Milling issues with live tooling

Guess this will be my question of the day...

Live tooling on my Doosan Lynx. Trying to mill a profile on the end of an aluminum bar with mixed results. Yes, I'm getting it to cut, but it is squealing like a pig. Doesn't seem to matter what speeds or feeds I try, the finish is pretty bad. Everything from 6000rpm 50ipm to 4000rpm 25ipm...all different variations. Tried to just skim off .001" up to 25% tool radius. From full depth (.425") profiling, to steps of .15" deep. I used 3/8" aluminum specific endmills from Maritool, with .030" corner radius and ZrN coating (destroyed one of them). I've got only the flutes sticking out of the collet. Tried both my Heimatec and Eppinger live tools. Are the ER20 and ER25 collets just not rigid enough? When I run 3/8" on my mill I always put them in ER32's.

Am I just expecting too much with live tooling? I know rigidity isn't what a machining center would be, but this kinda sucks. Should I try different endmills? Bigger diameter? Endmill holder instead of collets? Variable flute? I need the .030" radius for a feature on my part. Not too many .030" corner radius variable flute endmills out there for aluminum.

As usual, I'm all ears.

Thanks,
Eric U

When you get squealing you should cut your speed, that normally seems to have better results than anything else. I know it sounds counter productive but try cutting your rpm by half...dont let the chip load get too high or your endmill will be shorter yet. I would wonder how stiff is the aluminum bar you are milling and how much of it is sticking out in the breeze?

Charles

CBlair said:

When you get squealing you should cut your speed, that normally seems to have better results than anything else. I know it sounds counter productive but try cutting your rpm by half...dont let the chip load get too high or your endmill will be shorter yet. I would wonder how stiff is the aluminum bar you are milling and how much of it is sticking out in the breeze?

Charles

Click to expand...

Charles,

I've only got 2" of bar sticking out of the chuck. This is the same 1-3/4" x 1/2" wall tube that I had in my video, but that one was sticking out 3.25". I was taking pretty big cuts with that facemill on that other part with no vibration issues at all. Is it just the side cutting endmill that is the issue?

Thanks,
Eric U

Is the main spindle locked during milling? C-axis holding power can be questionable.

Sol,

I'll give that a try tomorrow. I didn't have any issues with my other part, but I wasn't milling with the side of an endmill either.

Thanks,
Eric

Do you have any other tools? My go to for live tooling especially 30-35* helix endmills. MA FORD, Hanita, Helical, Melin.....

I don't have any other aluminum endmills with my needed .030" corner radius. I could get something overnighted tomorrow and have it by Friday...if I can get a consensus of what would work better than what I've got.

Thanks,
Eric

Also consider your chuck/workholding...

Milling tubing can be tough, easy to get a harmonic vibration started and hard to stop it, best luck I have had is to keep the feedrate up and the rpm down...not the only answer but it works.

Charles

Im in the you need variable flute high helix camp. Have you bored out the stock at this point?

Orange Vise said:

Is the main spindle locked during milling? C-axis holding power can be questionable.

Click to expand...

Will the live tools even run with it not locked or synced? I believe mine gives me an alarm if I forget to put the M command in.

Over time the components in the live tooling heads themselves start to break down and in my experience if you can't get good results, no matter what you try, the tool head itself has developed problems that need to be attended to. I've started rebuilding live tools myself and offer it as a service through my business, Metal Metal Worx. I suggest that you try everything else you can think off before having the head rebuilt, because it can get expensive. However, I try to keep my prices lower than other businesses that I've heard of that offer the same service. If your interested personal message me or go to my website at http://www.metalmetalworx.com

Hertz said:

Will the live tools even run with it not locked or synced? I believe mine gives me an alarm if I forget to put the M command in.

Click to expand...

Mine will run when the spindle is not locked, as will most. (can't do polar on the face with a locked spindle).

It does have to be synched though.

Hertz said:

Will the live tools even run with it not locked or synced? I believe mine gives me an alarm if I forget to put the M command in.

Click to expand...

They won't run if not sync'd but they will if sync'd but not locked (clamped), since the control doesn't know if you're cutting with a simultaneous rotary axis or just indexing.

Orange Vise said:

They won't run if not sync'd but they will if sync'd but not locked (clamped), since the control doesn't know if you're cutting with a simultaneous rotary axis or just indexing.

Click to expand...

Right, gotcha.

Well I tried everything everyone suggested. First I changed the order of operations so the profile milling was the first operation. I also made sure the spindle was clamped. I ran it with just those two changes first...no change. Next I cut the rpm in half and ran the endmill at the suggested .004" ipr. Helped but not completely fixed. I lowered the rpm to 2500 and that pretty much got rid of the squealing. However, now my cycle time is a bit too much for my liking.

So, I threw another axial live tool on to try the majority of the facing and all the profiling with a variable flute endmill. I would just do a skim face cut and profile the alignment tab with my .030 radius endmill. I had a couple of 3/8" Lakeshore Carbide variable flute endmills laying around so I gave one of them a try. This is the first time I ran this live tool, so I did a bit of a break-in on it. About 20 minutes, ranging from 100 to 6000 rpm. This is when I discovered an interesting thing...my Heimatec axial live tool runs backwards! Need M4 for them to cut correctly. That explains a lot. The endmill I destroyed yesterday was because I ran it backwards at 6000rpm and 50ipm. I thought it was because the collet nut unscrewed itself, but now I know the reason it unscrewed itself. I had the same problem on my Eppinger axial tool with the chattering 3/8" endmill if I didn't get it REAL tight so I didn't think to check anything else. Funny thing is I've been running my engraving tool in that same Heimatec tool backwards from the beginning. No wonder I had so much burr!

Anyway, success! The variable flute Lakeshore Carbide cuts like butter. 6000rpm contouring full depth (.425") at 50ipm just purrs.

Thanks for all the help,
Eric U

You have other live endwerking tool(s) that use M3?


-------------------

Think Snow Eh!
Ox

Yes. The Eppinger tool that came with the turning center uses M3.

We have ran into that before.....I think (not 100% certain so sdont beat me up) some of the live heads run backwards so that you can use an M3 depending on whether your machine is a twin spindle and you are running on the sub spindle.

Well I've never seen a face tool that ran CW on M3 before.
I guess it depends on which side of the bevel gear you mate with eh?


--------------------

Think Snow Eh!
Ox