I've been having a good amount of success using my TAIG CNC to cut aluminum when I'm stepping over 50% (10IPM, 8000 RPM, 0.05" DOC with a 1/8" 2 flute end mill).

I need to make a series of cuts in the middle of a part where I will plunge straight down (cannot ramp), then traverse across the part. The main difference is that I'm using the WHOLE endmill to cut (so a 1/8" endmill is making a 1/8" wide pass). I've been having problems breaking endmills; the bit seems to be "grabbed" by the aluminum and, somehow, pulled down (the endmill is NOT moving in the collet, so could it be the z-axis? the part is well-fixtured).

Anyways, my question is how much harder is it on the mill & endmill to make this type of cut?

Thanks.

Plunging without a lead in is typically bad form, especially for smaller end mills.
I have been having good luck in steel and aluminum with some China made 3 flute end mills from 800 Watt on Ebay.
Dirt cheap. Maybe less than a couple bucks each. It don't hurt so bad when you break those.

I think what is happening is there is a build up in the tip of the endmill when plunging. Okay when done fast and rigidly, but not as good for slower feeds. Especially without coolant.

I am not following why you can't use a lead in though. Sheetcam can lead in even into an arc and then back up to start to clean out and go from there. That would seem to solve some of your trouble.

Lee - I can't use a lead in for the following reason: I have a 4" x 4" aluminum block. I need to make a 2" long cut in the middle of the block with the 1/8" endmill. So the only lead in I could do is a ramp, but my CAM software (BobCAD) doesn't have that functionality.

The plunging itself isn't the problem; the cutter usually makes about 75% of the distance on the first pass, then runs into trouble (seems to be getting caught up / pulled down by material)

drill where your going to plunge

Drilling the plunge is a good suggestion. Are you using any type ccolant or lube? If not, some WD40 would go a long way to helping out.

Ramp is actually what I meant when I said lead in. That is a common and critical function of a Cam software. If it isn't available in Bodcad/cam now, I have a suggestion for them on the next release. ;)

I think part of the problem could also be deflection. I do not have a taig, but it is conceivable that deflection in the column and vibration could cause this to happen.

You could do pretty well by using a ball end mill for all the roughing work, then tidy up with a regular end mill. Also, the high helix mills work wonders with plunge cuts because the material is extracted much more efficiently than normal with the same rpm.

Thanks. The problem is not the plunge, but rather once the cutter has made its well into the cutting path. I have the same problem if I lead in from the side (not a ramp, just a side lead in) on a cut that starts at the edge. Once again, I'm wondering how much "harder" it is to cut using the FULL width of the endmill versus the "normal" process where you're just using ~50%. I suppose you could say I'm climb milling and conventional milling at the same time...

than cutting on one side only. Use your highest RPM setting, and cut the depth in half. The nice thing about CNC is that you can take small repeated bites; you don't have to cut the whole thing in one go. And if you can do this with a bigger tool, that's less likely to break. I'm assuming you are using plenty of lube/coolant, and you've got a grade of aluminum that is fairly machinable - some are just gummy, and tend to grab cutters. If you have a choice, get a known-machinable alloy that's had some heat-treating; 6061 T6 is popular. It sounds like this is pretty simple G-code; it's probably not that hard to edit in a ramp where you need it; just give it a combined X/Z move from a certain height. Also, 50% is a pretty hefty stepover -25% is easier on the tool.

Good Luck,

Andrew Werby
www.computersculpture.com

Well, if your making it most of the way through the cut, I would think it's a heat buildup problem due to insufficient lube or coolant. The flutes will load up, be unable to eject their chips and 'SNAP'. (that wonderful sound....) Does the sound of cutting change just before the tool dies?

Cutting the full width of the endmill shouldn't be a big deal. Whenever you pocket, the tool has to do this at least once anyways.

Maybe take a smaller DOC and see if the problem goes away.

Paul

If it's performing a significant part of the cut OK then it sounds like buildup on the cutter. Your feed rate maybe to fast or in fact to slow, you maybe recutting chips (a problem in blind slots so you need to keep them clear) or maybe you are using the wrong coolant.

Examine the cutting edges of the broken cutter for buildup under a magnifier.

10 ipm at 8,000 rpm maybe a tad fast. Try 8 ipm or rise the rpm to 10,000

What do you actually see that tells you the cutter is being "pulled in" Photo would help.

Cutting full width is of course a bit more tricky but not that difficult.

Phil

Thanks. The problem is not the plunge, but rather once the cutter has made its well into the cutting path. I have the same problem if I lead in from the side (not a ramp, just a side lead in) on a cut that starts at the edge. Once again, I'm wondering how much "harder" it is to cut using the FULL width of the endmill versus the "normal" process where you're just using ~50%. I suppose you could say I'm climb milling and conventional milling at the same time...