[TechMonkey]

Hello all,

I have been trying to use high speed machining methods on a older vf2. the machine is good for 10,000 rpm, but I cant feed much more than 120 inches per minute without alot of jerk and stutter.

I am cutting 48hrc H13, and I use HSM Advisor to get my speeds and feeds. Parameters follow


Endmill, Garr 4 flute Squar Tialn 3/8" 1" Flute
Speed 7000rpm
feed 115 ipm
step over 8%
depth 1x.
cut style : plunge into open through hole, dynamic mill paths mastercam. g187 p2 e.01


I am cutting pockets and I only get about 20 minutes of tool life out of an endmill which is only 2 pockets. (pockets are 2"x1.5" x .750 deep) So, not a lot of material moved. and the tool is on the hot side of warm after a couple minutes cutting, so I think its rubbing.

I think maybe I need to increase speed to activate the coating. 7000rpm is about 700sfm, but is that hot enough? I also think I should take a heavier cut, but I am feed limited at 120ipm, so should i increase stepover, to say 12%?


I would love to hear how you guys would make this cut. How long would you guys expect this endmill to last in 48HRC material?

Thanks!!

[Jim Dawson]

You might take a look at the Garr tech page for that end mill, looks like cutting speed should be in the range of 60-90 FPM. I think you're turning a bit fast. https://www.garrtool.com/doc/pdf/tec...ling_guide.pdf About half way down the page.

[TechMonkey]

You might take a look at the Garr tech page for that end mill, looks like cutting speed should be in the range of 60-90 FPM. I think you're turning a bit fast. https://www.garrtool.com/doc/pdf/tec...ling_guide.pdf About half way down the page.

That doesnt make any sense??? thats 600rpm, and no where close to turning on the coating.

[Jim Dawson]

I get 917 RPM and 7 IPM. But I'll bet you could use 40% stepover

[RCaffin]

7000 RPM at 115"/min?
You are making the pocket by abrasion, not by cutting!!! Wildly out.

Cheers
Roger

[TechMonkey]

7000 RPM at 115"/min?
You are making the pocket by abrasion, not by cutting!!! Wildly out.

Cheers
Roger

thats a .004 chip load which is much above what the manufacturer recommends. however maybe the stepover isnt high enough. can you tell me where you would run it?

[dertsap]

no where close to turning on the coating.

rpm turns on the coating ??

A standard end mill with a coating on it is still a standard end mill . It's no different than trying to drag race a lada against the big blocks , you can replace the gas with alcohol but your still racing a lada . Garr carbides are soft in my opinion and you need a better quality carbide that has a variable flute variable helix , robjack , gorilla mill etc . Either vibration is killing the end mill or there is enough heat being generated to cook the coating , or both
Maybe try positing a video of what your trying to accomplish

[RCaffin]

I would probably start around 2000 rpm and 100 mm/min. Your DOC of 1x is a bit heavy unless you have the power and rigidity.

With an 8% stepover there is serious potential for a lot of rubbing without cutting unless you are climb milling. You should be climbing. With climb milling I would be looking at a stepover of maybe 20%.

If Dertsap is right about the Garr carbide, that could also be a problem. I use carbide cutters from CarbideChiu on eBay, rated at HRC65 (not HRC55 or HRC45). They are not 'traditional Chinese' by any means: German or Swedish carbide stock I think. Quite expensive compared to the cheaper stuff on eBay. The difference is very noticeable.

Cheers
Roger

[RCaffin]

Can't edit my posting. Mumble.
Once you have reasonable cutting with suitable chips, then start to go up in speed. But watch the chips: don't let them get too small.
Cheers
Roger

[zero_divide]

Hello all,

I have been trying to use high speed machining methods on a older vf2. the machine is good for 10,000 rpm, but I cant feed much more than 120 inches per minute without alot of jerk and stutter.

I am cutting 48hrc H13, and I use HSM Advisor to get my speeds and feeds. Parameters follow


Endmill, Garr 4 flute Squar Tialn 3/8" 1" Flute
Speed 7000rpm
feed 115 ipm
step over 8%
depth 1x.
cut style : plunge into open through hole, dynamic mill paths mastercam. g187 p2 e.01


I am cutting pockets and I only get about 20 minutes of tool life out of an endmill which is only 2 pockets. (pockets are 2"x1.5" x .750 deep) So, not a lot of material moved. and the tool is on the hot side of warm after a couple minutes cutting, so I think its rubbing.

I think maybe I need to increase speed to activate the coating. 7000rpm is about 700sfm, but is that hot enough? I also think I should take a heavier cut, but I am feed limited at 120ipm, so should i increase stepover, to say 12%?


I would love to hear how you guys would make this cut. How long would you guys expect this endmill to last in 48HRC material?

Thanks!!

I am away from computer now and can't check your numbers.
But why such high SFM?

On my FSWizard i am getting much more reasonable
430 SFM and 0.006 ipt feed

[TechMonkey]

I am away from computer now and can't check your numbers.
But why such high SFM?

On my FSWizard i am getting much more reasonable
430 SFM and 0.006 ipt feed

I have always thought that anything under 450 sfm or so was coolant territory. I base that only on my lathe days from when I tried to turn between 350-450 sfm. and it was all coolant and the tools lasted forever. getting upwards of 500 sfm and you would start to see tool degradation but more parts faster. I also saw other sources that run their Tialn endmills from 1200-1600 sfm, along with the appropriate feed of course.

So my question then is, if you recommend 450sfm, then how do I get to the next step and get more out of the tool?

HSM advisor with chip thinning and hsm checked, gives me 4057rpm(398sfm) at 56 ipm with an 8% step(climb).

Increasing to 7000 takes the surface speed to 687sfm and 96ipm. I was running 115ipm to try and keep the chip load up.


I'm really curious how some people get these tools up to 200+ipm. maybe they aren't doing it with anything this hard. (which i dont consider 48 to be all that hard. )

[zero_divide]

I have always thought that anything under 450 sfm or so was coolant territory. I base that only on my lathe days from when I tried to turn between 350-450 sfm. and it was all coolant and the tools lasted forever. getting upwards of 500 sfm and you would start to see tool degradation but more parts faster. I also saw other sources that run their Tialn endmills from 1200-1600 sfm, along with the appropriate feed of course.

So my question then is, if you recommend 450sfm, then how do I get to the next step and get more out of the tool?

HSM advisor with chip thinning and hsm checked, gives me 4057rpm(398sfm) at 56 ipm with an 8% step(climb).

Increasing to 7000 takes the surface speed to 687sfm and 96ipm. I was running 115ipm to try and keep the chip load up.


I'm really curious how some people get these tools up to 200+ipm. maybe they aren't doing it with anything this hard. (which i dont consider 48 to be all that hard. )

This is what you get with your tool (150% sfm and feedrate):

Material: H13 Tool Steel 45-50 RC
Tool: 0.500 in 4FL Carbide TiAlN HP/Roughing End Mill
Speed: 540.0 f/min / 4127.4RPM
Feed: 0.0059 in 0.0237in/rev 97.82 in/min
Chip Thickness: 0.0036 in
Reference Chip load: 0.0016 in
Engagement: DOC=1.00 in WOC=0.05 in
Effective Dia: 0.500 in
Cross Section: 0.20 x Dia.
Power: 7.3HP
MRR: 4.89 in³
Torque: 9.29 ft-lb
Max Torque: 7.90 ft-lb
Cutting Force: 445.9 lb
Deflection: 0.0009 in

The reason the tool lasts so little in your case is that SFM is too high and it burns the tool. I normally would not go over 150% from recommended especially on demanding materials.
At the same time you can not push the feedrate too high because 48Rc is pretty hard. You will just chip the edges.

To increase the productivity you need to increase the Depth of cut and the number of flutes.
Absolutely same conditions for a 7 flute endmill would yield 164.80 ipm

Most manufacturers provide high-flute count endmills for hard milling for this very reason.

Also for this very reason people try to avoid roughing a lot of hardened material.
I used to machine a lot of 45-50 Rc hardox plates and they would eat cutters in a matter an hour. So the strategy was to try to get as much work done withing that time frame.

Attachment 385184

[RCaffin]

Power: 7.3 HP
Cutting Force: 445.9 lb

Just so!

I suggest HSM makes a lot more sense on cast aluminium.

Cheers
Roger

[zero_divide]

Power: 7.3 HP
Cutting Force: 445.9 lb

Just so!

I suggest HSM makes a lot more sense on cast aluminium.

Cheers
Roger

What do you expect ? This is not a Tormach-level material.
And it is the opposite. HSM makes a lot more sense with tough and hard materials than with soft ones:

https://www.emastercam.com/forums/to...r-hsm-request/

[RCaffin]

Oh my, frightening stuff!
I don't have that sort of power in my spindle, and see no need for my sort of interests.
But fascinating all the same (in an Addams Family way?).

Cheers
Roger

[RCaffin]

Mastercan URL
Oh my, frightening stuff!
I don't have that sort of power in my spindle, and see no need for my sort of interests.
But fascinating all the same (in an Addams Family way?).

Cheers
Roger

[TechMonkey]

This is what you get with your tool (150% sfm and feedrate):


The reason the tool lasts so little in your case is that SFM is too high and it burns the tool. I normally would not go over 150% from recommended especially on demanding materials.
At the same time you can not push the feedrate too high because 48Rc is pretty hard. You will just chip the edges.

To increase the productivity you need to increase the Depth of cut and the number of flutes.
Absolutely same conditions for a 7 flute endmill would yield 164.80 ipm

Most manufacturers provide high-flute count endmills for hard milling for this very reason.

Also for this very reason people try to avoid roughing a lot of hardened material.
I used to machine a lot of 45-50 Rc hardox plates and they would eat cutters in a matter an hour. So the strategy was to try to get as much work done withing that time frame.

Thanks for that info. My tool was a 3/8 but I get your point nonetheless. So I guess when your talking about the critical surface speed of tialn coated tools (ie, the point when the coating is activated and working) I guess what it boils down to is that it just happens at a lower speed in hardened h13 than in some other materials.


I would like to present this video, in which robbjack is running 700sfm on a 1/2" 7 flute tool. with a 5-10% step over. Note at the end of the video, the tool is not hot. This material is 6 rockwell points higher than my material. He is running this tool at 125ipm. (So my chipload was quite a bit higher, and a bit lower in surface speed.)

https://www.youtube.com/watch?v=JATjRSzXgjw


This could very well be a much better tool than what I am using though.

[zero_divide]

Thanks for that info. My tool was a 3/8 but I get your point nonetheless. So I guess when your talking about the critical surface speed of tialn coated tools (ie, the point when the coating is activated and working) I guess what it boils down to is that it just happens at a lower speed in hardened h13 than in some other materials.


I would like to present this video, in which robbjack is running 700sfm on a 1/2" 7 flute tool. with a 5-10% step over. Note at the end of the video, the tool is not hot. This material is 6 rockwell points higher than my material. He is running this tool at 125ipm. (So my chipload was quite a bit higher, and a bit lower in surface speed.)

https://www.youtube.com/watch?v=JATjRSzXgjw


This could very well be a much better tool than what I am using though.

There are several reasons why they are able to cut such hard material so "fast"

1) they are using AlTiN coating that is harder than TiAlN and more temperature-resillient.

2) Because of the toolpath configuration they are onpy cutting 20% of the time or so. Rest of the time tool spends cutting air and cooling.

3) I do not know if it is really h13 56Rc and Have no idea how long it will last any way.

Calculator can not give ideal parameters outright.
It is supposed to land you in a comfortable zone at about 75%-100% of the available capacity.

[RCaffin]

And don't forget - he is using a trochoidal cutting path too (as zero has pointed out). That is a lot different from a straight plowing.
Hum - seems to be a bit of a glow from the tool though - fun stuff.

Cheers
Roger

[TechMonkey]

And don't forget - he is using a trochoidal cutting path too (as zero has pointed out). That is a lot different from a straight plowing.
Hum - seems to be a bit of a glow from the tool though - fun stuff.

Cheers
Roger

As I mentioned in the first post. I was using the same strategy.