[TravisR100]

I'm trying to make the profile cut on these parts with a 1/8" endmill. As you can see from the pictures I'm getting some chatter. I've tried both a 2 flute and 3 flute carbide endmill. The endmill sticks out of the ER32 holder only about 3/4" of an inch. The total depth of the profile is .26". The bottom two parts I used a .055" step down level to get to my .26" total depth and left .012" for a finish pass. As you can see the finish pass has a bunch of chatter. I then tried simply leaving no material for a finish pass but still using the .055" step down (the top part in the picture).

I'm running the speed at 10,000 RPM, 13ipm feed rate (.000625 per tooth). It's 6061 aluminum.

Any ideas?

[Delw]

with that depth of cut drop it down to 3-5k rpms and 10ipm then work on it form there. 3 flutes are the best
also make sure your holding in a collet and make sure your tool holders locate properly
I had the same problem with the haas on all endmills at anything over 5k rpms all my holders were JUNK. once i got new holders I can fly through parts like that.
also make 2 finish pass's last one being .005 and one dry pass


Add'd

on alum, when ever you get chatter on small endmills cut the rpms down to half keep the feed about the same run it. if you still get chatter cut them in half again and run it., you can always work up with the overrides once you get it to were your happy with it. then edit your program if need to to reflect the changes.
some things I have noticed with small endmills are that coolant will make a small endmill chatter so run it to the side just dripping off the part, collet chucks work the best on small endmills ( I would have never thought so either untill I tried it). I use TG collets das done work except on brass at low rpms and ER'S are marginal.
one thing I noticed about a new haas is that the taper on the spindle is freaking tight and if you buy less that quality holders you will get lots of chatter, that wil drive you nuts for weeks.

[TravisR100]

Thank you! I backed it down to 5000 RPM, cut it dry, and set the finishing cut to .005. It helped a lot but didn't get rid of it. Finally went with 4000 RPM, .005 finishing, and coolant and that seemed to do the trick.

[crabbass]

Why are you using an 1/8" endmill, and why do you need to have it extended from the collet 3/4"? If the fillet radius in the center of your dog-bone profile is about 1/16" I can understand the use of an 1/8" endmill. However, if you can afford to fit a larger diameter cutter in the fillet you could get serious with your feeds! At least use a 1/4" dia to rough this out. I think I would use a 3/8" 3flute stub length cutter (you only need .26" axial DOC). If your fillet is 1/16" then you could use a 1/8" endmill to finish. (If the parts can be designed with a larger radius this might help). If I can I will program slightly larger than nominal radii in corners so that a nominal cutter can still interpolate. For example in this case with a 1/16" radius (.0625") I would draw it close to the max allowable by tolerance (print says +/- .01") so I would draw a .07" radius. This does a couple things for me, one It allows me to start the program with a .125" endmill with up to a +.015" in the cutter comp( I use diameter compensation). and two, it reduces potential chatter when you interpolate when changing directions in the x-y plane.(because the tool engagement angle is better maintained). I do not use feed rate calculators like some,(and never will) but you can certainly do what you were doing at 10K, change the endmill to a stub length (min .26") and load the flutes appropriately. You could achieve a nice finish at around .001" per tooth, and with a three flute that is about 30ipm. Furthermore, you must like opening and closing the doors on the machine, If it was me I would make a fixture to hold as many as machine x-y travels permit!!!
Nice work though you are doing fine.

[Delw]

+1 on what crab bass says also dont forget to deburr the part too while its in the machine.

[Matt@RFR]

I'm betting that you do not need to slow down. I run 2 flute 1/8" endmills in 6061 at 12,000 RPM and 60 IPM, .090" DOC, slotting. No chatter.

I bet that your only problem is how far you have the cutter sticking out of the collet.

[TravisR100]

Crab, you're right that I should be using a 1/4" endmill. I'm out of 1/4" collets. Was just using what I had available. I'll try getting a shorter 1/8" endmill since I'm sure it will come in handy anyway. I have to have it sticking out at least a 1/2" because even though the depth of cut is only .260 the bottom of the collet has to clear the screw and washer I'm using to hold the part to the fixture.

I am indeed roughing it out with a 3/8" endmill and leaving about .030 for the 1/8" to take care of.

I'll keep that in mind with respect to the radii on any fillets. Makes sense.

On the first and second op I'm just holding each part individually in the vise. Certainly a fixture to hold more parts would be nice but I'm only going to be running about 200 of these in total. I did the 3 part fixture on the 3rd op just because I happened to have a piece of aluminum sitting around that was the right size.

I went back and read some posts on using G52 and that's what I'm using for the 3 part fixture.

[crabbass]

[QUOTE=TravisR100;679823] I have to have it sticking out at least a 1/2" because even though the depth of cut is only .260 the bottom of the collet has to clear the screw and washer I'm using to hold the part to the fixture.

I use button head screws a lot for this exact reason. If I remember right the difference in a 1/4" socket head cap screw and 1/4" button head is about .125".
Another thing to consider is an 1/8" end mill with a 3/8" shank.

The work you are doing looks to be pretty small stuff in aluminum. I am not too familiar with the design/construction of the SMM-2 other than seeing pictures of them. Why did you decide on using ER-32 collet holders in your machine? I think this is a bit large for 1/8" endmills.

[TravisR100]

I've got a couple of ER16 collet chucks as well and have more on order. Again, that's just what I happened to have available at the time. Yep, buttonheads would bethe way to go. IIRC they are half the head height of standard socket head cap screws.

[Matt@RFR]

Also consider a solid endmill holder for work like this as well. No, the runout won't be as good as a collet, but good endmill holders will surprise you. All of mine from Mari Tool have less than .0006" TIR.

Also, you can machine endmill holders to fit odd stuff. I've machined them with a taper that only had about .050" wall thickness at the end to miss other features. You can't run them as hard when you do that, but with an 1/8" endmill, it will likely be a non-issue.

[TravisR100]

Speaking of choosing collet size series, is it best to choose the smallest series that will hold the tool size in question? For instance, an ER11 collet will go up to 1/4". Is it best to use an ER11, ER16, ER20, ER32 for holding that 1/4" endmill?

[behindpropeller]

Speaking of choosing collet size series, is it best to choose the smallest series that will hold the tool size in question? For instance, an ER11 collet will go up to 1/4". Is it best to use an ER11, ER16, ER20, ER32 for holding that 1/4" endmill?

I have this one for my 1/4" EM. Makes it past all of my clamps.....etc. Mostly for light DOC in aluminum.

[crabbass]

Speaking of choosing collet size series, is it best to choose the smallest series that will hold the tool size in question? For instance, an ER11 collet will go up to 1/4". Is it best to use an ER11, ER16, ER20, ER32 for holding that 1/4" endmill?

In general the shortest, is best. As far as diameter is concerned, if you are using a ER11 you have the maximum radial clearance, with the minimal radial strength. The ER32 is the stoutest option for radial support, but because the collet is so large, the tool holder has to be a little longer, and collets FLEX! Having the large collet nut associated with ER32 holders is sometimes a pain as far as clearance goes.
What I was getting at when I said I thought it was large, is with a 2-20mm range suggests you were planning to use up to a 3/4" tool. This would be a poor holder choice for milling with a 3/4" endmill. If you are going to use 3/4" endmills, get a power milling chuck.

[TravisR100]

Crab, again thanks. Good information. I'll keep this in mind when ordering toolholders. Yeah, I saw the milling chucks but just didn't really understand their purpose. It seems like you'd use the ER32 for up to about a half inch and then end mill holders for anything larger.

[Matt@RFR]

Travis, it just all depends on the situation. Normally for roughing, I hold 1/2" endmills in an ER-32. Let's say, though, that you've got a small pocket that is 1" deep to rough with a 1/2" endmill hanging out 1.25". Coolant access will be a problem, so I would go with an ER-25 and slow my roughing feeds down a bit.

That's a fake scenario just to get you thinking about it. In actuality I would use a solid endmill holder. I have 45 tool holders for my VF-2ss, and I'm always buying more.

[gpcoe]

I have an 1/8 running 12k @30ipm .8 out of holder in a REGO-FIX PG holder cutting 2024 aprox .5 deep. Using the in house cutters I couldn't get above 2000 RPM or so without chatter and surface finish and cycle time suffered greatly. I ordered an Accupro end mill 1/8 in 2 fl 45 deg helix endmill and was able to ramp the spindle up to max with a fantastic finish. I've used the same brand 3 flutes that solved several other issues with some of our in house tooling on the same part. Cut a one hour, fifteen minute cycle to less than forty-five minutes. Collet holders are a must on small tools at high RPM. Lack of concentricity will cause chatter and the small tool body doesn't have enough mass to damp out the vibration. I've had great luck with the PG holders as far as concentricity. Most indicate zero with a .0001 indicator. Flutes are subject to manufacturing error. Unfortunately their not cheap. I've tried to get the people in power to get some more, but they cry about cost. Anyway, don't ignore the cutting tool in the equation.

Greg

[fattybean]

IMO your feed rate is way too slow for your rpm, I would try about 7000 rpm with a feed rate of 50-60 for the finish pass(may be too aggressive for roughing). And choke up to the flutes of the mill whenever possible.