[Terry G]

Going to try and keep this short and to the point.

Using a Haas Mini Mill and have been running the exact same program for almost 2 years. Have ran 1000's of these parts. Aluminum has always been purchased from the same place (6061 T6). Same mixture and brand coolant. Also, same clamping and fixtures as I have always used.

I run 4 small pockets and 4 .130" slots .185" deep in 3 steps (.062 each pass) in each part. Feed is 19.5 ipm, RPM 6000.

I used to use a pretty cheap brand 1/8" 2 flt carbide end mill and was pretty happy with it. Then I switched to a high performance SwiftCarb 2 flt end mill and was extremely happy with it. I ran over 1500 parts with it in the last 4 months. It cut very quite and left a great burr free finish. Then it finally broke. Figured it was getting old.

I purchased two more of the exact same end mills that same day. Stuck one in the same tool holder and collet, made sure it extended out of the collet the same and started up my program.

The tool broke in the middle of the 2nd pocket. Clean break right at the collet.

Took my second tool, used a different tool holder and a brand new collet. Started the program and the tool sounded very loud while cutting. I stopped the machine after 10 seconds or so and checked the cut. There was a HUGE burr for an 1/8" EM.

I pulled this tool out of the holder, stuck in another new collet just to be sure, ran the tool again, and the cutter broke after a few inches of cut.

Back to the local shop, purchased a cheap double sided SGS carbide 1/8" EM, stuck it in the same tool holder (2nd one) with yet another new collet, and ran another 100 or so parts and it is still going strong. Though even with this SGS EM, it is leaving a very large burr (right off the bat). But at least it is not breaking. I run a .002" chamfer on all my parts, so the burr goes away, but the cut is still much louder than ever before.

Couple questions:

1. Could it be my aluminum? I did try another piece from the last batch of parts I ran a few months ago, and it did the same thing.

2. Trying two different tool holders and 3 collets with the same results. Don't think it can be that

3. And all my other tools are cutting just fine. 1/2", 1/4", couple drills, and 1/4" 90 deg. chamfer. Clean cut and finish.

I'm focusing on the fact that I broke my old EM, then 2 brand new ones, and the 3rd new SGS is still cutting, but loud with a large burr.

Anything obvious here that I may be overlooking? Just want to get the clean and quite cuts again with an 1/8" EM. Not sure what else to try.

Thanks!

[davereagan]

I know you said same brand and mixture of coolant, but have you checked your coolant concentration with a refractometer? Are the endmills galling and then breaking or just snapping with no adhesion of aluminum to the flutes? Are you checking your endmill runout in the spindle with an indicator ?

[txcncman]

Are you absolutely sure all cutting conditions are the exactly same? Was feed rate override set the same as with the old tool? Are you aiming your coolant nozzle(s) exactly the same? When the tool(s) broke, was it pulled out of the collet causing the cut to be deeper than programmed? You said you changed collets, but a cracked collet nut can be a problem. Is the helix angle the same on the new tools as the old one? Different helix angle might mean different feed rate is needed. Are you using exactly the same work holding as before?

[a1diesinker]

#1 collet holders suck you have a big nut right in the way of the coolant
plus i'll bet it runs out aleast .0005 proably more use a tool holder.
#2 .06 deep with .0016 chipload thats with no runout is asking a lot of a 1/8 em
better have coolant right on the cut

[extanker59]

If you had an endmill break in a holder, the first thing I would do is check run out like others have said. I've seen the collets get ruined when the tool broke.
Rats. Just re-read your post. New collet and holder. Sorry. Ignore this.

[Terry G]

Thanks for all the quick replies.

Yes I do have a refractometer and keep the coolant concentration at the recommended 5%. I also run a skimmer every night to handle the oils.

The endmills are not galling, when they break, they are actually just sitting right on the part, so I have both of the new end mill broken ends and they look perfectly clean.

I did not check runout after I broke my 'old' 1/8" EM. Though I did replace the tool holder and collet.

All cutting conditions were exactly the same. We just ran through about 200 parts, the tool broke, pulled the tool holder out, replaced the tool, re-set the offsets, and continued with the program. The coolant nozzles were all completely flooding the cut as they have always been. I also checked that the overrides were not on. That was one of the first things I did!

No, the tool was not pulled out of the collet causing it to go deeper. For this particular tool, I had it measured exactly to accommodate the depth of cut, keeping it as short as possible and still allowing full coolant to flood the cut. And when I put the broken piece back together it was at the same length.

Same exact work holding, and same exact tool (manufacturer and part number). I definitely play with the feeds on my different brand tools, but I had this one dialed in perfect. Could barely hear the cut and left perfect edges (no burrs) before the old one broke.

I understand the drawbacks of collets, but I have been running this same setup for almost 2 years and thousands of parts without any issues using the same DOC and chipload. So it has been working for me. Something changed, and just trying to figure it out.

It really seems like I am all of a sudden pushing the tool to hard. I don't know if my old faith-full 1/8" EM broke because it was old (though the cuts still looked excellent right down to the last part), or if something went wrong with the setup. Which would indicate why I broke the next 2 EMs instantly, and even the 3rd SGS brand EM I am using is not cutting that great. Though it does not have a high helix cutting angle which may make it stronger.

After reading these replies and the talk about run-out I have one other thought I overlooked. There is a good chance that something could be stuck up in the spindle causing some run-out. I do wipe it every time I change tools, but maybe it is something really stuck.

It could be such a small run-out that my larger tools are not affected by it, just my 1/8" EM. Could be why I broke tools with 2 different tool holders and collets.

First thing I'll check the run-out on all my tools and see how much they vary, especially the 1/8" EM. Then I'll see if there is anything in my spindle and re-check run-out.

It really feels like something just went bad in the middle of running parts. Also noticed that when the first EM broke (my old one), it broke right at the beginning of that operation, just like the other two new EMs! Tool went into the tool holder, then broke really quick after that. So I am hoping it is simply a chip or something in there. Kind of makes sense I think.

Thanks again for all the replies. I'll post back what I find.

[txcncman]

Are you plunging into the slot? What feed rate? Have you tried ramping instead?

[Terry G]

Yes, I'm plunging into the slot at 9.5 ipm. It's just a 2 flute cutter. I do ramp on some of my other 3 flt cutters, but this program has been working for years on thousands of parts without any issues.

[txcncman]

Understood. For years. On thousands of parts. But you have no clue as to what changed.

I would venture that 9.5 IPM for a 1/8" diameter end mill is too fast, even if you were turning 10k RPM. I never plunge any end mill faster than about 4 IPM. That is because I do not like when they go POP. How you got away with it for years and thousands of part, I have no idea. Plunging with an end mill is basically the same as drilling with a flat bottom drill. How fast would you feed a flat bottom drill?

You can keep asking why, or you can change something and get back to making parts. Your choice.

[Terry G]

I appreciate all the great feedback and definitely take everything into consideration. You are very correct, I do not know what changed.

In general, if I were plunging too fast into the material would I except the cutter to break during the plunge, right after the plunge at the start of the cut, or well into the cut? Or any of the above? And would I notice anything on the edge of the cutter that would indicate I was plunging too fast. I do have the two new cutters I snapped for inspection.

Machine was down for 30 minutes or so and has continued to run over the last few days. I'm just not 100% satisfied with how this SGS cutter is cutting, and I don't want to snap any more of those $18.00 single ended high performance aluminum cutters. The cut looks OK, but leaves a burr and sounds loud while cutting. Chamfer tool cleans up the burr just fine, so the end results are perfect. But still something is a little off while cutting. Just want to figure out what caused those 3 cutters to snap in a row. Looking at the runout right now of my tool holders and tools.

Thanks again for the feedback.

[Terry G]

Checked the run out on a number of my tools and empty tool holders.

First I looked at the inspection sheets of the tool holders (for what it's worth) and saw the run out for inside the collet seat is better than .00018". And the run out at 1/2" from the collet with a 3mm end mill is better than .0006". (not sure how they check that)

I checked the run out right above the flutes while in the holders on my machine.

1/2" EM .0007" run out
1/4" EM .0015" run out
1/8" EM .0012" run out
1/4" chamfer top next to collet .0011", and at 1" length .0013"

I then checked two other tool holders without tools plus my 1/8" holder after removing the tool and measured the inside of the collet seats.

I measured from .0002" to .0015". This was on the same holder simply removing it and sticking it back in again. This is where I was a bit puzzled.

I carefully inspected the spindle and it looked great. And all the holders are carefully cleaned and inspected before putting into the spindle.

I have my indicator in a solid base right on the table and touching off on the tool holders / EM very carefully, so I am sure the measurements are accurate. But I'll probably pick up another indicator just to be sure.

[Machineit]

Contrary to what a lot of people here just love to say, collets are not the accurate way to go, good tool holders are.

Don't mean to start another big debate, but the truth is the truth.

Mike

[Terry G]

No debate necessary. I'm sure there are a lot of different ways to run the machine better and with more time and money it would be fun to experiment and get that optimal setup.

Until 3 days ago, the machine was cutting excellent with an 1/8" EM. Something changed and now it is a little less great sounding (louder), but still cutting just fine with a bit of a burr.

Larger diameter tools still leave a perfect finish. I run my 3 flt 1/4" Iscar at 56ipm and .100 DOC and the finish is really nice. Been using the same tool for over 6 months! I inspect everything with a 10x magnifier, and can see the flute marks, but with the naked eye it has a nice polished finish.

I could definitely switch to an 1/8" EM holder, which may have better runout, but I also don't want to mask a potential problem I may have.

I'm going to look into the spindle a bit more. Maybe check the runout of the actual spindle which I forgot to do. I'll take one step at a time and hopefully make some sense of it!

Once the problem is fixed (as minor as it may be), then I can for sure look into better holders, etc... Always want to improve our parts where I can.

Thanks!

[davereagan]

I have a feeling your first endmill had a much better than average gash/center cutting feature which tolerated a really high plunge rate all this time. Also, 5% is low concentration for aluminum in my experience, although you said the endmill is not galling. I have had 3/8" endmills gall, then I cleaned it up, increased my coolant concentration and everything was great. Is your coolant a full synthetic, semi, or soluble oil? Aluminum likes real oil. I would like to compliment you on your thoroughness in describing the problem and as many paramaters as possible so we can help. Sometime it takes a week to get all the info from a guy.

[Kenny0529]

Maybe try to pre drill a hole to get rid of the plunge and extend your tool life???? If that's an option for you. Also a good tool holder would be a suggestion. Take your collet out and look for bugs in or on it. Is the spindle making more noise than usual? Maybe years Of use have loosened up your bearings a bit even if it is still running quietly

[Terry G]

Thanks again for the quick replies.

Yes, I am using a soluble oil, and have never had any issue with galling on any of my tools. 5% is the recommended mixture ratio, and I keep it very close. My tools last a really long time, at least what I think is a long time. I keep track with number of parts machined. My last 1/8" EM went a good 4 months with well over 1500 parts until it snapped running at the same DOC, plunges and loads as previously described. And I am now pretty sure it snapped because of a machine issue, not because it was worn. I lost the piece when it snapped so I couldn't check it. The final cuts before it snapped looked really good. My 1/4" and 1/2" are much older and no signs of needing new ones. I have had the same luck with other brand tools as well, not just the ones I'm using now.

I see that I may need to improve on my plunging techniques, which I will take into consideration, though I don't feel this is the issue here.

I spent some time with the Hass technician and ran a number of tests on the spindle. So far the spindle runout is perfect and right at spec at just under .0002" (measuring at about 10 spots inside the spindle). I also did the pull test where you pull on the tool holder at the collet, and it was within .0005" again right where it should be.

Next step is to test the spindle drawbar force. Now I'm stuck. Can't find a gage locally, so I need to get a service rep in and have them check it. 2 hours of driving to get to my place plus the standard service fee. Oh well. Guess I have to get it done!

The reason I feel it may be something in this area is because I can take a number of tool holders, stick them in the spindle, measure the runout in the collet seat, which has been around .0008" or worse and way out of spec. Then remove the tool, and stick it right back in again, and it will change up to .0015" of runout. I can go in and out with the tool holder keeping everything else consistent (table not moving, indicator not moving, just the Z axis going up and down and always to the exact Z height as before.) and the reading will vary on the same tool holder.

I did spend some time cleaning and polishing the spindle just to make sure I couldn't find anything obvious in there.

When I checked the runout of my tool holders yesterday, I found one that seemed to be a little better than the others. So I actually took my 1/8" EM and stuck it into this holder. This definitely made a difference on the cut. So I know I'm going in the right direction and my issues are with excessive runout.

The Haas tech also said all the runout measurements I was taking on the tool holders was some what invalid until I get the drawbar pressure checked, which makes sense. If the tool is not going up all the way, I will get a different reading.

But maybe that one tool holder was newer than the rest and happened to seat a little better? Who knows, just guessing right now.

Thanks again and I'll post back what I find out in hopes it helps other users in the future.

[haastec]

Next step is to test the spindle drawbar force. Now I'm stuck. Can't find a gage locally, so I need to get a service rep in and have them check it. 2 hours of driving to get to my place plus the standard service fee. Oh well. Guess I have to get it done!

You might check pricing of the gage. With what you will spend to have someone check it, you might be better off putting that money towards a gage you can have on hand and check at any time.

Some other food for thought is the torque value of the pull studs. There are several posts here about the effects of over torquing them in regards to runout.

[Terry G]

Ya, I looked at a few gages and they were all around $1000.00 or more once you purchased all the pieces. Service call will be about $300.00. I think that covers 1 hour of labor plus the 2 hours of driving. I have a call in with them just to make sure.

I'll keep looking for gages, maybe I can find something less expensive.

I did read about the torque on the pull studs. That is definitely something too check. I've been using the same holders and pull studs for about 2 years. But I guess things can change over time. I'll pull out the studs and re-torque them.

Thanks.

[Delw]

Terry
might want to change all your pull studs. I have had problems over the last 8-14 months on small dia stuff as well. changed the pull studs and problems vanished. These are parts that I have ran for 10+ years.( in fadals and haas)
One of my endmill holders I replaced and havent broken a endmill yet and there 1/32. I was breaking one about every week or so. for the last 2 months.
Also on collet holders and small endmills if you change them alot over the years they wear causing problems. stick with HIGH QUALITY collet holders Like kenmetal most of the ones us shop tools sell dont repeat after a few years including parellac(sp)

Pulling out the studs and putting them back in wont make any difference, as they are already bent/used, there throw away items. get new ones and make sure there quality ones. Pull studs are a important part for small endmills that I been finding out.

funny thing about pull studs. My vf2ss wouldnt cut alum with out chatter on long endmills in 1/2" dia above 1000 rpms. I tried a ton of different tool holders. Talked to a guy on here that sells pull studs and figured WTF I will try it. Popped one on and I am cutting alum at 10,000- 12000 rpms 50+ ipm with out chatter now. 1.5-2.25 depth of cuts .050- .075 side cuts.
you can even hear the difference in unclamping with different pull studs.
My machine is a 2009
Delw

[Terry G]

Hi Delw,

Thanks for the great info. I actually have an appointment on Oct 12 for the Haas service guy to come and check it out.

Next week I will go and buy a couple new pull studs and do some quick before and after measurements. I do replace collets every once in a while. Though the runout I am measuring is right inside the tool holder collet seat, so I'm removing the collet and tool from the equation.

But if the pull stud were not perfect, I can see why my runout would vary every time I stuck the tool holder into the spindle. Sounds much better than having a problem with the drawbar pressure! This could also explain why I stuck my 1/8" EM into a different less used tool holder, and it ran better!


I'm out of town this weekend, but next week I am going to try the pull studs. If I can get one or two of my worst holders to run true, I'll cancel my appointment with Haas. Would be way cheaper to buy all new pull studs if that solves the problem!

Thanks again.