Need Help!- Feeds and Speeds for small endmills

[flathead]

Any suggestions for machining 6061 aluminum with small (1/16") 2 flute carbide endmill? During my first attempt with such a small cutter, I have just broken the only two that I had.

I know that endmills this size need to be run much faster, but my mill is limited to 3600 rpm. I used the feed and speed calculator in Mach3 to determine the cutting conditions I used. The first one broke @3600 rpm, 36 ipm, .031" doc. I assumed the doc was too much so I tried 3600 rpm, 16 ipm, .015" doc, but it broke too. Both broke on the first pass while cutting a 1" square.

Considering my rpm limitation, what should I try next?

By the way, I made some cuts with an 1/8" cutter @ 3600 rpm, 36 ipm, .031" doc with no problems at all.

[dertsap]

your chip load is way too high

these are the speeds we suggest for the CGS standard mills which is pretty standard for any carbide in the same ballpark ,for aluminum 600-1300 sfm with a chip load of .0002-.002 (for up to 1/4" ) , generally if your in the midpoint for a chip load then you should be fairly safe

[Glacern]

I'm somewhat surprised that you were able to feed the 1/8" cutter at 36 IPM (0.005 IPT). That's about as fast as you'd want to go with a 1/4" endmill.

I'd take it way down to 4 IPM for the 1/16" EM. You should be able increase your DOC to 1xD (about 0.063) without any problems.

-Sol
Glacern Machine Tools

[flathead]

Thanks for the replies. What you are saying makes a lot of sense. I'm still very new to machining and so far feeds and speeds have definitley been the hardest part for me to get a good grasp on. I've been relying on mostly on the speed and feed calculator within Mach3 to determine my settings, but I'm finding that the suggestions it gives me are not always usable.

Does anyone know of a speed and feed calculator that takes cutter size into account? (ie when you input a cutter size of .0625", then it will suggest a more reasonable IPT) The default in my Mach3 is .005.

Also, what about the fact that suggested SFM for aluminum is 600-1300 and I am limited to 3600 rpm on my mill. The rpm limitation means that I can only achieve 59 SFM with a .0625" cutter. What effect does the very low SFM have on my IPT or other settings such as DOC?

[vanm]

I found this web page to be pretty useful as a starting point. http://www.whitney-tool.com/html/cal...SpeedFeed.html

[flathead]

Vanm,

Thanks for the reply. But, Mach3 has a speed and feed calculator built in already. That's what I've been using. I guess what I need is some good guidelines to prevent a dummy like me from entering bad information into the calculator. The calculator can only put out information as good as the information that is put into it.

thanks again

[Andre' B]

When you are not sure set the feed per cutting edge at 0.5% of the tool diameter, works well enough for most jobs.

[flathead]

OK, I haven't been able to put any of your advice into practice until today when I received 3 new 1/16" carbide 2 flute bits from the UPS guy. I just managed to break 2 of them tonight. I'm not about to try the third one until I get more advice.

After my last post, I went back and adjusted my settings based on what I learned here. Tonight my settings have been set to the following: spindle speed is still 3600 rpm (can go no faster). Feed rate is set way down to 7 ipm. This is based on ipt of .001. (I have attached a couple screen shots of my settings and my g-code).

Both times tonight the bits broke while the cutter is engaging the cut (ramping in). I'm ramping the bit down just like I do with any other cutter. Its only plunging at 5.2 ipm. What now? I can't believe I'm still having problems with this.

I only have one bit left. I need to get this job finished. Any help is appreciated.

thanks

ats5-4.txt

[extanker59]

In my experience, carbide doesn't cut with the same feed per tooth as HSS. My charts only go down as far as 1/4" (says "up to") and it says .0002 to .002. for carbide endmills in aluminum. I'd go down to .0003-.0004 per tooth and no more than .03 DOC. Max your RPM (3600?) The smaller the cutter, the more important it is to minimize run out. Very important!
Make sure that there is plenty of coolant in the cut.

[Andre' B]

This is what I would do at this point.

Set your feed rate to 3.5IPM, set the Z step to 0.010", and cut your ramp angle to about 25% of whatever it is.

Next I would look for a spindle speeder or side mount high speed spindle, etc. for the next job of this sort.

Plotting your code it looks like your first pass is at Z-0.0625, then the second and third are each 1/32 steps down.
Also looks like the ramp for each starts at Z0.0312, I would look for a way to drop that down to about 0.003" and make it incremental from the previous pass, saves a little air cutting time.

Edit:
And ya, make sure the runout is less then about 30% of the feed per tooth.

[flathead]

Well, I'm 0 for 5. Number 5 broke @ 2 ipm

I suspect runout may be my problem. My mill is set up with an NT30 taper spindle. Normally I use holders for all my tooling. But my smallest holder is 3/16", so for these small bits I'm using an 1/8" ER40 collet. Just now, I flipped the last broken bit around in the collet and let it protrude about an inch. I measured .003" (+.0015 -.0015) of runout with my super-accurate Chinese dial indicator.

What I'm trying to cut out is a logo for a valve cover for a car going to the SEMA show in Las Vegas next week. I think at this point I'm going to have to start over and make the logo bigger so that I can cut the entire thing out with an 1/8" bit (hopefully I can scale up the logo and still make it fit). For some reason, I seem to have no trouble at all running the 1/8". Interestingly enough I'm running the 1/8" bit in the exact same collet.

I guess I'll have to make an adapter that will allow me to mount a high speed spindle to the mill or better yet, never accept another job that requires a bit smaller than 1/8".

[Cartierusm]

You have everything you need to do it correctly. Firstly don't try to go to fast, with a 1/16" bit I would go 5 IPM and a depth of .005 and you MUST USE COOLANT, mist or flood, aluminum gums up bits like crazy. You should be using a 2 flute, which I think you are and go as fast as you can. My CNC only goes 3000 and I have no problem. Now the only thing that can go wrong is runout as others have suggested.