What's new
What's new

Breaking 1/32 end mills in 6061-T6

604Pook

Hot Rolled
Joined
Sep 14, 2022
Location
BC CANADA
Having some issues with breaking .0312 4 flute and 0.0394 2 flute end mills in 6061 t-6 plate. I am machining some small D shaped pockets, .04" deep that aren't much wider than the tools.

I am running this part on my Fadal 4020, 10,000 rpm spindle. I do very similar jobs in brass, and I can run these end mills full depth of cut .04-.06", 12ipm, 2ipm on the plunge at 10,000 rpm for many many parts with no issue with tool breakage. I have run similar aluminum versions of these parts in the past, and on a bigger part I may end up breaking an end mill or two doing the whole job.

For aluminum I usually drop the depth of cut to .02" and do it in steps.

On this job I got 1/3 through the part ( 150 little pockets approx.) and now have broken 5 end mills on the next 20 pockets. I didn't see any part of the broken end mill in the pocket after the first break, so I went back at it with the same parameters. Tool broke. I have adjust feed rate up and down, plunge rate up and down. Tried adding some rubber shimming to dampen any possible vibrations. I changed to a brand new tool holder and collet just to rule that out. I started pocketing from the other end of the job to stay away from the partial hole where it broke last time.

Any suggestions on feeds and speeds? Depth of cut? step over? things to try?
 
I would check the runout of the tool with a tenths indicator on the flutes. I had a job in the past making small parts with similar size tools in stainless shim stock and .0005" runout was the difference between making 400 parts or 30 parts. I was also doing this job in a fadal like you and I would indicate in the tool every time I changed it out. My spindle had .0003" runout normally and I would orient a cheap collet to even out the runout down to .0001" or less.
 
Domestic or Chinese aluminum? Had a similar mystery problem that I posted about elsewhere. Drilling and tapping holes in 1/2" square aluminum rail. It started breaking drills or taps randomly. Our suspicion is that it was recycled material that had contaminates in the remelt. Bought a new batch of domestic aluminum and didn't break another cutter.
 
Domestic or Chinese aluminum? Had a similar mystery problem that I posted about elsewhere. Drilling and tapping holes in 1/2" square aluminum rail. It started breaking drills or taps randomly. Our suspicion is that it was recycled material that had contaminates in the remelt. Bought a new batch of domestic aluminum and didn't break another cutter.

I will take a look on the mill stamps on the other piece I have when I head out to the shop to see if the current cutter survived.
 
I would check the runout of the tool with a tenths indicator on the flutes. I had a job in the past making small parts with similar size tools in stainless shim stock and .0005" runout was the difference between making 400 parts or 30 parts. I was also doing this job in a fadal like you and I would indicate in the tool every time I changed it out. My spindle had .0003" runout normally and I would orient a cheap collet to even out the runout down to .0001" or less.

I will see what I am getting for runout in the machine. Thanks
 
Last edited:
So l was able to finish the pockets with the tool I had in there, looks like the run out on the current tool is just a hair over .0001" My spindle is pretty new and is an upgraded model from ITS.

To bad I can't tell what the previous end mills that broke where. I am not going to touch this one as I got more work for it to do right now, but moving forward I will double check the run out.

I also had taken some aluminum blocks the same size that the material is resting on and added one layer of a cut up thin nitrile glove and wedged that in some space I had between the clamps and other blocks thinking maybe i had some vibration. Not sure if that helped at :skep:
 
Did you find the broken piece of cutter to check for chip welding?

No, couldn't find any of them. I am wondering if maybe one was buried in the pocket and broke the a couple of the other cutters. It's pretty tiny would be pure luck to find it.
 
How's your coolant flow and concentration?

Lot of coolant flow, 4 jets at it, concentration is at a 6 on my refractometer thing, should be around 4, but I was doing a lot of tapping last week and ran it richer.

Would it being richer cause issues? Tanks is still to full to water it down, unless I move some to the lathe.
 
What end mills? What you are doing shouldn't be difficult with the right tools. My go to for this size is Harvey. 3 flutes for aluminum and the shortest flutes to do the job.
 
What end mills? What you are doing shouldn't be difficult with the right tools. My go to for this size is Harvey. 3 flutes for aluminum and the shortest flutes to do the job.

Performance Micro Tools. I have had very good results with these end mills for years now. Just this current job I am having issues.

I spoke with them today and they told me some stuff to try as well as asking for the trace number on this batch I am using, and said to let them now how things go and that they would send me some new end mills on Monday free of charge. Great service, they are very helpful.
 
I run small tools like this in Aluminum molds all the time, my 2 cents.
runout, runout, runout
carbide quality? I use Harvey for this size, 3 or 2 flute uncoated, Aluminum geo.
you said "plunge" I don't ever plunge an end mill in material, but especially with tooling this small, ramp or helix.
as mentioned 12ipm is .0006 ipt, this is a little quick, more like .0003" especially if the cut path has any full width cuts even at the start.

2 cents
 
Performance Micro Tools. I have had very good results with these end mills for years now. Just this current job I am having issues.

I spoke with them today and they told me some stuff to try as well as asking for the trace number on this batch I am using, and said to let them now how things go and that they would send me some new end mills on Monday free of charge. Great service, they are very helpful.
Is the EM coated?

Regards.

Mike
 
I run small tools like this in Aluminum molds all the time, my 2 cents.
runout, runout, runout
carbide quality? I use Harvey for this size, 3 or 2 flute uncoated, Aluminum geo.
you said "plunge" I don't ever plunge an end mill in material, but especially with tooling this small, ramp or helix.
as mentioned 12ipm is .0006 ipt, this is a little quick, more like .0003" especially if the cut path has any full width cuts even at the start.

2 cents

PMT actually told me to raise my rate from the slowed down 10ipm to 12ipm.

I think it was maybe a case of run out in the old tool holder and collet, and possibly hitting a hidden chunk of the old end mill.

I ran for another 3 hours last night with the same end mill, and she is now going good on the next portion of the job.

I am definitely going to spend more time when running aluminum getting the run out better.
 
QT: (I ran for another 3 hours last night with the same end mill, and she is now going good on the next portion of the job.)

Is the tool life/fail chartable, and a number target made. Then resharpening?
do you visualiy inspect ends of new end mills, defects sometimes are easy to see.
 
QT: (I ran for another 3 hours last night with the same end mill, and she is now going good on the next portion of the job.)

Is the tool life/fail chartable, and a number target made. Then resharpening?
do you visualiy inspect ends of new end mills, defects sometimes are easy to see.
IMO nothing under 1/2" is worth resharpening (used to be 3/8", but the cost of quality cutters has come down). When you figure in the cost of sorting, packing, paperwork, shipping, comping in, and the fact that a resharpened tool almost never performs as well or as long as a new tool, it's cheaper to use a new tool.
 
50 ops then failures on almost every one, this points to the metal, all other parameters remain the same. I worked in both Ali and Brass manufacture and can assure you that even the best produces do get inclusions.
The risk is greater with extrusions than rolled products. I would change the metal and try again.
 








 
Back
Top