult or criticism

Run err as fast and hard till she breaks or burns up

Adjust speed and feed accordingly

When you stop smoking tooling, tossing parts off the table, and breaking shit you've found the acceptable speeds and feeds of a particular setup, machine, and tool.

After awhile you'll be able to make some wiser decisions based on experience.

Nobody ever learned nothin by not cooking a tool or two.

Thats the speech I got when I first started in a machine shop, apparently this is the first your hearing it

Horsepower/Torque at the tool, Setup rigidity, Length of tool, runout, etc, etc, etc are all going to fuck with whats on this magical chart you want.

As far as MFG guidelines/recommendations: Always start at the high end and work your way down. Chances are 90% of the time the high end won't ever work, but you'll be happy the few times it does

I'm with CarbideBob.

To get good feeds and speeds, you need two things: a good calculator and calibration.

As some have said, the calculator will get you a starting point. It performs an even more important role though, which I'll come back to in a second. First, let's look at this idea of calibration.

Calibration means bringing the real world experience and data into the equations that the calculator uses. A feeds and speeds calculator starts with its own internal tables of what the chiploads, surface speeds, tweaks for different materials, and all the rest should be. That's a database, and the best calculators will make it possible to "calibrate" that database with your experience, your tooling, and your shop's best practices.

You can plug in your tooling manufacturer's recommendations right away to the database. There's a few other things to plug in as well if the calculator is able to take them, such as what the spindle power curve looks like.

But then the experience and shop best practices have to kick in. Every time you make a cut, you have the opportunity to learn something. Make it a little faster than you did the last time. Fiddle the variables. And keep a record of it. Whether the cut works well or breaks the cutter, both are important as they're helping to map out the envelope for that cutter, that machine, and that tooling under your shop's best practices. All that information needs to go into a database that's linked to calculator for best results. Done right, it's easy to track and easy to take advantage of. That calculator + database should do most of the record keeping work.

Once you have some of that data to go from, the real value of the calculator emerges. While a lot of variables have to be calibrated, there are also a lot that can be calculated and that are very predictable. Radial chip thinning is a real effect that works the same every time on every machine. The role of different tool engagement angles for HSM toolpaths are well understood. Tool deflection is predictable and can be calculated.

This means your precious data collected from real jobs is reusable in new jobs that may have slightly different parameters. The stepover or depth of cut may need to change for a new job, and maybe you will only make one or a small number of the parts so no experimentation is possible. Take your calibrated database which is hopefully built into the calculator and let the calculator tell you what to do there. Since it's been calibrated by your real world experiences in your shop with your tooling, it's going to be pretty bang on right about it.

Combining a database with a calculator that considers a lot of variables (about 50 at last count) is what G-Wizard does.

Cheers,

BW

Makes me wonder how I've survived this long without a 'calculator', short of my trusty TI-89.

It does seem redundant to me to use a starting point, develop tool paths, record that data in a database when most are using CAM systems with this technology on-board.

The procedure I use...

1. Record tool holder, gage length, tool ID, machine tool
2. Pick starting chip-load & rpm
3. Pick axial DOC for testing (this will not change for this portion of test)
4. Test cut at set radial DOC; say 0.5mm
5. Increase radial cut by set increment; say 0.5mm
6. Record stable and unstable cutting modes (no chatter present)
7. Rinse and repeat at +500 rpm

What you will find are the stable cutting speeds, and from there, you can increase the axial DOC to find best MRR for that material with that combination of tool, holder, etc..

It use to take me ~30 minutes to run through this procedure once the machine was ready to go. Harmonic software negates the step-increment to find stable lobes, which speeds things up considerably.

Anyhow...

All of this data goes into the CAM system... because all of the setup data should come out OF the CAM system for the operators; ie, the gage length, holder ID, tool ID, etc..

All of the data is logged into the CAM system for the type of cut being performed as a "process" or whatever your system supports, such that a separate database is simply not necessary.

Warning: stable lobes will tax machine HP, so pay attention to your load meter. A good cutting condition will remain stable right up to the machine's limits, especially with large cutters.

There are plenty of variations on this technique and I'm all eyes to reading them, but my point in all of this is that most have the capabilities right there in their CAM system to log 'best' conditions for future reference.

My 2.5 centavos