how much do you increase SFM when radial engagement milling?

lowCountryCamo · Apr 11, 2018

I am programing a large part in 17-4 Rockwell 38 - 44. I'm using a .75 VarifluteII .06cr 1-2 inches deep. Right now I am stepping over .04" 75ipm at 400SFM. How do you figure SFM as step over decreases. I have a lifetime license of HSM Advisor but not sure I am using it correctly.

macds · Apr 11, 2018

sfm is sfm. You dont change that. Its measured at the periphery of the tool.
I think what you are trying to get at is radial chip thinning?
This technique takes advantage of tangential engagement of the cutter to thin the chip, and allows for higher feedrates utilizing smaller stepovers.

I hope im not beating a dead horse.

I use HSM advisor A LOT. If you have any specific questions, please ask.
Eldar is a great dude, and lingers here from time to time. You could likely contact him directly if you have questions, but the software is pretty straight forward.

Those cut parameters sound a little aggressive to me at a 2" DOC, but if you have a rigid machine\setup, go for it.

Cheers

BROTHERFRANK · Apr 11, 2018

I have run a 5 flute, 3/8" in 15-5 and 17-4, H900, dry (air blast), 1" depth of cut, .015" stepover, 14500 rpm (1425 sfm), 650 IPM very successfully. If you apply these parameters to your 3/4" end mill, you will be at 7250 rpm, 325 IPM (if 5 flute) and .03" stepover. I got the parameters from Mastercam Dynamic milling and it was using the Iscar tool Library. Tool was Iscar All In One 5 Flute Chatter Free they called it at the time I believe. Why not run a less costly 5/8" or 1/2" end mill? They can handle the depth and handle tighter radii tool paths.

CarbideBob · Apr 12, 2018

I find SFM mostly trial and error and looking at used tools under a microscope.
SFM is tool life, too much and your burn up the tool. Too little and you are not efficiently using the tool.
When you reduce the WOC you can use a higher SFM for the same tool life.
What tool life you want or need depends on you and the application. You can play with SFM to align tool changes to breaks, shifts, or number of parts so the tool is changed at a convenient time. Google "Taylor tool life curve".

Simplified and not quite correct but think of this:
If you have a very hot part you can touch it quick and not burn yourself.
Holding that same part in your hand for a minute maybe very painful.

In a long engagement the tool is in contact a long time. As the stepover is decreased the tool is in contact for a shorter time sort of like quickly touching something.

It is all way more complicated than this but tool life is the concern and upping speeds until the tool life is unsatisfactory or you see signs of wear you do not like is faster than slogging through the theory and math.
Bob

zero_divide · Apr 12, 2018

Chipload seems ok (maybe a little low).
I would try faster sfm, though.

How much faster depends on how much tool life is important in your case.

exkenna · Apr 12, 2018

If that's a 4 flute tool you're showing .0092 IPT but actual chip thickness is around.0041 due to radial chip thinning. If fixturing and tool holding method allow you might be able to get away with a 25% increase in feed.
So 97 IPM = .012 IPT would be an actual chip load of .0054 @ .040 radial DOC.

If it's a 5 flute, then 122 IPM (.012 IPT) would give an actual chip load of .0054 per tooth.
A 3/4" variable geometry design should handle this.

Remember, heat is always and everywhere the killer. The only acceptable mode of failure is predictable abrasive wear.
Always strive to make gains with feed or DOC before looking at higher SFM.

DMF_TomB · Apr 12, 2018

lowCountryCamo said:
I am programing a large part in 17-4 Rockwell 38 - 44. I'm using a .75 VarifluteII .06cr 1-2 inches deep. Right now I am stepping over .04" 75ipm at 400SFM. How do you figure SFM as step over decreases. I have a lifetime license of HSM Advisor but not sure I am using it correctly.

.
i increase sfpm when side milling compared to full width slotting but hard to say how much cause a lot depends on machine, part, fixture, tool and tool holder and vibration chatter. sometimes go by sound or noise level and finish left on the part as well as how tool gets dull. corners breaking off compared to even dulling of cutting edges

mhajicek · Apr 12, 2018

When applying high feed rates you have to increase RPM a bit just to keep SFM the same. If climb cutting with a 1/4" endmill at 800 IPM, you have to spin at 1019 RPM just to keep the flute stationary in the material, rolling along like a wheel. So start by adding that. Then you'll find that since the tool is continuously contacting fresh, cool material, the heat dissipates faster, so you have to spin even faster to keep the optimal heat. In many tool and material combinations you'll actually have shorter tool life if you don't generate enough heat.

litlerob1 · Apr 13, 2018

mhajicek said:
When applying high feed rates you have to increase RPM a bit just to keep SFM the same.

The "same" as what exactly? You say "increase the RPM to keep the SFM the same", again the same as what? Surface Footage has nothing to do with Motion as it were it has to do with Rotation (as it were).

You can feed the Tool zero IPM and the SFM is the same as if you were feeding it 100 IPM.

Matt@RFR · Apr 13, 2018

mhajicek said:
When applying high feed rates you have to increase RPM a bit just to keep SFM the same. If climb cutting with a 1/4" endmill at 800 IPM, you have to spin at 1019 RPM just to keep the flute stationary in the material, rolling along like a wheel. So start by adding that. Then you'll find that since the tool is continuously contacting fresh, cool material, the heat dissipates faster, so you have to spin even faster to keep the optimal heat. In many tool and material combinations you'll actually have shorter tool life if you don't generate enough heat.

VERY interesting, I think this is the first time I've seen this brought up. Is there a calculator that you're aware of to convert RPM to IPM based on tool diameter?

Lastu · Apr 13, 2018

litlerob1 said:
The "same" as what exactly? You say "increase the RPM to keep the SFM the same", again the same as what? Surface Footage has nothing to do with Motion as it were it has to do with Rotation (as it were).

You can feed the Tool zero IPM and the SFM is the same as if you were feeding it 100 IPM.

This is splitting hairs, but technically feedrate also changes SFM if you consider the relative motion of the workpiece to the periphery of the cutter.
So when climb milling the feedrate "slows" the SFM and conventional milling speeds it up. But realistically the effect is negligible...

litlerob1 · Apr 13, 2018

Lastu said:
This is splitting hairs, but technically feedrate also changes SFM if you consider the relative motion of the workpiece to the periphery of the cutter.
So when climb milling the feedrate "slows" the SFM and conventional milling speeds it up. But realistically the effect is negligible...

Here we go again. right? If you are trying to make a point that you are a smart guy, great, heres your Trophy :soapbox:

There is a reason we use the Formulas that we do. KISS

swarf_rat · Apr 13, 2018

Matt@RFR said:
VERY interesting, I think this is the first time I've seen this brought up. Is there a calculator that you're aware of to convert RPM to IPM based on tool diameter?

D x Pi x rpm = IPM isn't it? So rpm = IPM / (D x Pi). For climbing cuts.

It isn't inconsequential, depending on the circumstance. In the 1/4 endmill feeding at 800 IPM case, turning at 1000 rpm it will be running backwards against the material. What do you call that, negative SFM? Not going to be good for tool life....

Motion and SFM are related, as SFM is defined as the difference in speed between the tool cutting surface and the work. No other definition makes sense. If the work is moving relative to the tool, it will change SFM.

litlerob1 · Apr 13, 2018

swarf_rat said:
D x Pi x rpm = IPM isn't it? So rpm = IPM / (D x Pi). For climbing cuts.

It isn't inconsequential, depending on the circumstance. In the 1/4 endmill feeding at 800 IPM case, turning at 1000 rpm it will be running backwards against the material. What do you call that, negative SFM? Not going to be good for tool life....

Motion and SFM are related, as SFM is defined as the difference in speed between the tool cutting surface and the work. No other definition makes sense. If the work is moving relative to the tool, it will change SFM.

No it's not

https://www.google.com/url?sa=t&sou...TCAIQFgggMAE&usg=AOvVaw1BhEfduxU2Wif9fi3b_y8q

DMF_TomB · Apr 13, 2018

been my experience increasing things you reach a point where you get sudden tool failures and even if they happen 2 to 10% of the time it can cause major problems.
.
i record all sudden tool failures and if they happen twice or more i tend to back off til they dont happen as much.

Matt@RFR · Apr 13, 2018

litlerob1 said:
No it's not

Think about a car tire (cutting tool) rolling along the road (material). If the tire is not skidding or doing a burnout, just rolling along like normal, then no matter the speed the tire is going (typical SFM), the surface speed of the tire RELATIVE TO THE ROAD (in the cut) is zero.

lowCountryCamo · Apr 13, 2018

DMF_TomB said:
been my experience increasing things you reach a point where you get sudden tool failures and even if they happen 2 to 10% of the time it can cause major problems.
.
i record all sudden tool failures and if they happen twice or more i tend to back off til they dont happen as much.

You got a picture of that 2%-10% sudden tool failure.

Mtndew · Apr 13, 2018

lowCountryCamo said:
You got a picture of that 2%-10% sudden tool failure.

I'm sure he'll post that pic of the drill going thru the control screen since he loves to show it.

swarf_rat · Apr 13, 2018

litlerob1 said:
No it's not

https://www.google.com/url?sa=t&sou...TCAIQFgggMAE&usg=AOvVaw1BhEfduxU2Wif9fi3b_y8q

This does not support your position in the slightest. ALL motion is relative. NO motion is absolute. Even when your tool is stopped (relative to the table), it is traveling at over a 88,000 ft/min (relative to the center of the Earth) and nearly 3 million ft/min relative to the sun. The only reference frame that makes sense for a tool is the work. That's what it's rubbing against. That's what counts for wear, heat, and anything else. That is why is it the same for a lathe (tool stationary, work turning) and a mill (work stationary, tool turning). SFM is the relative motion between work and tool.

litlerob1 · Apr 13, 2018

swarf_rat said:
Motion and SFM are related, as SFM is defined as the difference in speed between the tool cutting surface and the work. No other definition makes sense. If the work is moving relative to the tool, it will change SFM.

My "No it's not" comment was about the definition of SFM.

They are related, not defined by each other. And if you work out the Formulas as provided by Swarf-rat's #13 post, you'll se that it is meant as a slight joke. Whether the whole post is funny or not, I'm not sure.

There is a whole 'nother Thread about the exact same thing even a reference to Cars and Tires going around corners, guess what it was the exact same argument except about Feedrate instead of SFM.

Maybe we need to use the term 'V'elocity, for the action of Motion while Rotating Tools complete Linear and Arc moves.

We separate them for a reason.

how much do you increase SFM when radial engagement milling?

Stainless

Hot Rolled

Stainless

Diamond

Stainless

Stainless

Diamond

Diamond

Diamond

Titanium

Plastic

Diamond

Titanium

Diamond

Diamond

Titanium

Stainless

Diamond

Titanium

Diamond

Similar threads