What's new
What's new

Newbie Carbide Endmill Questions

niq0316

Plastic
Joined
Dec 7, 2016
I work at a job shop and am running a haas tm-1 with a 4000 max spindle. I believe its a 2005 model. There is only 4 employees total and I really gotta figure things out on my own. I feel like sometimes im pushing my tools too much or not enough etc.

Anyways I got a (probably china) .500 carbide endmill with about an inch of cutting flute. Im using 200 SFM and .002 feed per tooth and came up with 1528 RPM and 12.0 feed. I am side milling A-2 with a height of .750 and only taking .030 at a time. It is in a brand new er32 collet and im chucked right above the flutes so about 1.1 sticking out. For some reason when my parts get above .500 in height (in this case .750) I get crazy chatter and it sounds awful. This endmill should be able to take this cut? Am I doing something wrong? Side milling is a pretty basic operation for squaring up the last two sides. ANY advice at this point is appreciated.Thanks in advance.
 
I work at a job shop and am running a haas tm-1 with a 4000 max spindle. I believe its a 2005 model. There is only 4 employees total and I really gotta figure things out on my own. I feel like sometimes im pushing my tools too much or not enough etc.

Anyways I got a (probably china) .500 carbide endmill with about an inch of cutting flute. Im using 200 SFM and .002 feed per tooth and came up with 1528 RPM and 12.0 feed. I am side milling A-2 with a height of .750 and only taking .030 at a time. It is in a brand new er32 collet and im chucked right above the flutes so about 1.1 sticking out. For some reason when my parts get above .500 in height (in this case .750) I get crazy chatter and it sounds awful. This endmill should be able to take this cut? Am I doing something wrong? Side milling is a pretty basic operation for squaring up the last two sides. ANY advice at this point is appreciated.Thanks in advance.

Your probably feeding too little and just bouncing along the part. Trying going .03 a tooth.
 
Your probably feeding too little and just bouncing along the part. Trying going .03 a tooth.

99.9% sure this is meant to say .003 instead of .03 (.03 would be 183 IPM). :D

Also I would check the Collet and the Holder for dirt, grime, grease and nicks and dings. Make sure your pull stud is tight, check the taper of the Machine and the Holder for same dirt and dings. I think your chip load is about fine for A2 assuming it's Annealed and not Post Treat. Inspect the Tool itself for chipped corners. If it's got sharp corners I would get one with radii.

Plus, sorry but that isn't the most rigid mMachine out there. SFM seems fine, but you can always back off the spindle speed a little and maintain the DOC and WOC. But generally I don't see anything that is WAY off. It just takes time to get everything dialed in, and that is what experience is for.

R

And once y ou get everything loaded in the Machine you can run an indicator on the Endmill to check for runout.
 
99.9% sure this is meant to say .003 instead of .03 (.03 would be 183 IPM). :D

Also I would check the Collet and the Holder for dirt, grime, grease and nicks and dings. Make sure your pull stud is tight, check the taper of the Machine and the Holder for same dirt and dings. I think your chip load is about fine for A2 assuming it's Annealed and not Post Treat. Inspect the Tool itself for chipped corners. If it's got sharp corners I would get one with radii.

Plus, sorry but that isn't the most rigid mMachine out there. SFM seems fine, but you can always back off the spindle speed a little and maintain the DOC and WOC. But generally I don't see anything that is WAY off. It just takes time to get everything dialed in, and that is what experience is for.

R

And once y ou get everything loaded in the Machine you can run an indicator on the Endmill to check for runout.

Both my collet and the holder are new. This endmill is also new. I have a bunch of them and they all do the same thing. I actually got two different .5 endmills but it just has a faster helix. The machine is pretty old and is definitely not the best but its what I have to work with. My boss is a manual kinda guy and has no clue how to even turn it on I bet.

I been getting by using a cutter and incrementing down .050 at a time but it is a slow process. I will try your suggestion of lowerering the rmp. I usually plunge at 1200 with it no problem maybe ill try that. I appreciate the help.
 
This is very "rule of thumb", but for just about any steel that isn't hardened, I run a 1/2" coated carbide endmill at 3000 RPM, so that gives about 400 SFM. Off the top of my head, I'd be feeding somewhere between 15 and 30 IPM (somewhere around 0.0012 and 0.0025 IPT if I have my math right) depending on the tool engagement and how things are sounding and feeling. Feed too slow often causes squealing because you're just rubbing the tool, not keeping it loaded.

I can't speak to the machine rigidity, as I'm not familiar with what was mentioned. Of course, this plays a big role too.

If rigidity is the problem, reduce the amount of tool engagement. At the same time you can probably bump up the feed. Fast, light cuts are often more impressive to others watching than slow heavy ones. One perceives that work is being done quicker, even if the material removal rate is actually less. ;)
 
Maybe even bump down to 3/8” diameter... 1/2” just may be too much for the TM.

I like this idea best, and for the sake of your own sanity and the future of the processing, get a 3/8 from a reputable maker, or talk your boss into popping for 1 very high end Tool for the sake of understanding what the problem is. Eliminate a thing at a time to get where you need to be. Other than the Maker(thanks Bob :dunce:) and Size of the Endmill, I don't really see a problem. Your parameters are pretty conservative if anything, but just fine.

Annealed A2 will not work harden, but that doesn't mean the Tool isn't deflecting because of a low feedrate.

I would try Either increasing the feed or decreasing the RPM first with the Tool you have. Then WHEN that doesn't work, I would get yourself a high quality 3/8" solid carbide, 4 Flute, corner radius Endmill, to see if that's it.

R

Blip> OT but Bob this is another one I can smell cutting, sorry OT from a different thread.
 
If you program for .0025 chip load, at this radial DOC your actual chip thickness will be .0012 because of the radial chip thinning effect. You are rubbing the part, the chip is not thick enough to carry the heat away. The cutter is retaining the heat and will fail prematurely.

You'll need to run at .0052 IPT to maintain an average .0025 chip thickness. That's about 32 IPM.
If you can't feed that hard you can double the radial DOC to thicken the chip.
The heat has to go somewhere.. ideally it should go out in the chip.
 
I work at a job shop and am running a haas tm-1 with a 4000 max spindle. I believe its a 2005 model. There is only 4 employees total and I really gotta figure things out on my own. I feel like sometimes im pushing my tools too much or not enough etc.

Anyways I got a (probably china) .500 carbide endmill with about an inch of cutting flute. Im using 200 SFM and .002 feed per tooth and came up with 1528 RPM and 12.0 feed. I am side milling A-2 with a height of .750 and only taking .030 at a time. It is in a brand new er32 collet and im chucked right above the flutes so about 1.1 sticking out. For some reason when my parts get above .500 in height (in this case .750) I get crazy chatter and it sounds awful. This endmill should be able to take this cut? Am I doing something wrong? Side milling is a pretty basic operation for squaring up the last two sides. ANY advice at this point is appreciated.Thanks in advance.

some machines chatter when you cut above certain amounts. a Bridgeport series 1 mill is famous for having about a 1hp limit. anytime you approach using that much hp it starts to chatter. obviously if you increase rpm feed and try to take more metal off per minute the problem only gets worse
 
This is very "rule of thumb", but for just about any steel that isn't hardened, I run a 1/2" coated carbide endmill at 3000 RPM, so that gives about 400 SFM. Off the top of my head, I'd be feeding somewhere between 15 and 30 IPM (somewhere around 0.0012 and 0.0025 IPT if I have my math right) depending on the tool engagement and how things are sounding and feeling. Feed too slow often causes squealing because you're just rubbing the tool, not keeping it loaded.

I can't speak to the machine rigidity, as I'm not familiar with what was mentioned. Of course, this plays a big role too.

If rigidity is the problem, reduce the amount of tool engagement. At the same time you can probably bump up the feed. Fast, light cuts are often more impressive to others watching than slow heavy ones. One perceives that work is being done quicker, even if the material removal rate is actually less. ;)

Nobody at my shop uses math but me to get feeds/speeds so the 200 SFM is just something that has worked for me for MOST things. My thought was pretty much what your saying because my machine is not exactly rigid/strong I do light fast cuts. My 1 inch facemill I can run at 2400 and a feed of 60-70 no prob. I will try increasing the feed, lowering the spindle and finally doubleing my cut.
 
Saying "1/2" carbide endmill" is a lot like saying "2 door car". Could be a Geo Metro, could be a Koenigsegg. They're going to perform very differently. Add to that that there are carbide endmills made specifically for different types of material, and using a cutter designed for aluminum to cut steel or vice versa will not yield acceptable results.
 
Are you climb milling?

You said held in a ER32 Collet...what the gauge length? Is it a fairly stubby collet holder or a long 2-3" one...makes a big difference.

Have you tried using an endmill holder?

What about going down to a 3/8" tool? More tool in the work gives a smoother cut...


You didn't mention setup? Is the part rigid or dangling in the wind.


You said you tried all your New 1/2" EM's...did you try an decent older one from another manufacturer?


New isn't always better...
Cheap China Crap can sometimes be Cheap China Crap that works well...works ok or just crap.


Last thought...when something is not working.

I try not to repeat doing the same thing over and over hoping for a better result...switch it up a bit, BUT only one thing at a time...decide if it better, worse or the same then move forward.

Small steps down like you said...it works...but slow AND you wear out the end of the endmill leaving a pristine top part. Light duty machine...keep tool, tool holder, work piece all short as possible to maximize rigidity. Sometimes smaller tooling is better..less force needed, less rigidity required...make up for it with faster lighter cuts.
 
I figured it out with all the help! I can take about .050 - .06 at a time now with a spindle of 1500 and a feed of 20 ipm before it started to complain. I think I need to put a scrap piece in and fiddle around till I reach my limit. It's just hard messing around with the boss breathing down my neck all the time. Truth be told if I wanted different tooling id probably have to buy one myself and prove it works. What are some brands that work well? What am I looking for? Thanks again guys!
 
Sounds to me you need a better job. The guy you work for, is the guy most of us are putting out of business.

I have that exact machine. Rigidity is non existent. If your using a coated tool, go ahead and turn it up.
 
I figured it out with all the help! I can take about .050 - .06 at a time now with a spindle of 1500 and a feed of 20 ipm before it started to complain. I think I need to put a scrap piece in and fiddle around till I reach my limit. It's just hard messing around with the boss breathing down my neck all the time. Truth be told if I wanted different tooling id probably have to buy one myself and prove it works. What are some brands that work well? What am I looking for? Thanks again guys!

See that ExKenna guy up there.. That responded earlier.. He can hook you up.. He's got all the good stuff at good
prices. He won't sell you crap unless you specifically request crap. For a quick single endmill, Maritool is good..
His endmills are pretty solid. You are looking for the variflute, corner rads, coated all that fun stuff..

Quality tools don't COST money... They MAKE money..

Your boss sounds like an idiot.. Tripping over dollars to pick up nickels.
 
See that ExKenna guy up there..

I liked his post!

Must be somewhat of a special deal on the side milling threads with smaller toolroom mills this week? This is the second thread with a problem getting nowhere with pretty low settings. In post#17 Motorsports likely has it right “Rigidity is non existent”. The proving for me would be when a lower setting get shitty with a low HP setting, turn it around & take a conventional cut (up milling).

If that works at least you know that if you absolutely have to have a .030”doc by .750” pass you could make it by up milling. Then I'd plan the cuts to load the machine harder with the climb milling or buy a better endmill or machine.

I won’t pee on the variable pitch & helix solutions because they work (also not that new). However, if I’m failing with a little .33HP cut like the OP had originally (with a perfectly good milling machine), I’m thinking hell no… I’d be prone to get out a 3/4” 6 flute (they more money too) and try to run for 4+ HP on a climb (7.5 machine should do it no problem).

The OP is still a little low on the SFPM compared to conventional profiling in the 1960’s. (recommended citations back then attached)They showed 300SFPM & .0025" tooth load for A-2 & like tool steel.

Good luck,
Matt
 

Attachments

  • ProfEmill_SpeedFeed_ToolSteela.jpg
    ProfEmill_SpeedFeed_ToolSteela.jpg
    101.6 KB · Views: 70
  • ProfEmill_SpeedFeed_ToolSteel_Crop.jpg
    ProfEmill_SpeedFeed_ToolSteel_Crop.jpg
    82.4 KB · Views: 64
Last edited:
I liked his post!

Must be somewhat of a special deal on the side milling threads with smaller toolroom mills this week? This is the second thread with a problem getting nowhere with pretty low settings. In post#17 Motorsports likely has it right “Rigidity is non existent”. The proving for me would be when a lower setting get shitty with a low HP setting, turn it around & take a conventional cut (up milling).

If that works at least you know that if you absolutely have to have a .030”doc by .750” pass you could make it by up milling. Then I'd plan the cuts to load the machine harder with the climb milling or buy a better endmill or machine.

I won’t pee on the variable pitch & helix solutions because they work (also not that new). However, if I’m failing with a little .33HP cut like the OP had originally (with a perfectly good milling machine), I’m thinking hell no… I’d be prone to get out a 3/4” 6 flute (they more money too) and try to run for 4+ HP on a climb (7.5 machine should do it no problem).

The OP is still a little low on the SFPM compared to conventional profiling in the 1960’s. (recommended citations back then attached)They showed 300SFPM & .0025" tooth load for A-2 & like tool steel.

Good luck,
Matt

At this point I have way too many questions to ask in one post because it seems I might be running most my tools too conservatively. Where did you happen to get the images from? Do you know of a good resource I could get generalized starting points? Slotting, boring etc? Most my cutters come from ingersoll and I use the numbers from their website pretty reliably but my inserts dont seem to last that long :)
 








 
Back
Top