Glacern Indexable Endmills
Ok,
I finally broke down and decided I was going to buy a top quality indexable endmill. I had been using HSS and carbide but I wanted to get an indexable endmill and be able to start pushing the speeds and feeds. So I bought a .750 indexable endmill from Glacern and the aluminum inserts
That being said I am having some problems with this endmill. It does not cut well and chatters enormously. Gwizard says I can run this endmill at 5500 rpm 77 ipm with a .25" doc and a .5" cutting width in 6061 aluminum. So I plugged this data in the milling machine and it went about 3" and snapped an insert. So I emailed glacern and told them what speeds and feeds I was running and asked them what they suggested. They said that those speeds and feeds were well in the range for that endmill and that I must be having a chip evacuation problem and to cut the rpm down to 2250, 38 ipm and a .1" doc. So I go back and try this data. The endmill chattered so bad that the screws holding the inserts on were coming loose and cut quality was terrible. The only way I can get this endmill to seem to cut smoothly is with a rpm of 2500, 35 ipm and a .01 doc. I run 2 flute HSS endmills at 2800 rpm 40 ipm and .25" doc without an problems but I cannot get this endmill to cut with any quality. Maybe my expectations were too high for this endmill but I still think it should exceed a HSS endmill.
I tried increasing feed and decreasing rpms and vice versa with no effect. I'm not sure what else to do. I emailed glacern for a 2nd time but they have not responded. Any suggestions?
Similar Threads:
Are you using an endmill holder or collet to hold the tool? Is the tool length too long? Are you using flood coolant? Any evidence of aluminum loading on the inserts? Are you sure you have the proper inserts/seats/screws for the holder? Is the workpiece held securely?
Just my initial thoughts...
Diplomacy is the art of saying "Nice doggie" until you can find a rock. - Will Rogers
No, I'm not using flood coolant only air blast with a squirt of wd-40. I'm using a collet holder. I have a cat40 spindle, the piece is held securely in a vise. The inserts I bought from Glacern when I purchased the endmill. The endmill sticks out of the holder 3" which I plugged into g-wizard to get the 5500rpm and 77 ipm to which Glacern said the endmill is well capable of those speeds and feeds. Again, I can take a cheap HSS 2 flute endmill and out perform this inserted endmill. So, it has to be something I'm doing wrong otherwise people wouldn't buy these types of endmills if the cheap stuff out performs them.
Can you take a video with your phone and post it? Or take a picture of the end mill with a close up of how the insert is mounted?
Hi dlenardu, sorry you're having a bad time with this indexable endmill.
I agree that this endmill ought to be able to do better for you.
What's troubling is the chatter issue. Chatter will break down tooling fast, especially those sharp aluminum inserts. They're fairly delicate, all things considered.
G-Wizard shows this to be a 2 HP cut. Your CAT40 should be able to handle that fine, but its not a trivial cut. Makes me wonder a few things:
- You really need to take care with an ER collet chuck to get it take the 2 HP. A lot more torque than you'd think to tighten it. Clean the tool shank thoroughly. Yada, yada. Here are two good links to get the best performance from your collet chucks:
Getting the Best Performance from ER Collet Chucks « CNCCookbook
Toolholding in Collets: How to Avoid Tool Pullout « CNCCookbook
- Are you able to run 2 HP without chatter using some other cutter?
- Did you try setting the G-Wizard gas pedal all the way down to max conservative? That'd be about 38 IPM at same rpm.
- Can you try remounting this endmill in another holder? Maybe something is way off with that particular collet chuck. If you have one, I'd try a Weldon holder just to be sure the collet isn't slipping.
- Can you beef up the workpiece/workholding rigidity?
- Can you see the chatter marks in the workpiece well enough to measure how far apart they are? If you can, you can use G-Wizard's Chatter Pitch calculator to try to figure a spindle speed that minimizes the chatter.
- What are the chances you have a drawbar issue (weak belleville's)? That can make it easy to get chatter on older machines.
I hope those ideas help. It's got to be possible to get that endmill working better for you. Don't give up on it!
Cheers,
BW
Try G-Wizard Machinist's Calculator for free:
http://www.cnccookbook.com/CCGWizard.html
you biggest problem is not having flood coolant, you cant spray wd on the insert fast enough.Originally Posted by dlenardu
Get a mister or make one at the very least. other wise rig something up for flood
If I remember correctly the partner 1 machine ( I read you used that machine in the past)you are using is not a real rigid machine( small frame base) there great machines and plenty strong however when turning a big endmill that is tipped with carbide thats going to bounce a tad. then combine that with alum build up on inserts due to NO coolant your going to be chattering alot.
also for that machine you width of cut shouldnt exceed more than half of the cutter dia.
The reason you can take a highspeed or tool steel endmill at that speed is due to the endmill loads up and BENDS so to speak) keeping a load on the machine at all times. Carbide will NOT it bounces causing chatter.
this chatter your getting is also a good indication to check your gibs and backlash. cause if there worn and your table is loose it will cause the same problems.
First I would start with less than hald width of cuts at .1 doc. if you make it through that go .2 doc.
On older machines(loose) sometimes new fancy tooling wont work near as good as a hghspeed endmill.
I had acrolocs that did the very same thing, once I put in highspeed I never had a problem, you have to end up working with the machine to figure out what best suits your machine. something ust cause mre problems than there worth.
Bob,
Thanks so much for the info, again you always contribute so much. I torqued the collet down tighter than ever and still had the problems. Also tried using the same rpm and backing the feed down to 38 ipm, still chattered. Next I put the endmill in a weldon shank endmill holder and repeated the procedures and the results were worse than the collet. The best I can measure the chatter marks is about .o42" wide.
Delw,
Yes I have a partner 1 but I still think the machine is pretty rigid. I have seen the IH mills run .25" doc .5" wide cut at 100 ipm and I know that the milltronics machine is more rigid than the IH, given that it weighs about 4500lbs, but I maybe wrong in my thinking. Also my machine has linear rails so no gibs to adjust. I did check the backlash in all directions. In the X axis i commanded a .002" move, the machine moved .002, then programmed back to zero and the machine went to a little less than .0001 the y-axis was spot on, except when I commanded a .002" move it went .0021 but then it went back to 0.
I had a three flute carbide endmill that I use to run at 3600 rpm and 50ipm and it would cut like butter, just smooth.
I'm attaching a video and pics for you to look at
5500 rpm 77 ipm .5"width, .25" doc
5500rpm77ipm.mp4 video by dlenardu - Photobucket
Pic of chatter marks at 77ipm
http://i585.photobucket.com/albums/s...rpm77ipm-1.jpg
Video of 5500rpm 38 ipm
5500rpm38ipm.mp4 video by dlenardu - Photobucket
Pic of chatter marks at 38ipm
http://i585.photobucket.com/albums/s...rpm38ipm-1.jpg
Weldon shank marks at 38ipm
http://i585.photobucket.com/albums/s...shank38ipm.jpg
Nasty looking!
If I plug your numbers into the chatter calculator in G-Wizard, it suggests 2 speed possibilities for the collet chuck based on SFM of 1080, 2 flutes, and 0.046" separation between the chatter marks:
4694 rpm and 2347 rpm.
The chatter calculator is on the Quick References tab.
Note that the chatter profile will change if the stickout of the tool is changed (i.e. if you remount it back in the collet chuck). I would therefore go ahead and remount it, make another pass, remeasure the chatter, and do a new calculation.
I would also try seriously choking up on the endmill. Take it down to 1" of stickout and see how it does. Changing the stickout is another way to "tune" the chatter, which is a resonance phenomena. Choking up will also make it more rigid.
I will also say that for the run where you measured the chatter, the chatter low points are predicted for 7041 and 4694 (there's a whole list, actually). The midpoint between those two is 5867. The chatter peak is likely near there and you were running 5500 rpm, so that's a bad spot. Hate when that coincides with the spindle max rpm.
I agree that it would seem like you ought to be able to do better on this machine. I got a bud with a partner. His is nearly new and he runs the heck out of it without problems. If we can't get it tuned up better changing rpms, I'd try a different brand of inserts. My buddy has had a real hard time with the Glacern inserts on his.
It's a hassle dialing in, but once you get it figured you'll be able to go from there.
Best,
BW
PS The partner may not be the most rigid VMC in the land, but you are sure right it is a LOT more rigid than an IH mill, LOL!
Try G-Wizard Machinist's Calculator for free:
http://www.cnccookbook.com/CCGWizard.html
Bob,
Thanks again. I will try the changes. The machine actually has a max rpm of 6000 but I set it at 5500 so that I wouldn't always run it at the max. The endmill that I got from glacern has a cutting depth of 3" so I can't choke up on it any more, which I needed the depth because I needed to machine a pocket that was 2.5" deep. Yeah I was kinda wondering about some different insert, these are suppose to be the ones for aluminum but I'm sure there is something better out there to try. I also just ordered a mist coolant system so maybe that will help although it doesn't seem to be chip buildup because after the pass the inserts do not have aluminum on them. I do think I am going to look for some other inserts also, I'm trying to learn the differences between inserts. do you have a link that explains them better? I know this says it take an APMT 1135, but they sent a APGT 1135, I have found APKT, APMT 1035, so I assume that those will fit but don't understand the difference.
Your endmill looks to be smaller than you carbide inserted endmill ( not a good comparison) use the same size solid carbide and see what happens.
your not using coolant its very obvious that your endmill is loading up with chips, in all the pics.
Linier guides are much weaker than boxed ways and will chatter alot more than a box way machine. I could put a sloppy 1986 acroloc box way machine up against a brand new hass VF2 ss and out cut it on heavy cuts with big endmills. just because it has liner guides.
Higher rpms also causes the alum to load your cutter up and cause bad finish and chatter.
until you get the coolant issue solved your wasting your time and money. if you cant get coolant on that machine cut slower and live with it by brushing oil or wd 40 on it.
I am not trying to be a dick, but it boils down to using a mill the correct way with the correct tooling and coolant for that type of material you are using. air blast dont work very well on alum. the only way you would have a slight chance of cutting liek you are with good finish is to buy a coated 3 flute endmill and use light oil, that will work for a while but not a long time.
one of my cnc mills I dont have coolant hooked up as I use it for tooling, steel ss, and plastic parts.( kinda use it as a hand mill) I cut lots of alum in it. however I dont push it when cutting alum and I brush oil on it or use a spray bottle with coolant, wd-40 cans are so so but wont last that long. I dont have any problems and I use both inserted face mills and COATED 3 flute endmills. the alum will build up on it if I dont use enough coolant.
I have a Glacern 1" EM and I noticed you have to be very careful putting the inserts on it. They fit tightly against the shoulder and can be crooked or not seated all the way if your not careful, just something to check.
I have not tried the alum inserts yet, but I have run the standard inserts. The 1" EM REALLY vibrates my mill (Series II Bridgeport Manual) cutting mild steel. The same machine cuts the same material like butter when using a 6 flute 1.25" HSS rougher. Im thinking 2 flute cutters like the Glacern need 8-10K rpms to peform well.
I would think you could get MUCH better productivity from a 5 or 6 flute HSS/Carbide EM in your machine.
Delw
The endmill that I was comparing was a 3/4 3 flute carbide endmill using the same .25"doc and .5" width. I did not have Gwizard when I did the speeds and feeds with this endmill, so I did a standard chipload calculation and was a bit conservative but the endmill cut like butter, no coolant just air. This indexable endmill I cannot get to perform even at a slower feedrate than that carbide endmill. Even when Glacern told me to back the depth down to .1" doc 2250 rpm and 38 ipm the endmill still chattered. I am not denying that a Box way machine is much more rigid than linear rails, no doubt. However, I still feel this machine is rigid enough for this endmill to perform. I run a 3/4" 6 flute through steel with no problems either. I understand what you are saying and I went and checked the backlash on the machine and it checked out great. I do agree that I need to find the sweet spot for this endmill but it has been very discouraging. According to Glacern "The high positive axial rake reduces cutter flex and vibration while conserving spindle horsepower." So I feel there is no reason I should not be able to make this endmill work and be at least as effective as a regular carbide endmill, but then again maybe it won't work well in aluminum due to lack of chip evacuation.
Inventit,
A 6 flute endmill will not really work for me, I'm cutting aluminum and there is not enough room for chip evacuation with 6 flutes.
The APGT should be a polished/ground insert for aluminum, should have very sharp edges. The APMT should be a pressed insert, normally coated and will have an edge which is not extremely sharp.I know this says it take an APMT 1135, but they sent a APGT 1135, I have found APKT, APMT 1035, so I assume that those will fit but don't understand the difference.
The size is an 11. You cannot use 10 size inserts in a 11 sized pocket.
I cannot tell but make sure you do not cut on the exact half diameter of the endmill as it will slap the inserts. This will be pronounced if it is a two flute cutter.
i might not be much help, since i use mitsubishi indexable endmills, but I tend to always opt for the ones with slots so i can use a set screw to lock it down. the heavier i go with a collet setup, the more vibration i get. another trick i have learned is when you have to deal with vibration, its been better for me to go deeper cut and less axial, so im not riding the corner of the insert so much, more of the whole side.
with that being said, in aluminum, i like to use my half inch atrax carbide coated 4 flute endmill (.5x.5x1.25"loc) whenever possible, because I can push it as hard as i want and still get a decent finish. with the indexable, i still feel the need to hit it with a fluted endmill to get the finish, so why waste time. I run that atrax full doc most of the time, whether in aluminum or doing peel milling in stainless 304 for clevis slots, etc. shoot, 5500 rpm, 35ipm, doc @ 1.25", .03" stepover with .03" radius into cut for peel milling a stainless clevis, 2 inch slot done in a minute or 2, compared to slow straight passes.
so in other words, keep playing, find something that works good and takes abuse, and try new tricks! I love finding new ways to skin the same old cat!
3/4" endmill
Hi dlenardu, I cut a lot of aluminum (6061, 6105, 7075) and I have a couple of replacebale insert end-mills that I don't use. I found that for roughing applications a minicut endmill works best. I use 3/4" (p/n tc930-2416) on most applications. My cutting data is 6000RPM F106.875 0.5DOC my Radial DOC varies but stays within 75%. I get my best MRR with my 3/4" minicut, I start runing out of power with my 1" minicut (I run it at 5500RPM and feeds aroun 100IPM). I found that runing these endmills in production to be better than the replacible isert endmills. The downfall is the initial investment is a little higher because you need keep a couple to rotate between sharpening and production. I found that if I need to take out a lot of aluminum that a small face mill works best, I have a 50mm unit with inserts that have a wiper that I run at 2911RPM 70IPM (rough) and a 0.2 "DOC 70% radial depth of cut.
However if you do try the minicut endmills asuming you do a lot of aluminum a couple of things:
- use a weldon holder, on my machine for whatever reason they do not work on er collets.
- Go for the coated or the polished flute for pocketing ship evacuation is key (they are 3 flute mills)
- Do not go easy on them run them at values close to the mfg recomendations else they do not work well.
- They have an interupted flute, thus they work great in interupted cuts.
- You can purchase direct form TD-International.
- They say "center cuting" however does not work very well ramp or helical into cut, they birdnest like crazy if not, and the corners chip if you feed down into cut.
- They flex like crazy, I kid you not .006" worth or deflection on a 1/2" endmill. So if you are planing a finish cut take measurement before your tool change so you are aware of the amount of material you are removing.
I wish you the best of luck, but for my shop I use minicut for roughing/semi-finishing, and if their is no spec finishing followed by a trip to the vibratory fininishing machine and anodizing. I use a hand full of finishing endmills, and a lot of face mills.
I had the sandvik rep come by and talk about the coromill (the replacebill carbide head) endmill. He knows I like minicut and not the insert endmills he said this is best of both worlds have not tried yet, but maybe you can give both a try.
Reply with Quote
