What's new
What's new

Sanity Check: Breaking Tools on a Simple Milling Op

Johnny SolidWorks

Hot Rolled
Joined
Apr 2, 2013
Location
Rochester
Looking for a sanity check, because I've broken a couple of endmills, and I'm apparently too stupid to understand why on my own.

Full disclosure: I'm just starting to use more carbide tooling in the mill (Haas VMC) but have never had issues like this with HSS/Cobalt tooling.

I'm using the endmill in the picture below: 1/2" bullnose, 3 flute, carbide, 1 5/8" flute length.

Material is 1" x 2.5" x 8" 1018 CRS bar stock clamped in soft-jaws for clearance to put a scallop (1 5/16" radius half hole) in at the centerpoint of one side. I keep an eye on it to clear chips, otherwise they like to build up in the pocket (i.e. I don't just walk away.)

Dataflute's recommendations are shown here:

Untitled.jpg

I used the same speeds/feeds to square off both ends of the stock, and while it is alarmingly fast to a guy used to running HSS tooling gently, the chips looked good, no nasty harmonics or noises, and the cutter seemed perfectly happy.

I'm doing everything full depth, bottom of the cutter .05" below the bottom of the stock. 2D adaptive clearing operation via HSMWorks. 325 SFM, .0035 IPT, .25 X Diameter Optimal Load (Diameter times .25, not .25") [Edit]

Rapids to scallop, cutter starts to engage and bang - handful of scrap for the (rapidly accumulating) carbide bucket.

Go back to Dataflute, take speed adjustment to minimum: recommends 200 SFM, but chip load and radial depth of cut recommendations stay the same. Ok, lets give her a shot.

Well, now I'm 2 carbide endmills down.

Should I just dial this all the way back to HSS speeds and feeds and work my way up? I feel like I should be able to push way, way harder than that without issue. What stupid, idiotic, obvious mistake am I making? Do I have too much cutter engagement for their recommendations? Is there a rule of thumb for when you have 2xD cutter engagement for reduction to speeds/feeds? I really don't think it's my setup, but disabuse me of that notion if I'm wrong. I just don't know how I could make that much more rigid.

Thanks All
 
Last edited:
Looking for a sanity check, because I've broken a couple of endmills, and I'm apparently too stupid to understand why on my own.

Full disclosure: I'm just starting to use more carbide tooling in the mill (Haas VMC) but have never had issues like this with HSS/Cobalt tooling.

I'm using the endmill in the picture below: 1/2" bullnose, 3 flute, carbide, 1 5/8" flute length.

Material is 1" x 2.5" x 8" 1018 CRS bar stock clamped in soft-jaws for clearance to put a scallop (1 5/16" radius half hole) in at the centerpoint of one side. I keep an eye on it to clear chips, otherwise they like to build up in the pocket (i.e. I don't just walk away.)

Dataflute's recommendations are shown here:

View attachment 208194

I used the same speeds/feeds to square off both ends of the stock, and while it is alarmingly fast to a guy used to running HSS tooling gently, the chips looked good, no nasty harmonics or noises, and the cutter seemed perfectly happy.

I'm doing everything full depth, bottom of the cutter .05" below the bottom of the stock. 2D adaptive clearing operation via HSMWorks. 325 SFM, .0035 IPT, .25*Diameter Optimal Load

Rapids to scallop, cutter starts to engage and bang - handful of scrap for the (rapidly accumulating) carbide bucket.

Go back to Dataflute, take speed adjustment to minimum: recommends 200 SFM, but chip load and radial depth of cut recommendations stay the same. Ok, lets give her a shot.

Well, now I'm 2 carbide endmills down.

Should I just dial this all the way back to HSS speeds and feeds and work my way up? I feel like I should be able to push way, way harder than that without issue. What stupid, idiotic, obvious mistake am I making? Do I have too much cutter engagement for their recommendations? Is there a rule of thumb for when you have 2xD cutter engagement for reduction to speeds/feeds? I really don't think it's my setup, but disabuse me of that notion if I'm wrong. I just don't know how I could make that much more rigid.

Thanks All
.
usually you lower depth and width of cut if cutter chatters so much corners are breaking off
.
i lower sfpm next if chatter too much
.
usually i lower ipt feed rate last and usually i keep ipt in a certain range. above max ipt corners break off. what is max ? if corners still break off at low width and depth of cut at low sfpm then ipt is too high
1/2 dia end mill roughly .003 ipt is max with 1018 steel
.
i have excel chart with standard setup tools, tool holder length and stickout are tight specs. performance specs then are recorded with sudden failures noted. so i look at chart see 10 different feeds and speeds and see the sudden tool failures noted at the max settings.
.
really a simple chart recording what works good and not so good is often the best
.
some tools can take much higher ipt feed. big inserts on soft cast iron can take .013 ipt feed on ductile iron maybe .010 max and on 1018 steel .008 max. in general harder material ipt lower before corners break off. all tools even end mills have similar properties at too much, corners break off
 
Your optimal load in HSM is the basically the stepover amount between passes. With the info you provided, you are going full depth (1.0") and trying to take a .250" wide pass, with 1.625" flute length?? NO

First try and get a 1.25" flute length, then change your optimal load to about .05" at full depth. Also, 325sfm sounds low to me for 1018. I would probably be around 500sfm, if you have the rpm and a rigid setup.

Coolant? Air blast? Nothing? Is everything tight - stock in vise, vise to table, endmill in (hopefully sidelock) holder..?
 
.
usually you lower depth and width of cut if cutter chatters so much corners are breaking off
.
i lower sfpm next if chatter too much
.
usually i lower ipt feed rate last and usually i keep ipt in a certain range. above max ipt corners break off. what is max ? if corners still break off at low width and depth of cut at low sfpm then ipt is too high
1/2 dia end mill roughly .003 ipt is max with 1018 steel

It wasn't that I was getting chatter, or chipped corners - I completely grenaded both of these cutters. Broke them off in the holder, and into several pieces besides.
 
usually better to program conservatively and after making a good part the next part you try going faster often only 10 or 20% faster at a time
.
for example 4" facemill might start out at 30 ipm feed and end up at 60 ipm feed. but i often see problems at 30 ipm feed and need to reduce rpm and feed. better to start safer and work your way up. with facemill if i take 0.500 depth of cut it will choke. not meant for over 0.200 and .150 better depth. each tool has a max depth and width of cut max
.
if programmer programs at max setting you better warn the operator first. he dont want to be in the way of flying broken tools
 

Attachments

  • BrokenTool.jpg
    BrokenTool.jpg
    33.8 KB · Views: 152
Your optimal load in HSM is the basically the stepover amount between passes. With the info you provided, you are going full depth (1.0") and trying to take a .250" wide pass, with 1.625" flute length?? NO

First try and get a 1.25" flute length, then change your optimal load to about .05" at full depth. Also, 325sfm sounds low to me for 1018. I would probably be around 500sfm, if you have the rpm and a rigid setup.

Coolant? Air blast? Nothing? Is everything tight - stock in vise, vise to table, endmill in (hopefully sidelock) holder..?

Correct me if I'm wrong: 25% stepover (Optimal Load) on a 1/2" cutter is going to be 1/8", right? I guess it still seems like a lot, but not as aggressive as 1/4" stepover, that's for sure.

Ok, so I just need to run the stepover way below their recommendations (of 25%-40%) - I'm fine with that, and it makes sense. I was just trying to 'push' these, because (in my mind) that's kind of the point of carbide. Apparently I'm just an idiot who expected magic.

Is 10% stepover (your .050") a decent rule of thumb to start on long engagement like this? That's actually about what I run my HSS stuff at for this operation, without too much trouble.

Flood coolant, Parlec sidelock 1/2" endmill holder, standard length, checked for runout with a tool in it, found to be minimal. Vise, jaws, everything's tight. Sounds like I was just going for way, way too much stepover.

I'll try .05" stepover and see what I get. If everything looks good, I'll start dialing up the SFM. I don't think the speed was the issue - so I'm sure I have a ways to go to crank that up.

Thanks!
 
I'm doing everything full depth, bottom of the cutter .05" below the bottom of the stock. 2D adaptive clearing operation via HSMWorks. 325 SFM, .0035 IPT, .25*Diameter Optimal Load, now I'm 2 carbide endmills down.

1. Decrease from 25% to 8-10% engagement
2. Increase SFM to 500
3. Either increase explicitly the IPT to .007" or .008", or select the radial chip-thinning option in your CAM

This will work IF you have a rigid setup, and your CAM makes a nice HSM toolpath, and your control can keep up. If your control can't keep up, if the control pauses in the cut trying to catch up, at 500 SFM running dry, the carbide will burn up. Not sure what your Haas is capable of in this regard.

Regards.

Mike
 
Ok, so I just need to run the stepover way below their recommendations (of 25%-40%) - I'm fine with that, and it makes sense. I was just trying to 'push' these, because (in my mind) that's kind of the point of carbide.

Flood coolant, Parlec sidelock 1/2" endmill holder, standard length, checked for runout with a tool in it, found to be minimal.

Yes, for HSM to work, you need a low stepover/engagement
NO COOLANT! In an HSM scenario, the cutter edge and the chips will momentarily get very hot. If you try to flood, you will thermally shock the carbide and it will chip.

Regards.

Mike
 
I'm with these guys, Radial engagement is too high.

.25*.5= .125 At full axial engagement, that's the red flag I'm seeing.

Try a 10% radial engagement.
 
1. Decrease from 25% to 8-10% engagement
2. Increase SFM to 500
3. Either increase explicitly the IPT to .007" or .008", or select the radial chip-thinning option in your CAM

This will work IF you have a rigid setup, and your CAM makes a nice HSM toolpath, and your control can keep up. If your control can't keep up, if the control pauses in the cut trying to catch up, at 500 SFM running dry, the carbide will burn up. Not sure what your Haas is capable of in this regard.

Regards.

Mike

got to watch the large ipt feed rate. many tools will flat out chatter when pushed too hard . when side milling you obviously pushing on the side of cutter. many long tools AND long tool holders positively chatter easy that way. when you hear it 100 feet away you got a problem.
.....chip thinning theory dont mean much if cutter chattering loud hear it 100 feet away. old timer method chip thinning. as it milling slowly increase feed til its loud and back off a bit. you might be surprised at what the loudness test says
.
you then figure out what the ipt max feed the cutter can take (by loudness).....ultimately i figure max setting by the sudden tool failure rate. i often have backed off settings as changing tools every 20 minutes is annoying. ought to last longer and it will with the correct settings
.
tool holder length and machine and part rigidity effect max sfpm. often slow cause chatter too high. chatter can easily be different with different length stickout. length tool holder, different part shape, different machine
 
1. Decrease from 25% to 8-10% engagement
2. Increase SFM to 500
3. Either increase explicitly the IPT to .007" or .008", or select the radial chip-thinning option in your CAM

This will work IF you have a rigid setup, and your CAM makes a nice HSM toolpath, and your control can keep up. If your control can't keep up, if the control pauses in the cut trying to catch up, at 500 SFM running dry, the carbide will burn up. Not sure what your Haas is capable of in this regard.

Regards.

Mike

I'm good with #1 & #2, but man, .008 IPT seems scary...then again, I thought I'd get away with .125" radial depth of cut.

It's an 01, so my guess is the controller won't keep up with that - might be worth a shot sometime when I feel like making some more scrap carbide though.
 
I'm good with #1 & #2, but man, .008 IPT seems scary...then again, I thought I'd get away with .125" radial depth of cut.

It's an 01, so my guess is the controller won't keep up with that - might be worth a shot sometime when I feel like making some more scrap carbide though.

.
got to watch "recommended" setting by tool salesman. they just want to sell you tools
.
often can tell alot just by the loudness of noise
 

Attachments

  • BrokenTool.jpg
    BrokenTool.jpg
    33.8 KB · Views: 45
Yep, gotta be careful cause a Ø1/2" endmill will totally do that.

.
as a operator i often see bad settings. too slow or light cutting at least stuff not breaking or flying through the air.
.
sure i increase settings slowly. i often record 5% of parts have problems. you dont always get 100% failure rate, just a slight increase in sudden tool failure rate. i have often seen trying to save a few minutes caused hours of rework and expensive tool failures.
.
i record or log jobs after a 100 or more part runs or after a year i use data to tell me is going faster actually faster or is going slower ultimately faster and cheaper. cause i log remaking parts or reworking part times in total time to make parts. i average the times
.
i have often seen backing off max setting was faster and cheaper by the end of the year. boss giving me 7 pay raises in 5 years agrees too.
 
maytag

maytag repairman settings.
.
you want program to just run and not have any drama of sudden tool failures. something to be said for programs that just work dependable without problems. even 2% sudden tool failure rates can be big problems.
.
not every bad setting gives 100% sudden tool failure rates. operator who are smarter look at programmers name. some programmers create trouble filled programs. once saw job feed increase saving 1 minute was actually creating 1 hour of lost time remaking part. obviously that was not saving any time
 
Try using the Helical Milling Advisor. You have to input one of their tools, but you can pick their item # that most closely matches what you're using. It will recommend depth, step, speed, and feed. I've been using it's numbers in 17-4 H900 and Ti6Al4V on a VF-3SS with good results.
 








 
Back
Top