Milling 4130 I keep breaking Endmills

Hello first time posting, I am milling some 4130 34 HRC. I am using a Helical 83108 .500 dia 2.0 LOC chip breaker endmill with a Schunk Hydraulic Holder using high efficiency milling running 3050 rpm and feed rate of 30 ipm with a 4% radial and full axial. Now these endmill are running for about 7 hours before they break at around 31% spindle load. Should I be expecting more? the helical website suggest I run the tools way faster like 8950 rpm at a feed of 72 with a 8% radial engagement. I am running in a HAAS UMC 750 15k Spindle BTW. I have a lot of these parts to make so any help would be appreciated

Normally breakage like that is due to dull tools. 7 hours is not bad, but you might increase tool life by speeding things up a bit. You have plenty of machine there, why don't you try running at the recommended cutting parameters. Your MRR will increase dramatically.

i can try running at helical specs just a little hesitant. I am mostly a 6061 guy. Steel is new to me. My other thought was to go full bore 15k rpm like a 200+ feedrate but a super small radial like 2%. I know in stainless you have to take a decent cut or the tool with rub but not sure about 4130.

4130 will work harden also. It takes adjusting your mindset to start making some major chips.

Maybe this will help :D Titans of CNC has a lot of videos about how to increase production.

https://www.youtube.com/watch?v=WcOkOWO2wb0

Quote:

---

Originally Posted by danrandall

i can try running at helical specs just a little hesitant. I am mostly a 6061 guy. Steel is new to me. My other thought was to go full bore 15k rpm like a 200+ feedrate but a super small radial like 2%. I know in stainless you have to take a decent cut or the tool with rub but not sure about 4130.

---

7 Hours is more than what the manufacture would give you, if you run it at full blast, you may get 30 minutes, the sparks will be flying at those speeds, you need to change out the cutter before it breaks so it can be resharpened so just change it out every 5 or 6 hours you can increase the speed and feed a little and see how it cuts, but it won't last any longer cutting 4130

Quote:

---

Originally Posted by Jim Dawson

4130 will work harden also. It takes adjusting your mindset to start making some major chips.

Maybe this will help :D Titans of CNC has a lot of videos about how to increase production.

https://www.youtube.com/watch?v=WcOkOWO2wb0

---

Watch in the video when it is doing the slot in the Y axes and see the whole tool holder flex starting at 0.33, the high-speed examples is normal that most good shops do if they have VoluMill software
They also don't show many of the failures they have and the scrap that they produce

Don't believe what you see they go through tooling like it is free, well most of the tooling and cutting fluid these guys use is free to them, so they can afford to run at crazy speeds, time for a reality check when you post stuff like this without knowing the background of this company, it's all about advertising for the different tooling companies

Quote:

---

Originally Posted by mactec54

Watch in the video when it is doing the slot in the Y axes and see the whole tool holder flex starting at 0.33, the high-speed examples is normal that most good shops do if they have VoluMill software
They also don't show many of the failures they have and the scrap that they produce

Don't believe what you see they go through tooling like it is free, well most of the tooling and cutting fluid these guys use is free to them, so they can afford to run at crazy speeds, time for a reality check when you post stuff like this without knowing the background of this company, it's all about advertising for the different tooling companies

---

Of course it's advertizing, and their tooling and possibly the machines are free to them.. But I was making a point. You can push a little harder and find the sweet spot for your application. The OP has a substantial machine. Program for the manufacturer recommended speeds & feeds, then back down the feed and speed to about 70%, then bring it up until you and your machine are happy. But keep the chip load up so the chips carry away the heat.

On the other hand, you are correct, 7 hours is really too long for any endmill in steel. I don't know what the number should be, but you need to look at cut quality and listen to the machine to tell you when you need to do a tool change.

Quote:

---

Originally Posted by Jim Dawson

Of course it's advertizing, and their tooling and possibly the machines are free to them.. But I was making a point. You can push a little harder and find the sweet spot for your application. The OP has a substantial machine. Program for the manufacturer recommended speeds & feeds, then back down the feed and speed to about 70%, then bring it up until you and your machine are happy. But keep the chip load up so the chips carry away the heat.

On the other hand, you are correct, 7 hours is really too long for any endmill in steel. I don't know what the number should be, but you need to look at cut quality and listen to the machine to tell you when you need to do a tool change.

---

He is already running at around 70% of manufacturers specs, he can increase both speeds and feeds, by doing this his tool life will be less, trying to run like the video he would get about an hour of cutting time with the same cutter, if that, you can try it yourself if you have a machine that can go that fast, the machine in the video uses a HSK-A63 tool holder and 60Hp spindle you can't compare a 40 taper 30hp spindle machine and expect to come close to a machine like this.

Well I ran the tool at the manufacturers specs of 1009 sfm .0015 chip load at 9% radial engagement. Tool lasted around 20 mins. The routine was 2 mins long instead of 9 mins but c'mon. So back to my original numbers of 500 sfm .0016 chip load at 6-8% radial that got me roughly 6-7 hours. I might try a shorter stickout with a shorter beefier hydraulic sleeved holder which means I'll be adding another tool to my program but if it last longer it's worth it.

7 hours of machine time for one tool is pretty good

can you not throw an insert mill into the mix ? It's difficult to determine where improvements can be made without seeing the parts and the process , especially tool paths . Typically manufacturer specs are fairly optimal , at least with any quality cutters . If manufacturer specs fail miserably then it's worth looking at where the process might be failing
First thing I'd do is ditch the holder and put the cutter into a side lock . 0016 sounds like an awful light load and it should be running at at least .003 , it's a rougher and if it can't do that then toss it .
It might be worth trying a few other brands to see if there is a difference that can be found . Gorilla mill for example has the sasquach which is a rougher / finisher and I've seen them outshine all the top brands under extreme conditions . Also their support is excellent and a quick phone call can get you some pretty good numbers to start with , otherwise their online calculator is pretty good to .

Then there is coolant no coolant , which is always debatable . I personally lean towards using heavy concentrates , but some circumstances indicate that running dry is better

Hi Dan!

You definitely have it setup right running a 5 Flute Chipbreaker Rougher in a Hydraulic Chuck, that is awesome! I have also found Helical's Speeds/Feeds to be really aggressive in the HEM Toolpaths. Your parameters look good to me and 7 hours of run time is really good! Here is where I would be at to give you a comparison:

https://www.toolhit.com/pages/optimi...loy-steel-long
Axial DOC: 2"
Radial DOC: .035"
SFM: 500
RPM: 3,820
CLPT: .002"
IPM: 38.1

We did put together a quick HEM Speed/Feed Calculator that gives conservative starting speeds/feeds for using VoluMill, DynanicMill, iMachining or Adaptive Clearing or any HEM Toolpath. We found that most calculators are aggressive and wear out tools quick so we created this. All you have to do is select Material and Diameter x LOC and it will give you speeds/feeds that have tested well for us:
https://www.toolhit.com/pages/volumi...g-speeds-feeds

Hopefully this helps!

Mike

You're probably getting all of the tool life you can under the your current operating parameters, though increasing cutting speed a few percent might help a little bit. You specified the spindle load at which a tool breaks, but you didn't specify the spindle load with a new tool, and you didn't specify the spindle load when the tool is rotating but not in the cut. If you change your way of thinking about what the spindle load meter is telling you, you should be able to learn when to change tools before they break. It takes a certain amount of power just to turn the spindle when it is not cutting, but the load on a dulling tool increases at a much higher percentage rate than does the load on the machine spindle, particularly on machines with as much spindle powers as yours. Let's say that your machine shows a 17% load when cutting air with a fresh tool and 26% with the cutter engaged in the workpiece, If the load meter later reads 31%, the load on the machine has increased only 5%, but the load on the tool has increased by (31-26)/26 or 19.2%. You'll of course have to use your own real numbers, but if my example was correct for you, it would be a good idea to replace your cutting tool at say 30% spindle load or a tool load increase of 15.4%.

Quote:

---

see the whole tool holder flex starting at 0.33

---

oau macted, your right; i just watched it, and i think they where close to a failure; definetly not ok to use the machine like that

Quote:

---

t's all about advertising for the different tooling companies

---

yup ... kenametal is one of their favourites :)

i think is a bit tricky to find those specs that make the toolhoder flex, but the tool not to break

Quote:

---

Tool lasted around 20 mins. The routine was 2 mins long instead of 9 mins but c'mon. So back to my original numbers

---

if this trial lead to early fail, don't return to your initial specs; is obvious that those are too light :)

have patience, take record of your trials, and balance productivity versus costs

Quote:

---

You specified the spindle load at which a tool breaks, but you didn't specify the spindle load with a new tool, and you didn't specify the spindle load when the tool is rotating but not in the cut.

---

that's a good point : monitor the actual load because of cuting; a load warning would help, so to avoid having to constantly check the displayed load meter / kindly :)

Quote:

---

i think is a bit tricky to find those specs that make the toolhoder flex, but the tool not to break

---

haha ... i have been thinking on this : is needed a hss tool, with section bigger than pulstud, or even a biger carbide endmill

thus, you need to know that you can rely on tool, to break last